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Welcome to CivilKit CAD

CivilKit CAD is a parametric CAD application that runs in your web browser. You sketch on a plane, turn the sketch into a solid, add holes, fillets and patterns, and every step is kept in a history you can edit later. This page says what CivilKit CAD is, what it needs, how this guide is organised and where to look when something does not work.

What CivilKit CAD is

A part in CivilKit CAD is a list of features: sketches, extrudes, holes, fillets, patterns and so on. The list is the model. Change a dimension in an early sketch and CivilKit CAD rebuilds every feature after it. Nothing is baked into a mesh, so you can come back to a part months later and change it.

You can:

  • sketch with lines, arcs, circles, splines, text and more, and control the sketch with constraints and dimensions;
  • build solids and surfaces from sketches, and shape them with fillets, chamfers, shells, drafts, patterns and mirrors;
  • link dimensions to named variables and keep several configurations of one part;
  • put parts together in assemblies with mates, and make drawings from them;
  • measure, check and inspect a part, and run design checks against rules you choose;
  • import STEP, SolidWorks, SketchUp, STL, OBJ, GLB, 3MF, DXF and SVG files, and export STEP, STL, OBJ, 3MF, glTF and DXF;
  • drive the whole application from scripts or from an AI agent.

What it runs in

CivilKit CAD runs entirely in a current desktop web browser that supports WebGL. Nothing has to be installed.

  • The geometry kernel runs inside your browser. The built-in kernel is compiled to WebAssembly, so your parts are built on your own computer and stay there. If you want more speed you can instead connect to a kernel service running on the same computer. See The local kernel service.
  • Your work is stored in the browser and in files you save. The app keeps an automatic backup while you work, and saves parts as .ckpart files that you keep wherever you like. See Saving and opening.
  • It can be installed and used offline. See Install as an app and work offline.
  • One feature needs a Chromium browser. Listing the fonts installed on your computer (for the Text tool) only works in Chrome and Edge. Everything else is the same in any browser that runs the app.

How this guide is organised

Read the first two parts in order the first time; after that, use the guide as a reference.

PartWhat it covers
Getting startedA complete first part, a tour of the window, moving around the model, selecting, and settings.
SketchingStarting a sketch, every sketch tool, constraints and dimensions, offsets, text, and what to do when a sketch will not solve.
ModellingSolids, edges, holes, patterns, transforms, surfaces, bodies, variables and the feature tree.
Assemblies and appearanceAssemblies and mates, materials and colours.
FilesSaving, opening, importing, exporting and drawings.
Checking your workMeasure, inspect, checks and design checks.
Library and wizardsSample parts, parametric wizards and catalog parts.
AutomationScripting, the MCP server for agents, and the local kernel service.
ReferenceEvery command and shortcut, offline use, languages, troubleshooting, limits and a glossary.

Button and menu names are in bold; some bold words are run-in headings. Keys are written as Ctrl+S; on a Mac, Ctrl means the Command key wherever CivilKit CAD accepts either.

All dimensions are in millimetres. Angles are in degrees.

The kernel book

The geometry kernel and the part format have their own book, published beside this guide at /docs/cad/kernel/. You do not need it to use CivilKit CAD. Reach for it when you want to know exactly what is stored in a .ckpart file (the part format), how a program talks to the kernel (the protocol), or what a validation check or error code means (validation).

Getting help

  • Command search. Press F, or click Search commands in the top bar, and type part of a command’s name. Every command in the application is listed there with its shortcut. See The interface.
  • Tooltips. Hover a button to see its full name, its shortcut and a one-line description.
  • The Diagnostics tab. When an edit breaks the model, open the drawer (\) and choose Diagnostics. It names the feature that failed first, says why in plain words, and offers Undo this change. See Checks and diagnostics.
  • Troubleshooting. Troubleshooting lists the problems people meet most often, and Limits and known gaps lists what CivilKit CAD cannot do yet. If a sketch will not behave, start with When a sketch will not solve.
  • Library. Click Library in the top bar to open finished parts, bundled samples and the libraries you added, and take them apart. See The Library.

Who this guide is for

It is for someone who wants to model, import, export and check parts. You do not need to know how the application is built. If you have used another parametric CAD system you will find the ideas familiar (sketch, feature, constraint, history), and the tour in The interface shows where CivilKit CAD puts them.

Next

Your first part

In this tutorial you build a small plate: you sketch a rectangle, give it dimensions, extrude it into a solid, drill a hole, round one edge and save the part. It takes about ten minutes and uses the main ideas of CivilKit CAD. The steps assume the application’s default layout, with the ribbon along the top.

1. Start with a blank part

The application opens with a blank part called Part1, so you can start from it. If you have been working, click New part at the left of the top bar to get a fresh one (it is numbered Part2, Part3 and so on). The shortcut Ctrl+N exists, but browsers often keep it for themselves, so it may not work in a normal browser tab; use the button.

A blank part shows a card titled Start here that says “Pick a plane, then sketch on it.” It has three buttons: Sketch on Front Plane, Sketch on Top Plane and Sketch on Right Plane.

Double-click the part’s name in the top bar to rename it.

2. Sketch a rectangle

  1. Click Sketch on Front Plane. The ribbon is replaced by a single tab named Editing New sketch. The Line tool is already active.
  2. If the view is at an angle, press N (or click Look normal (N)) to turn the view square to the sketch plane.
  3. In the Draw group, click Rectangle, or press R.
  4. Click once to place one corner, move the pointer away, and click again for the opposite corner. A rectangle appears, drawn in blue.

The blue colour means the shape can still move. The chip in the Status group counts the degrees of freedom that are left, for example 4 DOF.

3. Dimension the rectangle

A dimension fixes a size. You will fix the width and the height.

  1. In the Dimension group, click Dimension, or press D.
  2. Click the bottom edge of the rectangle. A value box appears holding the length you drew.
  3. Type 60 and press Enter. The edge is now exactly 60 mm and a dimension label is drawn beside it.
  4. Click the left edge, type 40 and press Enter.

The rectangle’s sides were already kept horizontal and vertical when you drew it. Two freedoms are left: where the rectangle sits on the plane. They do not matter for this tutorial, but you can remove them. Click Fully define in the Status group. CivilKit CAD adds the relations and dimensions it needs to pin the rectangle down and reports how many it added. The chip then reads Fully defined and the lines turn dark.

If a sketch does not behave the way you expect, see When a sketch will not solve.

4. Extrude it

  1. In the Make group of the sketch tab, click Extrude. This finishes the sketch and opens the Extrude editor in the left panel.
  2. The solid appears as a preview. The defaults are Add (selected in the Operation control, next to New body and Cut), an end condition of Blind and a Depth of 10 mm. Leave them.
  3. If the solid grew the wrong way, tick Flip direction.
  4. Click the check mark (Confirm) at the top of the editor.

The ribbon returns to its normal tabs. In the feature tree you now see the Extrude, with its sketch tucked beneath it. Press 7 to look at the part from the Iso view, and Z to fit it in the window.

5. Add a hole

  1. Press Q to choose Face selection.
  2. Click the large flat face on one side of the plate. It lights up.
  3. On the Home tab, in the Create group, click Hole, or press Shift+H.
  4. A new sketch starts on that face with the Point tool active. Click once near the middle of the face to place the hole’s centre.
  5. Click the check mark in the Finish group (Confirm sketch), or press Enter.
  6. The Hole editor opens. The defaults are Simple, size M6, fit Normal and end condition Through. The editor shows the resulting Hole diameter.
  7. Click Confirm.

To move the hole later, double-click its sketch in the feature tree, change the point’s position or dimension it from an edge, and finish the sketch again. For several holes see Holes and threads.

6. Round an edge

  1. Press E to choose Edge selection.
  2. Click one of the four short edges of the plate, the ones that run across its thickness.
  3. On the Home tab, in the Modify group, click Fillet, or press Shift+F.
  4. The Fillet editor opens with a small radius (about 0.5 mm for this plate). Change Radius to 5. Leave Tangent chain on.
  5. Click Confirm.

The corner is now rounded. If you picked the wrong edge, click Undo in the Edit group, or press Ctrl+Z, and try again.

7. Save the part

  1. Click Save in the top bar, or press Ctrl+S.
  2. Your browser either asks where to put the file or downloads it. The file ends in .ckpart.

To save under another name, open More file actions (the three-dot button in the top bar) and choose Save as.

CivilKit CAD also keeps an automatic backup in the browser while you work. After a crash it offers Restore your last session. The backup is a safety net, not a replacement for saving to a file. See Saving and opening.

What you did

Each step is a feature in the tree on the left: the sketch, the Extrude, the hole’s point sketch and Hole, and the Fillet. Double-click any of them to reopen its editor and change a value. CivilKit CAD rebuilds everything after it. Try it now: open the Extrude’s chevron in the tree to reveal its sketch, double-click the sketch to reopen it, double-click the 60 label, type 80, press Enter, and finish the sketch. CivilKit CAD rebuilds the plate and every feature after it.

Next

The interface

This chapter is a tour of the CivilKit CAD window: the top bar, the ribbon, the feature tree and other side panels, the viewport, the status bar, the bottom drawer, command search, the Display menu and document tabs. It describes the default layout; Units and settings shows how to rearrange it.

Layout at a glance

From top to bottom:

  1. The top bar: file buttons, the document tabs (one per open part), the Part / Drawing switch, command search and settings.
  2. The ribbon: tabs of command groups, directly under it.
  3. The working area: the left panel (feature tree and friends), and the viewport. When you open a feature, its editor appears as a floating card over the viewport. The raw inspector panel on the right is off by default.
  4. The drawer (hidden until you open it).
  5. The status bar.

The side areas can be resized by dragging the thin handle between them and the viewport. Double-click a handle to reset it. Drag a panel to nearly nothing and it folds away. See Units and settings for the layout presets and Reset layout.

On a phone or tablet

The same app adapts to the screen. It chooses a layout from the window width and the pointer: a phone (narrower than 700 px, or a touch device whose short side is under 500 px), a tablet (narrower than 1100 px, or any touch device) or a desktop. Change it in Settings > Layout > Screen layout if the automatic choice is wrong for you; the choice is remembered, and your panel settings are not changed by it.

  • Phone. The drawing takes the screen: one slim bar at the top and one bar at the bottom, nothing else. The top bar has the file menu (new, open, save, export, library …), the title of the document (a dot after it means unsaved changes; tap it for the list of open documents and New part), undo, redo and more (search commands, Part or Drawing, rename, settings). The bottom bar has Tools, Tree, Properties and Diagnostics. Tools opens the ribbon as one strip just above the bar: the tabs as chips, then the tools of the chosen tab in a single row with their names that you scroll sideways; picking a tool, or tapping the drawing, closes it again. The tree, the properties (or the editor while you edit a feature) and the diagnostics open as sheets that share the screen with the drawing: the drawing shrinks to the room above the sheet and keeps its framing, so the model stays in view and updates while you change a value. A sheet that edits something rises to about 60% of the screen at most; the tree and diagnostics lists can go higher. Drag the handle at the top of a sheet to move it between its heights, drag it down to close it, or use its close button. When the on-screen keyboard is up the bars give way, and the sheet and the field you are typing in stay visible above the keyboard. Dialogs such as Samples and Settings fill the screen, and the Settings tabs scroll sideways.
  • Numbers on a phone. Every number field opens the digit keypad with a Done key. Fields that take a formula or a variable have an ƒ key beside them that switches to the full keyboard (and 123 back), and a ± key where the keypad has no minus. The label on the drawing (for example “Depth 20 mm”) is a button too: tap it to type an exact value in place.
  • Sketching with a finger. While a sketch tool is active, one finger belongs to the tool: press the first point (a circle’s centre), drag to size the shape with a live preview and lift to place it, or tap, then tap, as before. Two fingers pan and pinch the sketch view. A circle dragged out this way is selected with its radius field focused, so you can type an exact size. A touch the system cancels, or a second finger that lands, drops whatever the first one began. The bar above the bottom bar has Done, Cancel shape, Undo and Delete, because a phone has no Enter, Escape or Delete key. Points are picked from twice as far as with a mouse.
  • Tablet. One top bar row, the ribbon compact (tabs, then its tools) and the tree and the properties docked at the sides, as on a desktop but narrower. A single open document has no tab strip.
  • Touch on the model. One finger orbits (or draws, with a sketch tool), two fingers pinch to zoom and pan, a tap selects. One finger dragging the view cube turns the model; a tap on a cube face, an edge or a corner snaps to that view. The arrow ring around the cube has finger-sized buttons (44 px): four arrows that turn the view a step (hold to keep turning), two roll arrows and Home. On a phone it is open by default, 160 px square in the top right corner so the middle of the drawing stays clear; its menu button (three dots) hides the arrows when you want the room, and sets the step size. See Moving around the model. Putting a second finger down cancels whatever the first one began, so a pinch never selects or moves anything. Buttons are at least 44 px; the hide and suppress buttons of tree rows are always visible, since a finger cannot hover.

On an iPad

CivilKit CAD runs in Safari on an iPad, with a finger, the Apple Pencil, or both, and with or without a hardware keyboard.

  • Install it. Open the app in Safari, tap Share, then Add to Home Screen. It then opens full screen from its own icon and works offline once it has been opened online (see Install as an app and work offline).
  • Sketching with the Pencil. The Pencil works like a finger on the sketch tools: press the first point, drag to size the shape and lift to place it, or tap, then tap. A hand resting on the screen while the Pencil draws is ignored, and the Pencil hovering over (or lifting off) the drawing does not drop the shape you are in the middle of.
  • The value field opens after you lift. When a circle you dragged out is placed, its radius field opens on its own and the on-screen keyboard comes up with the number keys, so you can type an exact size at once; the same goes for the value of a dimension picked with the Dimension tool. For the other tools tap the field that appears next to the shape.
  • A minus sign. Where the number keys have no minus, a ± key appears above the keyboard (and next to formula fields) and changes the sign of what you have typed. Fields that take a formula or a variable have the ƒ key to switch to the full keyboard.
  • Updates. The installed app is mostly suspended rather than closed; when you open it again it checks for a newer version and, if nothing is unsaved or open for editing, reloads by itself and tells you “Updated to …”. With unsaved changes or an open edit you get a Reload note instead. Settings > General > Update automatically turns this off (see Updates).
  • Gestures. One finger orbits (or draws, with a sketch tool active), two fingers pinch and pan, and a long press does not select text or open a copy menu on the model. The page itself does not zoom when you pinch or double-tap.
  • Hardware keyboard. With a keyboard attached the desktop keys work: type a number while a sketch tool is waiting for a size and it goes into the first field (Tab moves to the next field, Enter confirms, Escape cancels, the arrow keys step the value), Enter and Escape finish and leave a sketch, Ctrl or Cmd with Z undoes, and the one-letter tool keys (L line, A arc, C circle, R rectangle, T trim; see Sketch tools) work as on a desktop.

The top bar

From left to right:

ControlWhat it does
New part (Ctrl+N, which a browser tab may keep for itself)Opens a blank part in a new tab, or in the current tab if that is still blank.
Open (Ctrl+O)Opens a part file.
Save (Ctrl+S)Saves the part.
Export (Ctrl+E)Opens the Export menu. See Exporting.
More file actionsA menu with Save as, Save geometry in file, Recover earlier versions…, Import STEP / STL / OBJ / GLB / 3MF / SolidWorks / SketchUp, Import SketchUp with hidden geometry and Rotate imported model.
LibraryOpens the Library picker: the sample parts and the libraries you added.
Part nameDouble-click to rename the part. A dot after the name means unsaved changes.
Part / DrawingSwitches the document between the model and its drawing. See Drawings.
Search commands (F)Opens command search.
SettingsOpens the settings dialog.

When a newer version of the application is available the bar shows a note with Refresh and Later. When your browser allows it, an Install button appears. See Install as an app and work offline.

Document tabs

On a desktop the open parts are tabs in the top bar, between the file buttons and the Part / Drawing switch. You can keep several parts open and switch between them without losing undo history.

  • + opens a new blank part after the current tab.
  • ×, or a middle click, closes a tab. A tab with unsaved changes asks Save, Don’t save or Cancel.
  • Double-click the active tab to rename the part. Right-click a tab for Rename, Close and Close the other tabs.
  • Drag a tab to reorder it. The ▾ button lists all open parts when the strip overflows.
  • Ctrl+Alt+1 to Ctrl+Alt+9 jump to a tab (9 is the last), Ctrl+Alt+T opens a new part and Ctrl+Alt+W closes the current one. Ctrl+Tab and Ctrl+Shift+Tab step through the tabs, but browsers reserve them and they may not reach the page in a normal tab; they work in the installed app.
  • Opening a file, a sample or an import uses the current tab if it is blank and a new tab otherwise.
  • You can have at most 32 tabs.
  • Switching tabs while a sketch is open finishes the sketch and keeps it.

Closing the browser page while any tab has unsaved changes makes the browser ask first.

The ribbon

The ribbon is a row of tabs; each tab holds groups of buttons. On the Home tab many buttons stand for a family of commands (the Surfaces tab and most of the Features tab show every command as its own button): the button shows the one you used last, and a small arrow, a long press or a right click opens the others. For example the Extrude button also holds Extruded cut.

TabGroups
HomeSketch, Create, Modify, Pattern, Edit
FeaturesReference, Create, Modify, Bodies (the commands in Reference, Modify and Bodies are plain buttons)
FrameFrame (Frame and Cut list)
Sheet metalRules, Create, Flatten, Export
SurfacesCreate, Edit (one plain button per command)
ViewViews, Display style, Appearance (lighting, background and Show), Workspace
SelectPick, Expand, Position
EvaluateMeasure, Surface analysis
AssemblyComponents, Review

The Frame tab is where the structural Frame tool lives: Frame builds a frame from a sketch of lines and a stock profile, and Cut list opens a drawing of it with the numbered pieces, the cut list and the bill of materials. On a phone the same tab is in the tool sheet.

The Assembly tab appears when the part contains inserted components, and opens by itself when you open an assembly.

Three things change the ribbon:

  • While a sketch is open the ribbon shows one tab, named Editing followed by the sketch name. Its groups are Select, Finish, Import, Make, Draw, Dimension, Constrain, Modify, Reference and Status. Select and Finish stay pinned at the left while the other groups scroll. See Starting a sketch.
  • While a feature editor is open the commands that create or change geometry are greyed out. Undo, Redo, view, selection and inspection commands stay available. Confirm or cancel the editor first.
  • A command that cannot run is greyed, and its tooltip says why: for example Fillet says “Select edges, or two or more faces, to round”.

The ribbon has two sizes, Full and Compact, and can be turned off, in which case you reach every command through command search. File commands are in the top bar, not on a ribbon tab.

The tool rail

The tool rail is a column of tools down the left edge of the view: the modelling commands without the ribbon. It is off on a first visit. Turn it on with Tool rail in Settings > Layout (the presets set it: Plasticity-style has it on, Classic ribbon and Minimal leave it off).

The rail sits directly against the left panel (the tabbed outliner, features and editor) and follows it: when the panel opens, folds or is resized, the rail moves with it. With a floating panel it sits beside the panel.

Folding the left panel

A handle on the edge of the panel and rail (a chevron, at least 44 px high on a touch screen), the panel button at the left of the top bar, and the [ key all fold and unfold the left panel; Side panel on the ribbon’s View tab does the same. The canvas takes the freed width. The choice is remembered on this device, and the fold animates unless your system asks for reduced motion.

When the panel is folded the tool rail shrinks to one narrow column of icons if it is your only tool surface (the ribbon is off, as in Plasticity-style); if the ribbon is on, the rail folds away with the panel. The handle always stays on the screen to bring the panel back.

Getting your tools back

The tools can never all disappear. A stored layout with the ribbon and the tool rail both off (other than Minimal, which shows a Show tools button in the top bar) gets the compact ribbon back when the app starts, turning one of them off in Settings while the other is off turns the other on, and Reset layout (in Settings > Layout, in the … menus and on the ribbon’s View tab) unfolds the left panel, restores the default sizes and brings the tools back. On a tablet the ribbon is never fully off while the tool rail is off too.

Undo and Redo on a tablet

On a tablet Undo and Redo are always on the screen as a pair of 44 px buttons at the top left of the canvas, above the tool rail, whatever panels are open or folded and also while a sketch is open; they grey out when there is nothing to undo or redo. A phone keeps them in its top bar.

Overlays do not overlap

Everything that floats over the model (messages, the new-version note, the busy indicator, hints, the start card, the selection modes, the sketch bar, the readouts) lives in one layer with named regions: notices stack downward from the top, between the tool column and the view controls; messages stack upward from the bottom, above the keyboard and any strip along the bottom; the view controls stay at the right edge. Items stack instead of covering each other, at most three messages show at once (the rest wait their turn, identical ones merge into one with a count, errors go first), each disappears by itself after a few seconds, and the layer respects the screen’s safe area and the on-screen keyboard.

  • Sections run down the rail: Edit, Sketch, Create, Modify, Frame, Surfaces, Pattern, Inspect, Assembly and Select. A section that would be empty in this build is skipped.
  • One cell per family. A cell shows the tool you used last from that family (the Extrude cell is fixed and always shows Extrude); the rest open from it with a long press, a flick to the right, a right click, or the triangle in its corner. The last tool is remembered per family and shared with the ribbon.
  • For selection sits at the top while something is selected: the commands that apply to what is selected, most relevant first, in the order of the right-click menu among the commands that can run now; commands that cannot run move to the end. Its memory is per kind of selection, so the tools you used on a face come back when you pick another face.
  • Button labels (Settings > Layout) switches the rail between Icons and text and Icons only (label on hover), as it does the ribbon.

While a sketch is open the rail keeps Edit and, when the ribbon is off, gains the sketch sections (Select, Draw, Dimension, Constrain, Modify, Reference); with the ribbon on the sketch tools stay on the ribbon. See Starting a sketch.

File, export, camera and display commands have no cell on the rail: they stay in the top bar, on the View tab and in command search.

Common problems

SymptomFix
There is no railIt is off by default. Settings > Layout > Tool rail
A family opens a tool you did not wantThe cell opens on the last tool of that family. Long press, right click or press the corner triangle to pick another
The rail is missing while sketchingWith the ribbon on, only Edit is shown there; the sketch tools are on the ribbon. Turn the ribbon off to carry them on the rail
A command you look for is not on the railFile, export, view, layer and display commands are not on it by design. Use the top bar, the View tab or command search (F)

The left panel

The left panel can be docked, floating over the viewport, or hidden. Press [ to show or hide it. When tabs are on (the default) it has these tabs. They are icon buttons in a row at the top of the panel, in the order below; the name of each is its tooltip, and the active tab also shows its name.

TabContents
OutlinerThe parts, mates and patterns of an assembly.
FeaturesThe feature tree, described below. While a feature editor is open it takes this place.
EditorThe editor of the selected feature.
CatalogShapes and library parts to drop onto the model. See Catalog parts.
VariablesNamed values and configurations. See Equations and variables.
ScriptA script box. See Scripting.
BodiesThe bodies of the part, with colour, opacity and finish. See Bodies and combining.

The feature tree

The tree lists the history of the part in build order. At the top are fixed rows: Material, Front Plane, Top Plane, Right Plane and Origin. Below them is one row per feature. A sketch that a feature uses is tucked under that feature.

  • Click a row to select it, Ctrl-click to add to the selection, Shift-click to select a range.
  • Double-click a row to open its editor. Double-clicking a sketch reopens it for editing.
  • Hover a row to see its buttons: Select in viewport, Edit, Roll back to here, the eye (Hide (view only) / Show), the pause button (Suppress (rebuilds) / Unsuppress (rebuilds)) and Remove.
  • A failed feature is red with its reason underneath. Features that fail only because an earlier one failed are muted and say “blocked by” the cause.
  • Drag the model is here marker to roll the model back to an earlier step. See The feature tree and history.
  • Use the search box to find a feature by name, type or id.
  • F2 renames the selected feature, Delete removes it, Ctrl+Shift+U suppresses or unsuppresses it, and Ctrl+G groups several neighbouring features into a folder.

The inspector panel

Opening a feature (double-click it in the tree, or use its pencil button) shows its editor as a floating card over the viewport, with labelled fields, drop-downs and sections. The left panel keeps the feature tree, so the Editor tab is not shown on a desktop screen. A phone and a narrow tablet keep their single panel or sheet for the editor.

The inspector is a separate column on the right that lists the selected feature’s properties as plain fields. It is Off by default. A layout saved by an earlier version had it docked; it is switched off once when you first open this version. To bring it back, set Inspector panel to Docked right or Floating in Settings > Layout. The Classic ribbon preset docks it. It shows only while a feature is selected.

The viewport

The viewport shows the model. Over it you find:

  • The view cube in the top right corner, with its arrow ring (turn, roll, home) and the Fit and projection buttons under it. See Moving around the model.
  • The Display button (an eye icon), described below.
  • The selection list at the bottom right when something is selected. See Selecting things.
  • On-canvas handles: arrows and dots you can drag to change a depth, a fillet radius, a shell thickness or a hole diameter. They can be turned off in the settings.
  • Notices and a busy indicator with a Cancel button when a rebuild takes long.

Right-click the viewport for a menu of the commands that apply to what is selected. With nothing selected it offers the three New sketch commands, Extrude, Extruded cut, selection commands and Fit.

If you turn on the Selection mode bar in the settings, a small bar appears at the top of the viewport with Auto, Face, Edge, Corner, Body, a Box select button and a filter button.

The status bar

The status bar runs along the bottom.

ItemMeaning
Ready / BusyWhether the kernel is working.
Hover nameWhat is under the pointer.
NoticesThe latest message, for a few seconds.
SelectedA summary of the selection, such as 3 faces, 12.4 cm².
Features, Faces, TrianglesSize of the part.
Cached viewShown while the stored view of a part is on screen during a rebuild.
Design check chipThe result of the last design check. See Design checks.
KernelShown only when you use the local kernel service. Click it to open the kernel settings.
Last rebuildHow long the last rebuild took.
ErrorsThe number of failed features, in red when not zero.
DrawerOpens and closes the drawer.
Licences, DocumentationLinks to the licence list and to this guide, at the right end of the bar.

In a sketch the bar also shows the pointer position on the sketch plane, the active snap, the Snap and Grid switches, the Zoom and the grid Spacing. Click Spacing to type a grid spacing; 0 or empty means automatic.

The drawer

Press \ or click Drawer in the status bar to open the drawer at the bottom of the window. It has five tabs:

TabWhat it shows
HistoryEvery edit as a step, with filters All, You, Agent and Failed. Click a step to go back to it.
DiagnosticsWhy a failed feature failed and what to try. See Checks and diagnostics.
InspectMeasure, mass properties, section view and interference. See Measure and inspect.
CheckDesign rule checks. See Design checks.
ConsoleRecent messages.

Badges on the tab names count entries; red means problems.

Press F, or click Search commands, to search every command by name, group or tab. Type a few letters, move with the arrow keys, press Enter to run the highlighted command and Esc to close. Greyed commands cannot run in the current state. Before you type, the search offers a short list of pinned commands: Iso, Fit, Undo, Redo, Samples and Workspace settings.

Command search is the one place that lists everything. If you cannot find a button, search for it. Commands and shortcuts lists the commands and their keys.

The Display menu

The Display button in the viewport opens a panel with these sections:

  • Style: Shaded, Shaded with edges (the default), Wireframe, Hidden lines removed and Ghost, with an opacity slider for Ghost.
  • Appearance: a colour and a material finish for the part, or for the selected component of an assembly.
  • Scene: lighting presets Studio, Flat, High contrast and Technical, Light strength, and Reflections.
  • Edge width and Silhouette outline, and the Background.
  • Surface analysis options. See Surfaces.
  • Show: switches for Edges, Sketches, Curves, Planes, Axes, Grid, Relations, Overall size, Threads and Design issues.
  • While a sketch is open, a Sketch section with Dimensions, Relation glyphs, Reference dimensions, Colour by definition and Constraints panel.

These settings change only how the part looks. They are never written into the part’s geometry.

Getting help

A round ? button is next to the name of whatever you are working with, so help is one tap away and matches the tool you chose.

  • In an editor or wizard. The ? sits in the header of the panel (Extrude, Fillet, Hole, Gear, Spring, Case, 3D Sketch and the rest), next to the name.
  • While you sketch. The ? sits in the Status group of the sketch ribbon (and on the sketch bar on a phone). It explains the tool you have active; with no tool active it opens the sketch overview.
  • Anywhere. The ? in the status bar, at the right, opens the contents of this guide.
  • From the keyboard. Press F1, or ? when no text box has the focus, for the tool or editor you are in.

The button opens a small card with the name, one sentence, and Open the guide. That link opens the matching page of this guide, at the right section, in a new browser tab (in the desktop app it opens in your default browser). Press Esc or tap outside the card to close it. Each button is at least 44 px square on a touch screen.

Next

Moving around the model

This chapter covers how to orbit, pan and zoom the 3D view, how to jump to standard views with the view cube, the number keys and the ribbon, how to switch between perspective and parallel projection, and how the display styles help you see what you are doing. None of this changes the part: navigation and display settings only move the camera and change how the model is drawn.

Mouse and keyboard

In the model view:

To do thisDo this
OrbitDrag with the left or the middle mouse button.
PanDrag with the right mouse button, or Shift + middle button.
ZoomScroll the wheel, or hold Ctrl and drag with the middle button (drag up to move in).
Orbit in stepsPress the arrow keys. Each press turns the view 15 degrees.
Pan in stepsPress Alt + an arrow key.
Fit the modelPress Z.
Open the context menuRight-click without moving.

The arrow keys work when the focus is on the viewport or the page, not in a text field or a panel, and not while a sketch is open.

In a sketch

While a sketch is open the left button is used for drawing and picking, so the other buttons navigate:

To do thisDo this
OrbitDrag with the right mouse button.
PanDrag with the middle mouse button.
ZoomScroll the wheel. The view zooms towards the pointer, so you can reach a small detail without panning first.
Square the view to the sketch planePress N, or click Look normal.

The view cube

The view cube sits in the top right corner of the viewport and follows the camera. It is a chamfered cube labelled RIGHT, LEFT, TOP, BOTTOM, FRONT and BACK, with coloured arms for the +X, +Y and +Z axes. It has 26 targets, and the one under the pointer (or under your finger while you press) lights up in the accent colour:

  • Click a face to look at the model from that side.
  • Click an edge (the bevel between two faces) to look from 45 degrees between those two sides.
  • Click a corner (the small triangle where three faces meet) for an isometric-style view from that corner.
  • Drag the cube to orbit the model.

Around the cube are the arrow ring buttons, in four groups you can switch on or off (see the menu below). On a phone only the left and right arrows are on to begin with, which keeps most of the drawing clear; a tablet and the desktop start with all four groups.

ButtonWhat it does
Four triangles (left and right: Turn left/right; up and down: Turn up/down)Turn the view one step. The model moves the way the arrow points, as it does when you drag that way: the right arrow brings the model’s left side towards you. Click and hold to keep turning.
Two curved arrows at the top corners (Roll)Roll the view clockwise or counter-clockwise about the direction you look. Click and hold to keep rolling.
Home (bottom left; Home)The isometric view of the whole model.
Menu (bottom right, three dots)The checkboxes Turn left/right, Turn up/down, Roll and Home switch each group on or off (a group that is off takes no room; with all four off only the cube and the menu button remain); Step sets how far one click turns the view (15, 30, 45 or 90 degrees, 90 by default). Look normal is here too while a sketch is open. The groups and the step are kept for this browser.

From a face view, four 90 degree steps in the same direction come back to where you began. From an edge or corner view, left and right keep the tilt of the view and turn it to the next side; up and down tilt the view and stop on the Top or Bottom view rather than turning the model upside down. Once the view is rolled, or on Top or Bottom, the arrows turn about the screen’s own axes. Dragging the cube or the model orbits from wherever the view is and takes the roll out again.

Turning, snapping and Home are animated; with the system setting for reduced motion they jump.

The Fit and projection buttons sit under the ring (beside it on a narrow canvas of a desktop window). The cube, the ring and these buttons are laid out so they never cover each other or the selection readout.

Standard views

The number keys jump to the standard views. They work when the focus is not in a text field and no sketch tool is using the keys.

KeyView
1Top
2Front
3Right
4Back
5Left
6Bottom
7Iso
ZFit (the whole model fills the window)

The same commands are in the Views group of the View tab, and in command search. The Views button shows the view you used last.

The standard views follow the camera’s up axis, not the names of the reference planes. By default Y is up. With Z up, Top looks down onto the XY plane. See below to change it.

Perspective and parallel projection

Click the projection button under the view cube’s arrow ring, click Projection in the Views group of the View tab, or press P, to switch between a perspective view and a parallel (orthographic) one. In a sketch, P is the Project edges tool instead; use the button there.

Up axis, orbit mode and orbit centre

Open Settings and choose the Navigation tab (or click Up axis on the View tab to switch the up axis quickly).

SettingChoicesWhat it does
Up axisY up (SolidWorks style) (default), Z up (Onshape, Fusion, Blender style)Which axis points up on screen. It turns the camera, the ground grid and the view cube.
Orbit modeTurntable (no roll) (default), Trackball (free rotation)Turntable keeps the up axis upright and stops just short of the poles. Trackball rotates freely and can roll or go over the pole.
Orbit aroundModel centre (default), Point under the cursor, SelectionThe point the camera turns about. With Point under the cursor the pivot is the point of the model under the pointer when you start the drag. With Selection it is the middle of the selected faces or edges.

The up axis changes only the camera. Parts, sketches, reference planes and exported files are exactly the same on either setting, and a part saved with one opens correctly with the other.

Display styles while you work

Display styles do not move the camera, but they decide what you can see.

StyleShortcutGood for
ShadedAlt+1A clean look without edge lines.
Shaded with edgesAlt+2The default.
WireframeAlt+3Seeing through the part. Hidden edges are drawn faint. You can still pick faces.
Hidden lines removedAlt+4A drawing-like view.
GhostAlt+5A translucent part, so you can see sketches and features inside. An opacity slider appears in the Display menu.

Choose a style in the Display style group of the View tab, in the Display menu on the viewport, or with the shortcut. Picking and hover work in every style.

To hide the body of the selected faces, or the selected sketch, plane or curve, press H. Press Alt+H to show everything again. This changes the view only and is not saved. To hide one feature from the tree, use the eye button on its row. The Show switches in the Display menu hide whole kinds of things, such as Planes, Axes or Sketches. See The interface.

The lighting presets (Studio, Flat, High contrast, Technical) and the background (Theme, Light, Dark, Gradient) are in the Appearance group of the View tab.

Tips

  • If you lose the model, press Z to fit it.
  • If you are used to a program where Z points up, set Up axis to Z up so the standard views and the orbit feel familiar.
  • Double-click a face to select the feature that made it and open that feature’s editor. Alt+click selects the whole body. See Selecting things.

Next

Selecting things

Most modelling commands act on what you have selected: a fillet needs edges, a shell needs faces, a hole needs a face. This chapter covers the four kinds of thing you can select (faces, edges, corners and bodies), how hovering and clicking work, how to select several things at once, how to select more of a kind with one command, and how a selection feeds a command.

What you can select

KindWhat it isKey
FaceA flat or curved surface of a body.Q
EdgeA line, arc or curve where two faces meet.E
CornerA point where edges end.V
BodyA whole connected solid or surface body.B

A body is a connected set of faces. Two solids that do not touch are two bodies, and a surface body is its own body. Bodies are named in the selection list as Body 1, Body 2 and so on, or Surface body 1; a body that has a name from a script or from the Bodies tab uses it.

Auto pick, and picking one kind

By default CivilKit CAD is in Auto mode: as you move the pointer, the corner, edge or face nearest to it lights up, and a click selects it. The selection takes the kind of what you clicked, and does not mix kinds.

To pick only one kind, press its key or choose it on the Select tab in the Pick group: Face, Edge, Corner or Body. Choosing a kind turns Auto off. The pick buttons are also on the optional Selection mode bar, together with an Auto button, a Box select button and a filter button. Turn the bar on in Settings > Layout.

Hover and click

  • Hover over something to light it up. The status bar shows its name.
  • Click to select it. The previous selection is replaced.
  • Shift-click or Ctrl-click (Cmd-click on a Mac) adds to the selection. To take something out again, click its Remove from selection button in the selection list.
  • Click empty space to clear the selection and close any properties panel.
  • Esc clears the selection. Deselect all (Ctrl+Shift+A) does the same.
  • Alt-click selects the whole body. The Select body command does the same without the mouse.
  • Double-click a face to select the feature that made it and open that feature’s editor.

A very transparent body is not picked by a click when something lies behind it.

Selecting several things

Box select

Press X, or click Box select, and drag a box in the viewport instead of orbiting. You can also hold Shift and drag from empty space without turning the mode on. Press Shift to add to the current selection.

  • Drag to the right for a window box (solid blue): it selects only what is fully inside.
  • Drag to the left for a crossing box (dashed green): it selects everything the box touches.

Box select works through the model, so faces hidden behind others are picked too. In Face mode it picks faces, in Edge mode edges, in Corner mode corners, and in Body mode whole bodies.

Select all, invert and none

CommandShortcutWhat it does
Select allCtrl+AEverything of the current kind.
Invert selectionCtrl+IEverything of the current kind that is not selected.
Deselect allCtrl+Shift+AClears the selection.

Select more

The Expand group of the Select tab, command search and the right-click menu all offer commands that add to the selection. They work on faces and edges. If one cannot run, its tooltip says why: Select something first or Works on faces and edges.

CommandFacesEdges
Select tangentFaces joined across an edge where they meet smoothly, such as a fillet chain.Edges that continue each other with a smooth turn.
Select parallelPlanes facing the same way (either way round), and cylinders with parallel axes.Straight edges with the same direction, and circles with parallel axes.
Select similarThe same kind of face with the same area (a cylinder also needs the same radius).The same kind of edge with the same length (a circle or arc also needs the same radius).
Select loopSwitches to Edge mode and selects the edges around the selected faces.The edges that join end to end around the neighbouring face.
Select connectedEvery face of the body.Every edge reachable through shared corners.
Select same sizeEvery cylinder of the same diameter and kind as the selected cylinders.

A toast tells you how many items were added.

Filters

The funnel button on the Selection mode bar opens switches for Faces, Edges, Corners, Bodies, Sketches and Planes. A kind that is off cannot be picked: its mode button is disabled, a box ignores it, and with Planes off a reference plane cannot be picked in the view. A badge shows how many kinds are off. Sketches is in the list but does nothing yet: sketches are chosen from the feature tree.

The selection list

When something is selected, a list appears at the bottom right of the viewport. It shows a count and one chip per item (Face name, Edge number, Corner position, Body number), each with a Remove from selection button. Clear empties it, and the arrow folds the list away. Hovering a chip lights that item in amber. Click a chip’s name to Show in tree.

The status bar summarises the selection, for example 3 faces, 12.4 cm², 2 edges, 14 mm or 1 body. Areas and lengths come from the displayed mesh, so they are exact for flat faces and close for curved ones. For exact numbers use Measure and inspect.

How a selection feeds a command

Commands read the selection when you run them. Greyed commands tell you what they are missing.

CommandWhat it needs
Fillet, ChamferOne or more edges, or two or more faces (then the edges the faces share). Corners count as the edges that end there.
ShellOne or more faces to leave open (Face mode).
HoleOne face, or an earlier sketch of points.
ThreadOne or more cylindrical faces, such as the wall of a hole.
Sketch on selected face or plane (S)One face, a reference plane, or a plane feature.
Draft, Delete face, Delete bodyFaces.
Pipe cutEdges, or faces whose rim is cut.
Move / rotate ballA body, a face, or a move feature. Edges and corners cannot be moved.
Linear pattern, Circular pattern, MirrorThe feature selected in the tree, or else the last feature.
MeasureOne or two faces, edges or corners.

With Tangent chain on in a fillet or chamfer, edges that continue the selected edges smoothly are rounded too, and the editor says how many were added.

The right-click menu changes with the selection. With a face selected it offers Sketch on selected face, Hole, Shell, Fillet, Chamfer, the patterns and the select-more commands. With edges it offers Fillet, Chamfer and the select-more commands. With a body it offers Select body, Move body, the patterns and Shell.

Faces from the tree

Hovering a row in the feature tree tints what that feature made. The row’s Select in viewport button picks those faces, and a folder’s Select all faces of this group picks every face its features made. In the other direction, hovering a face in the viewport marks the row of the feature that made it.

Next

Units and settings

This chapter explains the units CivilKit CAD works in and every setting in the settings dialog: theme and language, the layout of the window, sketching, navigation, the move ball and the geometry kernel. It also covers automatic backup, which has no setting.

Open the dialog by clicking Settings (the gear) at the right of the top bar, by choosing Workspace settings in command search, or from the Workspace group of the View tab. Changes apply at once. The dialog remembers the tab you used last.

All settings are kept in your browser, for this site only. They are not saved in part files, and they do not follow you to another browser or computer. Clearing the site’s data in your browser resets them.

Units

CivilKit CAD works in millimetres and degrees. There is no unit setting. Part files store millimetres, and sizes in editors and on the status bar are shown in millimetres.

You can still type a value in another unit. A number field accepts a unit after the number: mm, cm, m, in for lengths, and deg or ° for angles. CivilKit CAD converts it to millimetres. For example 2 in becomes 50.8 mm, and 1.5 cm becomes 15 mm. A field also accepts simple arithmetic and variable names, such as =width*2+3. See Equations and variables.

The grid Spacing field in the status bar accepts units in the same way, for example 0.25 in.

General tab

SettingChoicesDefault
ThemeMatch system, Light, DarkMatch system
LanguageThe languages installed.Shown only when more than one language is available. At present English is the only one.

The theme changes the colours of the whole application, including the viewport background when the background is set to Theme. See Languages.

Layout tab

The layout tab controls which parts of the window are shown. Start with a preset, then adjust.

SettingChoicesWhat it does
PresetPlasticity-style, Classic ribbon, Minimal, Custom (your own mix)Applies a whole set of the settings below at once. It shows Custom when your settings match no preset.
Panel sizesReset layoutRestores the default widths and heights, unfolds a folded or switched-off left panel and brings the tools back if the ribbon and the tool rail were both off.
RibbonOff (command search), Compact, FullOff hides the ribbon and relies on command search and the tool column.
Left panelDocked, Floating, HiddenWhere the feature tree and its tabs sit.
Inspector panelOff, Docked right, FloatingThe raw property column for the selected feature. Off by default: a feature is edited in a card over the viewport. Phones and narrow tablets ignore it.
Button labelsIcons and text, Icons only (label on hover)How ribbon and palette buttons look.
Left panel tabs (Outliner, Features, Assets, Editor)on / offOne list, or tabs. With tabs on, the left panel offers Outliner, Features, Editor, Catalog, Variables, Script and Bodies.
Tool railon / offA column of modelling tools down the left edge.
Tool palette in sketcheson / offA floating palette of sketch tools on the right edge while sketching. Off: the Sketch tab carries the tools.
Selection mode baron / offThe bar with Auto, Face, Edge, Corner, Body, Box select and the filters.
Bottom drawer openon / offWhether the drawer is open.
Direct-manipulation handles on the canvason / offThe arrows and dots you drag to change a depth, radius, thickness or diameter.
Floating panel opacity15 % to 100 %How see-through floating panels are.
Highlight line thickness1 to 8The width of selection and hover lines.
Backdrop blur0 to 30Blur behind floating panels.

The presets set the following:

Plasticity-styleClassic ribbonMinimal
RibbonOffFullOff
Left panelDocked, tabs onDocked, tabs onFloating, tabs off
Inspector panelOffDocked rightOff
Tool railOnOffOff
Selection mode barOnOffOff
Bottom drawerOpenClosedClosed

A first visit starts with a mix of these: the full ribbon, a floating left panel with tabs, the inspector panel off, no tool rail, no selection mode bar and a closed drawer. Because it matches no preset, the dialog shows Custom (your own mix). If you saved a layout in an earlier version with the inspector docked, it is switched off once when this version first opens; set Inspector panel to Docked right to bring it back.

Drag the handles between panels to resize them. The sizes are remembered. Drag a panel below its minimum and it folds away; the keyboard works too: focus a handle and use the arrow keys, Home and End, and Enter to reset. [ shows or hides the left panel and \ the drawer.

Sketching tab

How the sketch editor takes input. See Sketch tools and Constraints and dimensions.

SettingChoicesDefault
Infer constraints while drawing (Shift at a click turns it off)on / offOn
Line to tangent arcRest the pointer on the end, Keys and drag only, OffRest the pointer on the end
Values beside the pointerDimensions, Dimensions and positions, OffDimensions
Snap to the gridon / offOn
Keep the view when entering a sketch (Look normal squares it up)on / offOn
Auto look normal for new sketcheson / offOff

The Snaps menu in the Status group of the sketch tab holds the rest: which kinds of snap are on (End points, Centres, Midpoints, Quadrants, Intersections, Perpendicular, Tangent, On curve, the model snaps, Alignment guides and Grid), Add constraints from snaps, and Auto-constrain from guides.

The Up axis, Orbit mode and Orbit around settings. See Moving around the model.

Positioning tab

Settings for the Move / rotate ball. See Moving things: the move / rotate ball and handles.

SettingDefault
Snap distance (mm)10
Snap angle (degrees)15

Hold Ctrl while dragging a handle of the ball to move in whole steps of these sizes.

Kernel tab

The geometry kernel is the part of CivilKit CAD that builds solids. By default it runs inside your browser. See The local kernel service for how to run the faster service.

SettingWhat it does
Kernel to useBuilt-in (runs in this browser) or Local service (faster, runs on this computer).
Service addressWhere the local service listens. Shown with the local service.
Access tokenThe token the service printed or saved when it started. It stays in this browser only.
Test connectionChecks the address and token, and reports the kernel version, the protocol and the number of cores, or why it cannot be used.
Try the service againAppears after a failure.

Switching kernels reopens the open part on the other kernel. If the service stops or turns out to be a different build from the app, the built-in kernel takes over and a notice tells you. While the local service is selected, the status bar shows a Kernel chip: Local with a version, Connecting, or Built-in (service off). Click the chip to come back to this tab.

Messages

Messages from the app (a finished import, a refusal and the reason) appear once, in a stack at the bottom right. A long message wraps, with Show more for the rest and Copy for an error. A message stays long enough to read, pauses while the pointer is on it, and closes with x or Esc. The status bar shows only an Alerts count; click it to list the last 50 messages.

Backup and saving

There is no autosave setting. A moment after you change a part, CivilKit CAD writes a backup of every changed part to the browser’s storage, and again when the page is hidden. After a crash or reload the app offers Restore your last session, with Restore, Start new and Earlier versions…. Each changed part returns in its own tab.

The backup has limits you may meet:

  • It is capped at about 3 MB. A part larger than that is not backed up, and a notice says so.
  • If the browser has no room left, or does not allow storage, the notice says that too.
  • The undo history is not part of the backup.

Save to a file for anything that matters. More file actions > Recover earlier versions… lists versions kept in the browser from a few minutes ago.

Next

The Mac app

CivilKit CAD is also available as a Mac app (Apple silicon and Intel). It is the same program as in the browser, in its own window. It works offline, and your parts stay on your computer.

Download the .dmg from the Releases page of the project: the aarch64 file for Apple silicon (M1 and later), the x64 file for Intel Macs. Open it and drag CivilKit CAD to Applications.

The first start

The app is not signed with an Apple Developer ID yet, so macOS asks you to confirm it once:

  1. Open the app. macOS says it cannot check it or that it is blocked.
  2. Open System Settings > Privacy & Security, scroll to the message about CivilKit CAD, choose Open Anyway and confirm.
  3. From a terminal you can instead remove the quarantine mark: xattr -dr com.apple.quarantine "/Applications/CivilKit CAD.app".

On older macOS versions, right-clicking (or Control-clicking) the app and choosing Open also works. Newer ones no longer offer that route for an unsigned app.

What is different from the browser

  • Export and Save a copy open the system Save dialog. Open uses the system file dialog, and File > Open Part File does the same.
  • Double-clicking a .ckpart file opens it in the app.
  • The app does not update itself; download the new version to update. The version is at the bottom of Settings.
  • Online libraries (Poly Haven textures and environments) stay off until you turn on Use online libraries; the app contacts only Poly Haven for that.

Linux and Windows

There is no Linux or Windows app yet. Use the Install button in your browser’s address bar to install CivilKit CAD as an app from the web page.

Starting a sketch

A sketch is a flat drawing on a plane or on a face of the part. Extrudes, revolves, holes, sweeps and lofts all start from sketches. This chapter shows how to choose where a sketch goes, how to enter it, how to finish or abandon it, how to reopen it later and how to show or hide sketches.

Choose a plane or a face

Every sketch sits on one of:

  • A reference plane. A new part has three: Front Plane (the XY plane), Top Plane (XZ) and Right Plane (ZY). They are the first rows of the feature tree, below Material.
  • A plane feature that you made yourself with Plane (Features tab, Reference group): an offset plane, an angled plane, a plane through three points and so on.
  • A flat face of a body. Cylinders and spheres also work: CivilKit CAD makes a plane that touches the surface at the point you clicked and sketches on that. For any other curved face, make a plane first.

A body that was imported from STEP, SolidWorks or SketchUp is view-only. You cannot sketch on its faces, only on reference planes. See Importing.

Enter a sketch

There are several ways in; all of them open the same sketch editor.

FromHow
A blank partThe Start here card offers Sketch on Front Plane, Sketch on Top Plane and Sketch on Right Plane.
The ribbonOn the Home tab, in the Sketch group, click the sketch button. It holds Sketch on selected face or plane, Sketch on selected face, and New sketch: front plane, top plane and right plane, New sketch from DXF and New sketch from SVG. The button shows the one you used last.
The keyboardSelect a plane (click its row in the tree) or a face, then press S. If nothing is selected, the three origin planes appear in the view to pick from (see below).
Pick in the viewPress S with nothing selected, or use New sketch: pick a plane in the view (the Pick plane entry of the sketch button, also in the command search). Front, Top and Right are drawn as translucent sheets at the origin with the axes; the sheet under the pointer turns orange and shows its name. Click a sheet to sketch on it. You can also click a flat face of the part, or a plane you made yourself. On a touch screen, tap: a tap near a sheet’s outline counts, so an edge-on sheet is still easy to hit. Esc or Cancel in the bar at the top gives up.
The viewportSelect a face and click the Sketch on this face chip that appears over the viewport. For a plane feature the chip says Sketch on this plane.
The right-click menuWith a face selected, choose Sketch on selected face. With nothing selected, the menu offers the three New sketch commands.

When you start a sketch from a face, edges and faces you had selected are remembered. The Project edges tool can bring them into the sketch (see Offsets and references).

What you see inside a sketch

  • The ribbon changes to one compact row, the sketch bar, with one tab named Editing followed by the sketch name (a new sketch is called New sketch while you edit it). Its groups are Select, Finish, Import (Import DXF and Import SVG), Make, Draw, Dimension, Constrain, Modify, Reference and Status. Select and Finish stay pinned at the left while the other groups scroll. The tools are described in Sketch tools and Constraints and dimensions.
  • The Line tool is active, so you can start drawing at once.
  • The body is drawn faded, to a quarter of its opacity, so you can see the sketch in front of it.
  • Mouse buttons change: the left button draws and picks, the right button orbits, the middle button pans, and the wheel zooms towards the pointer. See Moving around the model.
  • The status bar shows the pointer position on the sketch plane, the active snap, the Snap and Grid switches, the zoom and the grid Spacing.
  • A small label beside the pointer says the same position (for example 5.61 mm, -7.13 mm), at the snapped point when a snap is active. It appears only for a mouse or pen, not for a finger, and goes when the pointer leaves the view. Turn it off with Show the pointer position beside the pointer under Sketching in the settings.
  • If the view is angled to the sketch, a Look normal (N) button appears on the sketch bar (it is not shown while the view is already square to the plane). Click it, press N, or choose Look normal in the right-click menu of the sketch, to turn the view square to the plane. Turn on Auto look normal for new sketches in the settings to do this automatically, and turn off Keep the view when entering a sketch if you want the view to square up whenever a sketch opens.
  • If Sketches had been hidden in the Display menu, they are shown again so that you can see what you draw.

If the ribbon is off, the sketch controls sit in a small bar at the top of the viewport instead. If you use the Tool palette in sketches setting, the tools are also on a palette at the right edge.

Finish or cancel

To do thisDo this
Keep the sketchClick the check mark in the Finish group (Confirm sketch), or press Enter when no tool is in the middle of a shape.
Keep the sketch and extrude itClick Extrude in the Make group. The sketch is finished and the Extrude editor opens on it.
Keep the sketch and revolve itClick Revolve in the Make group. The sketch needs a construction line for the axis; if it has none, CivilKit CAD says “Draw a construction line for the axis.” Draw one with the Centreline tool.
Throw away this session of editingClick the cross in the Finish group (Cancel sketch).

Esc steps out in stages. While a tool is in the middle of a shape, Esc abandons that shape. With a tool chosen but idle, Esc returns to the Select tool. With nothing chosen and nothing selected, Esc cancels the whole sketch, discarding what you did since you entered it. If that is not what you want, use Ctrl+Z to undo steps inside the sketch instead.

Undo inside a sketch (Ctrl+Z) steps back through the sketch’s own edits.

Switching to another document tab while a sketch is open finishes the sketch and keeps it.

Reopen and reuse a sketch

  • Edit it again. Double-click the sketch’s row in the feature tree. A sketch that a feature uses is tucked under that feature; the features that depend on it rebuild when you finish.
  • Use it again. Extrude and the other sketch-based commands use the sketch selected in the tree, or else the last sketch that no feature uses yet. If every sketch is already used, CivilKit CAD says so: select a sketch in the tree to use it again, or draw a new one (S).
  • Rename it. Select the row and press F2.
  • Delete it. Select the row and press Delete. If a feature uses it, CivilKit CAD refuses and names the features that depend on it.

Show and hide sketches

  • The Show section of the Display menu has a Sketches switch for all sketches, and Curves, Planes, Axes, Relations and Overall size switches for other helpers. Turning Sketches off does not delete anything.
  • To hide one sketch, click the eye on its row in the tree. This hides it in the view only; it is not saved. Alt+H or Show all brings everything back.
  • Select a sketch and press H to hide it.
  • Finishing a sketch while Sketches is off turns the switch back on, with a notice, so a sketch you just made cannot vanish.
  • Inside a sketch, the Display menu also has a Sketch section: Dimensions, Relation glyphs, Reference dimensions, Colour by definition and Constraints panel. These change only what is drawn.

Check

After you finish a sketch, the feature tree shows it. If you then extrude and nothing appears, the sketch probably has no closed outline. See When a sketch will not solve.

Next

Sketch tools

This chapter describes every tool in the sketch editor: how to draw lines, arcs, circles, rectangles, polygons, ellipses, slots, splines and points; how to trim, extend, fillet, chamfer, mirror, offset, pattern, move, copy, rotate and scale; how to project edges of the part into the sketch; and how to mark geometry as construction. Dimensions and constraints are in Constraints and dimensions.

Choosing a tool

All tools are on the Editing tab of the ribbon while a sketch is open, in the groups Draw, Dimension, Constrain, Modify and Reference. Select and Finish stay pinned at the left end while the other groups scroll between them, and the scroll arrows sit beside the tools rather than over them. They are also in command search while you sketch.

  • Several tools share one button. The button shows the tool you used last. A small arrow, a long press or a right click opens the family with names and keys.
  • Some tools have a single key. Press it while the pointer is over the viewport.
  • Select (in the Select group) returns to selecting and dragging. Esc also goes there when no shape is in progress.
  • A tool stays active after it finishes a shape, so you can draw the next one. Click Select or press Esc when you are done.
KeyTool or commandKeyTool or command
LLineDDimension
RRectangleHHorizontal
CCircleVVertical
A3-point arcTTrim
QTextEExtend
OOffsetXConstruction
PProject edgesNLook normal

Typing values while you draw

Most tools show small fields beside the pointer while you draw, labelled with short names such as len, ang, w, h, rad, dia. Each tool’s fields are listed in its entry below, in the order Tab visits them: Line len, ang; Rectangle and Centre rectangle w, h; Rounded rectangle w, h, corner; Circle rad, dia (either one ends the circle); Ellipse major, ang, then minor; Slot len, ang, then w. Type digits (or . or -) and the first field takes them; letters are not typed into fields, and with no field on screen D switches to the Dimension tool. Press Tab to lock the value as a driving dimension and move to the next field, or Enter to lock it. A value you type but do not lock only previews. Esc clears typed values first, then the shape. A field also accepts an expression or a variable name, such as =width/2.

The setting Values beside the pointer chooses whether the fields show dimensions only (the default), dimensions and positions, or nothing. See Units and settings.

In a field that holds a plain number, ArrowUp and ArrowDown change it by 1 (Shift by 10, Alt by 0.1) and the preview follows. A formula or a variable name in the field is left alone.

Snaps and inferred constraints

As you move the pointer, CivilKit CAD snaps to existing points and curves and shows a marker and a name: endpoint, centre, origin, midpoint, quadrant, intersection, perpendicular, tangent, on curve, aligned and grid. The same markers appear for model geometry: model endpoint, model midpoint, model centre, model quadrant, model crossing, mid-extent, body centre and mid of extrusion.

  • Hold Alt while you click to turn snapping off for that click.
  • With Infer constraints while drawing on (the default), the tools add horizontal, vertical, coincident and tangent constraints as you draw. Hold Shift at a click to turn that off for the click. A snap to a guide places only the point, unless Add constraints from snaps and Auto-constrain from guides are on.
  • Hold Shift while you click a model snap to attach the point to the model: a fixed reference point is added there and your point is made coincident with it.
  • The Snaps menu in the Status group switches each snap kind on or off.

Draw

ToolHow to use it
Line (L)Click to start, click for each next end. The chain continues from the last end. Click the first point again to close the outline. Horizontal and vertical are inferred within 2 degrees. Type len and ang for an exact segment. Press M or A to continue with a tangent arc, and L or M to return to lines; with Line to tangent arc set to Rest the pointer on the end (the default), resting the pointer on the end of the chain switches too.
CentrelineTwo clicks make a construction line. It is never extruded. Use it as the axis of a revolve.
3-point arc (A)Click the start, then a point the arc passes through, then the end. Collinear points are refused.
Centre arcClick the centre, the start (this sets the radius), then the end. The shorter way round is drawn unless the pointer goes past half a turn.
Tangent arcClick the free end of a line or arc, then click where the arc should end. It is made tangent to that curve.
Circle (C)Click the centre, then click for the radius. Type rad or dia to set it exactly.
EllipseClick the centre, click the end of the major axis, then click (or type) the minor radius.
Rectangle (R)Click one corner, then the opposite corner. Type w and h. The four sides are kept horizontal and vertical.
Rounded rectangleClick a corner, then the opposite one, like Rectangle. The four corners are rounded; the field corner is the radius (it stays for the next one, and is held to just under half the shorter side unless you type it). A typed radius becomes a driving dimension on each corner arc.
Centre rectangleClick the centre, then a corner. The rectangle is symmetric about the centre.
SlotClick the first centre, the second centre, then set the width with the pointer or by typing. The result is two lines and two arcs.
Arc slotA curved slot, in the Slot button’s flyout. Click the arc centre, click the start point (it sets the radius and the start angle; len and ang fields), click the end of the arc (the sweep field; the arc follows the pointer round, either way), then set the width with the pointer or by typing (w). The result is two concentric arcs joined by two half-round ends, all kept tangent. A typed radius and width are held as dimensions. To change the slot later, click one of its arcs in the sketch: the fields rad (radius of the centre arc), ang (start angle), sweep and w (width) appear, and typing a value and pressing Enter reshapes the whole slot, keeping it tangent.
PolygonClick the centre, then a second point: its distance is the radius and its direction the rotation. The default is 6 sides. Press + to add a side. The fields, in order, are radius (or apothem), ang and sides: type digits for the first and press Tab to lock it and move on, and so reach sides. Press M to switch between a polygon whose corners touch the circle (radius) and one whose sides touch it (apothem). The sides are kept equal.
Add spline pointClick a spline where it should get one more point. The new point lies on the curve between its two neighbours, and you can drag it to bend that part. The spline is fitted through all its points again, so it can shift slightly.
SplineA smooth curve through the points you click. Press Enter or click the last point again to finish. Click the first point to close the curve. Esc cancels.
Control-point splineA curve shaped by control points; it passes through the first and last only. Same keys as the spline. The degree is 3; it cannot be changed in the interface.
Bridge curveClick a free end of one curve, then a free end of another. A smooth spline joins them. Press 1 for tangent continuity (the default) or 2 for curvature continuity.
Equation curveClick where the curve starts, then type formulas x(t) and y(t) in its panel. See Equation curves.
PointEach click adds a point. Points mark where Hole will drill.
Text (Q)Click where the text goes. See Text.

Select and edit by hand

With the Select tool:

  • Click a line, arc, circle or point to select it. Shift-click or Ctrl-click adds to the selection.
  • Drag on empty space to draw a box. Drag right for a window box that picks what is fully inside; drag left for a crossing box that picks what the box touches.
  • Ctrl+A selects everything; Delete or Backspace removes the selection; Esc clears it.
  • Drag a point to move it. If the sketch is fully defined, CivilKit CAD says so and does not move it: remove a constraint first. If the move would break a constraint, it says “This move conflicts with the constraints”.
  • With one item selected, type a digit to start editing its size.

Modify

ToolHow to use it
Trim (T)Click a part of a line, arc or circle. It is removed back to the nearest crossings with other curves. A part with no crossings is deleted. A circle needs two crossings. Hover shows what will go. Splines and ellipses are not trimmed.
Extend (E)Click a line or arc near the end you want to lengthen. It runs on to the first curve it meets. A circle cannot be extended.
Split entityClick a place on a line, arc, circle or fit spline. It is broken there into two pieces that share one new point, so an outline through it stays closed and still extrudes. Picking an end of the curve is refused. Control-point splines and ellipses cannot be split. Constraints that cannot carry over to both pieces are dropped, and the status line names them.
FilletClick two lines that meet at a corner (or click the corner), then type or accept a radius to replace the corner with a tangent arc. A radius you type before picking is applied as soon as you pick the corner and is kept as a dimension.
ChamferThe same picks as the fillet. The distance is the length cut from the corner along both lines.
Offset (O)Click a line, arc, circle or spline. For lines and arcs, the whole connected chain is selected. Press Enter, then move the pointer to the side you want. The pointer’s distance is the offset distance, or type digits for the single field, dist, and press Enter to lock it. F flips the side. Click to place. See Offsets and references.
MirrorClick the entities to mirror (click again to unselect), press Enter, then click the mirror line. The source geometry stays.
Linear patternSelect entities, press Enter. A panel opens with the same groups as the Linear pattern feature: see Patterns below.
Circular patternSelect entities, press Enter, click the centre. A panel opens with the count and the angle: see Patterns below.
Move, Copy, Rotate, ScaleSelect entities first (or click them in the tool), press Enter, click a base point (the centre for Rotate), then move the pointer and click, or type the values. The fields, in order, are dx, dy and copies for Copy; dx and dy for Move; ang and copies for Rotate; factor and copies for Scale. Type digits for the first field and press Tab to lock it and move on. Copy, Rotate and Scale take a number of copies (at most 99); with 0 copies, Rotate and Scale change the selected geometry in place.

Patterns

The Linear pattern makes a grid of copies, in columns and rows. Pick the shapes (click them, or select them first), press Enter, and the pattern panel opens, with a live preview of every copy on the canvas.

  • Direction 1 (columns): Count (the number of instances, the first one included), Angle (typed, or press Pick a line and click a line of the sketch to take its direction; horizontal until you set it), and the distance. Spacing is the distance between neighbours; switch to Total length to give the distance from the first copy to the last (the spacing follows the count).
  • Direction 2 (rows): the same group. Its count starts at 1, which means no rows; raise it to make rows. Its angle starts at 90 degrees to direction 1. Spacing and total length work as above.
  • Enter or OK makes the pattern. Esc first clears what you typed, then goes back a step; Cancel leaves the tool.

The shortcut still works: before you move onto the panel, the pointer sets direction 1 (where it sits is where the second copy goes) and a click on the canvas makes the pattern. Digits typed go into the fields next to the pointer: count, space and ang of direction 1.

The result is real geometry with these constraints:

  • Each step along direction 1 is a driving dimension (a horizontal and vertical distance from the previous copy; a horizontal or vertical constraint instead when one of them is 0).
  • With rows, direction 2 adds ONE dimension, the step from the first copy to the first copy of row 2. Every other copy in the rows repeats that step again from the copy below it, as a dashed construction line kept parallel and equal to the first step. Editing a spacing dimension (double-click it) moves every copy that depends on it; no other dimension is added.
  • A count cannot be changed afterwards: delete the copies and make the pattern again. The pattern is also not linked to the shape you started from.
  • At most 99 in one direction and 200 copies in all. The two directions must not be parallel.

The Circular pattern panel has the Count (the first one included), the angle and an Angle type: Step angle (the angle between neighbours, negative for clockwise) or Total angle (the turn from the first copy to the last; 360 spreads the copies right round). The step angle is a driving dimension between construction lines from the centre.

What the edit tools do to constraints

  • Trim and Extend bind the new end to the curve it stops at. A length dimension or equal constraint on a trimmed line is dropped, because its length changed. Horizontal, vertical, parallel and perpendicular constraints stay.
  • Fillet and Chamfer replace the corner point; a dimension or coincident constraint on that point goes with it. The fillet arc is tangent to both lines.
  • Offset keeps the copy parametric: each copied line gets a parallel constraint and a distance dimension; each copied arc or circle shares the centre of its source and keeps a radius difference.
  • Mirror ties each copied point to its source with a symmetric constraint, and the radius of a copied circle to the source radius.
  • Patterns write the spacings or the step angle as visible dimensions. The copies follow those, not later changes to the shape of the source.
  • Move, Rotate and Scale re-measure dimensions that mention what changed. A fixed point cannot be moved. Relations to geometry that did not move are kept, so the solver can pull the shape back; if it refuses, press Ctrl+Z.

Reference

ToolHow to use it
Project edges (P)Hover an edge of the part to preview its projection onto the sketch plane and click to project it. Press Enter to project the edges and faces you selected before opening the sketch. The result is fixed reference geometry, drawn dashed, that is not extruded.
Construction (X)Click a line, arc, circle, ellipse or spline to switch it between normal and construction. Shift-click switches the whole connected chain.

The Construction button in the Reference group is a mode: while it is on, new geometry is drawn as construction (dashed, not extruded). With geometry selected, Make construction switches the selection between normal and construction. Points cannot be construction.

Project edges is a snapshot. If the part changes later, the projected geometry does not follow it. Edges that are square-on to the plane project to nothing and are skipped, and a tilted circle becomes a spline.

Importing a drawing

While a sketch is open, the Import group of the ribbon has Import DXF and Import SVG. Import DXF into sketch (also in command search) adds the lines, arcs, circles, polylines and splines of an ASCII DXF file to the current sketch. New sketch from DXF makes a new sketch from a file. Binary DXF is not supported. Import SVG into sketch and New sketch from SVG do the same for an SVG drawing: paths (curves become splines, circular arcs stay arcs), rectangles, circles, ellipses, lines and polygons, with the file’s size in millimetres, centimetres or inches. See Importing.

3D sketch tools

A 3D sketch is a separate tool: it is not one of the flat sketch tools above. It draws lines, arcs and splines whose points have three coordinates, for use as a sweep path. See 3D sketches and, for a first walk-through, Introduction to 3D sketching.

Next

Constraints and dimensions

Constraints and dimensions are the rules that hold a sketch in shape. A constraint such as Parallel or Tangent relates two pieces of geometry; a dimension fixes a size or a distance. This chapter lists every constraint and dimension, shows how to add, change and delete them, and explains how CivilKit CAD tells you how well defined a sketch is.

Why constrain

A sketch with no constraints is only a drawing: drag one point and the shape distorts. Constraints let the sketch keep its meaning when you change a value. A rectangle that stays a rectangle, a hole that stays centred and a slot that stays 10 mm wide are all constraints at work. In a parametric part you change a dimension and everything after it follows.

You do not have to constrain everything. A sketch can be extruded while it still has freedom. But a fully defined sketch behaves predictably, and CivilKit CAD marks it as such.

Geometric constraints

Geometric constraints are in the Constrain group of the Editing tab. Choose a tool, click what it needs, and CivilKit CAD adds one constraint and waits for the next set of picks. Picks can be points or curves; a click on an existing point wins over a click on a curve.

ToolPicksWhat it does
Horizontal (H)A line, or two pointsMakes the line horizontal, or the two points level.
Vertical (V)A line, or two pointsMakes the line vertical, or the two points one above the other.
CoincidentTwo pointsMakes the points the same point. A circle or arc stands for its centre.
MidpointA point and a line, in either orderPuts the point at the middle of the line.
FixA pointPins the point where it is now.
EqualTwo lines, or two circles or arcsMakes the lengths equal, or the radii equal.
ParallelTwo linesMakes the lines parallel.
PerpendicularTwo linesMakes the lines meet at a right angle.
CollinearTwo linesPuts both lines on one straight line.
TangentA line and a circle or arc, or two circles or arcsMakes the curves touch smoothly. Two lines cannot be tangent. When the two share an end point, the tangent is at that point.
ConcentricTwo circles or arcs, or a circle or arc and a pointGives them the same centre.
SymmetricTwo points and a line, in any orderMakes the points mirror images of each other across the line.

The constraint list also shows Point on line and Point on circle. You do not add these with a tool: they come from snapping to a curve while you draw, and from Trim and Extend.

When a constraint is refused

A constraint that would add nothing, or would contradict what is already there, is refused and the sketch is left unchanged. The hint line tells you why:

  • That constraint is already there.
  • That would add nothing: the sketch already implies it.
  • That conflicts with the existing constraints.
  • That cannot be picked here, Pick a different item or Nothing to pick there, when a click does not fit what the tool needs.

Dimensions

The Dimension tool (D) is a smart dimension: you click what to measure and it chooses the right kind. It then offers a value box holding the measured value.

ClickYou getNotes
A lineDistance: the length of the lineA second click on a point or line refines it.
Two pointsDistance between themPress H for the Horizontal distance, V for the Vertical distance, or A for the aligned distance (the default).
A point and a linePoint to line: the distance to the (infinite) line
A circleDiameterPress R to dimension the Radius instead.
An arcRadius
Two linesAngle between them, in degreesThe angle at the point where they meet.
An edge of the partThe edge is projected into the sketch first, then measured like a line, arc or circleClick a point or circle of the sketch and then the part’s outer edge to dimension its position from that edge.

To set the dimension:

  1. Click what you want to measure.
  2. Type the value you want, or leave the measured one.
  3. Press Enter or Tab. The geometry moves to the new value.

A body edge you click is projected as fixed, dashed reference geometry (the same as Project edges), once only: a second dimension to the same edge reuses it, and it adds no degrees of freedom. An edge square-on to the sketch plane has no line in it and cannot be used.

Esc first clears a typed value, then the picks. A dimension that already exists for the same things is refused. A value must be a positive length, or an angle of 0 up to but not including 360 degrees.

A value can be a number, an expression such as =width*2+3, or the name of a variable. A dimension linked this way shows fx. See Equations and variables.

Change or delete a dimension

  • Double-click the dimension label in the view, type a new value and press Enter.
  • Or select the item in the Constraints list and double-click its row.
  • Delete a dimension or any other constraint with the × button on its row in the list.

When you change an Angle dimension by a lot (more than about 90 degrees from the present angle), the solver can end on the opposite solution, with the line pointing the other way. Change the value in steps if that happens.

Reference dimensions

A reference dimension measures but does not constrain. It shows in italic brackets, for example (20). It is a way to read a size that other constraints already fix.

  • When you add a dimension that the sketch already fixes, or that would conflict, CivilKit CAD adds it as a reference dimension and tells you.
  • To turn a driving dimension into a reference one, click the arrows button on its row in the Constraints list, or right-click its label.
  • To turn a reference dimension back into a driving one at its present value, double-click its label, or click the button again.

The Display menu has a Reference dimensions switch.

How defined is the sketch

The Status group of the Editing tab shows a chip with the state of the sketch. The chip always shows its short text (such as 2 DOF); hover it for the longer hint.

ChipMeaning
N DOFThe sketch is under-defined. N is the number of degrees of freedom: the number of independent ways the shape can still move or change size.
Fully definedNothing can move: every point and every size is fixed by constraints.
Over-constrainedSome constraints conflict with, or repeat, others.

In the Constraints list the same states are worded N degrees of freedom, Fully defined, Over-constrained and Does not solve.

With Colour by definition on (the default), the geometry is coloured to match:

ColourMeaning
BlueSomething about this item can still move or change.
Dark (light on a dark background)Fully defined. Nothing can move.
RedA constraint that names it conflicts with others.

An item is blue if it is not fully determined; one dimension can fix a line’s length while its position stays free. CivilKit CAD works out the colours by testing each point against the solver, a moment after you stop editing, and never changes the sketch while doing so. A point that is fixed in only one direction, such as a point on a circle about a fixed centre, counts as under-defined.

Sketch Report

Sketch Report (in the Status group, and in the command search) opens a summary of the sketch. On a desktop it is a small window over the view; on a phone or tablet it is a sheet from the bottom edge. Either stays open while you keep editing and follows the sketch.

  • The sketch name and its state: Fully defined, the number of degrees of freedom, Over-constrained, Conflicting constraints or Does not solve.
  • Counts of points, lines, arcs, circles, splines, construction entities, Closed profiles (the shapes Extrude can use) and Open chains (loose ends).
  • The number of constraints, then Driving dimensions and Reference dimensions, and the constraints counted by kind.
  • Conflicting and redundant constraints: click one to select the geometry it names in the sketch. Delete it from the Constraints list.

Fully define

Fully define in the Status group adds relations and dimensions until the degrees of freedom reach zero, but only the ones the solver accepts.

  1. It first adds relations that your drawing already shows: horizontal and vertical within one degree, parallel and perpendicular within one degree, and equal lengths and radii.
  2. It then adds dimensions one at a time, taken from the present geometry: radii, line lengths, angles at shared corners, and finally positions from the origin.

The message says how many relations and dimensions were added, and how many degrees of freedom remain if no dimension could remove them (a spline, for example). The button does nothing, and says so, if the sketch is already fully defined or has conflicts. The whole step can be undone in one go. Because the dimensions copy your drawing, review them before you rely on them.

The Constraints list

Click the chip to open the Constraints list. It also opens by itself the first time a sketch becomes over-constrained. Each row shows the kind of constraint, the things it names, and its value. Hover a row to light the geometry it names in the view.

  • A row in red is a conflict: it cannot hold together with the constraints before it. Delete it, or one of the others.
  • A row in amber is redundant: the sketch already implies it. It does no harm, but it counts toward over-constrained.
  • × deletes a constraint.
  • The arrows button switches a dimension between driving and reference.

When the sketch is over-constrained the list also names the blamed constraints under Conflicting or Redundant, each with a delete button. See When a sketch will not solve.

The list is a pop-over. The Constraints panel switch in the sketch Display menu turns it off.

Seeing constraints in the view

Relation glyphs (H, V, =, tangent and so on) are drawn on the geometry, and driving dimensions are drawn as labels. The Sketch section of the Display menu has switches for Dimensions, Relation glyphs, Reference dimensions, Colour by definition and Constraints panel. They change only what is drawn. A few constraints that tools add automatically, such as the placing constraints of a pattern, are hidden in the view and shown only in the list.

Limits

  • You cannot edit a constraint’s picks. Delete it and add it again.
  • The glyph switches work per kind (dimensions, relations, reference), not per type of constraint.
  • A fully defined sketch cannot be changed by dragging. CivilKit CAD says so: remove a constraint first.
  • Constraints between a sketch and the part itself are a snapshot, not a live link. See Offsets and references.

Next

Offsets and references

This chapter covers three ways of building a sketch from geometry that already exists: Offset, which draws a parallel copy of a curve; Project edges, which brings the edges of the part into the sketch as reference geometry; and Construction geometry, which helps you draw without becoming part of the shape. It also explains what these references are not: they are a snapshot, not a live link to the part.

Offset

Offset (O, in the Modify group) draws a copy of a curve at a set distance. It is the quickest way to make a wall, a pocket inside an outline, or a clearance around a shape.

  1. Choose Offset.
  2. Click a line, arc, circle or spline. For lines and arcs, CivilKit CAD selects the whole chain of lines and arcs connected end to end with it (with no branches). Click the chain again to unselect it. Shift-click toggles a single entity, which must stay connected to the rest.
  3. Press Enter.
  4. Move the pointer to the side you want. The distance from the chain to the pointer is the offset distance, and the side the pointer is on is the direction. Or type digits: the one field, dist, takes them, and Enter (or Tab) locks the value. Then click on the side. F flips the side.
  5. Click to place the copy.

Esc drops a typed value first, then the selection.

How the copy behaves:

  • Where neighbouring curves meet, the offset curves are joined at their intersection, trimmed or extended as needed. A closed chain stays closed.
  • A piece that would collapse at this distance (an arc whose radius would reach zero, or a line that would reverse) is left out, and the hint says so.
  • The copy is parametric. Every copied line is made parallel to its source and gets a point-to-line distance dimension with the offset distance. Every copied arc or circle shares the centre of its source and keeps the difference in radius. Change a distance and the copy follows. Each segment carries its own distance, so there is no single dimension that changes them all.
  • The copy keeps the construction flag of its source.
  • The source geometry and its constraints are untouched.

Chains that mix a spline with lines or arcs cannot be offset. Pick the spline on its own. A spline is copied as a new spline through points taken on the exact offset curve (at most 48 points), and it is a free curve, not linked to its source. When the distance is larger than the curve’s local radius of curvature, or two sides of a narrow neck would cross, nothing is drawn and the hint says the offset folds over itself: use a smaller distance or the other side.

Offset a reference outline

You can offset things that are not yet in the sketch:

  • Edges of the part. Hover an edge of the part. The whole outline of edges in the same plane, joined end to end, lights up. Click it to project it into the sketch and select it, then continue as above: Enter, side, distance.
  • Curves of other sketches, including sketches an extrude has already used. These are not drawn in the 3D view, but Offset and Project can still pick them.
  • The outline of the face you are sketching on. If you started the sketch from a planar face, choose Offset and CivilKit CAD takes that face’s outer outline, inward, with a distance of 1 mm. The hint reads “Face outline offset inward: type a distance, press F to flip the side, Enter to apply”. Enter applies, a typed value changes the distance, and Esc drops the typed value so the pointer drives the distance.

The projected outline is fixed and counts as a real edge of the sketch’s shapes (it is not construction), so the ring between the outline and its offset is a region you can extrude or cut.

Cut a pocket or a wall

When a sketch holds an outline and an offset inside it, the extrude and cut editors list the Shapes by how they nest:

  • Inside the offset (pocket): the area inside the offset.
  • Wall between outline and offset: the ring between the two.

For a cut, Shift+C on such a sketch chooses the pocket by default. The wall would remove material whose outer face is the body’s own wall, which a pocket does not need. Tick both shapes if you really want the ring.

Project edges

Project edges (P, in the Reference group) flattens edges of the part onto the sketch plane and adds them to the sketch.

  • Hover an edge to preview its projection and click to project it.
  • Press Enter to project the edges and faces you selected before opening the sketch. That includes the boundary of the face you are sketching on.
  • A click on an edge that is already projected says so.

What you get:

  • Fixed points: projected geometry never moves and adds no degrees of freedom.
  • A line, arc or circle where the projection is one, otherwise a spline.
  • Construction geometry, drawn dashed, which is not extruded. A circle is fully defined by its projection.

Limits to know:

  • It is a snapshot. If the part changes, the projected geometry stays where it was. Project again, or redraw.
  • An edge square-on to the sketch plane projects to a point and is skipped, and “That projects to nothing on this plane” appears.
  • A circle seen at an angle becomes a spline, not an ellipse.
  • Body picking is off while you sketch, so select edges and faces before you open the sketch if you want to use Enter.
  • A free-form edge is rebuilt from the part’s display mesh and follows the true curve only to about 0.01 mm, unless it is the wall of an extruded sketch spline, which projects exactly. Cutting a ring made from an edge that is only that close can fail; cut the inside loop instead.

Construction geometry

Construction geometry is dashed, takes part in constraints and snaps, and is never extruded or revolved. Use it as an axis, a guide or a mirror line.

  • Centreline draws a construction line directly.
  • Construction mode, the Construction button in the Reference group, makes everything you draw next construction until you turn it off.
  • Make construction (shown when geometry is selected) switches the selection between normal and construction.
  • The Construction tool (X) flips one curve at a time; Shift-click flips the whole connected chain.

Points cannot be construction. See Sketch tools.

Model snaps

While a sketch is open, the part offers places to snap to, in a different colour from the sketch’s own snaps. They come from the part’s edges projected into the sketch plane: model endpoint, model midpoint, model centre, model quadrant, model crossing, mid-extent (a dashed guide half way across the part), body centre and mid of extrusion. They are on by default and can be switched off in the Snaps menu.

A model snap only positions your point. Hold Shift while you click to attach it: a fixed reference point is added there, and your point is made coincident with it. The attachment is also a snapshot.

Locking a placed shape to the part

When you place a shape from the catalog, its size box has a Lock to list of nearby points (hole centres, corners, edge midpoints). Choosing one adds a fixed reference point to the shape’s sketch and holds the shape at the same horizontal and vertical distance from it. The distances are ordinary dimensions in the shape’s sketch, so you can edit them there. They record the position at the moment you lock; if the part changes so that the point moves, the shape does not follow. See Catalog parts.

What does not exist yet

References that follow the part when it changes (an associative link from a sketch to an edge or a face) are not available. Everything above is a snapshot. If you need a feature to stay tied to a part’s dimension, drive both from a variable. See Equations and variables.

Next

Introduction to 3D sketching

This page teaches the 3D Sketch tool with two short projects. When you want the full list of options, see the 3D sketches reference.

What a 3D sketch is

A normal sketch is flat. It lives on a plane or a face, and every point has two coordinates. You draw a closed outline in it and extrude, revolve or cut.

A 3D sketch has no plane. Every point has three coordinates, X, Y and Z, so the curve can rise, fall and turn in any direction. You cannot extrude it, because it has no outline. It is a path or a guide: a line in space that other features follow.

2D sketch3D sketch
Lives onA plane or a faceNothing: it floats in space
A point hasX and YX, Y and Z
Used forProfiles to extrude, revolve or cutPaths to sweep along, lines to measure against
Constraints and dimensionsYesNo (you place and type points)

When you use one

  • Sweep paths. A pipe, a hose, a wire, a spring or a handrail that bends in all three directions. This is the main use.
  • Guide curves. A line in space that you want to keep for reference, to snap other points to or to look at.
  • Curves drawn on a mesh. A seam, a cut line or a groove on an imported scan or SketchUp model. You click across the surface and the curve lies on it.
  • Frames and skeleton lines. The centre lines of a frame or a rack, drawn once as lines in space.

Project 1: a pipe along a rising curve (5 minutes)

You will draw a curve that climbs in space, then sweep a circle along it.

1. Open the tool. On the Home tab, in the Sketch group, choose 3D Sketch. The panel opens on the left. The ? button in its header shows a short reminder and a link to this page.

2. Choose Spline. In Draw, press Spline. A spline is a smooth curve that passes through every point you click.

3. Click the first points on the ground. Under Where you click, Work plane is Ground and Height above plane is 0. Click four points in the 3D view in a rough circle. Each click lands where your pointer meets the work plane. The Points list gains a row for each one, with its X, Y and Z. The up axis is Y.

4. Lift the curve. Set Height above plane to 20 and click a fifth point, then set it to 40 and click a sixth. Each click now lands higher (the points get Y 20 and 40). You can also type a point exactly: under Add by coordinates, enter X, Y and Z and press Add.

5. Check the points. Every point is a row in Points with its X, Y and Z. Type a new number to move a point. Drag a diamond in the view to move it in the work plane.

6. Finish. Leave Also add a plane normal to the start ticked and press Create (or press Enter). The feature tree now has a 3D sketch and a Plane at the start of the curve, square to it.

7. Draw the pipe’s cross-section. Select that plane (F2) in the tree and choose Sketch on the Home tab. Choose Circle, click the origin, type 4 for the radius and press Enter. Press Esc, then the green tick to finish the sketch.

8. Sweep. On the Home tab, in the Create group, open the list of the Loft button and choose Sweep (or press Shift+W). Profile (closed) is the circle sketch and Path (open) is the 3D sketch (F1); both are usually already chosen. Confirm with the green tick. The circle is carried along the curve and you have a pipe.

To change the pipe, double-click the 3D sketch in the tree, move a point, and press Update. The sweep follows.

Project 2: a curve on an imported mesh

Use this to mark a seam or a groove on a scan or a SketchUp model.

  1. With a part open, import an STL or SketchUp file as a Reference mesh (see Importing). Pick the unit the file was made in. Lower the mesh Opacity if you want to see your curve through it.
  2. Choose 3D Sketch and press Spline.
  3. Click across the surface. Under Mesh, Draw on the imported mesh surface is ticked, so each click that lands on the mesh sits on its surface. Click four or five points in a loose wave.
  4. Your clicks are far apart, so between them the spline can drift off the surface. Under Mesh, choose how to lay the curve (To the nearest surface point, or Along the work plane normal) and press Fit curves. The spline is resampled into many points and each one is placed on the surface.
  5. Press Create.

A curve that still has a stretch that misses the mesh cannot be fitted. The panel says so. Add a point on that stretch and fit again.

The ideas behind the tool

Work plane. Your mouse is flat and the model is not, so each click lands where the pointer’s line of sight meets the Work plane: Ground, Front, Top, Right, or any plane of the part. A plane selected in the tree is the starting choice.

Height above plane. Slides the work plane along its own normal. At 40 on the ground, the next clicks land 40 mm up. Change it between clicks to build a curve that rises and falls.

Snapping. With Snap to model and sketch points on, a click near a model corner, an edge end or middle, a point of another sketch, or a point you already placed snaps to it in space, whatever the work plane is. A green cross shows a snap; a yellow cross shows where a click will land on the plane.

Line, Arc, Spline, Control spline, Points.

  • Line joins the points you click with straight segments.
  • Arc takes a start, a point on the arc and an end.
  • Spline passes through every point. Use it for paths you want to hit exactly.
  • Control spline is pulled towards the points but does not touch them. It is smoother and wobbles less; use it when the exact points do not matter.
  • Points places single points to snap to.

Editing points. Click a diamond to select it (its row in Points lights up; clicking a row selects the diamond too). Drag a diamond to move a point in the work plane. While you are drawing a chain, clicking an existing point continues the chain through it, closes on it or ends there. Type in its X, Y or Z field to move it exactly in any direction. Select it and press Backspace or Delete, or press the bin button in its row, to remove it. Undo point removes the last point of the chain you are drawing. Ctrl+Z (Cmd+Z on a Mac) steps back through the tool.

Why a sweep path must be one spline. The kernel sweeps along one smooth curve. A 3D sketch with a single spline is offered by Sweep. A sketch with a polyline, an arc, or two splines is not, because the profile would have no single direction to follow. If you need a path with straight runs, draw it as one spline.

Tips and troubleshooting

  • A point is not where you expected. It landed on the work plane, not at the depth you pictured. The up axis in the app is Y: check the point’s Y in Points and type the value you want. Or change Height above plane, or orbit the view and look from the side.
  • The point jumped to something. Snap took it. Untick Snap to model and sketch points, or click away from corners and edge ends.
  • The curve wobbles. A spline passes through every point, so points placed too close or at uneven spacing make it ripple. Delete some points, space them evenly, or use a Control spline.
  • Sweep does not list your sketch. It holds more than one curve, or a line or arc. Delete the extras so one spline remains.
  • How do I undo? Undo point or Ctrl+Z inside the tool. Esc drops the chain you are drawing and a second Esc cancels the tool. After Create, use the normal Undo: the whole sketch is one step.
  • No point gets placed on the mesh. Check that Draw on the imported mesh surface is ticked and the mesh is shown.

Next

3D sketches

This is the reference page. If you are new to 3D sketching, start with Introduction to 3D sketching.

A normal sketch is flat: it lies on a plane or a face. A 3D sketch is not: its points have three coordinates, so it can run in any direction. It has no profile and cannot be extruded. It is made to be a path, for example for a sweep along a curve that bends in all three directions, like a handrail, a hose or a wire.

Quick start

  1. Choose 3D Sketch (Home tab, Sketch group, or command search). The tool opens in the left panel.
  2. Pick a mode (Line, Arc, Spline, Control spline or Points) and the Work plane to draw on.
  3. Click in the 3D view to place points. Each click lands where your pointer meets the work plane. To go off the plane, raise Height above plane or type X, Y and Z under Add by coordinates.
  4. Press Enter or Create to finish. Esc drops the chain you are drawing and a second Esc cancels the tool.

The keys the tool uses are:

KeyWhat it does
EnterFinish: the 3D sketch is added to the part.
EscDrop the chain being drawn; press again to cancel the tool.
Backspace or DeleteRemove the selected point (not while you are typing in a field).
Ctrl+Z / Cmd+ZStep back through the tool (the last point), not through the part.
Shift+click on a pointStart a new chain from an existing point.

The tool has no axis keys or gizmo: to move a point along the third direction, type its coordinate.

Drawing one

Choose 3D Sketch on the Home tab, in the Sketch group (on a phone, on the Sketch tab of the tools sheet), or search for “3D Sketch” in the command search. The tool opens in the left panel and takes over the 3D view.

Pick what to draw:

ModeWhat it makes
LineA polyline: click the corners. Click the last point again, or End chain, to stop; click the first point to close it.
ArcClick the start, a point on the arc, then the end. An arc of more than half a turn is made of several arcs that join up.
SplineA smooth curve that passes through every point you click. End chain stops it; clicking the first point again closes it.
Control splineA curve pulled towards the points but not through them. Set its Degree (3 by default; fewer points give a lower degree).
PointsSingle points.

Draw on the Work plane: Ground (the plane of the grid), Front, Top, Right, or any plane of the part. A plane you selected in the feature tree is the starting choice. Each click lands where your pointer meets the work plane.

Lifting points off the plane

  • Height above plane moves the work plane along its normal: set it to 40 and the next clicks land 40 mm above the ground. Change it between clicks to build a curve that rises and falls.
  • Under Add by coordinates, type X, Y and Z and press Add (or Enter): the point goes there, wherever it is.
  • Every point is in the Points list with its three coordinates. Type in a field to move it.

Snapping

With Snap to model and sketch points on, a click near one of these snaps to it, in space, ignoring the work plane:

  • a corner of the model (the end of an edge) and the middle of an edge;
  • a point of another sketch, flat or 3D;
  • a point you have already placed in this sketch (the click then reuses it, so lines and curves join).

A yellow cross shows where a click will land on the plane; a green cross shows a snap.

Editing while you draw

  • Drag a diamond to move that point in the work plane. For the third direction, type its coordinate.
  • Hover a diamond and it brightens and grows slightly. Click it to select it: the diamond turns red and its row in the list is highlighted (clicking a row selects the diamond too). The click area is larger than the drawn diamond, and larger again on a touch screen.
  • While you draw a chain, a click on an existing point does not select it: it joins the chain there, so the line or spline continues through that point, a click on the chain’s first point closes the outline, and a click on the last point ends the chain. Shift+click an existing point with no chain under way starts a new chain from it. Placing a new point clears the selection.
  • Select a point (click its diamond or its row) and press Backspace or Delete, or press × in the list, to remove it. A polyline closes up over the gap; a spline just loses that point.
  • Undo point removes the last point of the chain you are drawing. Ctrl+Z (Cmd+Z) steps back through the tool, not through the part.
  • Enter or Create finishes: one 3D sketch feature is added, as one undo step. Esc drops the chain you are drawing, and a second Esc cancels the tool.

Double-click the 3D sketch in the feature tree to open it again, with the same tools, and press Update. It is hidden, shown and suppressed like any other sketch, and drawn as a teal curve (the Curves display layer).

Sweeping along a 3D sketch

The kernel sweeps along a 3D sketch that holds exactly one spline (and nothing but points). A polyline or arcs in a 3D sketch are fine for reference, but cannot be a sweep path; the Sweep editor does not list them.

The introduction walks through this step by step with pictures. In short, a pipe along a curve:

  1. Open 3D Sketch, keep Spline, and click four or five points. Lift some of them with Height above plane. Leave Also add a plane normal to the start ticked, and press Create. You now have the 3D sketch and a Plane at its start, square to the curve.
  2. Select that plane in the tree and choose Sketch. Draw a circle (or any closed outline) around the origin and finish the sketch.
  3. Run Sweep (Home tab, Create group, in the list of the Loft button; Shift+W; or the command search). Profile is the new sketch; Path (open) offers the 3D sketch. Confirm.

The same path list is used by Path pattern.

What cannot use a 3D sketch

Guide curves of a sweep or loft, loft sections, Project curve and Rib take curves of flat sketches only; they do not list 3D sketches.

Not in the tool

The constraint solver for 3D sketches is in the kernel, but the tool does not offer constraints: you place and move points directly. Constraints already in a 3D sketch (for example from an import) are kept when you edit it, except ones that refer to a point you delete.

Next

Text

Lettering on a part, such as dial numerals, captions, nameplates and part numbers, is a text item in a sketch. This chapter covers placing and editing text, choosing a font and adding your own, laying text along a circle, and turning it into an engraving or a raised emboss. It also says plainly what CivilKit CAD cannot do with text yet: wrap it onto a curved face.

How text works

The kernel turns the letters of a font into closed outlines. Because they are closed loops like any other sketch profile, everything that works on a sketch works on text: Extruded cut engraves it and Extrude embosses it.

Place and edit text

  1. Open a sketch on a plane or a face. See Starting a sketch.
  2. Choose Text in the Draw group, or press Q.
  3. Click where the text should go. A text item holding the word TEXT is placed at once, and its panel opens. The lettering is drawn in the sketch colour and follows every change.
  4. Edit it in the panel:
FieldMeaning
CharactersThe string, one line, 1 to 500 characters.
Cap heightThe height of a capital letter, in millimetres.
FontThe font. See below.
AnchorA 3 by 3 grid: which point of the text sits on the point you clicked (left, centre, right across; top, middle, baseline down).
AngleRotation about the anchor, in degrees.
SpacingThe letter pitch as a factor; 1 is the font’s own spacing.
MirrorFlips the text, for the back of a clear part.
On an arcLays the letters along a circle. See below.
Along a curveLays the letters along a line, arc or curve of the sketch. See below.
  1. Click Done, press Enter in the string field, or press Esc to leave the panel. To edit the text later, choose the Select tool and click the lettering.

Delete text removes the text and its anchor point.

The anchor is a normal sketch point. You can drag it, fix it, dimension it, or snap other geometry to it. The Copy, Move, Rotate and Scale tools and the patterns take text along; Rotate moves the anchor, so also set Angle if you want the letters to turn.

Warnings and errors

The panel and the hint line say what is wrong, and what to change:

  • Under 0.8 mm cap height the strokes are too thin to engrave or print.
  • Some characters are not in the font and were skipped. Only Basic Latin and Latin-1 letters are covered by the built-in fonts, including the degree sign.
  • The text was cut to 500 characters.
  • Neighbouring letters were moved apart so they do not touch, and Letters still overlap on this radius: on an arc, use a larger radius or more spacing.
  • The text is empty, The cap height must be above 0 and similar, for a bad value.
  • Strokes of this font overlap inside letters; engraving or cutting may fail validation. Try another font.

Text on an arc

Tick On an arc to lay the letters along a circle, as on a dial or a badge.

FieldMeaning
RadiusThe radius of the baseline.
DirectionThe angle, in degrees, of the middle of the text seen from the centre; 90 is the top.
Centre X, Centre YThe centre of the circle. Or click Pick centre, then click a sketch point or any place.
SideOutside (reads clockwise): the tops of the letters point away from the centre. Inside (reads counter-clockwise): the tops point towards it.

Text along a curve

Draw a line, arc or spline where the text should run (a construction one is best: it does not become part of the part), then select the text and tick Along a curve.

  1. Click Pick the curve, then click the line, arc, circle or spline. The letters turn to follow it and stay on it when you drag or constrain the curve.
  2. The anchor grid places the text on the curve: left starts at the start of the curve, centre centres the text on it, right ends at its end. Slide along moves it along the curve by a distance (negative moves it back).
  3. Other side travels the curve the other way, so the letters stand on the other side of it and read the other way.

Each letter keeps its shape and is turned as a whole to the direction of the curve, so tight curves need a larger letter spacing; the panel says when the letters were moved apart. Past the end of the curve the letters carry on straight. On an arc and Along a curve are alternatives: choosing one clears the other.

Fonts

The Font list has three groups.

GroupWhat it holds
Built inGauge (sans), a condensed sans-serif, and Engrave (serif). They are always available and look the same everywhere.
LibraryTen open-licence fonts hosted with the app: Barlow, Barlow Condensed, Source Sans 3, Bebas Neue, Anton, PT Serif, Special Elite, IBM Plex Mono, Great Vibes and Satisfy. A library font is fetched when you pick it, so it needs a connection the first time. The browser then keeps it.
This partFonts you have added to this part.

Below the list are two ways to add more:

  • Add font file… loads a .ttf, .otf or .ttc file (the first face of a collection) from your disk.
  • System fonts… lists the fonts installed on your computer, with a filter. This needs the browser’s Local Font Access feature, which only Chrome and Edge have. In other browsers CivilKit CAD says so, and you should use Add font file… instead. The browser asks for your permission when you click the button, never before.

A font file you add is stored inside the part file, so the part opens anywhere. A font larger than 1.5 MB is stored as a subset that holds only the letters the part’s text uses; the panel then says so. If you later type characters that were not in the subset, add the font file again. A library font is stored as a reference only, and fetched again when the part opens. If it cannot be fetched (you are offline), the part still opens; the lettering reports that the font is not loaded until you open the part online or pick the font again.

Check the licence. Fonts you add or take from the system are embedded in the part file. Make sure you may embed them. The panel reminds you.

Font notes the panel can show: kerning pairs and ligatures are ignored; a variable font gives only its default style; a collection gives its first face; a font whose licence flags forbid embedding or subsetting is reported. WOFF and WOFF2 files are not supported; use the TrueType or OpenType file. A font file can be at most 24 MB, and at most 64 fonts can be loaded at once.

Engrave and emboss

Finish the sketch, then:

  • Engrave. Use Extruded cut on the sketch, with the depth of the engraving. A depth of 0.1 to 0.5 mm is typical. The cut goes into the face the sketch lies on.
  • Emboss. Use Extrude with the height of the raised letters. If you start the sketch on a plane a little above the face (an offset plane), the lettering becomes a body of its own, with its own name and colour in the Bodies tab.

The extrude and cut editor lists the lettering as one shape per text item, so one text in a sketch can be cut and another embossed.

Keep lettering in a sketch of its own. The outlines of text are not trimmed against, merged with or made into holes by the other curves of the sketch. One sketch can hold several texts, for example one per numeral on a dial.

Text in scripts

A script can place text with s.text(...), choosing the font, height, anchor and an arc. See Scripting.

Limits

  • Text is flat. It lies on the plane of its sketch. CivilKit CAD cannot yet wrap lettering around a cylinder or a cone. A cut from a flat sketch removes material straight along the cut direction, so lettering cut into a curved face is not bent to follow it.
  • Text is one line per item.
  • Kerning and ligatures are ignored; letters are placed with their plain advance widths. Bold and italic are separate font files.
  • Fonts whose strokes overlap inside a letter, and connected script faces, can fail validation when engraved.
  • Very small text can fail to engrave cleanly. Keep the cap height at 0.8 mm or more.
  • While a sketch is open, the lettering outlines come from the kernel. A finished sketch in the tree shows the cut or extruded result, not the lettering curves.

Next

Equation curves

An equation curve is a curve you describe with two formulas instead of drawing it: x(t) and y(t). Think of t as a clock that moves a pen; as t runs from its start to its end, the pen draws the curve. Circles, ellipses, waves, spirals and gear involutes are all a line or two of formula.

The part keeps the formulas, not the points. When a variable used in a formula changes, the curve is drawn again from the formula.

Draw one

  1. Open a sketch. See Starting a sketch.
  2. Choose Equation curve in the Draw group (with the splines).
  3. Click where the curve should start. A wave is placed there at once and its panel opens.
  4. Type the formulas, or pick a curve in Start from (wave, circle, ellipse, spiral, gear involute, Lissajous figure) and change it.
FieldMeaning
x(t), y(t)Formulas of t, in millimetres.
t from, t toThe range of t. A number, or a formula of your variables.
ToleranceHow far the drawn curve may be from the formulas, in millimetres (0.01 by default).

While you type, the panel checks the formulas and says how many points the curve needs, or what is wrong. A change only goes into the sketch when it works, so a typing mistake never breaks the sketch.

  1. Click Done. To edit the curve later, choose Select and click it. Delete curve removes it.

Writing formulas

Formulas use the same rules as every number field: + - * / ^, brackets, sqrt, sin, cos, tan, abs, min, max, pow, atan2, exp, ln and the others, and pi.

Angles are in degrees. sin(90) is 1, and a full turn is t from 0 to 360.

Curvex(t)y(t)t fromt to
Circle, radius 2020*cos(t)20*sin(t)0360
Ellipse30*cos(t)12*sin(t)0360
Wave, 40 longt/95*sin(t)0360
Spiral, three turnst/36*cos(t)t/36*sin(t)01080
Parabolatt*t/40-3030

Using variables

Any name other than t must be one of the part’s variables (see Equations and variables). With a variable R, the circle R*cos(t), R*sin(t) follows every change of R, and so does anything built on it.

From curve to part

  • A curve that ends where it starts (a circle, an ellipse, a flower) is closed: extrude it straight away.
  • An open curve needs lines to close it. Its end points are ordinary fixed sketch points, so draw lines that snap to them. They stay joined when the formula changes.
  • An open curve can also be extruded as a thin wall.

When something goes wrong

The panel says what to change:

  • A formula is not right: a bracket is missing, or a name is not a variable. The message names the unknown name.
  • A formula has no value somewhere in the range: for example a square root of a negative number, or a division by zero. Narrow the range of t.
  • The range of t is not right: the start and the end are the same, or one of them cannot be read.
  • The tolerance cannot be met: the curve would need more than 200 points. Use a larger tolerance, or split the range into two curves.
  • The curve crosses itself: it still draws, but it does not make one region to extrude.

For scripts and agents: s.equation({ x, y, t: [start, end], tol }) in the script API, and the kernel’s equationCurve request.

When a sketch will not solve

This chapter helps when a sketch misbehaves: it moves when you do not want it to, it refuses a constraint, it says it is over-constrained, or it will not extrude. It explains what under-constrained, over-constrained and conflicting mean, how an open or crossing outline affects extrusion, and where CivilKit CAD tells you what is wrong.

First, read the signs

CivilKit CAD shows the state of the sketch in three places. Check them before you change anything.

  • The chip in the Status group of the Editing tab: N DOF, Fully defined or Over-constrained.
  • The colours of the geometry (with Colour by definition on): blue can still move, dark is fully defined, red belongs to a conflicting constraint.
  • The Constraints list, opened by clicking the chip. Red rows are conflicts, amber rows are redundant. Hover a row to see what it names.

The hint line, in the status bar or under the sketch bar, says why the last action did not work. The table at the end of this page lists the hints.

Under-constrained: it moves too much

A sketch with degrees of freedom left (N DOF, blue geometry) can still change. Dragging one point may move others; changing a dimension may slide the shape. That is normal for a sketch in progress, and a sketch does not need to be fully defined to extrude.

To pin it down:

  1. Click Fully define in the Status group. CivilKit CAD adds relations your drawing already shows, then dimensions taken from the present geometry. Check them afterwards: they copy your drawing, so a line that is 59.98 mm long gets a 59.98 mm dimension. See Constraints and dimensions.
  2. Or add the constraints yourself. Blue items tell you where something is missing: a line with no length, a circle with no radius, a corner with no position.
  3. If Fully define adds nothing for part of the sketch, that part may be a spline or another curve that dimensions cannot pin; the message says how many degrees of freedom remain.

If you cannot drag a point, the sketch may be fully defined, and CivilKit CAD says “Sketch is fully defined: remove a constraint to move this point.” Delete a constraint or dimension first.

Over-constrained and conflicting

A sketch is over-constrained when two constraints cannot both hold, or when one repeats what the others already imply.

  • A conflict is a constraint that contradicts the ones before it. For example, two Distance dimensions between the same two points, one 30 mm and one 40 mm. The chip turns red and reads Over-constrained; the geometry named by the conflict turns red; the Constraints list opens by itself and shows the culprits.
  • A redundant constraint is one the sketch already implies, for example a Parallel on two lines that are already horizontal. It is shown in amber. It does no harm to the shape, but it counts as over-constraining and may become a conflict if you change a value later.

When you add a constraint with a tool, CivilKit CAD checks it first. It refuses a constraint that is already there (“That constraint is already there”), one that adds nothing (“That would add nothing: the sketch already implies it”) and one that contradicts a known orientation (“That conflicts with the existing constraints”). Conflicts that arise later, from a value you change, are found by the solver, which blames the later of the clashing constraints.

To fix it:

  1. Open the Constraints list. The rows under Conflicting are the ones to look at.
  2. Delete one conflicting constraint with its × button. Usually the one you added last is the right one. Or change its value.
  3. If you only wanted to read a size, make the dimension a reference dimension instead: click the arrows button on its row. A reference dimension measures and never conflicts. CivilKit CAD does this automatically when you add a dimension the sketch already fixes, and tells you.
  4. If you are not sure what changed, press Ctrl+Z to undo steps inside the sketch.

If the chip or the list says Does not solve, the constraints cannot all be met at once at any shape. Typical causes are a dimension larger than the shapes around it allow, a Tangent between two lines, and a triangle whose sides cannot meet. Delete the last constraint you added and try a different value.

A conflict does not stop the part from building: the sketch is used as it was last drawn and the rest of the model continues. But the dimensions no longer mean what they say, so fix it.

A value change goes the wrong way

When you change an Angle dimension by a large amount (more than about 90 degrees from the present angle), the solver can land on the other solution, with a line pointing the opposite way. Change the angle in smaller steps.

It will not extrude

Extrude, Revolve and the other sketch features need closed outlines. These are the usual reasons they do not work.

The outline is open

The Extrude editor shows a card titled This profile is open: “A solid needs a closed loop. Give the curve a wall thickness, close it, or make a surface from it.” It offers three ways out:

ButtonWhat it does
Make thin wallGives the open curve a wall thickness, so it becomes a thin solid.
Close with a lineAdds a line across the gap between the two loose ends. If the sketch has no single chain with two loose ends, CivilKit CAD says so.
Extrude as surfaceMakes a surface instead of a solid.

If the gap is small, the card tells you how big: “Almost closed: the ends are 0.02 mm apart.” That is almost always two end points that look joined but are separate points. Fix it in the sketch by making the two end points Coincident, or by drawing the outline with one chain of the Line tool and clicking the first point again to close it.

In the Diagnostics tab and on the feature, the same problem reads The sketch is not a closed outline. Close the gaps, then try again.

The curves cross

CivilKit CAD finds closed regions by cutting every curve at its crossings. A line that crosses a rectangle divides it into two regions, and the parts of the line outside the rectangle are dropped as loose ends. Circles that overlap make several regions, and a figure-eight outline becomes two loops. This is not an error. Choose what to extrude:

  • In the Extrude editor, the Shapes list shows each region, with a note on how it nests (for example Inside shape 1). Click a shape in the list, or click its area in the viewport, to switch it on or off. “Click regions to choose what to extrude (outer, inner or both)”.
  • A shape inside another: the outer alone is a filled disc, the inner alone is the inner disc, and both together make a ring.

If you want one outline, remove the stray crossings with Trim, or delete the curve that crosses.

Two exact duplicates are merged. Curves that overlap along a line without crossing are not split, which can leave a region closed in the wrong place; delete the overlap.

Something is construction

Construction geometry (dashed) is never part of an outline. If a shape you need is dashed, select it and click Make construction to turn it back to a normal curve. Projected edges are construction too; see Offsets and references.

The cut removes nothing

A cut needs the sketch to overlap the body. If it does not, the editor says “Nothing to cut: no body under this sketch” or “Nothing to cut: this cut does not reach any body”, with an Add instead button, and a hint “The cut does not touch the body in this direction. Flip?”. Tick Flip direction, move the sketch so it overlaps the body, or change the End condition.

The revolve has no axis, or crosses it

A revolve needs a construction line as the axis (“Draw a construction line for the axis”) and a profile on one side of it (“The profile crosses the axis”).

Text

Lettering that does not engrave usually has overlapping strokes, a cap height under 0.8 mm, or sits in a sketch with other curves. See Text.

How CivilKit CAD tells you

WhereWhat you see
The sketch chip and coloursThe degrees of freedom, fully defined, or over-constrained.
The Constraints listThe conflicting and redundant constraints, each with a delete button.
The hint lineThe reason the last click was refused.
The editor of the next featureA card with the problem and, where it can, a button to fix it.
The feature treeA feature that fails turns red with its reason underneath. Features built on it say “blocked by” the cause.
Diagnostics in the drawerThe first failed feature, the cause in words, advice, Undo this change, and a list of the later features that failed because of it.
The status barErrors, counting the causes.

The Diagnostics tab is described in Checks and diagnostics.

Hints you may see

HintWhat it means and what to do
Too small: move the pointer fartherThe shape would have no size.
The three points lie on one lineA 3-point arc needs points that are not in a row.
Not enough points for this curveA spline needs more points; a control-point spline needs more than its degree.
A polygon needs at least 3 sidesPress + to add sides.
These two lines do not meet at a cornerFillet and Chamfer need two lines that share an end point.
The lines are parallelThe two lines never meet, so there is no corner.
The radius is too large for these lines / The distance is too large for these linesUse a smaller radius or distance.
A circle needs two cuts to trimTrim a circle where two other curves cross it.
Nothing ahead to extend toNo curve lies in the path of the end.
Start from the end of a line or arcA tangent arc continues from a free end.
Already tangentThe end is straight along the tangent: an arc would have an infinite radius.
Pick a free curve endThe bridge curve joins open ends.
The offset collapses the whole chain / The offset curves no longer meetUse a smaller offset distance.
Pick lines and arcs that form one chain (no branches)Offset needs a connected chain.
That projects to nothing on this plane (it is square-on to it)The edge is edge-on to the sketch plane.
Select edges or faces before the sketch, or click an edgeNothing was selected to project.
Type a valid valueA dimension must be a positive length, or an angle from 0 up to 360 degrees.

Next

Extrude, revolve, sweep and loft

These four features turn sketches into solids: Extrude pushes a profile in a straight line, Revolve turns it about an axis, Sweep drags it along a path, and Loft blends between several profiles. You can use each one to add material, cut material, or start a separate body.

How every solid feature works

  1. Draw the sketch (or sketches) first. See Starting a sketch.
  2. Run the command. The feature is added to the feature tree straight away with sensible defaults, the Editor opens on it, and the model shows a live preview.
  3. Change the options. The preview follows every change.
  4. Click the tick at the top of the Editor (or press Enter) to confirm, or the cross (or Esc) to cancel. Confirming is one undo step.

If the kernel cannot build the first attempt (for example Loft with profiles it cannot join), the feature still opens in the Editor as a draft with the reason shown, so you can fix the values. Cancel removes the draft.

Which sketch is used. The command uses the sketch you selected in the feature tree. With nothing selected it uses the newest sketch that still has shapes no feature has used. If every sketch is already used, the app says “Every sketch is already used by a feature. Select a sketch in the tree to use it again, or draw a new one (S).” With no sketch at all it says “Draw a sketch first”.

While you are inside a sketch, the Make group of the Sketch tab has Extrude and Revolve buttons. They finish the sketch and start the feature in one step.

Ribbon buttons with several tools. Some buttons hold a family of tools, for example Loft and Sweep. The button shows the tool you used last. Click the small triangle on it, right-click it, or press and hold to open the list. The Extrude button is the exception: it always runs Extrude, and Extruded cut is chosen from its list.

Extrude

Extrude pushes the closed shapes of a sketch along the sketch normal.

Start it from Home > Create > Extrude (Shift+E). Extruded cut (Shift+C) is in the same button’s list and starts with the operation set to Cut. Right-clicking empty canvas also lists both.

The Editor has these parts. Defaults are what a new feature starts with.

OptionWhat it doesDefault
Profile sketchThe sketch to extrude. Pick changes it.The sketch chosen as above
End conditionHow far the extrusion goes (see below).Blind
DepthLength in mm. Shown for Blind and Mid plane. For Mid plane it is labelled Total depth.10 mm
OperationNew body, Add or Cut (see below).Chosen from the situation
Body nameName of the new body. Shown for New body.Body 1, Body 2, …
Flip directionExtrude the other way. Not shown for Mid plane or Through all, both ways.Off
Draft angleTapers the walls, in degrees. 0 means straight. Not available for Mid plane or Through all, both ways.0
Draft outwardTapers the walls outward instead of inward. Shown when the draft angle is above 0.Off
End scaleScales the whole outline, holes included, in a straight line to this factor at the far end: 1 means none, 0.5 ends at half size, 1.2 grows. Works with Blind, Mid plane and Flip; hidden with Draft angle or Twist, Through all and Up to next, and not available for a surface extrude.1
Thin wallBuilds a wall around the curve instead of filling it (see Thin walls).Off
ShapesOne checkbox per closed shape in the sketch. Shown when the sketch has two or more shapes.All checked

Number fields accept expressions and variables. The draft angle is the exception: it takes a plain number. See Equations and variables.

End conditions

End conditionThe extrusion goes
BlindThe Depth you type, from the sketch plane.
Mid planeHalf the Total depth each side of the sketch plane.
Through allFrom the sketch plane through the whole body.
Through all, both waysThrough the whole body on both sides of the sketch plane.
Up to nextTo the next face of the body in the extrusion direction.

With no body yet, Through all uses a length of 1000 mm. Up to next with no body, or with no face ahead of the sketch, fails with a message in the Editor.

The kernel also knows the end conditions Up to face, Offset from face and Up to point, but it does not cut them yet, so the app does not offer them. To end a boss at a face, use Through all or Up to next, or set a Blind depth.

Add, cut or new body

The Operation control decides how the solid meets the body you already have.

  • Add joins the new solid to the body.
  • Cut removes the new solid from the body.
  • New body keeps the new solid as a separate body, even where it overlaps or touches another body. It gets a name (Body 1, Body 2, …) that you can edit. To merge bodies later, use Join in the Bodies panel. See Bodies and combining.

A new Extrude starts as:

  • Cut when you used Extruded cut.
  • Add when it is the first solid of the part, or when the sketch plane reaches the existing body.
  • New body when the part already has a solid and the sketch plane does not reach it.

You can always change it in the Editor.

Only Extrude chooses its operation this way. Revolve, Thin revolve, Sweep and Loft always start as Add; switch to Cut or New body in the Editor if you need it.

The direction is chosen for you. A boss grows away from the face its sketch sits on. A cut tries both sides and keeps the one that actually touches the body. Tick Flip direction to reverse either.

If a cut removes nothing, the Editor says “Nothing to cut: no body under this sketch.” or “Nothing to cut: this cut does not reach any body.” The second message comes with a one-click Add instead button, and a Flip direction fix is offered when the cut misses in this direction.

Draft and tips

A draft angle tapers the extrusion toward its end. A drafted extrusion of a circle comes to a point at some height. If you type a taller depth, the app lowers it to that height and says “Limited to the tip (N mm)”. Lower the angle or the depth to avoid it.

Shapes (regions)

A sketch can hold several closed shapes, and shapes inside shapes (a circle in a rectangle). By default all are extruded and inner shapes become holes. In the Shapes list, untick a shape to leave it out, or untick the outer one to extrude only the inner disc. One shape must stay ticked. Hovering a row lights the shape in the view. This also lets one sketch feed several features: a new Extrude picks up the shapes nothing has used yet.

The depth arrow

While the Extrude editor is open, an arrow on the preview sets the depth. Drag it, hold Ctrl to snap to whole millimetres, or type the number in the Editor to be exact. It is shown for Blind and Mid plane only, and not when Depth holds an expression.

Thin walls

Thin wall builds a wall of a given thickness around the curves instead of filling them. It works on open curves (a C-shape, a polyline), where it gives a wall in one step, and on closed curves, where it gives a hollow wall. It is available in Extrude, Extruded cut and Revolve. The Thin extrude, Thin cut and Thin revolve commands (Home > Create, the button after Extrude) start with it on.

OptionWhat it doesDefault
Thin wallSwitches the wall on.Off
Wall thicknessThickness in mm.About 10% of the profile size, at least 1 mm
SideInside, Outside, Both or Mid. Inside is the inner side of a bend, or the interior of a closed loop. Mid centres the wall on the curve.Inside
Other side thicknessThickness of the second side. Shown for Both.Same as Wall thickness
End capsFlat or Round. Shown when the sketch has an open chain.Flat
CornersMitre or Round.Mitre

A thickness the curve cannot take (thicker than a bend radius, or eating a short segment) shows a hint with the largest thickness that works.

If you extrude an open sketch without Thin wall, the Editor shows a card “This profile is open” with three buttons:

  • Make thin wall turns the option on.
  • Close with a line adds the missing segment to the sketch, and shows the gap in the view. It is disabled when the sketch has no single chain with two loose ends.
  • Extrude as surface turns the feature into an extruded surface (Extrude only). See Surfaces.

For the exact definition of Extrude and its thin walls, see the kernel book: extrude, thin walls.

Revolve

Revolve turns a closed profile about a line of the same sketch.

  1. In the sketch, draw the closed profile on one side of a construction line. The construction line is the axis. See Sketch tools for how to make a line a construction line.
  2. Choose Home > Create > Revolve (Shift+R), or the Revolve button in the Sketch tab.

The axis is the first construction line of the sketch. With none, the app says “Draw a construction line for the axis” and creates nothing. The Axis field in the Editor shows the line in use.

OptionWhat it doesDefault
Profile sketch, AxisThe sketch and its axis line.First construction line
End conditionBlind turns from the sketch plane by the Angle. Mid plane centres the turn on the sketch plane.Blind
AngleDegrees of turn. For Mid plane it is labelled Total angle.360
Operation, Body nameSame controls as Extrude. A new Revolve always starts as AddAdd
Flip directionTurn the other way. Not shown for Mid plane.Off
Thin wall, ShapesAs for Extrude.Off, all

A full 360 degree turn has no end caps. A profile that crosses the axis fails with “the profile crosses the axis”: move it to one side. Revolve has no draft and no other end conditions. See revolve in the kernel book.

Sweep

Sweep moves a closed profile along an open path.

  1. Draw the path as an open chain of lines and arcs in one sketch, or, for a path that bends in all three directions, as one spline in a 3D sketch.
  2. Draw the profile as a closed shape in a second sketch on a plane that is perpendicular to the path at its start.
  3. Choose Home > Create > Sweep (Shift+W), or pick it from the Loft button’s list.

With nothing selected, Sweep takes the newest unused closed sketch as the profile and the newest unused open sketch as the path. The Editor lets you change both.

OptionWhat it doesDefault
Profile (closed)The profile sketch.Newest unused closed sketch
Path (open)The path sketch.Newest unused open sketch
Guide curvesOpen sketches the profile scales to follow. Add guide adds one; the guide must be as long as the path.None
Twist over the pathDegrees of turn along the path. Hidden when there are guide curves.0
Operation, Body nameAs for Extrude.Add

Common failures: the profile is not perpendicular to the path start, the path has a sharp kink, or a corner between a line and an arc is not tangent (make the arc tangent). Sweeping into a sheet is not available. A helix (see Reference geometry) cannot be chosen as the path in the Editor: its Path list shows open sketches only. See sweep in the kernel book.

Loft

Loft joins two or more profiles in order, like a skin stretched between them.

  1. Draw one sketch per profile, each closed, on its own plane (for example offset planes).
  2. Select the profile sketches in the tree in the order you want, using Ctrl-click, or leave nothing selected.
  3. Choose Home > Create > Loft (Shift+O).

With no selection, Loft takes the unused closed sketches drawn since the last solid feature, in tree order, or else the two newest unused ones.

OptionWhat it doesDefault
ProfilesThe ordered list of sketches. Each row has a drop-down and up, down and remove buttons. Add profile adds a row. At least two.The sketches chosen as above
Auto-orderAppears when the profiles do not follow each other along the loft. One click sorts them.
Guide curvesOpen sketches the loft follows along its length. Add guide adds one.None
Make a surface (not a solid)Builds a sheet instead of a solid. Profiles may then be open curves, all of one kind.Off
Operation, Body nameAs for Extrude. Hidden for a surface.Add
Start tension, End tensionHow strongly the loft leaves the first and last profile along its normal. 0 means free.0

Points. The first or the last profile may be a sketch holding a single point. The loft then comes to a tip there. Only one end can be a point; a point cannot be in the middle, and it cannot be combined with guide curves or with a surface loft. The Editor explains whichever rule you break.

Order. If the profiles do not run in order along the loft it would fold back on itself. Use Auto-order. A loft can only use sketches that come before it in the tree. If you pick a later sketch, the loft moves to just after it and the app says “Loft moved after …”.

Each profile must be one closed region. Profiles with holes make a hollow loft; they need the same number of holes. See loft in the kernel book.

Sphere

A sphere needs no sketch. Choose Home > Create > Primitives > Sphere and click a face or plane, or open the Catalog (Shift+K), go to Primitives, and drop Sphere (adds material) or Dimple (removes material, a spherical pit). A solid ball is a Sphere feature centred where you drop it. A hollow ball (set Sphere wall (mm) above 0 and below half the size) is built from a revolved profile instead, and has the Revolve options. See Catalog parts.

Double-click a Sphere feature in the tree to edit it:

OptionWhat it doesDefault
RadiusBall radius in mm.Half the size set when it was dropped
Centre X, Centre Y, Centre ZPosition of the centre in mm.Where it was dropped
OperationNew body, Add or Cut.As dropped (Add or Cut)
Body nameName of the new body. Shown for New body.Body 1, Body 2, …

A ball dropped on a face is centred on the spot, so it is half in and half out of the face: it adds a dome or cuts a pit.

Common mistakes

SymptomCause and fix
“Draw a sketch first”No sketch exists. Draw one, then run the command.
“This profile is open”The sketch is not a closed loop. Close it, use Thin wall, or make a surface. See When a sketch will not solve.
An extruded cut changes nothingThe sketch plane does not reach the body, or the cut goes the wrong way. Use Flip direction, or Add instead.
A new body appears when you wanted to addThe sketch plane did not touch the existing body. Switch Operation to Add.
Extrude with a draft is shorter than DepthThe taper closes to a tip. Lower the angle or the depth.
Revolve failsNo construction line, or the profile crosses it.
Loft twists or foldsProfiles are out of order, or start points differ. Use Auto-order.

Next

Torus

A torus is a ring made from numbers, with no sketch. Choose Home > Create > Primitives > Torus. It appears at the origin about the Z axis. In the Editor set the centre, the axis (x, y, z or a vector), the Ring radius (from the axis to the middle of the tube) and the Tube radius (smaller than the ring radius), and whether it adds, cuts or is a new body.

Pipe

A pipe is a round tube along an open sketch. Draw an open chain of lines and arcs, then choose Home > Create > Pipe (the picked sketch, else the last open one). Set the outer Radius; give it a Wall (thinner than the radius) to make the tube hollow. It is built like a sweep, with the round section at the start of the path.

Coil

A coil is a spring: a round wire wound round an axis, with no sketch. Choose Home > Create > Pipe > Coil. Set the Radius (axis to the middle of the wire), the Wire radius, the Pitch and the Revolutions (or a Height, which gives the turns), and Left hand. The pitch must be larger than the wire is thick, and the radius larger than the wire radius.

Bounding solid

A bounding solid is the box that just holds the bodies you pick. Pick a face on each body (or nothing, for every solid body) and choose Home > Create > Pipe > Bounding solid. It is always a new body; Padding grows it on every side, and a flat body needs some padding to have any thickness.

Dome

A dome raises a spherical cap on a flat face bounded by one circle. Pick that face and choose Dome (Features > Modify). Set the Height; a negative height cuts a dimple into the body. A face that is not a plain circle is refused, and an oval dome is not built.

Split face

Split face cuts flat faces in two without cutting the body: the solid and its volume stay, and each cut adds a face. Pick the faces and choose Features > Modify > Split face. It starts with the plane across the middle of the longest side; in the Editor change the plane and Offset, or cut by the lines of a sketch instead. Round faces are not supported, and a plane that misses every picked face is refused.

Reference geometry

Reference geometry is construction aid that has no volume of its own: planes to sketch on, axes to turn things about, and helix curves. You make them from the Reference group of the Features tab, which has a button each for Plane (Shift+N), Axis (Shift+A) and Helix.

None of these change the solid. They appear in the feature tree and in the view, and later features use them.

Plane

A reference plane is a flat sheet of any size that you can sketch on, mirror about, or hang another plane from.

Create one

The command picks its starting point from what you have selected:

You selectedThe new plane
Two facesA Midplane: halfway between them
One flat faceAn Offset plane, 10 mm from that face
A Plane feature in the treeAn Offset plane, 10 mm from it
The Front, Top or Right plane in the treeAn Offset plane, 10 mm from it
NothingAn Offset plane, 10 mm from the Front plane

The plane’s name is made from its settings, for example “Plane 10 from Front” or “Plane between F2.C1 and F2.C0”. It updates when you change the offset or base, until you rename it yourself.

The Plane editor

ControlWhat it doesDefault
ModeHow the plane is made: Offset, Angle, Midplane, Parallel, Three points. Origin and directions appears only for a plane that already uses itOffset (Midplane for two faces)
OffsetDistance in mm along the base plane’s normal. A negative value goes the other way10
AngleDegrees. Shown only for a plane that already has an angle
Flip directionTurns the plane around so it faces the other way. In Offset mode the base is flipped before the offset is applied, so the plane lies on the other side of the base (offset 10 flipped is 10 mm the other way). In Angle mode it negates the angle. Shown only for a plane that already has it set; a new plane starts without itOff
Base planeThe plane to start from: Front Plane, Top Plane, Right Plane, an earlier Plane feature, or the face it hangs on (“Face F2.C1”)The base chosen as above

Offset and Midplane are complete: pick the base (and, for a midplane, the two faces at creation) and the plane is built. The other modes need extra references that the Editor cannot set yet: Angle needs a line to turn about, Parallel needs a point, Three points needs three points, Origin and directions needs vectors. If you switch a plane to one of them it fails with a “missing reference” error and the plane is not built. Switch back to Offset or Midplane. For midplanes, the Editor can change the first base only; to change the second face, delete the plane and make it again.

The kernel has more plane modes (perpendicular, line and point, normal to a path or curve, tangent to a cylinder or sphere). The app uses the tangent plane by itself when you sketch on a curved face. See planes in the kernel book.

Using a plane

  • Sketch on it. Select the plane in the tree and press S, or choose Sketch on selected face or plane. The sketch origin is the plane’s origin. See Starting a sketch.
  • Mirror about it. Pick it in the Mirror editor. See Patterns, mirror and scale.
  • Draft against it. A plane can be the neutral plane of a draft. See Fillets, chamfers, shells and drafts.
  • Base another plane. Select it, then run Plane again.

Planes are drawn only while the Planes layer is on (View > Appearance > Show). A plane that follows a face moves when the face moves.

Limits

A plane made from a face needs that face to be flat. If an earlier edit removes the face or base a plane hangs on, the plane fails, and so do the sketches built on it. See The feature tree and history.

Axis

An axis is a straight reference line.

Create one

You selectedThe new axis
One cylindrical faceThe cylinder’s centre line
Two facesThe line where their planes meet
NothingThe line where the Front and Top planes meet (the X axis)

If you select one flat face, the command makes the axis, then the kernel reports that the face is not cylindrical and nothing is added. Select a cylinder, or two faces. Only the first two selected faces are used.

The Axis Editor has no fields: the references are fixed when it is created. To change them, delete the axis and make another.

Using an axis

An axis is drawn while the Axes layer is on. The kernel lets a plane in Angle mode turn about it, but the app’s editors do not yet offer an axis feature in a list. The Circular pattern axis is a choice of the X, Y or Z axis (through the origin or through a point), a typed direction, or a picked edge or round face, and Revolve uses a construction line in its own sketch. So an Axis is mostly a visual and measuring aid today. See Patterns, mirror and scale and Extrude, revolve, sweep and loft.

For the exact definition, see axis in the kernel book.

Helix

A helix is a spiral curve around an axis, such as the centre line of a spring or a screw. It adds no solid.

Create one

  1. Draw a sketch with a circle. The circle gives the radius and the centre. See Sketch tools.
  2. Choose Features > Reference > Helix.

The command uses the sketch selected in the tree, else the last sketch with a circle. It is greyed out if there is none. The helix runs along the sketch normal, through the circle’s centre, starting at the sketch plane.

The Helix editor

ControlWhat it doesDefault
Profile sketchThe sketch with the circleThe sketch chosen as above
Defined byWhich two sizes are set: Pitch and revolutions, Pitch and height, Revolutions and heightPitch and revolutions
PitchRise per full turn, in mmAbout 10% of the smallest body dimension, rounded to a tidy value (1 with no body)
RevolutionsNumber of turns5
HeightTotal rise in mm10
Start angleWhere the helix starts, in degrees from the sketch’s x axis0
leftHandCheck for a left-hand helix. The label is the raw field nameOff (right hand)
Reverse directionRises against the sketch normalOff

The third size is calculated from the two you choose with Defined by. With the default, Height has no effect.

Known gap: the kernel reads the Defined by choices as “pitch and revolutions”, “height and revolutions” and “height and pitch”. The app’s list names Pitch and height and Revolutions and height with different internal names, so for now those two choices behave like Pitch and revolutions. Use Pitch and revolutions, and set Pitch and Revolutions to get the height you want (height is pitch times revolutions).

Using a helix

A helix is a curve, drawn while the Curves layer is on. The kernel can sweep a profile along a helix to make a spring or coil. The Sweep editor in the app, however, lists open sketches only as paths, so you cannot pick a helix there. For threads, use the Thread feature instead. See Holes and threads. To sweep along a helix today, use scripting. See Scripting.

For the exact definition, see helix in the kernel book.

Next

Fillets, chamfers, shells and drafts

These features change a body that already exists. Fillet rounds edges, Chamfer bevels them, Shell hollows the body, and Draft tilts faces so a part can leave a mould. You select edges or faces on the model first, then run the command.

Selecting what to change

Pick modes decide what a click selects. The Select tab and the keys switch them: Face (Q), Edge (E), Corner (V), Body (B). The mode named Auto picks whatever is nearest the pointer. See Selecting things.

  • Fillet and Chamfer accept selected edges, selected corners, or two or more selected faces.
    • Edges: each selected edge is rounded.
    • A corner: every edge that ends at the corner is rounded, so rounding a cube corner rounds its three edges.
    • Two or more faces: every edge that two of the selected faces share is rounded. For two faces that is their common edges, including every arc of a ring that is split into arcs. If the faces share no edge, the command says “These faces do not share an edge” and adds nothing.
  • Shell needs one or more selected faces: the faces that are left open.
  • Draft needs one or more selected faces: the faces to tilt.

A command that cannot run is greyed, and its tooltip says why. The messages include “Select edges, or two or more faces, to round”, “Select a second face (or select edges) to round”, “Switch to edge selection to round edges” and “Select one or more faces to leave open”.

Each command is also in the canvas right-click menu: right-click an edge or corner for Fillet and Chamfer, and a face for Fillet, Chamfer, Shell and more.

Fillet

A fillet rounds the sharp edge between two faces with a smooth arc.

  1. Select the edges (or faces) as above.
  2. Choose Home > Modify > Fillet (Shift+F). Chamfer (Shift+B) shares the same button and is in its list: click the small triangle on the button.
  3. The Editor opens with a small radius, so the first preview shows only a slight rounding. Type the radius you want, then confirm with the tick or Enter.

A new fillet starts with a small radius: about 5% of the smallest dimension of the body, rounded to a tidy value (a 40 x 25 x 10 mm body gives 0.5 mm). Change it to the size you need. A new chamfer starts with the same small distance.

OptionWhat it doesDefault
EdgesThe list of edges. Use selection fills it from the model and keeps following the selection until you click Done.The selected edges
RadiusConstant radius in mm. For the Chordal profile it is labelled Chord width.About 5% of the smallest dimension
Variable radiusGives each edge a Start radius and an End radius that blend along it. The start is the end of the edge nearer where you picked it. These two fields take plain numbers, not expressions.Off
ProfileThe cross-section of the round (see below).Circular
Conic ratio (0 to 1)Fullness of a conic round. Shown for Conic.0.5
Shape (0.1 to 1)Shape of a curvature-continuous round. Shown for Curvature continuous (G2).0.5
Tangent chainAlso rounds the edges that continue the selected ones smoothly.On

Profiles.

  • Circular is the usual round, a circular arc.
  • Conic is flatter or fuller than a circle, controlled by the Conic ratio.
  • Chordal is sized by the width of the chord rather than the radius.
  • Curvature continuous (G2) blends into both faces without a visible change in curvature, controlled by Shape.

Tangent chain. With it on, selecting one edge of a rounded outline rounds the whole outline: edges that meet at a vertex and continue each other within 1 degree, and the other arcs of a ring split into arcs. The extra edges are lit before you run the command, and the Editor says “N more edge(s) added through the tangent chain”. Face selections are not chained. The choice is remembered in your browser. Switching it in the Editor re-applies it to the feature’s edge list.

Variable radius rules. Edges that meet at a corner of a variable fillet need the same radius where they meet. A radius of 0 at one end is built as a very small radius.

Corners. Where three rounded edges meet at a convex corner, the kernel adds a spherical patch. If edges meeting at a corner have different radii they end in a mitre, and the feature shows a warning.

Twisted extrudes. A fillet rounds the edges of an extrude with a Twist set (the helical gear and screw shapes) up to about 30 degrees of twist, and a ring of four edges, such as the top of a twisted square, up to about 45 degrees. A chamfer on twisted faces, and rings at 60 degrees and more, are still refused with the reason; reduce the twist or round before twisting.

Not offered: the corner (vertex) chamfer type and the full-round fillet between three faces.

Handle. With an edge selected, a yellow dot appears beside it. Drag it outward for a new fillet, or inward for a chamfer, and release to make the feature. With an edge next to an existing fillet or chamfer, drag the dot to change its size in place. Hold Shift for fine movement, Ctrl for whole millimetres, or type a number while dragging (a minus sign makes a chamfer) and press Enter. Esc cancels. You can switch handles off in the workspace settings.

See fillet in the kernel book.

Chamfer

A chamfer cuts a flat bevel along an edge. Select edges exactly as for Fillet and choose Chamfer (Shift+B).

OptionWhat it doesDefault
Chamfer typeEqual distance, Two distances, or Distance and angle.Equal distance
Distance (Distance 1)The leg of the bevel, in mm. Same default as a fillet radius.About 5% of the smallest dimension
Distance 2The second leg. Shown for Two distances.Same as Distance 1
AngleThe angle between the bevel and the first face, in degrees. Shown for Distance and angle.45
Tangent chainAs for Fillet.On

For Two distances and Distance and angle, Distance 1 is measured on the first face of each picked edge. If the legs end up on the wrong faces, swap the two values. See chamfer.

Shell

Shell hollows the body to a wall thickness and removes the faces you selected, leaving an open box or a cup.

  1. Switch to Face mode and select the faces to leave open.
  2. Choose Home > Modify > Shell (Shift+S).
OptionWhat it doesDefault
FacesThe faces to open. Use selection refills it.The selected faces
Wall thicknessThickness of the walls in mm.The larger of 1 mm and 2% of the smallest dimension, rounded to 0.1
Grow outwardBuilds the walls outward from the existing surface instead of inward.Off

With the shell selected, an arrow on the inner wall changes the thickness when you drag it.

A wall that is too thick for the part fails with “the wall is thicker than the part allows”. The Editor offers Use suggested thickness (N mm), the largest wall that works. Walls also fail where a tight inside curve is smaller than the wall: use a thinner wall, or round the curve first. See shell.

Draft

Draft tilts faces by an angle about a neutral plane. Use it on the walls of a moulded or cast part so it can be pulled out of the tool.

  1. Switch to Face mode and select the faces to tilt.
  2. Choose Features > Modify > Draft (Shift+G).
OptionWhat it doesDefault
FacesThe faces to tilt.The selected faces
AngleDraft angle in degrees.3
Neutral planeThe plane that stays fixed, and whose normal is the pull direction. Pick sets it from a selected face.The plane of the first sketch in the part

Faces keep their names when drafted, so later features still find them. A face parallel to the neutral plane cannot be drafted. An angle that turns an edge over fails with the kernel’s message “edge <faces> turns over”, naming the two faces that meet at the edge: use a smaller angle. Faces that continue a drafted face smoothly are drafted with it. See draft.

To check the result, use Draft analysis on the Evaluate tab. See Surfaces.

You can also taper an extrusion directly with its Draft angle option. See Extrude, revolve, sweep and loft.

Rib and lip

Two more edits sit beside Draft in Features > Modify.

  • Rib adds a thin wall from an open sketch line to the body. Draw a line or chain that reaches the body, then choose Rib. The Editor has Profile and Thickness (about 10% of the smallest dimension at first), and a Rib section with the side of the sketch plane the thickness goes to, a Fillet on the free edge, a Draft angle and, once the part has named bodies, Extend to (the bodies the rib grows to). A line that does not reach the body fails with “does not touch the body”. See rib.
  • Lip / groove adds a raised band along the rim of a flat face, or cuts a groove into it. Select the rim face (Face mode), then choose Lip / groove. It follows every edge of the picked faces. The Editor has Kind (Lip or Groove), Width and Height, both about 5% of the smallest dimension at first. See lip.
  • Split body (Features > Modify) cuts the body at a plane into two bodies, named Base and Lid. With a planar face selected the plane is that face; otherwise it is the standard plane that cuts the smallest side of the body, through the middle. The Editor has Plane (Front, Top, Right, a reference plane, or Pick to take a planar face), Offset along the plane normal, Reverse, the two body names, and Keep (both halves, or only one).
  • Lip joint (Features > Modify) does the same split and also gives the cut a tongue on one half and a groove on the other, for a shelled box and its lid. The Editor adds Tongue on (which half), Tongue height, Tongue width (a fraction of the wall, or millimetres), Centred in the wall (or a distance from the outer wall) and Clearance of the groove (0.2 mm at first), which makes the groove wider on each side and deeper by that much. The preview shows the two halves as you change the numbers. A tongue that does not fit the wall is refused with the reason (inset + width + clearance more than the wall), and a solid body, which has no wall, needs the width and the distance in millimetres.

The two-part case page builds a box and its lid with these and checks the volumes.

A bracket with a rib

This script builds a base plate with four holes, an upright block that carries a round boss with a bore, and a triangular rib that braces the block to the plate. It is the Script tab version of the Rib above, and it shows the things that most often go wrong.

part('Clevis')
  .sketch('top', (s) => s.rrect(140, 90, 8)).extrude(12)                          // plate
  .holes.points(face('>Y'), [[-55, -30], [55, -30], [-55, 30], [55, 30]], { diameter: 10 })
  .sketch('front', (s) => s.rect(30, 79, [15, 45.5])).extrude(60, { mid: true })   // block
  .sketch('front', (s) => s.circle(25, [15, 85])).extrude(60, { mid: true })       // boss
  .sketch('front', (s) => s.line([-50, 12], [-5, 70])).rib(15)                     // rib: ONE open line
  .sketch('front', (s) => s.circle(15, [15, 85])).cut(through(), { direction: 'both' }); // bore

The part is one valid body of about 335,157 mm³. The numbers are written out so the example stands alone; to make them editable, declare them with variables as described in Scripting.

How the rib works:

  • One open line. The rib is drawn as a single line, from [-50, 12] to [-5, 70]. It is centred on the sketch plane and 15 is its total thickness. Both ends are extended until they meet the body, and the result is fused to it, so the line may stop short of the block or lie a little inside the plate.
  • Not a closed triangle. A closed triangle in rib fails with ribNeedsOpenSketch. The opposite mistake is extruding a single open line: that fails with noClosedProfile. For a thin wall made from an open line, use thin on the extrude.
  • Feature order. The rib may come before or after the bore: the web stops at the outer wall of the body and never fills a bore the line runs through, so both orders give the same part.
  • Cut direction. The bore is sketched on the mid-plane of the block, so a cut through everything needs direction: 'both'. Without it the cut goes one way only and may miss.

The rib takes four optional settings, in the GUI and in the script call .rib(thickness, { fillet, draft, side, target, flip }):

SettingMeaning
side'both' (the default) centres the thickness on the sketch plane; 'right' puts all of it on the side the sketch normal points to, 'left' against it.
filletRadius of a round on the two edges of the free edge. It must be less than half the thickness.
draftTaper of the two side faces in degrees (0 to 45): the rib is thickness thick at the free edge and widens toward the body. It needs a sketch that is one straight line.
targetA body name or a list of names. The rib grows to those bodies only; the others are left alone. By default it grows to every body it reaches.

For example .sketch('front', (s) => s.line([-50, 12], [-5, 70])).rib(15, { fillet: 3, draft: 2 }) rounds the free edge of the clevis rib and tapers its sides. A rib on a part with named bodies can grow to one of them with target: 'Bracket'.

Two mistakes to avoid. Extruding one open line fails with noClosedProfile, and the error now says to use Rib for a web or Thin wall for a thin wall. And a through cut from a sketch on the middle of the part cuts one side only unless you give direction: 'both'; the script run warns about it.

When a feature fails

A fillet, chamfer or shell the kernel refuses still opens its Editor as a draft, with a plain-words reason. Cancel removes the draft.

MessageWhat to do
“the rounding runs off the faces beside it”The radius is wider than the neighbouring faces. Use a smaller radius, keep Tangent chain on so the round runs on through corners, or round fewer edges at once.
“the radius is too large for these edges”Use a smaller radius.
“the rounding could not be built”Try a smaller radius, fewer edges at once, or a different order.
“this edge or corner shape cannot be rounded yet”Try fewer edges, a chamfer instead, or leave the rounding to the end of the history.
“the wall is thicker than the part allows”Use a thinner wall, or click Use suggested thickness.
“a face or edge it uses no longer exists”An earlier edit renamed or removed what the feature was built on. Pick the edges or faces again, or undo. See The feature tree and history.

Rounding order matters. Large rounds first, small rounds and chamfers last, and rounds at the very end of the history are the least likely to break when you edit an earlier feature.

Next

Cases and moulds

A two-part case is a shelled box cut into a base and a lid, with a tongue on one half and a groove on the other so the halves locate and close. A mould is a block with the part cut out of it, split into two halves. Both start from the same step, a split of one body by a plane. This chapter builds a case with the commands and with a script, and describes the mould recipe. For a plain closed box with a lipped lid in one step, use the Case wizard (Features > Create > Case).

Split body

Split body (Features > Modify) cuts a body at a plane into two bodies. A picked planar face is the plane; with nothing picked it is the standard plane across the smallest side of the body, through the middle, which is where a case is cut. The two halves are named Base and Lid.

The Editor has:

OptionWhat it doesDefault
PlaneFront, Top, Right or a reference plane. Pick in the Plane section takes a planar face instead.Across the smallest side
Offset along the plane normalMoves the plane.The middle of the body
Reverse the plane normalTurns the plane round, which swaps the half below with the half above.Off
Body below the plane, Body above the planeThe names of the two halves. “Below” is the side the plane normal points away from.Base, Lid
Body to splitShown only when earlier features named several bodies.The only body
KeepBoth halves, or only the half below or above.Both halves

A plane that does not cross the body fails with cutNoEffect. The faces keep their names; the cut face of each half belongs to the Split feature. See split in the kernel book.

Lip joint

Lip joint (Features > Modify) does the split and then follows the outer boundary of the cut face, which for a shelled box is the outside of the wall, and makes:

  • a tongue on one half, standing out of the cut face by the tongue height, with a width and a distance from the outer wall;
  • a groove in the other half in the same place, wider by the clearance on each side and deeper by the clearance.

The Editor has everything Split body has, and:

OptionWhat it doesDefault
Tongue onThe half below or above the plane.Below
Tongue heightHow far the tongue stands out of its half, in mm. The groove is this plus the clearance deep.15% of the smallest dimension of the body, rounded
Tongue width asA fraction of the wall thickness, or millimetres.A fraction, 0.5
Centred in the wall / Distance from the outer wallCentred, or the distance in mm from the outer wall to the tongue.Centred
Clearance of the grooveThe gap between tongue and groove on each side and at the top, in mm.0.2

The wall thickness is measured on the cut face, at its narrowest. A tongue and its clearance that do not fit the wall are refused with the numbers (inset + width + clearance more than the wall). A solid body has no wall to measure: give the width and the distance in millimetres. The tongue and groove follow flat cut faces with a closed outline; a curved rim is refused in the way Lip / groove refuses it.

A two-part case with a script

This script builds a 80 x 50 x 30 mm hollow box with 2 mm walls and cuts it at mid height with a joint: a tongue 1 mm wide and 1.5 mm high, centred in the wall, and a groove 0.2 mm wider on each side and 0.2 mm deeper.

part('Case')
  .sketch('front', (s) => s.rect(80, 50)).extrude(30)
  .feature({ type: 'shell', faces: [], thickness: 2 })              // no open face: a closed cavity
  .lipJoint(at('front', 15), { height: 1.5, width: 1, clearance: 0.2, names: ['Base', 'Lid'] });

The result is two valid bodies, Base and Lid. The numbers that prove the fit:

Volume (mm³)
The hollow box before the cut29 104
Tongue added to the base: 1.5 x (the area between the outline offset by 0.5 and by 1.5)378
Groove removed from the lid: 1.7 x (the area between the outline offset by 0.3 and by 1.7)599.76
The two bodies together28 882.24

The total is the box plus the tongue minus the groove: 29 104 + 378 - 599.76. The groove is larger than the tongue by 221.76 mm³: that void, 0.2 mm on each side and at the top, is the clearance. The two bodies do not overlap (Evaluate > Overlap reports none).

The section below is the same joint on a small 16 x 12 x 10 mm case (the 0.2 mm gap would be two pixels wide at 80 mm):

What to know:

  • Shell first, with no open face. shell with an empty faces list closes the cavity, so both halves are cups. To get an open box, shell with faces: [face('>Z')] instead: the “lid” is then a ring of wall and the groove still follows it.
  • The plane is at('front', 15). front runs along +Z, so the offset is the height of the cut. The half under the plane is “below” and is named first in names.
  • Name the halves, then target them. names gives the two halves their names (Base and Lid unless you change them in the editor); they show in the Bodies panel and stay through later features. A cut made after the joint with no body named meets each half on its own, so the halves are not joined again where they touch. To change only one half, name it: from: 'Lid' in a script, or the Cut from list of a cut, which names the bodies of the part once a split has named them. In a test, a through cut with from: 'Lid' left the base unchanged and kept both names. A boss or other added solid that crosses the seam was not tested; add it before the split.
  • Wall thickness is read from the cut face. width and inset can also be given in mm; widthRatio (default 0.5) is a fraction of the wall.
  • Clearance for printing. 0.2 mm suits an FDM printer; use a larger value for a looser print, a smaller one for resin.
  • Not done yet. Snap fits, screw bosses and a seal groove are not part of the joint, and a split along a curved or tilted surface needs a different tool (the plane must be flat).

.split(plane, { names }) does the cut alone, and .lipJoint(plane, { height, width, widthRatio, inset, clearance, tongue, names }) takes the options above; both are in the script reference.

A mould from a part

A mould half is the part’s negative in a block. The steps use the bodies and booleans described in Bodies and combining:

  1. Make the part a body with Operation New body, named Part.
  2. Scale for shrinkage. Scale Part by 1 / (1 - shrinkage); a 2% shrinkage gives 1.0204. See Scale.
  3. Make a block around it, also as a New body, named Block.
  4. Cut the cavity. Combine bodies, Cut, target Block, tool Part, with Keep tools on, so the shrunk part stays next to the mould for checking.
  5. Split the block along the parting plane with Split body, names Lower and Upper.

As a script:

part('Mould')
  .sketch('front', (s) => s.circle(12)).extrude(20, { newBody: 'Part' })                   // the part: a 24 x 20 mm cylinder
  .feature({ type: 'scale', factor: 1 / (1 - 0.02), bodies: [{ body: 'Part' }] })         // 2% shrinkage
  .sketch(at('front', -10), (s) => s.rect(60, 60)).extrude(40, { newBody: 'Block' })      // the block, 10 mm past the part each end
  .combine('cut', 'Block', 'Part', { keepTools: true })                                   // the cavity
  .split(at('front', 10), { target: 'Block', names: ['Lower', 'Upper'] });                // the parting plane, half way up the part

Run on the kernel, the script gives three valid bodies and no warnings:

BodyVolume (mm³)
Part, the shrunk positive: π x 12² x 20 x 1.0204³9 613.11
Lower67 193.44
Upper67 193.44

Lower and Upper together are the 60 x 60 x 40 block (144 000 mm³) minus the cavity: 144 000 - 9 613.11 = 134 386.89. Each half holds half the cavity, so the cavity is the shrunk part. Here the part sits wholly inside the block, so the cavity is closed until the split opens it; a real mould leaves the part’s flat face on the parting plane or the block face.

What the recipe does not do: it adds no draft angle (draft the faces of Part on each side of the parting plane first, with Draft), it makes a flat parting plane only (a stepped or curved parting surface needs a kernel feature that does not exist yet), it does not detect undercuts, and sprues, vents, ejector pins and registration keys are modelled by hand with extrudes and cuts on Lower and Upper.

Holes and threads

The Hole feature drills plain, counterbored and countersunk holes at points you place on a face, using standard metric sizes. The Thread feature then marks a hole wall or a shaft as threaded, either as a drawing-style marker or as a real helical groove.

Make a hole

A hole is drilled at the points of a sketch. There are two ways to start.

From a face.

  1. Select one flat face of the body. Face mode (Q) makes this easy.
  2. Choose Home > Create > Hole (Shift+H).
  3. A new sketch opens on that face with the Point tool active and the hint “Place the hole centres with the Point tool or use Corner holes, then confirm the sketch”. Click to place one point per hole.
  4. Confirm the sketch with the tick. The hole is added and the Hole editor opens on it.

If you confirm a sketch with no point, the hint appears again and no hole is made. Cancelling the sketch adds nothing.

From a sketch of points. If the part already has a sketch that contains point entities, Hole with no face selected uses it at once. It uses the sketch selected in the tree, else the last sketch that has points. Draw such a sketch with the Point tool on a face or plane. See Sketch tools.

The direction is chosen so the hole goes into the body. If it points the wrong way, tick Flip direction in the Editor.

Hole is disabled until the part has a solid and you have either one face selected or a sketch of points. The right-click menu on a face also lists Hole.

Corner holes

When you start a hole from a face, a Corner holes card appears at the top right of the canvas. It places mounting holes on a rectangular plate in one click.

FieldWhat it doesDefault
InsetDistance from both edges to each hole centre, in mm.10
Match corner fillet (R x mm)Shown when the face has equal rounded corners. The inset follows the corner radius, so each hole sits concentric with its corner.On when shown
Holes along X, Holes along YHoles on each row and column, corners included. 2 and 2 is the four corners. 3 adds a hole in the middle of each side.2 and 2

Click Place holes, then confirm the sketch. Placing again replaces the earlier corner points, but keeps points you added by hand. When you reopen the hole later, the same card shows with Update holes, which re-places the points against the face as it is now (useful after the plate changes size) without touching the hole’s size or type.

The card refuses an inset of 0 or less, or of half the plate or more, and counts below 2. It warns when less than 1 mm of material is left at the edge. If the face is not a rectangle with equal corners, the holes are placed against its bounding box and the card says so. Slanted edges, unequal corners and slots all fall into this case. The inset is a plain number. The card is not shown for a sketch on a standard plane (use the Point tool).

The Hole editor

Double-click the hole in the feature tree to reopen it. The Editor has five sections.

ControlWhat it doesDefault
Hole typeSimple, Counterbore or Countersink.Simple
Counterbore diameter, Counterbore depthSize of the step. Counterbore only.Table values for the size
Countersink diameter, Countersink angleSize and included angle of the cone. Countersink only.Table diameter, 90 degrees
SizeM2 to M24, or Custom diameter. Custom is for Simple holes only.M6
DiameterHole diameter in mm. Custom only.
FitTap drill, Close, Normal or Loose. Tap drill is for Simple holes only.Normal
Hole diameterA read-out of the finished diameter from size and fit.
End conditionBlind, Through or Up to next.Through
DepthDepth in mm. Blind only.Twice the diameter, at least 10 mm
Drill point tip (118 degrees)Ends a blind hole in a drill-point cone. Blind only.Off
Flip directionDrills the other way.Off
ThreadedAdds a thread to the wall (see below). Simple holes only.Off

A new hole starts with the type, size and fit of the last hole you confirmed. A custom diameter is not remembered. Number fields take expressions and variables. See Equations and variables.

Sizes and fits

Choosing a size fills in everything that goes with it. The hole diameter depends on the fit: Tap drill suits a hole you will tap, Close and Normal are clearance for a bolt, and Loose is a generous clearance. All values are in mm.

SizeTap drillCloseNormalLooseCounterbore diameter x depthCountersink diameter
M21.62.22.42.64.3 x 2.34.4
M2.52.052.72.93.15.0 x 2.85.5
M32.53.23.43.66.5 x 3.46.5
M43.34.34.54.88.0 x 4.48.6
M54.25.35.55.810.0 x 5.410.4
M65.06.46.67.011.0 x 6.412.4
M86.88.49.010.015.0 x 8.616.4
M108.510.511.012.018.0 x 10.620.4
M1210.213.013.514.520.0 x 12.624.4
M1614.017.017.518.526.0 x 16.632.4
M2017.521.022.024.033.0 x 20.640.4
M2421.025.026.028.040.0 x 24.848.4

The counterbore values follow ISO 4762 socket-head screws, and the countersink diameters follow ISO 10642. Counterbores and countersinks always use an ISO size, so they have no Custom diameter. For them, Tap drill counts as Normal. You can type your own counterbore or countersink dimensions; impossible values (a step wider than the body, a cone with no room) come back as an error with a hint.

For a size that is not in this table, choose Custom diameter on a Simple hole.

Holes in a part with several bodies

A hole cuts every body it meets. A hole feature in a part file can carry a target that names the bodies it drills, as extrude and revolve do; the Hole editor does not have the field, so set it in the file or the script’s raw .feature({ type: 'hole', ... }). See the kernel book, “hole”.

End conditions

  • Blind drills to the Depth you type.
  • Through drills through the whole body. There is no bottom face.
  • Up to next is offered, but the kernel currently drills it the same as Through.

Several positions

A hole with several points shares one set of settings: editing it edits all positions at once. Each position has its own wall, which matters for threads.

The diameter handle

For a Simple hole, select the cylindrical wall of the hole in the view. A dot appears on the wall. Drag it to change the diameter, which then becomes a Custom diameter. Counterbore and countersink holes take their sizes from the table, so there is nothing to drag.

For the exact definition, see hole in the kernel book.

Teardrop holes for 3D printing

A hole printed on its side sags at the top, because the roof of a round hole has nothing under it. A teardrop adds a peak above the round hole, with sides no steeper than the printer’s overhang limit, so every layer rests on the one below. Teardrop hole puts that peak on a hole you already have.

  1. Select the wall of the round hole (face mode, Q) and choose Teardrop hole in the right-click menu (or the command search).
  2. Choose which way the peak points. Peak points toward is the direction that is up when the part is printed; it starts at the model’s up direction. The direction is projected onto the plane of the hole’s mouth, so the hole must not run along it (the dialog says so). Turn by rotates the peak about the hole’s axis, counter-clockwise seen from the mouth.
  3. Peak angle is each side’s angle from the peak’s axis. 45 degrees makes a 90 degree peak, the usual limit for printing without support. It can be 20 to 60.
  4. Tick Flat top to cut the tip off flat: a printed bridge across the top is easier than a sharp tip. Flat at is its distance from the hole’s centre, between the tangent points and the tip.
  5. When the hole is part of a pattern, Pattern adds the peak to all of its holes at once; untick it for the picked hole only. Press Add teardrop.

The round hole stays exactly as it is. The peak is cut along the same axis, as deep as the hole (through, or the blind hole’s depth), as a Teardrop folder in the tree: a plane, a sketch and a cut for each hole. Switch the folder’s eye off to see the plain hole again, or undo to remove it in one step. The peak is a cut, so it follows the hole only until you change the hole: if you move or resize the round hole later, delete the folder and add the teardrop again.

A 6.6 mm hole with the usual 45 degree peak reaches 4.67 mm from its centre (the radius times the square root of two), so leave that much wall above it. A peak that runs out through a thin wall is cut where the wall is; it does not fail.

Heat-set seat on a hole

A heat-set insert is pressed into a hole with a soldering iron. Heat-set seat starts the Heat-set insert panel from a hole you already have.

  1. Select the wall of the round hole (face mode, Q) and choose Heat-set seat in the right-click menu (or the command search).
  2. The panel opens with the insert at the hole’s mouth, going into the part along the hole’s axis, and with the size whose insert hole is nearest to your hole. Change the size, the dimensions or the thread there as for any insert.
  3. A hole narrower than the insert hole is opened up to it. A hole that is already as wide is left as it is. Press Add insert.

The hole must run along the X, Y or Z axis; for a slanted hole use Add heat-set insert and type its origin and axis. The insert table is from typical manufacturer data and has not been checked against a particular brand, so check the hole and insert sizes against the datasheet of the inserts you buy.

Threads

A thread feature marks a cylindrical face as threaded: the wall of a hole, or a shaft. It records the standard, size, class, length and hand. By default it is cosmetic: the model does not change, the thread appears as a marker in the view, and it is available to drawings and checks. If you turn on Model the thread, the kernel cuts a real helical groove.

Add a thread to a hole

The easy way is inside the Hole editor.

  1. Open the hole in the Editor and tick Threaded at the top of the Size section. Only Simple holes can be threaded.
  2. The hole is drilled to the tap drill of the thread. The size picker becomes a thread picker. A Thread options section appears with Length, Hand and Model the thread.
  3. Confirm. The hole and the thread are one undo step, and editing the hole later updates the thread with it.

Clearing Threaded puts the hole’s own size back and removes the thread. With several hole positions you get one thread per position, all with the same settings.

Add a thread to any cylinder

Use this for shafts, or for holes made some other way.

  1. In Face mode, select the cylindrical face. The command only enables for a cylinder, not for a flat face with a round hole in it.
  2. Choose Home > Create > Thread (Shift+T). It is in the Hole button’s list.
  3. The Thread editor opens. The new thread uses the metric size nearest the face diameter, full length, right hand, cosmetic.

You can select several faces first (Ctrl-click or Shift-click) and get one thread per face, all editable together. Select same size (Select tab, Expand group) selects every cylinder in the body with the same diameter and kind, so all holes of one diameter are one click.

The Thread editor

ControlWhat it doesDefault
StandardISO metric coarse, ISO metric fine, UNC, UNF, BSP parallel (G), NPT (tapered), Trapezoidal (Tr), Acme. Changing it picks the nearest size of the new standard.ISO metric coarse
Common sizesChips for the usual sizes of the standard.
SizeA search box. Type to filter (m6, 1/4, g1/2), use Up and Down, and Enter to pick. The sizes nearest the face diameter come first.Nearest to the face
ClassThe tolerance class. It is recorded with the thread and does not change the geometry.The standard’s usual class
LengthFull (the whole face) or Custom (a number in mm, held between one pitch and the face length).Full
HandRight or Left.Right
StartOpen end, Top or Bottom. Shown only when it matters, that is when both or neither end of the face is open.Open end
Model the threadCuts a real helical groove. Slower to rebuild. Remembered as the default for new threads.Off
Print clearanceShown with a modelled thread: None, Wider (a looser fit, for a thread that will be printed) or Narrower, with the amount in mm (up to 1 mm). A wider external thread cannot fit a shaft drawn at the nominal size, so it falls back to a cosmetic thread with a warning: draw the shaft near the loosened size.None

A read-out card shows the pitch and the diameters that matter: for a hole the tap drill and minor diameter, for a shaft the major diameter and root diameter.

Fit check. The thread editor compares the face with the thread. An internal thread wants a hole within 3 percent of the tap drill, and an external one wants a shaft within 3 percent of the major diameter. A green “Fits” line means it does. An amber line gives the kernel’s advice and a one-click Use M8 (or whatever is nearest) button. For example, a 6.5 mm hole with an M6 thread shows “hole is 6.5, M6 tap drill is 5”. Drill the hole to the tap drill, or pick the size that fits.

Length handle. While the Thread editor is open, a dot sits on the axis at the end of the thread. Drag it to set the length; at the face length it becomes Full. Ctrl snaps to whole millimetres. The value goes into the Editor, and you confirm as usual.

When threads are made together, or sit next to each other with identical settings, the Editor edits them as a group, and the face chip says “4 holes, Ø 5 mm”. To edit one alone, change its settings first, or give it its own Shift+T.

Cosmetic or modelled?

Cosmetic (default)Modelled
Body geometryUnchangedA helical groove is cut
In the viewDashed rings and lines at the thread, with the size as a label; hide them with View > Appearance > Show > ThreadsThe groove itself
Rebuild timeFastSlower, many more triangles
Good forNormal modelling, drawings, hole calloutsShowing or printing a real thread

Some threads cannot be modelled, and then the thread stays cosmetic and the Editor shows “Not built: …” with the reason. This happens for tapered NPT threads, threads of more than 60 turns, lengths shorter than one turn, a bore or shaft that does not match the thread, and a failed cut.

Patterns

A linear or circular pattern, or a mirror, copies the threads of the features it repeats. The copies are not separate tree rows. Edit the source thread and every copy follows. See Patterns, mirror and scale.

For the exact definition, see thread in the kernel book.

Common problems

SymptomFix
Hole is greyed outSelect exactly one flat face, or make a sketch of points first.
The hole goes the wrong wayTick Flip direction.
Thread is greyed outSelect a cylindrical face in Face mode. A flat face with a round hole in it is not a cylinder; select the wall inside the hole.
Amber “does not fit” lineThe hole or shaft diameter is not the thread’s tap drill or major diameter. Use the suggested size, or edit the hole.
“The thread tables are not loaded yet”Wait a moment and try again.
The Threaded box is disabledOnly Simple holes can be threaded. Counterbore and countersink walls are not a single cylinder.

Next

Patterns, mirror and scale

Patterns repeat a feature in a row, in a grid, around an axis or along a path. Mirror reflects a feature, or the whole body, about a plane. Scale makes the part larger or smaller. All three work on features and bodies that already exist.

Seeds: what gets repeated

Linear pattern, Circular pattern and Mirror copy features, not faces. The feature that is repeated is called the seed. A seed is a feature that made material or removed it: an extrude, a cut, a revolve, a hole, a sweep, a loft, or an earlier pattern.

  • The copies are combined with the body in the same way as the seed. Copies of a cut cut, and copies of a boss add.
  • A copy that falls outside the body does nothing. It is not an error, but the pattern gets a warning that lists those copies (see When copies miss, stand apart or overlap).
  • A pattern of a pattern is allowed.

The command chooses the seed for you: the feature selected in the feature tree, or if none is selected, the last feature that is not a sketch, plane, axis or pattern. Select the feature in the tree before you run the command if you want a different one. In the Editor the seed appears under Features to repeat, as a list of feature ids such as F4, separated by commas.

When a seed is a hole with a thread, the Editor shows what is meant (“Hole F4 + Thread F5”). See Threads in patterns.

Linear pattern

A linear pattern makes copies of the seed in a row.

  1. Select the feature in the tree (optional).
  2. Choose Home > Pattern > Linear pattern (Shift+L). You can also right-click a face or the body and choose it there.
  3. Adjust the Editor and confirm.

The Editor has a Direction 1 and a Direction 2 section. Each direction has the same options:

OptionWhat it doesDefault
DirectionWhat the copies run along: the X, Y or Z axis, a Direction vector (x, y, z) (any direction, such as (1, 1, 0) for 45 degrees; the length does not matter), or a straight edge or round face picked in the view with the Pick button (the copies run along the edge from its start to its end, or along the axis of the round face, and follow it when the part changes). Direction 2 also has None, which turns it off.Direction 1: the world axis along which the body is longest. Direction 2: None
CountNumber of instances along this direction including the seed. A count of 1 or less makes no copies.3 (Direction 2: 2 when you turn it on)
Distance typeSpacing: the distance between neighbouring copies. Extent: the distance from the seed to the last copy; the copies are spread evenly over it, and it stays the same when you change Count. To object: the last copy reaches a plane, a flat face or a point (see below).Spacing
SpacingWith Spacing: the distance between neighbours, in mm.About 20% of the body length along the direction, rounded to a tidy value (1, 1.5, 2, 2.5, 3, 4, 5, 6, 8 or 10 times a power of ten), at least 1 mm
ExtentWith Extent: seed to last copy, in mm. Must be above 0.The span the copies covered when you switched
ObjectWith To object: Front, Top or Right plane, an earlier Plane feature, or a face. Click Pick and click a flat face in the view.None (pick one)
OffsetWith To object: moves the end the way the copies go. A negative offset stops short of the object.0
Reverse directionCopies go towards the negative direction. Not shown for To object: the object sets the side.Off

The Editor also has Features to repeat (the seeds, as feature ids) and, when the part contains threads, Carry threads (see below).

With Direction 2 on, the pattern is a grid: Count x Count 2 instances. The two directions must point different ways (a direction along the first is refused).

To object

The last copy reaches the object, measured from the middle of what is repeated (the centre of the box around the seed). With a plane or a flat face, that is where a line from the middle along the direction meets it, so the face must lie across the direction, not along it. The copies follow the object: move the plane or the face and the copies spread out or close up to it. If the object lies behind the seed, the copies go the other way.

The pattern is refused, with a message, when the object runs along the direction (no copy can reach it), when it lies at the middle of the seed or the offset takes the end back past the seed, or when the face is curved.

The script API (see Scripting) can also give a point: linearPattern({ count: 3, to: [50, 0, 0] }).

Circular pattern

A circular pattern turns copies of the seed around an axis.

Choose Home > Pattern > Circular pattern (Shift+P). It is on the same button as Linear pattern: click the small triangle to open the list.

OptionWhat it doesDefault
Features to repeatThe seeds.The seed chosen as above
AxisThe X, Y or Z axis, Direction and point (x, y, z) for a typed direction (it can be oblique), or a straight edge or round face picked in the view with Pick (the copies turn about the edge, or about the axis of a round face such as a hole wall, and follow it when the part changes).The world axis along the body’s shortest dimension
Axis pointShown for the X, Y, Z and typed axes: a point the axis passes through. 0, 0, 0 is an axis through the origin; give the centre of a bolt circle to turn about it.0, 0, 0
CountNumber of instances including the seed.3
AngleWith Equal spacing: the total angle the copies are spread over. Without it: the step between neighbours. In degrees.360
Equal spacingOn: copies are spread evenly, so 360 degrees with 4 copies puts them 90 degrees apart, and any smaller total puts the last copy exactly at the Angle. Off: the Angle is the gap between neighbours.On
Reverse directionTurns the other way.Off
Carry threadsAs for Linear pattern.On

Known limits of the circular pattern:

  • The axis is not the centre of the part and not the seed’s own axis unless you say so: set the Axis point to the centre you want (a bolt circle round (40, 0) is the Z axis through the point 40, 0, 0), or pick the edge or the round face that marks it.
  • A seed that ends up outside the body after turning produces no change and no error.

Pattern on path

A pattern on path repeats the seed along an open sketch: a chain of lines and arcs.

  1. Draw the path as a sketch. It must be open: a chain with two loose ends.
  2. Select the feature to repeat in the tree (optional).
  3. Choose Home > Pattern > Pattern on path (on the same button as Linear pattern).

The command uses the newest open sketch, or the one selected in the tree, and spreads 3 instances over its whole length.

OptionWhat it doesDefault
Path sketchThe open sketch the copies follow.The newest open sketch
CountNumber of instances including the seed.3
Distance typeSpacing between neighbours along the path, or Extent from the seed to the last copy.Extent
Spacing / ExtentIn mm, measured along the path.The path length
Start pointDistance along the path (mm) or Fraction of the path (0 to 1). Where the seed sits along the path; the copies follow on from there. A fraction keeps its place when the path gets longer or shorter.0
Run from the other endThe path runs from its other end.Off
OrientationFixed: the copies are moved but not turned. Follow the path: the copies turn with the path, so a seed beside an arc stays beside it all the way round.Fixed

The path runs from its end nearest the seed. The seed does not have to sit on the path: each copy keeps the seed’s offset from the path (turned with it when Orientation is Follow the path).

A last copy that would lie past the end of the path is refused, and the message gives the largest spacing that fits. A start point outside the path is refused too.

When copies miss, stand apart or overlap

After a linear, circular or path pattern is built, the feature gets a warning (the triangle in the feature tree) when:

  • some copies change nothing: a cut copy misses the body, or a boss copy lies inside the material. The warning lists the copy numbers;
  • boss copies do not touch the body, so each stands as a body of its own;
  • copies overlap each other, because the spacing is smaller than the seed. For a linear pattern in one direction the warning gives the smallest spacing that keeps them apart.

These are warnings, not errors: the pattern is still built.

Mirror

Mirror reflects the seed about a plane. The copy is the seed’s mirror image on the other side.

  1. Select the feature in the tree (optional).
  2. Select one flat face if you want to mirror about that face (optional).
  3. Choose Features > Modify > Mirror (Shift+M).

With exactly one face selected, the mirror plane is that face. Otherwise it is the Right plane. The Editor has Features to repeat, Plane (Pick sets it from a selected face), and a checkbox whose label is the raw field name, body (there is no friendlier text for it). Tick it to reflect the whole body made so far and unite it with itself. A reflection that lies clear of the body is added as a separate body.

For the exact definitions of the features, see the kernel book: linear pattern, circular pattern, pattern on path and mirror.

Threads in patterns

A pattern or mirror carries the threads of its seeds onto the copies, so a threaded hole patterned six times has six threads. When the part contains threads, the Editor shows a Threads section that lists the seeds in words and has a Carry threads checkbox (on by default).

  • Off: the copies are plain holes and shafts. List a thread feature itself under Features to repeat to copy just that one.
  • The copies are not separate tree rows. The seed and its thread show a note “patterned by F7” in the tree. Edit the source thread and every copy follows. If you try to add a thread to a face that gets its thread from a pattern, the app edits the source thread instead and says so.
  • A drawing callout for a threaded hole that is patterned reads, for example, 4x M5 THRU.

See Holes and threads.

Scale

Scale makes the part bigger or smaller without changing how its features are named.

Choose Features > Modify > Scale. It is enabled when the part has a solid. A new Scale doubles the whole part about its centre of mass. Change it in the Editor.

OptionWhat it doesDefault
Same in every directionOne factor for all directions. Untick it for a factor per axis.On
FactorThe scale factor. A plain number. Must be above 0.2
Factor X, Factor Y, Factor ZOne factor per axis. Shown when Same in every direction is off.The same value as Factor
AboutThe point that stays fixed: Centre of mass or Origin.Centre of mass
BodiesWhich bodies are scaled. It shows “The whole part”.The whole part

Scale is exact for flat faces, for cylinders and cones stretched along their axis, for free-form faces, and for spheres and tori under a uniform factor. It is refused, with a hint, for the cases it could not keep exact: round faces stretched across their axis, a sphere or torus with different factors per axis, and surfaces made by revolving, extruding, screw or offset operations. The part is left as it was. Negative factors are refused: use Mirror instead.

Scale acts on the bodies as they are at that point in the history. Features added after it work on the scaled part. See scale in the kernel book.

Not available

These are known in the file format but cannot be built yet, so the app has no command for them:

  • Patterns driven by a sketch of points or a fill of a face.
  • Dome, split line and offset surface.

To copy whole bodies, use Copy in the Bodies panel. See Bodies and combining.

Common problems

SymptomFix
The pattern shows no copiesCopies fall outside the body; the warning on the feature lists them. Check Count, Spacing and Reverse direction.
“the object runs along the pattern direction”To object needs a plane or face across the direction. Pick another face, or a plane square to the direction.
“the last copy lies past the end of the path”Use the spacing the message gives, fewer copies, or an earlier start point.
The wrong feature is repeatedSelect the right feature in the tree before running the command, or edit Features to repeat.
“a face or edge it uses no longer exists”The seed was deleted or renamed by an earlier edit. See The feature tree and history.
Circular pattern rotates about the wrong centreSet the Axis point to the centre of the circle, or pick the edge or round face that is its axis.
A picked edge or face is refused (missingReference)A direction or axis needs a straight edge or a round (cylindrical) face. A flat face or a curved edge has no single direction.
The copies of an edge-direction pattern go the wrong wayTick Reverse direction: the edge runs from its start to its end as the kernel reads it.
Scale is refusedSee the cases above. Scale the sketch before extruding instead, or use uniform factors.

Next

Moving things: the move / rotate ball and handles

You can change a model by dragging it directly. The move and rotate ball moves, turns and copies a body, pushes a face, or shifts the sketch behind a feature. Handles that appear on a selection resize and reshape features on the canvas. Every drag is previewed live and becomes one undo step when you release.

Handles on the canvas

Select something and a small handle appears on it. Drag the handle and the part redraws as you go. Nothing is written until you let go. Esc puts everything back. A click on a handle that does not move does nothing.

SelectHandleDragging it
An edge, several edges or a cornerA yellow dot beside the selectionOutward makes a fillet, inward makes a chamfer. See Fillets, chamfers, shells and drafts
A face next to an existing fillet or chamferA dot on the blend faceChanges its radius or distance in place
The inner wall of a shellAn arrowChanges the wall thickness
The wall of a plain holeA dotChanges the hole diameter
A shape feature in the tree (extrude, cut, revolve, hole)The size box (below)Changes width, length and height, or moves the shape
An Extrude open in the EditorAn arrow on the previewSets the depth
A Thread open in the EditorA dot at the end of the threadSets the thread length
The whole bodyThe move and rotate ball (F10)See below

While you drag, a readout shows the number (“Fillet 3 mm”, “Depth 42 mm”). These keys work while you drag a handle:

KeyEffect
ShiftFine control: a tenth of the pointer movement
Ctrl (Cmd)Snap to whole millimetres, or 15 degrees for rings
Digits, ., -Type the exact value instead of dragging
EnterCommit now
EscCancel

Handles are hidden while you sketch and while a feature’s Editor is open, except the depth arrow and the thread length handle. To turn all handles off, clear Direct-manipulation handles on the canvas in the workspace settings.

The size box

Click a shape feature’s row in the feature tree (with nothing selected in the view), or select one of its faces, and its size box appears: a wireframe box around the profile and its depth, with a handle on every face centre and every cap corner.

  • Drag a face handle to change the width, length or height. Hover a handle to see its dimension. The three labels always show the numbers; click one and type an exact value, then press Enter, or the check or Done key of a phone keyboard (leaving the box also applies it; Escape cancels). If the value cannot be applied, a notice says why and the label keeps its old number.
  • A revolve shows R70, the radius (the outline’s distance from the axis), and a length along the axis that includes the rounded ends (150 for a cylinder 80 long with domes of radius 35). Typing a radius moves the outline toward or away from the axis, which stays where it is, and the round ends follow it so they stay tangent (a dome that is half the radius shrinks with it, so the length changes too). Typing a length moves the far end and the round end with it. The same labels show on the cylinder face, the end faces and the revolve’s row in the tree. Dimensions in the sketch follow the new size.
  • Drag a corner handle to change width and length together.
  • Shift or Ctrl snaps to a round step. Digits type a value.
  • A Resize about menu at the bottom left chooses what stays put when you change a width or length: Anchor (the profile scales about its anchor point), Symmetric (both faces move equally about the centre), or Opposite face (the opposite face stays; the default). The height always grows from the sketch plane.
  • To move the shape in its sketch plane, drag the flat four-arrow pad at the centre of the footprint, drag the shape itself, press Tab or double-click the pad and type an X offset, Y offset or a Distance from edge, or use the arrow keys (the grid step; Shift is 10 times larger, Alt a tenth). Shift while dragging keeps to one axis, Ctrl snaps to the grid, and Alt turns snapping off. Snap hints appear in the readout.

A resize or move edits the feature’s sketch (its points and its dimensions), so it is one undo step. If the sketch is also used by other features, they all move with it (undo reverts). A constraint that the change breaks is removed, and the app tells you which. A fixed point that would have to move refuses the edit.

Limits: Through all and Up to next extrusions get width, length and corners but no height handle. A revolve gets only the flat profile box. A hole gets a diameter handle only if it is Simple.

The move and rotate ball

The ball is a manipulator that follows a selection. Turn it on with F10, with Move / rotate ball (Select tab > Position), or with Move body in the right-click menu of a body. Esc turns it off. If it cannot act on the selection, the app tells you what to select.

You selectedThe ball acts onResult
The whole body (Alt+click, the Body pick mode B, or Select body)The bodyA Move or copy body feature
A Move or copy body feature in the treeThat featureEdits it in place
One or more facesThe facesA Move face feature: flat faces slide along their normal, curved faces grow or shrink. Only the face-normal handle is live
A feature built from a sketch on the Front, Top or Right planeThe featureShifts that sketch’s points in its plane. Everything else that uses the sketch moves too
Edges, corners or nothingNothingF10 is greyed out

While the ball is on, the contextual handles step aside. It hides during sketching and while an Editor is open.

Move, rotate and copy

The ball is a cyan ring that always faces the camera, with a centre dot and three axis stubs (X red, Y green, Z blue) ending in dots.

GestureResult
Click an axis end dotSelects the axis (the dot turns yellow). Click again or click empty space to deselect
Drag an axis end dotMoves along that axis
Drag a plane squareMoves in that plane
Drag the ringTurns about the view direction, or about the selected axis
Drag inside the ring with an axis selectedTurns about that axis
Ctrl while draggingSnap to the increments (10 mm and 15 degrees at first)
Shift while draggingA tenth of the movement
Digits, then EnterType the exact distance or angle
EscCancels the drag. A second Esc turns the ball off
SpaceAttaches or detaches the ball. A detached ball (white) moves only itself, to reposition it

Angles are right-handed about the axis. Move and rotate are combined: the turn is applied first, then the move.

Right-drag a handle instead of left-drag, and on release a menu offers Move Here, Copy Here, Create Radial Pattern (for a turn) or Create Linear Pattern (for an axis move), and Cancel. Copy Here keeps the source body and adds a copy. A pattern dialog (Repeated copy) asks for the Number of copies (the source body stays, so 5 copies make 6 bodies), the Distance or Angle, and for a radial pattern a Step up along the axis. A pattern is one undo step.

Right-click gives more:

Click onMenu
An axis end dotEdit Distance (type it, as a Move or Copy), Create Linear Pattern
The ringEdit Angle (about X, Y, Z or the view; Move or Copy), Create Radial Pattern, Snap Increments
An orientation dot (the stub end)Parallel to Axis (pick a cylinder), Perpendicular To Face (pick a flat face), Parallel To Edge (pick an edge), Reverse, Mirror (Copy)
The centre dotEdit Position (X, Y, Z), To Point (a corner), To Center Point (a circle edge), To Midpoint (an edge)

The orientation commands re-aim the ball only. They do not rotate the object. Use them to aim an axis along a direction you need, then drag.

The snap increments can also be set in the workspace settings, on the Positioning tab.

What each move writes

One gesture is one feature or one edit. A second plain move of the same bodies, right after the first, is folded into the existing Move or copy body feature. A copy is always a new feature. Select the feature in the tree and double-click it to open its Editor: it shows the bodies, how far they went (“by 10, 0, 0 mm”), and Make a copy with a body name. The amount is read-only there: change it by dragging the body again with the ball.

For the exact definitions, see moveBody and moveFace in the kernel book.

Press Pull

Press Pull (Features tab > Modify, or Press Pull in the right-click menu of a face) pushes or pulls the faces you picked along their own normals. It writes the same Move face feature as the ball above, with a distance, so it is the quick way to make a wall thicker, a boss taller or a hole bigger without sketching again.

  1. Pick one or more faces (face mode), then choose Press Pull. A Move face feature opens with a preview and a starting distance of about a tenth of the part.
  2. Type the distance in the options, or drag the face-normal handle on the canvas. Positive goes out of the body, negative goes into it.
  3. Press Enter or the tick.

What it does to each kind of face:

  • A flat face slides along its normal. The faces around it grow or shrink to stay joined, so a top face pulled up 5 mm on a 20 x 20 x 10 block makes a block 15 high.
  • A cylinder grows or shrinks its radius. A hole of radius 10 pulled by -3 mm becomes a hole of radius 7, and a post pulled by +2 mm gets 2 mm thicker.
  • Several faces move together, each along its own normal.

When it cannot be done the feature fails and says why, with the limit where there is one: pushing a face past the opposite one reports an edge reverses, and a cylinder moved further than its curvature allows reports move by at most 8 mm (for a radius of 10 mm). Choose a smaller distance and the feature builds.

Continue: Offset or Straight

The panel’s Continue choice says how the faces move:

  • Offset is everything above: the faces slide along their normals and their neighbours follow. It writes a Move face feature, and it is what Press Pull starts as.
  • Straight continues a flat face as if it were extruded. A positive distance joins a new piece out of the part, a negative one cuts a piece into it (0 is refused). The moved end keeps the face’s name and the new walls are named after the faces they meet, so later features that use them keep working. It writes a Press pull feature.
  • Along the walls (the end follows a bend in the walls) is listed as later and cannot be chosen yet.

Switching between Offset and Straight converts the feature and keeps the faces and the distance. Offset moves curved faces too; Straight needs flat ones and says so for a cylinder.

With Straight, Taper shapes the new walls:

  • None keeps them straight.
  • Draft tilts them by an angle between -85 and 85 degrees. A positive angle grows the outline along the run (the opposite sign to the Draft angle on Extrude), a negative one shrinks it, and holes do the reverse.
  • Scale takes the end to a size factor of the face (1.2 is 20 percent bigger, 0.5 half size), about the face’s centre of area and holes included. The panel shows the wall angle this makes at the face’s farthest point, so a scale can be compared with a draft.

A taper that closes to a point before the distance is reached is refused with the length at which it does (the taper closes to a point after 28.36 mm) and Use the largest size puts that in. A cut that would go through the body or join into other material is refused with the largest distance that builds. A refused edit leaves the part as it was.

In a script, Offset is .moveFace(faces, { distance }) and Straight is .pressPull(faces, { distance, taper }), with taper as { type: 'draft', angle } or { type: 'scale', endScale }:

part('Block').sketch('front', (s) => s.rect(40, 20)).extrude(10)
  .pressPull(face('>Z'), { distance: 8, taper: { type: 'scale', endScale: 1.2 } });

Limits

  • Link Here is disabled. Linked copies need instances, which the kernel does not have.
  • Mirror (Move) is disabled, because a mirror in this kernel joins the mirror image to the body. Mirror (Copy) works only when the handle points along X, Y or Z and the ball sits on that plane through the origin. For other planes use the Mirror feature. See Patterns, mirror and scale.
  • Only a whole body can be copied or patterned with the ball. A face can only be pushed.
  • Patterns made with the ball are chains of Move or copy body copies of the body, not the Linear and Circular pattern features.
  • Faces: there is no rotation and no copy, and several faces move together by the same amount. A face move the kernel refuses (for example, a face that would collapse) shows the reason and changes nothing. Moving a hole by sliding its cylinder sideways is not supported.
  • Moving a feature works only for sketch-based features on the three standard planes. Features on a face, 3D sketches and features without a sketch say so.
  • Free three-axis moves and free trackball rotation are not available.
  • Copy along a curve is not available.
  • The ball itself is not saved with the part.

Next

Surfaces

A surface is a sheet: it has faces and edges but encloses no volume. You build surfaces when a shape is easier to describe by its skin than by a solid, then trim, join and thicken them. This chapter covers the commands on the Surfaces tab, how sheets show in the view, and the tools that check a surface.

Surface bodies

A feature that makes a sheet leaves a surface body. Surface features are Planar surface, Extruded surface, Revolved surface, Lofted surface, Trim surface, Fill surface, Extend surface, Pipe cut, a Knit that is not made into a solid, and Delete face on a solid. A surface body is named after the feature that made it.

How sheets look and behave:

  • Sheets are drawn with a cool teal tint so you can tell them from solids. Both sides are lit.
  • You can pick the faces and edges of a sheet exactly as for a solid, including the border edges (one face) that Fill and Extend use.
  • H hides the body that holds the selection (a sheet or the solid), and Alt+H (Show all) brings everything back. Hiding is for the view only and is not saved.
  • Mass properties and interference counts solids only. A part with no solid reports that sheets have no volume or mass. See Measure and inspect.
  • A section view clips sheets, but a sheet has no inside, so the cut is not capped.

Where the commands are

GroupCommands
Surfaces > CreatePlanar surface, Extruded surface, Revolved surface, Lofted surface and Fill surface (Shift+I), each its own button
Surfaces > EditOffset surface, Extend surface (Shift+X), Trim surface, Knit, Thicken and Freeform, each its own button
Features > ModifyPipe cut
Features > BodiesDelete body and Delete face

Each command makes its feature at once, opens the Editor with a live preview, and is one undo step. A command that has nothing to work on says “Nothing to build this feature from: pick what it needs first”, or is greyed with a tooltip.

Making a sheet

CommandNeedsDefaults
Planar surfaceA closed sketch: the one selected in the tree, else the last that fitsA flat sheet filling the sketch
Extruded surfaceA sketch with curves, open or closedBlind, 10 mm
Revolved surfaceA closed sketch with a construction line as the axis360 degrees about the first construction line
Lofted surfaceTwo or more sketches, open or closed, all of one kindAs Loft, with Make a surface on. See Extrude, revolve, sweep and loft

An open sketch extruded as a surface gives a wall you can thicken later. The Editor for an Extruded or Revolved surface shows the sketch, the End condition and the Depth or Angle. A surface sweep (Sweep with a sheet result) is not available.

Trim, knit, thicken

Trim surface. Trim cuts a surface with a plane or with another surface and keeps one side.

  1. Select what trims. Either pick the faces of the two surfaces (the first is trimmed by the second), or pick a face of a solid (its plane is the tool).
  2. Choose Surfaces > Edit > Trim surface.

With nothing picked it uses the surface selected in the tree, then another surface, then the last reference plane. The Editor has:

OptionWhat it doesDefault
Surface to trimThe sheet that is cut.The target chosen as above
Trimmed byA plane (pick a face) or another surface.The tool chosen as above
Keep the other sideKeeps the part on the opposite side.Off
Trim both surfacesThe tool surface is trimmed by the first too.Off

If the tool no longer crosses the sheet, the trim fails with “the surfaces do not cut each other”. Move the tool or change the sheet.

Knit. Knit joins sheets along their shared edges into one sheet.

  • With faces picked, Knit uses the surfaces they belong to. Otherwise it uses the one selected in the tree, else every surface in the part.
  • The Editor lists the surfaces with a checkbox each.
  • Make a solid when the result is closed turns a sealed shell into a solid. It is off by default. If the shell still has open edges, the Editor reports that it is not closed.

Thicken. Thicken turns a sheet into a solid. The Editor has Surface, Thickness, Side (Front, Back or Both) and Operation (Add or Cut). Thickness starts at about 10% of the body size at first, or 1 mm with no body. A thickness larger than the surface’s tightest bend radius allows is refused, and the message gives the largest thickness that works (for example “its smallest radius of curvature is 3.63 mm, use at most 2.90 mm”). For a sheet that tight, set Side to Both instead.

Tick Variable thickness and the single thickness becomes a ramp: the sheet is thick at one end and thin at the other, which is what a blade or a tapered plate needs.

ControlWhat it doesDefault
Ramp alongX axis, Y axis or Z axis: the direction the positions are measured along. A direction that is none of those (set by a script, say) is shown as its vectorZ axis
PositionWhere a stop sits, in millimetres along that direction0, then 10
ThicknessHow thick the sheet is at that stop, in millimetresThe thickness you had, then half of it
Add stop, RemoveStops are added at the end and removed from anywhere: 2 to 6 in allTwo stops

The note in the editor gives the rules: “Thickness at positions along the axis (2 to 6, rising). The stops must cover the whole surface.” Between two stops the thickness is interpolated, so the sheet changes smoothly. Positions run from the smallest to the largest, and stops that do not reach across the whole sheet are refused.

Delete face. Select faces in Face mode and choose Features > Bodies > Delete face. The faces are removed; deleting a face of a solid leaves a sheet.

Fill and extend

Fill surface closes a loop of boundary edges with a patch. Pick the edges in Edge mode, or select a surface in the tree, and choose Fill surface (Shift+I). Without picked edges it uses the first open loop of the surface.

OptionWhat it doesDefault
ContinuityHow the patch meets its neighbours: G0 (touching), G1 (tangent), G2 (curvature), G3.G0
FairingHow the patch is smoothed: Smooth net, Thin plate, Curvature or Variation.Smooth net
Merge with the surfaceJoins the patch to the surface it fills.On
EdgesThe boundary edges, with Use selection.The picked edges

Extend surface continues an open border of a sheet along its own shape. Pick one border edge (or select the surface) and choose Extend surface (Shift+X). Distance is about 10% of the model size at first. The command extends the border edges you picked, or else the first open edge of the surface. In the Editor you can add more border edges with Use selection. The kernel extends each open border edge, but only one edge of any one face: two edges of the same face are refused with the code extendNotBoundary, and so is an edge that is not an open border (an edge shared by two faces). The kernel’s detail text is “only open boundary edges extend”. So pick border edges only, at most one per face, or make several Extend features. A wavy edge may report that it cannot be extended at the default distance; try a shorter distance.

Pipe cut

Pipe cut rolls a ball of a given radius along edges and cuts away everything it touches. Select edges in Edge mode, or select faces to use their rim edges, and choose Features > Modify > Pipe cut. Radius is about 10% of the smallest dimension at first. The solid becomes a surface body.

Offset surface

Offset surface makes a new surface body a set distance from faces. Pick faces of a solid (or choose a surface in the tree) and choose Offset surface (Surfaces > Edit). A positive Distance goes outward on a solid, a negative one into it; the source stays unless you turn Keep the source off for a surface. Only flat, cylindrical, conical, spherical and ring faces can be offset, and a distance that reaches the centre of a round face is refused with the limit.

Not available

  • Project curve, Edit curve and Freeform are covered in Curves on faces. Inside a sketch, the Project tool is a different thing: it projects model edges onto the sketch plane. See Offsets and references.
  • Cut with surface is not built yet.
  • Guide curves and strength for Fill are not offered.

For the exact definitions, see Surfaces and curves in the kernel book: knit, fill, trim surface, thicken, extend.

Surface analysis

Four views and a comb help you judge whether a surface is smooth. They colour or decorate the displayed mesh and are never saved with the part. Turn them on from Evaluate > Surface analysis.

CommandKeysShows
Zebra stripesAlt+ZStripes reflected in the surface. A break in a stripe is a break in tangency, a kink a break in curvature. Has a stripe density control.
Gaussian curvatureRed where the surface is dome-like, blue where saddle-like, white where flat or rolled.
Mean curvatureRed where it bulges out, blue where it dips in.
Draft analysisAlt+DColours faces by their angle to a pull direction: green has draft, red has none, blue faces the other way. Controls: Pull direction and Least draft (degrees).
Curvature combAlt+CTeeth along edges and sketch curves, as long as the curvature there. Smooth teeth mean a smooth curve. Has a Comb size control.

Use only one colour mode at a time; the comb can be added to it. The analysis reads the displayed mesh, not the exact surface, and it does not show continuity (G1, G2) between faces as a number. The Hidden-lines and Wireframe display styles draw no faces, so only the comb shows there.

Next

Curves on faces

Three commands reshape geometry without making a solid. Project curve lays a sketch or an earlier curve onto the faces of a part, Edit curve rebuilds edges and curves into one smooth curve, and Freeform pushes a face into a new shape with a control net.

Project curve and Edit curve sit in the Reference group of the Features tab, beside Plane, Axis and Helix. Freeform sits on the Edit button of the Surfaces tab, with Trim surface, Knit and Thicken. All three are in command search (F), and each is greyed out until it has something to work on. Each result is an ordinary feature: it sits in the tree, rebuilds with the part and takes part in undo.

Project curve

Project curve takes a curve that lies flat (a sketch, or a curve feature you made earlier) and lands it on the faces you choose. What comes out is one smooth curve lying on those faces, which a later Project curve or Edit curve can take as its source.

  1. Make a sketch that holds the curve, or select a curve feature in the tree.
  2. In Face mode (Q) pick the faces the curve should land on. Pick none to use every face of the part and of its surfaces.
  3. Choose Features > Reference > Project.
  4. Set the options, then press Enter or the tick.

OptionWhat it doesDefault
ProjectThe source: a sketch or an earlier curve. With none selected it takes the sketch selected in the tree, else the last sketch that holds a curve.The last sketch with a curve
Onto facesThe faces the curve lands on.The picked faces, else every face
DirectionBoth ways, Along the sketch normal or Against the sketch normal.Both ways
DegreeHow smooth the curve is. Must be between 2 and 9.3
Fit toleranceHow closely the curve follows the faces, in millimetres.0.001 mm

The note in the editor says what to expect: the result is one smooth curve lying on the faces, and a curve that misses every face is reported. If the result comes in several separate pieces, the editor’s note says so, but check the curve in the view. A projection that reaches no face is refused and the feature is left as it was.

Edit curve

Edit curve rebuilds a chain of edges, sketch curves or an earlier curve into one smooth curve, keeping the ends and the corners you ask it to keep. The pieces must meet end to end, in the order you add them.

  1. In Edge mode (E) pick the edges of the chain, or select a curve feature or a sketch in the tree.
  2. Choose Features > Reference > Edit curve.
  3. Set the rebuild and the keep options, add control point edits if you want to shape it, then press Enter.

OptionWhat it doesDefault
CurvesThe chain, one row each, with Add curve.The picked edges, else the sketch or curve feature selected in the tree, else the last one
Rebuild, Fit byTolerance follows the picks to a tolerance; Number of control points fits a fixed count.Tolerance
Degree, Tolerance or Control pointsThe numbers of the chosen fit. The degree must be between 2 and 9.Degree 3, tolerance 0.01 mm
Keep the ends, Keep the end tangents, Keep cornersWhat the rebuilt curve must match at its ends and at a corner.Ends and corners kept
Flatten onto a plane, PlanePuts the curve flat on a plane instead of following the picks.Off
Control point editsAdd edit, then a control point number, a direction (the world axes, or the curve’s tangent, normal and binormal), an offset and a weight. An edit past the last point is skipped.None

Freeform

Freeform rebuilds a face as a net of control points and lets you push some of them. Pick faces in Face mode (Q) and choose Surfaces > Edit > Freeform. The editor has two sections.

Control net

OptionWhat it doesDefault
FaceThe faces to rebuild.The picked face
Degree U, Degree VHow smooth the net is along each direction.3 and 3
Spans U, Spans VHow many pieces the net is cut into along each direction.2 and 2

The note under the fields gives the size of the net: with the defaults the face is rebuilt as a 5 x 5 net of points, numbered from 0. Rebuilding alone does not change the shape.

Point moves

  • Add move adds a row. Points (column,row) names the points to shift: 2,2, or 2,2; 2,3 for several, counted from 0 in the corner of the net.
  • Offset X, Offset Y and Offset Z move them by that many millimetres. Offset along chooses the frame: the world axes, the face (X and Y along it, Z out of it), or a plane with Plane.
  • Spread to neighbours shares the move with the points around it (0 is none). Mirror about repeats it across a plane. Skip this edit turns a row off without deleting it.

The outer ring of the net never moves, so the face keeps the border it shares with its neighbours. Moving points works on exactly one face: the editor says so when you have picked several. Several faces can be rebuilt at once, but their points cannot be moved by these edits.

Common problems

SymptomFix
Project curve is greyed outIt needs a body or a surface, and a sketch or curve to project. Start a sketch, or select one in the tree
The curve misses every faceMove the sketch over the part, or pick the faces the curve does cross, or change the direction
A degree is refusedThe degree must be between 2 and 9
Edit curve will not buildThe chain must meet end to end. Keep Keep corners on for a chain with a corner, and check the order of the rows in Curves
Freeform says to pick a single facePoint moves work on one face only. Clear the extra picks, or delete the moves
The face will not move at its borderThe outer ring never moves. Move points inside the ring
An edit does nothingAn edit past the last point of the net is skipped. Check the control point number

Next

Sheet metal

Sheet metal parts are made from one thickness of stock, bent along straight lines. You set a rule (thickness, k-factor and bend radius), make a first plate from a sketch, add flanges, hems and folds, and the kernel builds the folded solid, the flat pattern and the bend table from the same bend arithmetic. Cut, Corner and Convert to sheet shape the plate itself.

The Sheet metal tab

The Sheet metal tab sits between Frame and Surfaces. It has four groups:

GroupCommands
RulesRules
CreateBase flange, Edge flange, Contour flange, Convert to sheet, Hem, Fold, Cut, Corner
FlattenUnfold, Refold, Flat pattern
ExportFlat pattern DXF, Bend table (CSV), Bend table (JSON)

A part whose first plate you make opens on the tab. That is a suggestion, not a mode: the other tabs stay as they are. A command that cannot run is greyed out, and its tooltip says why (no first plate yet, the sheet is unfolded, no closed sketch). The tool palette has a Sheet metal section with the modelling commands; the three exports stay on the tab and in command search (F).

The features appear in the tree with these types, each with its own icon (a rule shows its own name): Sheet metal rules, Base flange, Edge flange, Contour flange, Hem, Fold, Convert to sheet, Sheet cut, Sheet corner, Unfold and Refold. Each command that changes the part is one undo step and opens its editor with a live preview, except Unfold and Refold, which are one edit with no editor; Flat pattern and the three exports only read the sheet.

The rule

Rules opens the one rules editor of the part; on a part with none it adds a rule named Sheet 2 mm (2 mm stock, k-factor 0.44). The form has two sections.

Stock fieldWhat it sets
Rule nameThe name the base and contour flange list and the tree show
ThicknessThe stock thickness
K-factorThe bend allowance factor, BA = (r + k t) a
Bend radiusThe inside radius of a bend
Use for the next base flangeThe active rule: the one a new base or contour flange starts with
Relief fieldWhat it sets
Relief widthThe width of a tear relief, and of the rectangular relief a partial-width flange cuts at its ends
Relief depthHow far a relief reaches past the bend line
Corner reliefThe size of the corner relief
Corner relief shapeNotch, Round, Rectangular or Tear
Gap between flangesThe gap left between two legs made by one edge flange, and between a partial flange and its neighbour
Hem gapThe inside radius of a hem

A field left empty follows the thickness: bend radius = thickness, relief width = thickness, relief depth = thickness / 2 and corner relief = 4 x thickness. Follow the thickness again clears those fields. Inside a rule, Thickness is that rule’s thickness, so a field may be an expression such as =Thickness*2.

The corner shape is stored with the rule. The kernel builds Round, Rectangular and Tear reliefs and shows them in the flat pattern and the DXF; a Notch is the open corner between two bends. The note under the field is older than the shaped reliefs and still says every corner is a notch: a round relief is the easy check, because it shows as an arc in the corner of the flat pattern.

A file or a script can carry more than one rule. The Rule list of a base or contour flange then offers The active rule or a rule by name.

Base flange

Base flange makes the first plate: a closed sketch (holes inside it are allowed) extruded by the rule’s thickness.

  1. Draw and close a sketch, or select it in the tree. With none selected the command takes the last closed sketch.
  2. Click Base flange.
  3. Set Rule (The active rule, or one by name) and Build on the other side of the sketch, then confirm.

A part has one base flange, and it is its first body feature. If the part has no rule yet, the command adds a 2 mm rule named Sheet 2 mm first, so the plate has stock to be made of.

Edge flange

Edge flange bends a flange on an edge of the plate.

  1. Press E and pick one or more edges of the plate. The edge list in the editor takes more picks: Use selection, or click them in the view, and press Done.
  2. Click Edge flange.
  3. Set the flange, then confirm.

You can also pick the free end of a flange, to add a second flange or a hem on it (a double fold): click the edge at the tip of the flange.

A flange bends towards the face its edge was picked on: an edge on the top (cap) side bends the leg up, an edge on the bottom side bends it down. Flip direction reverses that.

FieldWhat it doesDefault
HeightHow far the flange reaches, measured as Height measured says10 x thickness
AngleThe angle the leg turns through, more than 0 and less than 180 degrees90 degrees
Bend radiusThe inside radius of this bendThe rule’s bend radius
Height measuredTo the outer sharp, To the inner sharp or To the end of the bendTo the outer sharp
Flange positionInside the outline (the outer face stays within the plate’s edge), Outside the outline (the bend starts at the edge) or MiddleInside the outline
Flip directionBends the leg the other wayOff

Chained bends adds bends after the flange, each on the far edge of the leg before it: Bend 2 angle, Bend 2 height, its own Flip direction, and Add a bend (up to 16). Use it for a return lip or a Z section. The flange’s radius, Height measured and Flange position apply to the whole chain.

Four 90 degree flanges made in one feature keep the gap of the rule at their corners, so their legs do not meet. A flange made later next to an existing one trims the existing bend but not its leg.

Hem and fold

Hem folds an edge 180 degrees back against the sheet. Pick an edge and click Hem; the editor has Length (measured to the outer face of the hem), Gap (inside radius, the rule’s hem gap by default) and Flip direction. The leg is length - (gap + thickness) long, so a length below gap + thickness is refused. A hem on a neighbouring edge, or one whose flat layout overlaps another flange or hem, is refused.

Fold bends the plate along a sketch line. Draw a line in a sketch (the plate’s own outline does not count), select it, and click Fold. The editor lists Sketch and Line, then Angle (more than 0, less than 180 degrees; 90 by default), Bend radius, Line position in the bend (Centre of the bend, Start of the bend, End of the bend or Outer sharp (mould line)) and Flip direction. When the sheet has more than one panel the editor also offers Panel (Automatic, or P0, P1 …). The fold follows the sketch line when the sketch changes. The line may cross a hole or window of the plate: the window is cut through the bend, as a Cut across a bend is.

Contour flange

Contour flange makes the first plate from an open chain of sketch lines: the plate is bent at every corner and extruded by a distance.

  1. Draw an open chain of lines (an L, U or Z section).
  2. Click Contour flange.
  3. Set Rule, Distance (50 mm at first), the lines in Lines in the chain, Material on the other side of the line and Extrude against the sketch normal, then confirm.

It needs no plate yet and makes the first plate, so a part has either a base flange or a contour flange. The material lies to the right of the direction of travel; Material on the other side of the line puts it on the left. The chain is lines only: an arc in the chain is refused.

Convert to sheet

Convert to sheet turns an existing solid bent plate into a sheet, with panels, bends, a flat pattern, a bend table and DXF.

FieldWhat it does
ThicknessThe stock thickness. Empty: the kernel reads it from the body, as the gap between its facing flat faces
Use … of rule …Fills in the thickness of the active rule
Read the thickness from the bodyClears the field, so the thickness is read again
RuleThe rule that supplies the k-factor (the active rule by default)

The converted rule is named Converted and becomes the active rule. After it the part is a sheet: edge flanges, hems, folds, cuts and corners work on it, and Base flange and Contour flange are off.

The body must be a constant-thickness bent plate: flat panels, straight round bends and walls, one connected chain. Sharp corners between panels, cones, tori, free-form bends, reliefs and embossing are refused, and so is a rebuild whose volume differs from the body by more than 1 %. The card gives the kernel’s reason.

Panels

Once the sheet has more than one panel (a flange, a fold or a converted bend), the Edge flange and Hem editors get an Edge of a panel section, and the Fold editor gets a Panel list. The panels are numbered from P0, the base plate; the legs of a flange follow in the order they were made, and the pieces beyond a fold are appended as the folds are made.

ControlWhat it does
PanelPanel P0, Panel P1 …
Where on the panelFree end (tip), Start side, End side, a named wall (for example Wall e2), or Edge of the panel outline, by number
Edge numberThe edge’s number in the panel’s outline, for the last choice
Add this edgeAdds the pick to the edge chips

A pick in the view is found on the folded sheet; this section adds an edge the view cannot reach. The chips show what was added, such as P2.tip or P1 edge 3. With a single panel the section is not shown.

Cut

Cut cuts the closed regions of a sketch out of the sheet through the flat pattern, across bends too.

Draw the sketch on the plane of the base plate or on a plane parallel to it: its coordinates are flat coordinates, so read the position off the flat pattern, not off a folded leg. Select the closed sketch and click Cut. In the editor, tick the regions in Shapes, or click them in the view, then confirm.

A plain Extrude cut that goes all the way through the folded sheet (through all, or a depth of at least the thickness) and is sketched parallel to the plate does the same, so the part stays a sheet and still unfolds; a shallower pocket turns the part into an ordinary solid.

A slot that crosses a bend shows in the flat pattern and the DXF as a hole across the bend zone, and the folded solid loses the matching wedge of the bend. A rectangular cut along and across a bend is exact in the solid; another outline across a bend is a staircase of small wedges, though the flat pattern stays exact. A region that misses the sheet, removes or splits a panel, or holds an island is refused with the kernel’s reason.

Corner

Corner rounds or chamfers a free corner of a panel.

  1. Press V (vertex mode) and click the corners, or add them from the editor.
  2. Click Corner.
  3. In Corners, use Pick in view to pick more (click a corner again to take it out) and Done when finished.
  4. Choose the Treatment: Round with a Radius, or Chamfer with a Distance. The size carries over when you switch.

Both walls of the corner must be free of bends, the corner convex, and the walls at least as long as the radius or distance. A corner next to a bend is refused. The round is a true cylinder face in the solid and an arc in the DXF.

Mirror

A sheet metal part stays a sheet when you mirror it. In a script, mirror with body: true mirrors the whole part. Add replace: true to turn the part into its mirror image: it works about any plane, including a flat face of the sheet, and the flat pattern and bend table stay the same. Leave replace out to join the mirror image to the sheet: that works when the plane is square to the base plate and runs along a free, straight end of it with no bend, so an L-bracket mirrored about its far end becomes one channel whose flat pattern is twice as long and unfolds as a whole. A plane that cannot give one sheet (a face of the sheet, a plane parallel to the plate or tilted, a plane through a bend, or a flange that reaches the plane) is refused with the reason, and the part is unchanged.

Unfold and refold

Unfold flattens the body to its flat sheet; Refold bends it back from the bend table. Neither has an editor, and each is one edit. While the sheet is unfolded, flanges, hems and folds are refused with The sheet is unfolded: refold it first. Unfold then Refold gives the same solid back.

The flat pattern

Flat pattern opens a panel with the drawing of the blank: the outline and the holes, the bend zones in a light tint, and each bend line dashed, numbered and labelled with its angle. Up bends and down bends have different colours. The width and length of the blank are dimensioned on the drawing.

Under the drawing the panel gives the size and thickness, the rule and k-factor, the number of holes (when there are any) and a row per bend: direction, angle, radius, allowance and length. It follows the document, and while a feature editor is open it follows the draft, so a changed height or radius shows at once. Escape or Close closes the panel. The panel also carries Flat pattern DXF, CSV and JSON.

Export the flat pattern

Flat pattern DXF asks for the options and writes <part>-flat.dxf. The last choice is remembered.

OptionChoicesDefault
DXF versionR2000 or R12R2000
Unitsmm, cm, m, in or ftmm
LayersBy role (cut, bends) or All on layer 0By role
Layer namesCUT_OUTER / CUT_INNER or OUTLINE / CUTCUT_OUTER / CUT_INNER
Bend linesOn or offOn
Tangent lines (both ends of the allowance)On or offOff
Bend notes (number, direction, angle, radius)On or offOff
Note heightThe text height of the bend notes, in mm3

Write DXF writes the file; Cancel closes the dialog. Bend table (CSV) and Bend table (JSON) write <part>-bends.csv and <part>-bends.json, one row per bend with its angle, direction, radius, allowance, length and line in flat coordinates. Both exports are made by the kernel from the flat pattern; a refusal names the field.

Worked example: a small tray

The tray is 100 x 60 mm of 2 mm stock with 15 mm walls, a rolled rim and a round relief at each corner.

  1. The sketch. Start a new part named Tray and sketch a rectangle on the Front plane from (0, 0) to (100, 60). Close the sketch.
  2. The rule. Open the Sheet metal tab and click Rules. Set Rule name to Tray 2 mm, Thickness 2, K-factor 0.44, Bend radius 2, and leave Use for the next base flange on. Under Relief, set Relief width 2, Relief depth 1, Corner relief 4, Corner relief shape Notch for now, Gap between flanges 2 and Hem gap 0.01. Confirm.
  3. The plate. Select the sketch and click Base flange. Rule stays The active rule and Build on the other side of the sketch stays off. Confirm.
  4. The walls. Press E, pick the four outer edges of the plate (the rim of its top face), and click Edge flange. The editor lists 4 edges. Set Height 15, Angle 90, Bend radius 2, Height measured To the outer sharp and Flange position Inside the outline; leave Flip direction off. Confirm. The plate has four legs.
  5. The rim. Click Hem. Under Edge of a panel, set Panel Panel P1, Where on the panel Free end (tip) and press Add this edge. Set Length 5 and Gap 0.01; if the hem curls the wrong way, tick Flip direction. Confirm.
  6. The corner relief. Open Rules again and set Corner relief shape to Round, with Corner relief 4. Confirm: each of the four corners where two legs meet gets a 4 mm round relief.
  7. The flat pattern. Click Flat pattern. With the hem on one of the long sides the panel reads 123.05 x 88.83 mm, 2 mm thick (128.83 x 83.05 mm if the first leg is on a short side). Rule Tray 2 mm, k-factor 0.44 follows, then the bend rows B1 to B5: the four flange bends at 90 degrees and the hem at 180 degrees, each with its direction, radius, allowance and length. The four flange bends have an allowance of 4.523893 mm; the hem has 2.796017 mm.
  8. The DXF. In the flat panel click Flat pattern DXF. Keep DXF version R2000, Units mm, Layers By role (cut, bends), Layer names CUT_OUTER / CUT_INNER, Bend lines on, Tangent lines off and Bend notes off; click Write DXF. The file is Tray-flat.dxf. Bend table (CSV) writes Tray-bends.csv; Bend table (JSON) writes Tray-bends.json.

SolidWorks sheet-metal parts

A SolidWorks sheet-metal part opens as editable sheet-metal features as far as the kernel can read the feature tree back. The mapping is:

In the fileIn the tree
Sheet-Metal with a Thickness dimensionSheet metal rules: thickness, bend radius from D1 and k-factor from D2 (a k-factor outside 0 to 1 is dropped)
Base-FlangeBase flange, with the cap outline as the later features left it (corner rounds and rim cuts baked in)
Edge-Flange and its EdgeBendEdge flange with the leg’s outline as its profile, the bend’s angle and radius, and Flange position Outside the outline
Cut-Extrude or a round hole wizard hole through the plateSheet cut (a square cut in the rim is already in the base flange’s outline)
Corner rounds, Flat-Pattern, cut-list and bend-line sketchesNo feature: the rounds are in the outline, the rest has no geometry

A feature the reader cannot follow stops the read there: the steps before it are editable, and the file’s body stays as the imported remainder. That covers a mitre flange, a hem, a jog or a sketched bend, a flange on a curved edge, a leg with a hole made of other curves than a circle, and a bend cut through later. The flange heights and offsets in the file’s dimensions are not used; the faces are.

The part is then an ordinary sheet-metal part: the tab, the flat pattern, the bend table and the DXF work on it. See Importing.

Known limits

  • There are no commands for a jog, a mitre flange or a sketched bend, and the SolidWorks reader stops at one.
  • A flange needs a straight edge of the base. You can pick an arc, but the kernel refuses it; on a base whose outline has arcs, only the straight edges take flanges.
  • The Edge flange editor sets a flange on the whole edge with a straight leg. The kernel also takes a partial width (start and length, or from and to), a shaped leg (profile), holes in the leg and a relief cut at the ends; no field here sets them.
  • A hem on a neighbouring edge is refused, and so is a hem, flange or fold whose flat layout overlaps another. Give the corner a relief.
  • A corner of the panel inside a fold’s bend zone, and a fold across the edge a flange hangs on, are refused. A fold line that crosses both arms of a U or V shape is refused too: the pieces would be joined twice, so move the line so that it crosses one arm, or fold each arm with its own line. (A hole in the bend zone is cut through the bend.)
  • The Fold editor has no control for which side stays; the kernel’s fixed side is not in the form.
  • A contour flange takes lines only. An arc in the chain is refused.
  • A cut across a bend is exact in the flat pattern and the DXF. In the solid, an outline that is not rectangular is a staircase of small wedges; the sketch is not followed onto folded panels (use a plane parallel to the base); and a region that splits a panel or encloses an island is refused.
  • Convert to sheet takes constant-thickness bent plates of flat panels and straight round bends, in one connected chain. Sharp corners, cones, tori, free-form bends, reliefs and embossing are refused, and so is a rebuild more than 1 % away from the body’s volume.
  • A Corner is for the free walls of one panel, convex, with walls at least as long as the radius or distance. A corner across a bend is refused.
  • The flat pattern is a view: it cannot be dimensioned or put on a drawing sheet.
  • While the sheet is unfolded, flanges, hems and folds are refused. Refold first.
  • The relief shapes are stored with the rule; the form’s note about notches is older than the round, rectangular and tear reliefs, which the kernel builds.

Every Sheet metal command

CommandWhat it doesWhat it needs picked
RulesThe rule of the part: stock, relief and the active rule; adds one on a part with noneNothing; edits the selected rule if one is selected
Base flangeThe first plate: a closed sketch extruded by the rule’s thicknessA closed sketch (selected, else the last); no first plate yet
Edge flangeA bent flange on the picked edges, with chained bends if you add themA sheet, not unfolded; one or more edges, or an edge of a panel from the editor
Contour flangeThe first plate from an open chain of sketch lines, bent at every cornerAn open chain of lines; no first plate yet
Convert to sheetTurns a solid bent plate into a sheet with panels and bendsA solid body; no sheet yet
HemA 180 degree fold that lays the edge back against the sheetA sheet, not unfolded; an edge, or an edge of a panel
FoldBends the plate along a sketch lineA sheet, not unfolded; a sketch with a line
CutCuts closed sketch regions through the flat pattern, across bends tooA sheet, not unfolded; a closed sketch on a plane parallel to the base
CornerRounds or chamfers free corners of a panelA sheet, not unfolded; one or more corners (vertices)
UnfoldFlattens the sheet; no editorA sheet that is not unfolded
RefoldBends the flattened sheet back; no editorAn unfolded sheet
Flat patternShows the blank: outline, holes, bend lines and the bend tableA sheet
Flat pattern DXFWrites the flat pattern as a DXF with the options you chooseA sheet
Bend table (CSV)Writes one row per bend as CSVA sheet
Bend table (JSON)Writes one row per bend as JSONA sheet

The same commands, with their ribbon captions and the full availability rules, are in Commands and shortcuts.

Bodies and combining

A part can hold more than one solid. Each separate solid is a body. This chapter covers how bodies come about, the Bodies panel, and how to join, cut, intersect, copy and delete them. Colour, opacity and finish of a body are covered in Materials and appearance.

How a part gets several bodies

  • New body. The Operation control of Extrude, Revolve, Sweep and Loft offers New body. The new solid stays separate from the others, even where it overlaps or touches them. It gets a name such as Body 1, which you can change in the Editor. See Extrude, revolve, sweep and loft.
  • A sketch that misses the body. A new Extrude whose sketch plane does not reach the existing body starts as a New body. A sketch that meets the body starts as Add, and the first solid of a part always just adds.
  • Copy. The Copy button in the Bodies panel, and Copy Here on the move and rotate ball, make a second body from an existing one. See Moving things.
  • Sphere. A Sphere (from the Catalog) can also be a new body. See Extrude, revolve, sweep and loft.
  • Disjoint solids. Solids that share no face and no edge are separate bodies even if you made them with Add.

Two solids that are joined by Add become one body. A New body that you later want joined must be combined explicitly.

A body is a set of faces connected by shared edges. The Bodies panel lists the bodies the model currently has.

The Bodies panel

Open the Bodies tab in the left panel (next to Features, Variables and Script). The tab is available when the left panel tabs are on in the workspace settings. It lists one row per body, in the order they were created.

Part of the rowWhat it does
EyeHides or shows the body. Space on a focused row does the same. This changes the view only, not the model
Colour swatch and nameThe line under the name says which feature made the body (“made by Boss-Extrude1”). Click selects the body; Shift-click or Ctrl-click adds to the selection. Clicking a face in the view selects its row. F2 or a double-click renames. Up and Down move between rows
VolumeThe body’s volume, in cm³ or mm³. A sheet shows no volume
Isolate buttonHides every other body. Press it again on the only visible body to show all

Under the list:

ButtonNeedsWhat it does
Show allA hidden bodyShows every hidden body
Hide othersA selected body and two or more bodiesKeeps the selected bodies visible and hides the rest
CopyOne selected bodyMakes a copy in the same place, named after the source body with “ 2“. Move the copy afterwards
DeleteOne or more selected bodiesDeletes the bodies
Join, Cut, Intersect, SplitTwo or more selected bodiesCombines them. The first body you selected keeps the result, and the others are used up

Below those, the selected body shows its Appearance settings. See Materials and appearance.

Hidden bodies are not drawn and cannot be picked. Hiding a body in the panel is saved with the part, but it is not an undo step, and it does not change the geometry or what you export. Copy, Delete, Join, Cut, Intersect and Split are features: they appear in the tree, can be undone, and show in the History.

Names

A body that the part names (from the Operation control, a copy or a combine) shows that name, ahead of the feature name. Renaming it in the panel renames it in the feature that made it and in every feature that refers to it. A name another body already has is refused with “Another body is already called …”. A body that has no name in the part falls back to the feature that made it, or Body 1, Body 2, and so on.

Which body an Add or Cut acts on

An Add fuses with every body the new solid touches or overlaps; a Cut removes material from every body it reaches. An Add that reaches no body makes a separate one, and the first solid of a part just adds.

Once the part names at least one other body, the editors of Extrude, Revolve, Loft and Sweep show a control for it, and what it is called depends on the operation:

OperationControlChoices
AddTarget bodyAutomatic (every body the shape reaches), or one named body, which the operation then acts on alone (the others are left as they are)
CutCut fromAll bodies the shape reaches, or a ticked list of the named bodies: only the ticked ones lose material

Neither control is shown for New body, and neither appears until the part has a body it names. A body that the part no longer names stays in the list, so the feature still shows what it points at.

Parts converted from another CAD system

A part converted from another program can carry its stored solid (named Original (STEP)) on top of the body its history builds, so two identical solids lie on one another. Original (STEP) is hidden when the part is opened only if the body its history rebuilds is there and has the same volume (within 0.5%); if the history is suppressed, greyed, failed or a different size, it stays visible. Show or Hide in the Bodies panel changes that. An Add or Cut that is sketched on a face of one of two identical bodies acts on the body that owns the face, so a hole cut from a face does not meet its twin. When an Automatic cut cannot be made on all the bodies at once, it is made on each body in turn, the one that owns the face first; a body the tool misses, or whose hole already holds the tool, is skipped, and the cut is refused only when no body is touched.

Combine bodies

Join, Cut, Intersect and Split make a Combine bodies feature.

  1. Select the bodies in the panel. Click the target first: it is the body that keeps the result.
  2. Click Join, Cut, Intersect or Split.
OperationResult
JoinThe target and the other bodies become one
CutThe other bodies are subtracted from the target
IntersectOnly the volume shared by all of them is kept
SplitThe target is cut into two bodies: the part outside the other bodies and the part inside them. The other bodies are used up

Double-click the Combine bodies feature in the tree to open its Editor.

OptionWhat it doesDefault
OperationJoin, Cut, Intersect or Split.The button you clicked
Target bodyThe body that keeps the result. Read-only; shown in wordsThe first body selected
Tool bodiesThe other bodies. Read-only; shown in wordsThe other selected bodies
Keep the tool bodiesThe tools survive instead of being used upOff

Which bodies a combine acts on is set when you create it. To change them, delete the feature and make it again.

Typical failures:

  • A Cut that touches nothing is refused (“it cuts nothing”).
  • An Intersect of bodies that do not overlap leaves nothing.
  • A join can fail when the bodies only meet along a face. The Editor advises: “Make sure they overlap in a volume, not just along a face, or nudge one by a small amount.”

See combine in the kernel book.

Delete body

Two routes.

  • Select one or more bodies in the Bodies panel and click Delete.
  • Select faces in Face mode and choose Features > Bodies > Delete body. Every body holding a selected face is deleted.

The feature is called Delete or keep body. In its Editor the Mode drop-down switches between Delete and Keep. Keep removes all the bodies except the selected ones, which is the quick way to throw away everything but one body.

See deleteBody in the kernel book.

How other features treat several bodies

  • Add joins the new solid to the body it meets. New body joins nothing.
  • Shell hollows only the body that holds the faces you left open.
  • Patterns and Mirror repeat features. To copy whole bodies, use Copy or the ball. See Patterns, mirror and scale.
  • Scale can scale the whole part. See Patterns, mirror and scale.
  • Mass properties and Interference use the solid bodies. Sheets have no volume.

Interference check

To find bodies that overlap by mistake, use Evaluate > Measure > Interference check and click Check. It lists the “Bodies that share volume”. It needs two or more solid bodies. With one body it says so, and with none overlapping it says “No interference between N bodies”. See Measure and inspect.

Bodies that you made with New body can overlap without any warning while you model. Run the check before you export or make a drawing.

Common problems

SymptomFix
An extrusion became a separate body instead of joiningThe sketch plane did not reach the body. Change Operation to Add, or move the sketch plane onto the body
Two bodies merged into oneThey touch and were joined by Add. Make the second one with New body, or use Cut/Intersect afterwards
Join, Cut, Intersect or Split is greyed outSelect two or more bodies in the panel
A cut removes nothingThe tool body does not overlap the target. Check Interference first
A body cannot be picked in the viewIt is hidden, or it is almost transparent with something behind it. Check the eye and the opacity

Next

Frames, cut lists and connectors

The Frame feature turns a sketch of lines into a structural frame: every line becomes a member of standard stock (aluminium T-slot, Australian, US and European steel hollow sections, rolled beams, columns and channels, angle, flat or round bar), the corners are mitred or butted, and the hardware that joins the pieces is placed for you. The same frame gives a cut list and a bill of materials that match the model piece for piece.

Build a frame

  1. Draw the skeleton: a sketch (or a 3D sketch) with one line per member. A line that ends on the middle of another line becomes a tee.
  2. Choose Frame.
  3. Pick the Skeleton, tick the lines to use, choose the Profile and the Corners (mitre, or butt with the first line running through), and Create.

Choosing stock

The Region list picks which stock the Profile list shows: generic and T-slot (the default), Australia, United States, Europe, or all regions. The regional stock is several thousand profiles, so it is not loaded until you pick a region: the list shows “Loading the … profiles…” for a moment the first time, and the data is then kept for the session. A file that already contains a frame of a regional profile loads that region by itself when it opens, so the frame, its Edit panel and its cut list work at once.

The Profile list is grouped by region, standard and kind of section, and the box above it searches the region you picked: type any words of the name, designation, standard or grade (shs 50 c350, ub, hss 4x4, a500, w14x30, ipe 300, en 10219, t-slot) and only the matching profiles stay in the list. The US sections can also be found by their metric designation (W360X44). The profile you are using always stays listed. Under the list, a line shows the region, standard, grade and mass per metre of the stock, its material and whether its figures were checked against the published table. A row or grade that could not be verified wears an unverified badge; a hollow-section size that the catalogue marks “check availability” says so.

GroupStandardSectionsProfiles
Generic and T-slotnoneT-slot 20, 30, 40; SHS, RHS, CHS and aluminium tube, angle, flat and round bar in a few common sizes13
Australia, hollow sectionsAS/NZS 1163, grades C250L0, C350L0 and C450L0SHS 20 x 20 to 150 x 150, RHS 50 x 25 to 200 x 100, CHS 26.9 to 168.3 mm outside diameter221
Australia, rolled steelAS/NZS 3679.1, 300PLUSUB, UC and UBP (I sections), PFC (channels), equal and unequal angles, flat bar, round bar160
United States, rolled steelASTM A992 (W), ASTM A36 (S, C, MC, L)W 283, S 28, C 32, MC 40 and angles L 137 (AISC Shapes Database), imperial names (W14x30) with the metric designation520
United States, hollow sections and pipeASTM A500 Gr C (HSS), ASTM A53 Gr B (pipe)HSS square 107, rectangular 281 and round 128 (every size in the database), pipe 51 (STD, XS and XXS)567
Europe, rolled steelEN 10025-2, S355IPE 18, IPE A 18, IPE O 13, IPE AA 14, HE A 24, HE B 24, HE M 24, HE AA 24, IPN 21, UPN 18198
Europe, hollow sectionsEN 10210 hot-finished and EN 10219 cold-formed, S355J2HSHS 242, RHS 383, CHS 263888

Each profile is built with its outside size, wall or flange and web thickness and corner radii, so mass in the cut list agrees with the catalogue. Where the catalogue gives a mass per metre, the cut list and bill of materials use it (mass per metre times stock length), and stock without one (your own, the generic sizes) uses the modelled volume and the material density. Where the profile’s source is listed, Frame stock data and sources says what it is and what was left out.

Material of the stock

Each catalogue profile names the steel grade it is made of by default (its material_ref), a grade of the Material editor: ASTM A992 for W shapes; ASTM A36 for S, C, MC and L; ASTM A500 Gr C (shaped or round) for HSS; ASTM A53 Gr B for pipe; EN 10025-2 S355 for the European rolled sections; EN 10210 or EN 10219 S355J2H for the European hollow sections; AS/NZS 3679.1 grade 300 for the Australian rolled steel. These are defaults to confirm: they follow common practice for each family, not a statement by the catalogue, and the line under the Profile list, the bill of materials and the CSV say “default, confirm” next to them. The AS/NZS 1163 hollow sections name their grade (C350L0 and so on) but have no verified material record, so they show it as the grade only. The Australian profiles list grade 300PLUS (the catalogue’s name) and use the material AS/NZS 3679.1 grade 300; see Materials and appearance for the yield values.

When you create a frame from a catalogue profile and the part has no material of its own yet (nothing set, “steel” or Mild steel), the part’s material is set to the profile’s grade, so Mass properties in Inspect uses its density, and a notice says so. A part that already has another material keeps it, and Edit never changes it. The cut list and bill of materials mass of catalogue stock is the catalogue mass per metre times the stock length; the grade’s density is used for stock with no catalogue mass.

Hollow sections have rounded corners as the standards give them (outside radius 2 t up to 3 mm wall and 2.5 t above for AS/NZS 1163, 2 t for HSS, 1.5 t for EN 10210 and 2 t to 3 t for EN 10219), and the same hardware choices as the generic tube: a gusset plate by default, tube brackets where the tube is large enough, a plug for each free end, and a levelling foot where the bore can take its stud. Hardware is offered for hollow sections up to the size a frame is built from (rectangular up to 8 in = 203 mm, round up to 8.625 in = 219 mm outside); the larger structural sizes list none, like the open sections.

Open sections (UB, UC, UBP, PFC, W, S, C, MC, IPE, HE, IPN, UPN), angles and bars are mitred or butted like any other stock. Joints, cut angles, the cut list and the weld count work for them. The brackets, gussets, end caps and feet are made for tube and T-slot faces, so these profiles offer none: the Connectors section is not shown for them and the parts list holds no hardware. Beams and channels start with butt corners (the first line of a joint runs through). The flanges of an I section lie in the plane of a sketch drawn on a standard plane, and 90 degrees turns the web into it.

Each member is its own body, named like F3 M2. Editing the sketch moves the frame, and reopening the frame from the Features tree brings the panel back.

Connectors

The Connectors section of the panel lists the hardware the profile offers. A new frame starts with the profile’s defaults:

PlaceT-slot 20, 30, 40Steel and aluminium tube
JointsL corner bracket with a T-nut and a button head screw in each armGusset plate, welded
End capsCap over the section on every free endPlug-style cap on every free end
Levelling feetPad on a stud that goes into the bore of a leg standing on the floorSame, for steel tube

Set any place to None to leave it out.

  • At a node where three members meet at right angles, T-slot frames get one 3-way corner block (a cube with a plate on each member and a screw and T-nut in each) in place of two brackets; set 3-way corners to None to use brackets, or give one joint its own connector. Tubes offer the block and bracket choices, with weld gussets as the default.
  • Bracket on both sides at tees puts a second bracket on the other side of the through member. A tee row in the joint list has its own Both sides box.
  • For steel tube, choose a tube bracket or the corner block and tick Drill tubes and bolt the brackets: the members get through holes at each plate hole, and a bolt (length worked out for the tube) with a hex nut goes through. The cut list then shows the drilled volume. Without it the brackets are plates, to be welded or drilled later.
  • A bracket needs a 90 degree joint with the section square to the corner; a joint where it cannot go is listed with the reason (a gusset has no angle limit).
  • Click a bracket, a corner block or a member near a joint in the model to pick that joint: it lights up and its row in the Joints list is selected. Hover a bracket to light its joint; tap works the same on a touch screen. Click a row to light the joint in the model.
  • The Joints list shows every joint of the frame (the two lines, the angle and the corner type). Pick None or another connector for one joint; Default goes back to the frame’s choice. A tee joint takes one bracket, on the side the through line points to.
  • Feet go on the free lower end of a vertical member that stands on the lowest level of the frame. Other free ends get caps.
  • The Parts list under the Connectors updates with every change and is what the model holds: brackets, T-nuts, screws, caps and feet are real solids, each its own body (F3 H7).

Fasteners are modelled at their nominal size sitting in the existing slot and bore; threads are not modelled. Add your own stock and hardware to the library as described in apps/cad/src/frame/profiles.json.

Your own stock and fittings

Open My stock and fittings at the bottom of the Frame panel. Download example gives a small valid file to start from; Import file (or paste the text) adds your profiles, fittings and materials. The file is checked first: every problem is listed with its place in the file (for example profiles[0].section.t: needs a number above 0 (mm)), and nothing is imported unless it is all valid. A good library is kept in this browser and offered in the Profile list and the connector lists. Frames that use your stock keep a copy of it in the file, so someone who opens the file without your library still sees the right profile, hardware and bill of materials. Forget my library removes it from this browser only.

The file has three parts, all in millimetres:

{
  "materials": { "brass-cz121": { "label": "Brass CZ121", "density": 8.5e-6 } },
  "fittings": {
    "my-hex-m5": { "label": "Hex head bolt M5", "kind": "bolt", "spec": "ISO 4017 M5", "part": { "d": 5, "headD": 8, "headH": 3.5 } },
    "my-nut-m5": { "label": "Hex nut M5", "kind": "nut", "spec": "ISO 4032 M5", "part": { "af": 8, "t": 4 } },
    "my-bracket-30": { "label": "Bracket 30 tube", "kind": "bracket", "spec": "28 x 28 x 3 L angle", "part": { "kind": "lbracket", "arm": 28, "t": 3, "w": 26, "hole": 5.5, "holeAt": 17, "bolt": "my-hex-m5", "nut": "my-nut-m5" } },
    "my-cap-30": { "label": "Plug 30", "kind": "cap", "spec": "30 x 30, 3 thick", "part": { "kind": "cap", "t": 3 } }
  },
  "profiles": [{
    "id": "my-shs-30x30x2", "label": "My SHS 30 x 30 x 2", "family": "shs", "material": "brass-cz121", "corner": "mitre",
    "section": { "kind": "rectTube", "w": 30, "h": 30, "t": 2 },
    "fittings": [{ "id": "weld", "per": "joint", "qty": 1 }],
    "hardware": { "joint": ["my-bracket-30"], "cap": ["my-cap-30"] }
  }]
}
  • Sections are rect, rectTube, roundTube, roundBar, angle, channel, ibeam or tslot, with their dimensions (w, h, t, d, s…). rectTube also takes an outside corner radius r. channel takes one thickness t or its own flange tf and web tw, and a root radius r. ibeam has flanges w wide, depth h, flange tf and web tw thickness and root radius r. Optional catalogue fields on a profile (region, standard, grade, designation, mass_per_m_kg, source) are kept and shown in the list and the bill of materials.
  • Fitting parts are lbracket (arm, t, w, hole, holeAt), gusset (leg, t), corner3 (block, arm, t, w, hole, holeAt), cap (t) and foot (base, baseH, studD, studLen, neck). A bracket or block names its fasteners by fitting id: tnut and bolt for T-slot stock, bolt and nut for drilled tube. Bolts have d, headD, headH (the length is set by the model), T-nuts l, hex nuts af and t.
  • Hardware lists, per place (joint, corner3, cap, foot), the fitting ids a profile offers; the first is the default.
  • Ids must be new: the built-in ones cannot be replaced.

Cut list and bill of materials

Cut list opens the Drawings workspace on a drawing of the frame: isometric, front and top views with the pieces numbered, the cut list (profile, stock length, cut angles, quantity, mass) and the bill of materials. The bill of materials is grouped (stock, connectors, fasteners, caps and feet, process) and lists every bracket, nut, screw, cap and foot with its quantity and specification. Stock lines also give the standard, grade and material of the profile and the total mass of all its pieces in kilograms (catalogue mass per metre times stock length; stock without a catalogue mass uses its volume and density). Export it as PDF, SVG or DXF, or the two tables as CSV.

Frame stock data and sources

The Australian, US and European profiles of the Frame tool are built from published catalogue tables. This page lists where each figure comes from, how it was checked, what was left out, and how to rebuild the lists. Section sizes and masses are facts that manufacturers and standards bodies publish; the catalogues themselves, their text and their layout are not copied, and each profile names its source table.

Sources

StockStandard and gradeSource tableProfiles
Square, rectangular and circular hollow sectionsAS/NZS 1163, grades C250L0 (small round), C350L0 and C450L0Australian Tube Mills, Design Capacity Tables for Structural Steel Hollow Sections, August 2013, Tables 3.1-1 to 3.1-6 (dimensions and properties). The C450 tables are headed as designed to grade C450L0.221
Universal beams and columns, universal bearing pilesAS/NZS 3679.1, 300PLUSInfraBuild, Hot Rolled and Structural Steel Products, 9th Edition (2019), Tables 9, 11 and 1745
Parallel flange channelsAS/NZS 3679.1, 300PLUSsame, Table 1510
Equal and unequal anglesAS/NZS 3679.1, 300PLUSsame, Tables 19 to 2465
Flat bar, round barAS/NZS 3679.1, 300PLUS (merchant bar is made in several grades: confirm with the supplier)same, Table 5 (flats) and Table 3 (rounds)40
W, S, C, MC shapes and angles (L)ASTM A992 (W), ASTM A36 (S, C, MC, L)AISC Shapes Database, version 15.0 (November 2017; Steel Construction Manual, 15th edition), sheet “Database v15.0”, W, S, C, MC and L rows520
Hollow structural sections (HSS) and pipeASTM A500 Gr C (HSS), ASTM A53 Gr B (pipe)same database, HSS rows (516) and PIPE rows (51)567
IPE, IPE A, IPE O, IPE AA, HE A, HE B, HE M, HE AA, IPN, UPNEN 10025-2, S355 (dimensions to EN 10365)ArcelorMittal, Sections and Merchant Bars, sales programme (FR/EN/DE, PDF dated 2024-03), the dimension table and the “Dimensions and properties” table of each family198
Hot-finished and cold-formed SHS, RHS, CHSEN 10210 and EN 10219, S355J2HSCI P363, Steel Building Design: Design Data (Tata Steel, BCSA, SCI; reprinted 2015), tables for Celsius (EN 10210-2) and Hybox (EN 10219-2) sections; masses cross-checked against the Tata Steel Hybox S355J2H datasheet (TST95:0122, 2022)888

For each profile the list shows the region, standard and grade; the Frame panel shows the source table in a tooltip; the bill of materials prints standard, grade, material and mass.

To review. The AISC workbook could not be downloaded from the AISC site (the server refused automated requests, HTTP 403). The identical file, with the AISC disclaimer unchanged, was taken from a public redistribution (an MIT-licensed repository that packages it), and an independent copy of the same database matched it value for value. The terms under which the AISC data may be reused have not been reviewed; the profile figures are published dimensions and weights, but the question stays open until someone has read the AISC terms (see THIRD_PARTY.md).

What the figures are

  • Sizes are the nominal outside dimensions and wall (or flange and web) thicknesses. Mass per metre is the catalogue figure; for US stock it is the published weight in pounds per foot converted to kilograms per metre (1 lb/ft = 1.48816 kg/m). Inches convert at exactly 25.4 mm.
  • The US hollow sections and pipe are modelled with the nominal wall and an outside corner radius of two wall thicknesses, which reproduces the published weight to within 0.6 per cent. AISC tabulates the weight on the nominal wall but the area and section properties on the design wall (0.93 of nominal, ERW A500), so the catalogue weight is 5 to 11 per cent above the tabulated area times 7850 kg/m3. The bill of materials uses the catalogue weight; the design wall is not modelled.
  • US W shapes use the database’s flange, web and root-fillet sizes. S, C and MC shapes have tapered flanges: they are modelled with the database’s mean flange thickness and no root fillet, which keeps the modelled area within 3 per cent of the weight (C3X3.5 is the exception: the database’s own weight is 5.6 per cent under its area). European IPN and UPN are modelled the same way with the catalogue’s mean flange thickness and root radius (IPN 80, UPN 65 and UPN 80 come out 3.1 to 3.3 per cent heavy). EN 10210 SHS 50 x 50 x 8 and 80 x 80 x 12.5 come out 3.1 and 3.2 per cent heavy because the tube corner is built with inside radius outer minus wall where the standard has 1.0 t.
  • European hollow sections use the standard’s corner radii: hot-finished (EN 10210) 1.5 t outside and 1.0 t inside; cold-formed (EN 10219) 2 t up to 6 mm wall, 2.5 t above 6 and up to 10 mm, 3 t above 10 mm. The two standards give different properties for the same size, so each is its own group in the Profile list.
  • Australian hollow sections use an outside corner radius of 2 t up to 3 mm wall and 2.5 t above, with the inside radius 1 t and 1.5 t; the modelled area agrees with the table’s gross area.
  • Rolled sections include the root radius of the table (I sections and channels); angles are modelled with square corners (no root or toe radius), which keeps the modelled area within 1.3 per cent of the catalogue’s.
  • Strength properties (second moments of area, section moduli, capacities) are not stored or used. Check the current edition of the catalogue and the design standard for anything other than layout, cut lists and mass.

How it was checked

  • Each hollow-section row was read from the table text by a script that rejects a row when its mass differs from the area times 7850 kg/m3 by more than 1.5 per cent, or when the table’s own width-to-wall ratios do not match the size read for the row. One row of the C450 square table, 35 x 35 x 3.0, could not be read reliably from the text and is not included; the same size is in the C350L0 table.
  • Each rolled-section row is verified when the catalogue text has a line that carries both its mass and its gross area (angles, channels, I sections) or the mass in the right row and column of the size table (rounds and flats). All 28 beams, 13 columns, 10 channels, 65 angles, 34 flats and 6 rounds passed. The bearing piles were transcribed and machine-checked in a separate data set.
  • Each US row was taken from the database workbook; an independent CSV copy of the same database matched all 10412 compared values. Imperial values are converted exactly (25.4 mm/in, 1.48816394 kg/m per lb/ft) and rounded to four significant figures. The AISC metric columns agree with the conversion within 1.5 per cent except six small-section weights (rounding of small integers). The database’s HSS area equals the closed form with outside radius 2 t and inside radius t on the design wall within 0.4 per cent.
  • The European open sections were checked against the catalogue’s two tables (mass and properties agree for every section), against the second moments recomputed from the dimensions (within 0.09 per cent for the 159 parallel-flange sections) and against mass = area x 7850 kg/m3 (within 1.1 per cent). The hollow sections were checked against mass = area x 7850 (within 0.6 per cent) and against the Hybox datasheet masses: 283 of the 285 sizes found there agree within 1 per cent. Two differ and the SCI value is kept: RHS 100 x 50 x 5 (10.5 against 10.3 kg/m) and RHS 200 x 100 x 8 (33.9 against 43.2 kg/m, a misprint in the datasheet; 33.9 matches the area). SCI marks some sizes “check availability”; the profile carries that flag.
  • The tests also check every profile: unique ids, positive dimensions, hardware that exists, and the mass per metre within 3 per cent of the modelled area times 7850 kg/m3.

Left out

  • Cold-formed channels and zeds (C and Z purlins): their lipped section needs a section kind the Frame tool does not have. A follow-up.
  • Taper flange beams (TFB): the flanges are not parallel. A follow-up.
  • Welded beams and columns, and rolled sizes that the catalogues do not list.
  • Hollow sections larger than the range above (the tables go to 400 mm square and 508 mm round), and sizes that are not in the tube maker’s tables.
  • US and European sections that are not frame stock in the first lists: M, HP, WT, MT, ST and double angles; IPE 750 and the heavy HE series above 1000 mm; UPE; elliptical hollow sections; Hybox sizes outside SCI P363. The flat bar and round bar of the US and Europe have no public table of standard sizes, so none is listed.
  • Section properties (second moments, moduli, torsion constants) are in the verified data files but not in the profile lists: the Frame tool does not use them.
  • Hardware (gussets, plugs, feet) is offered only for hollow sections up to the size a frame is built from; larger structural sizes list none.
  • The 35 x 35 x 3.0 square section in the C450 table (see above).

Rebuilding the lists

The lists are generated and committed, so nothing is fetched while using the tool. To rebuild after a change in the data (developers):

  1. tools/extract_atm_hollow.mjs reads the hollow-section tables from the text of the PDF (pdftotext -layout) into apps/cad/src/frame/data/au-hollow-atm.json.
  2. tools/verify_au_sources.mjs re-checks the rolled-section rows against the catalogue text and records verified in data/au-sections.json.
  3. tools/steel_data/ holds the scripts that produced data/us-sections.json, data/eu-sections.json and data/steel-materials.json from the AISC workbook, the ArcelorMittal catalogue text and the SCI P363 text (they need those files, which are not in the repository, and write the verification reports beside them).
  4. tools/build_frame_profiles.mjs writes profiles.au.json, profiles.us.json and profiles.eu.json; tools/build_steel_materials.mjs writes apps/cad/src/materials.steel.json. --check compares them with the data and the tests run both.

Each regional list is a separate file that the app loads only when its region is used (so the program itself stays small): profiles.au.json about 170 kB, profiles.us.json about 500 kB and profiles.eu.json about 540 kB before compression (11, 39 and 26 kB compressed).

Add your own stock the same way as described in Frames, cut lists and connectors.

Materials

The steel grades of the Material editor (data/steel-materials.json) come from these sources. A grade is verified when its headline strengths agree between at least two independent public sources, or a mill catalogue that reproduces the standard’s table; the others carry an unverified badge.

GradeSourceVerified
EN 10025-2 S235, S275, S355EN 10025-2:2019 mechanical table as reproduced in the ArcelorMittal catalogue (thickness bands to 140 mm); E, Poisson’s ratio and density from SCI P363yes
EN 10210 and EN 10219 S355J2HSCI P363 section 5.2 (ReH by thickness) and the Tata Steel Hybox S355J2H datasheet (Rm 470 to 630 MPa)yes
ASTM A36Wikipedia article “A36 steel”, quoting the AISC Steel Construction Manual: 36 ksi, 58 to 80 ksiyes
ASTM A992Wikipedia article “ASTM A992” (cites A992/A992M): 50 ksi, 65 ksi, fy/fu at most 0.85yes
ASTM A572 Gr 50ASTM listing summary for A572/A572M and Wikipedia: 50 ksi, 65 ksiyes
ASTM A53 Gr Ban AISC magazine excerpt and an engineering reference: 35 ksi, 60 ksi; a single secondary sourceno
ASTM A500 Gr B (round 42 ksi, shaped 46 ksi) and Gr C shaped (50 ksi)A500-07 SI table as in Wikipedia, a fabricator summary and the Steel Tube Instituteyes
ASTM A500 Gr C round46 ksi (315 MPa) in the A500-07 to -18 summaries; the Steel Tube Institute says the 2021 revision gives 50 ksi (345 MPa) for all shapes. The record keeps 46 ksi and stores 345 MPa as the alternateno (edition conflict)
AS/NZS 3679.1 grade 300 and 350a third-party web printout of the standard’s property tables (fy 280 and 330 MPa, fu 440 and 480 MPa); the InfraBuild catalogue shows thickness-dependent yields, so these are conservative lower boundsno

The elastic constants of the European grades (E 210 GPa, Poisson’s ratio 0.3, G 81 GPa, expansion 12 x 10^-6/K) follow EN 1993-1-1 as summarised in design aids; the standard text itself was not read. The US constants (E 200 GPa, G 77.2 GPa, Poisson’s ratio 0.3) are the AISC 360 values and were not retrieved from a source; US thermal expansion is left empty. The ASTM, EN and AS/NZS standard texts are paywalled and were not read; the figures rest on the bodies and catalogues named above.

Defaults to confirm. Which grade a profile is made of by default (A992 for W; A36 for S, C, MC and L; A500 Gr C for HSS; A53 Gr B for pipe; S355 for the European rolled sections; S355J2H for the hollow ones; AS/NZS 3679.1 grade 300 for Australian rolled steel) follows common practice and is not a published fact about the profile. Each such profile is flagged material_default in the data and the bill of materials adds “default, confirm” to its material. The Australian catalogue lists grade 300PLUS; the material record names it 300, so the Australian profiles use as-nzs-3679.1-300, whose yield is the conservative lower bound described above.

Equations and variables

Any number you type into a feature can be a formula instead. You can also define named values (variables) once and use them in many places, so that changing one number resizes the whole part. This chapter covers variables, expressions in fields, units, evaluation order, and what the errors mean.

Typing a formula in a field

Every number field in the feature Editors accepts three kinds of input:

  • A plain number, such as 12.5.
  • A variable name, such as width.
  • An expression that starts with =, such as =width*2+3.

A number stays a number. Anything else is stored as an expression and re-evaluated whenever a variable changes.

While the text is an expression:

  • The field shows a blue fx badge. The evaluated value shows under the field (for example = 6 mm).
  • A bad expression shows its error and is not applied. The model keeps the last good value.
  • Variable names, the functions and pi complete as you type. Use the arrow keys with Enter or Tab, or click.
  • Click fx to keep the current value as a plain number and break the link.

Some fields take a plain number only, because the app itself calculates with them. These say “This field takes a plain number” if you type a formula. They are the draft angle, the Start and End radius of a variable fillet, the scale factors, the loft tensions, and the thread length.

Drag handles on the canvas (the depth arrow, the size box) are not offered for a field that holds an expression, so a drag cannot silently replace your formula. Remove the formula first if you want to drag.

Sketch dimensions

A sketch dimension takes the same text. Double-click the dimension label (or its row in the constraints list), and type a number, a name or =expression. The dimension is drawn with an fx mark, and the sketch is solved again whenever a variable changes. Typing a plain number unlinks it. The value boxes that follow the pointer while you draw accept an expression, but only its value is used there and no link is made.

Sketch point coordinates and circle radii in the sketch itself are plain numbers. To drive a size from a variable, dimension it and give the dimension an expression. See Constraints and dimensions.

The Variables panel

Open it from Home > Create > Variables (it shares the Catalog button) or from the Variables tab of the left panel.

Each row has:

ColumnWhat it is
NameLetters, digits and _, not starting with a digit. Case sensitive.
ExpressionA number or an expression. It can use other variables.
ValueThe evaluated result in mm or degrees. A small number beside it counts the places that use the variable. Hover for the list
UnitA label: blank, mm or °. It is a note for you. It does not change the value
CommentFree text

Click Add variable to add a row; a new one starts as 10 with the unit mm. Edit any cell in place. A cell commits when you press Enter or leave it.

  • Rename rewrites every use in one step: other variables, configurations, feature fields (=w*2 becomes =width*2) and sketch dimensions. Only whole names are replaced, so w does not touch w2.
  • Delete works only for a variable nothing uses. A used one is refused with “<name> is used by <places>. Change those fields first.”
  • Nothing is applied until the whole list evaluates. If it does not, the row shows the error and the part is unchanged.
  • If every row is valid but the part cannot rebuild with the new values (for example a depth that becomes zero), the whole change is refused with “The part would not rebuild with that change, so nothing was changed”, and the failing features are shown.
  • Each change is one undo step in the same history as feature edits. It appears in the History as Edit variables, Rename variable, Add variable and so on.

A worked example. Define t = 4 and d = t*2. Type =d into an Extrude depth. The depth is 8. Change t to 5 and the depth becomes 10.

Writing expressions

PartWhat is allowed
Operators+ - * / ^ and parentheses. ^ is right-associative and binds tighter than unary minus: -2^2 is -4 and 2^3^2 is 512
Functionssqrt, sin, cos, tan, abs, each with one argument in parentheses. Angles are in degrees. Names are not case sensitive
Constantpi
VariablesBy name. Variable names are case sensitive
Numbers12, .5, 1e3. A comma counts as the decimal point, so 1,5 is 1.5

Not available: min, max, round, and conditions. They are reported as unknown names.

Units in expressions

You can put a unit directly after a number. The unit converts the number to millimetres (or degrees):

UnitMultiplier
mm, deg, °1
cm10
m1000
in25.4

So =3 in is 76.2, =2 cm is 20, and =1.5 m is 1500. Length fields are in millimetres and angle fields are in degrees. The unit only scales the number. It is not checked against the kind of field, so =90 deg in a length field is just 90.

A unit has to follow a number. It cannot follow a name or a parenthesis. =3 mx and =width mm are errors. Variable names cannot be pi, a function name or a unit.

For the full grammar and a table of results, see Variables and expressions in the kernel book.

Order of evaluation

Variables can use each other in any order. You do not have to define a variable before you use it. The part works out the values by repeatedly evaluating every variable whose expression uses no unresolved variable.

  • a = b + 1 with b = 5 works whichever row comes first.
  • A cycle (a = b + 1 and b = a + 1) cannot be solved. The panel refuses it with “Circular reference between variables”.

Errors

MessageMeaning
Not a valid expressionA syntax problem: a missing parenthesis, sqrt 4 without brackets, a result that is infinite (1/0)
Unknown variableThe name is not defined (names are case sensitive: W is not w)
Invalid name: letters, digits and _, not starting with a digit, and not pi, sqrt, sin, cos, tan, abs or a unitThe variable name breaks the rules
Name already in useTwo variables share a name
Circular reference between variablesVariables depend on each other in a loop
This field takes a plain numberThe field is one the app calculates with

If a feature uses a variable that is missing or cannot be worked out, the feature fails and shows in red in the tree, with a message such as an invalid expression. Define the variable or correct the formula. See The feature tree and history.

Configurations

A configuration is a named set of variable values, such as Small, Standard and Large.

  • Add from current values captures the current expressions under the name you typed in New configuration name.
  • Click a configuration to switch the variables to its values. The part rebuilds in one undo step.
  • Save values stores the current expressions into that configuration. A configuration whose values no longer match the variables is marked modified.
  • Renaming or deleting a variable updates the configurations.

Configurations are saved in the part file, but other programs that rewrite the part may not keep them.

Next

The feature tree and history

Every part is a list of features, built in order from top to bottom. The feature tree shows that list. You can rename, reorder, suppress, delete and group features, step back in time with the rollback bar, and undo or redo any change. This chapter also explains what happens to later features when you edit an earlier one.

The feature tree

The tree is the Features tab of the left panel. At the top it shows the part name (double-click it, or press F2 with no feature selected, to rename the part), the number of features, and a count of failed ones in red. Below that come fixed rows for the material, the Front, Top and Right planes, and the origin, then one row for each feature.

A row shows the feature’s icon, its name, and its id (such as F4) in muted text. Some details:

  • A sketch is tucked under the first feature that uses it. Click the chevron to open or close it. A thread sits under its hole.
  • A note such as “patterned by F7” marks a feature that a pattern repeats.
  • A failed feature is red with the reason under it. A feature that only fails because an earlier one failed is muted and says “blocked by F3”: click it to jump to the cause.
  • An amber ! on a row is a warning. The feature still works. Hover for the text.
  • A suppressed feature is dimmed and in italics.
  • Hovering a row tints in the view what the feature made. Hovering a face in the view marks its feature’s row.

Select a row with a click. Ctrl-click (Cmd on a Mac) toggles one more, and Shift-click selects a range. With a row selected, the rows that depend on it get a thin marker at the left edge.

Press Ctrl+F in the tree, or click the magnifier, to search features by name, type or id (for example F62, revolve, lens). Enter or Down goes to the next match, Shift+Enter or Up to the previous, and Esc clears the search.

Row buttons

Hovering or selecting a row shows buttons on its right:

Button (tooltip)What it does
Select in viewportSelects the faces the feature made (not for sketches and planes)
EditOpens the feature’s Editor
Roll back to hereMoves the rollback line below this row
Hide (view only) / ShowHides or shows what the feature made. Nothing is rebuilt
Suppress (rebuilds) / Unsuppress (rebuilds)Suppresses or restores the feature. It shows a pause icon
RemoveDeletes the feature. It shows a trash icon

When several rows are selected, the buttons act on all of them.

Rename

Select a feature and press F2, or choose Home > Edit > Rename. Type a name and press Enter. Esc cancels. An empty or unchanged name cancels. Renaming is one undo step. A generated name for a plane or a sketch, such as “Plane 10 from Front”, keeps following its settings until you give it a name of your own.

Suppress

Suppressing a feature builds the part as if it were not there, without deleting it. Select it and press Ctrl+Shift+U, click its Suppress button, or choose Suppress / unsuppress from the right-click menu. With a mix of suppressed and active features selected, they all become suppressed. If they are all suppressed, they all come back. Suppress a feature to see the part without it, or to find out which later features depend on it. Like any edit, a suppress that would break a later feature is refused and the model stays as it was.

Delete

Select one or more features and press Delete or Backspace, or click its Remove button. A “Deleted F5” notice appears with an Undo button.

If a feature you did not select still uses the one you are deleting (a sketch used by an extrude, a seed used by a pattern), the delete is refused and the notice names what uses it, with a Delete both button that removes them together. You can also select them all first. Deleting is one undo step, and one Undo brings everything back.

Reorder

Drag a row onto another row to move it there. A feature travels with the sketches tucked under it. A move is refused, with a short message, when it would put a feature before one it uses, for example before its own sketch. A Loft that you point at a later sketch is moved for you, and the app says “Loft moved after …”.

The rollback bar

The model is here line in the tree marks how far the model is built. Drag it up between rows to see the part as it was at that point. Features below the line are greyed out and not built.

  • Drag the line, or focus it and press Up, Down, Home or End.
  • Click the Roll back to here button on a row to put the line below that row.
  • Click Roll forward on the line, or choose Home > Edit > Roll forward, to return to the end.
  • While rolled back, new features are added right after the line and the line moves past them.
  • A sketch you start while rolled back previews on the part as it is at the line.

The rollback line is only a view. Every feature is still in the part. The line is not saved and is not an undo step, and reloading the part puts it back at the end.

Folders

A folder groups neighbouring features under one collapsible row. It changes only the tree, not the order or the result.

  1. Select two or more features that are next to each other.
  2. Choose Group into folder (Ctrl+G, or Home > Edit, or the right-click menu).
  3. Type a name. It starts as “Folder”.

Click a folder to open or close it. Double-click it, or choose Rename folder, to rename it. A button on the folder row selects every face of the group in the view.

Drag a row onto a folder to put it at the end of that folder. Drag it onto a row in the folder to take that place, or onto a row outside to leave. Drag a folder header onto a row or another folder to move the whole folder. Folders do not nest.

Right-click onChoices
A featureEdit, Roll back to here, Hide in the view / Show in the view, Select its faces in the view, Select its bodies, Add fastener to hole (on a hole feature or a pattern of holes), Group into folder (Ctrl+G), Remove from folder (when in one), Rename (F2), Suppress / unsuppress (Ctrl+Shift+U), Delete, Collapse all folders
A folderRename folder, Ungroup, Export folder geometry (STEP, STL, part file), Extract folder as a part, Delete folder, Collapse all folders

Select its bodies selects the bodies the feature made that are still in the part (a body a later feature used up is not listed). Collapse all folders closes every folder but the one you clicked. Export folder geometry and Extract folder as a part take a folder out of the model as a file or a new document; see Exporting. Ungroup removes the folder and leaves the features where they are. Delete folder deletes its features, with the same rules and Undo notice as Delete.

A folder action is refused when the rows are not neighbours (“Only features next to each other can be grouped; folders do not change the build order”), when it would put a feature before one it uses, when the name is taken, or when it would split another folder. Whether a folder is open or closed is remembered in your browser for each part; long parts start with their folders closed.

Undo and redo

Every change is one undo step: a new feature, an edit confirmed in the Editor, a rename, a delete, a suppress, a move, a variable change, a folder action, or a whole drag. A drag is previewed first and only counts when you release it.

ActionKeysWhere
UndoCtrl+Z (Cmd+Z)Home > Edit
RedoCtrl+Shift+Z or Ctrl+YHome > Edit
Repeat last commandHome > Edit
RebuildCtrl+BHome > Edit

Rebuild builds the part again from the document and shows “Rebuilt”. Use it when something looks stale. The kernel does not keep a cache, so every build is a full rebuild.

Repeat last command runs the last command you ran again: the last feature you made, the last fillet, the last export, the last view. Press Enter to run it when nothing is in progress (no sketch open, no feature being edited, no dialog); the button has no other shortcut, and it says “No command has been run yet” until something has run. The command search itself is not remembered as a last command, and Repeat last command never becomes the last one either. The button is greyed out while the last command cannot run now.

The History log. Open the drawer (View > Workspace > Toggle drawer, or the backslash key) and choose History for a log of every edit. Filter by All, You, Agent (edits made through the MCP server, see Agents and the MCP server) or Failed. Click an entry to go back to that step: the later steps are undone, and Redo can bring them back. A “model is here” line shows where you are. Rejected edits appear in the log marked failed, so you can see what was refused.

Each open part (tab) has its own undo history. A part restored after a crash comes back without its undo steps.

Editing an earlier feature

Double-click a row, click its Edit button, or double-click one of its faces in the view (not while sketching). The Editor opens on that feature, with a live preview. Everything after it is rebuilt as you type.

What happens to later features:

  1. The values still work. Features keep referring to faces and edges by name (for example the top face of F2). Changing a depth, a radius or a sketch size keeps those names, so later features follow the change. A fillet on a box edge stays on that edge when the box grows.
  2. A name disappears. If the edit removes or reshapes what a later feature points at (for example you delete the feature that made the face, or change a sketch so that an edge no longer exists), that later feature fails with “a face or edge it uses no longer exists”.
  3. The app protects the model. While you type, the preview shows the problem. If the draft would break the model, the tick is greyed out with “This change breaks the model (F5). Cancel or adjust.” Holding Shift while you confirm tries it anyway. An edit that the kernel refuses is not applied at all: you get “This edit was not applied; your model is unchanged”, the cause and a list of things to try, and Undo this change, Cancel edit and Select F5 buttons.

Tips that make editing earlier features safer:

  • Put fillets, chamfers and shells late in the history.
  • Dimension and constrain sketches, and give features and sketches clear names.
  • Use variables for sizes that several features share. See Equations and variables.
  • Use Suppress to test whether a feature is the cause.
  • Use the rollback line to edit a feature “as it was” without looking at the later features.

Failures and the Diagnostics tab

Failed features are red in the tree. The drawer’s Diagnostics tab explains the cause first and lists the features that only fail because of it. Fix the cause and the others usually clear. See Checks and diagnostics.

Next

Plugins

A plugin adds a generator: a form that builds a part for you, such as a case, a spring or a cabinet. Two are built in: Enclosures (Case) and Springs. You fill in the fields, watch the preview, and Add it. It goes into the tree as ordinary features in one folder, and one Undo removes it.

Use a generator

  1. Open the Features tab and choose Plugins (or press the Features tab’s gear menu to pick a generator directly).
  2. Pick a generator, change the fields and watch the preview. A field left empty shows auto: the generator chooses.
  3. Choose Add. Position moves the result before it is built.

Back to the list and Cancel leave the model untouched.

Change or move a generated part

Right-click its folder in the tree:

  • Edit parameters… opens the same form with the values you used. Update rebuilds the folder in place, as one undo step. It is refused if something outside the folder depends on its faces.
  • Move folder (drag with the ball) shows the move ball: drag an arrow to slide the whole part, or type a distance and press Enter.
  • Move folder by distance… asks for X, Y and Z.

Install a plugin made by someone else

Installed plugins are off by default. In Plugins, switch on Allow plugins from other people, then add one from a packed zip file, from github:owner/repo@tag, or from a link to a zip. The app shows what the package contains, its hash and anything it could not check, and installs only after you confirm. Use a tag or a commit, not a branch, so the package cannot change later. Remove a plugin from the same panel.

A plugin with compiled code runs in a sandbox: it cannot reach the network, your files or your document, and it is stopped if it runs too long. Only install plugins from people you trust; the sandbox limits what a plugin can do, not whether its geometry is any good.

SolidCraft’s Woodwork

The app can run the SolidCraft Woodwork plugin (cabinets in sheet goods) by TomasDJo, MIT licence, once it is packed for this app. Its Cabinet form builds the boards, shelves, holes and colours from the material library. Doors and drawers do not swing, and its joinery and cut list entries are not available yet.

With an agent

An agent connected through the bridge can list the installed generators and run one on the open document with app_plugin_list and app_plugin_run. Running one changes the document, so it needs the box that lets the agent change it, and it is one undo step.

Limits

  • The sandbox has been checked in Chrome and Safari. Firefox is not checked yet.
  • In the Mac app, installing from github: works; links to other websites do not. The sandbox has not yet been checked inside the Mac app itself.

Assemblies and mates

An assembly is a part that holds other parts as components. You insert parts, place them, and tie them together with mates so that they move the way the real thing would. This chapter covers inserting and placing components, the mate kinds, reading the degrees of freedom that are left, editing a component’s own features, and the bill of materials, exploded view and interference check.

How an assembly works

Every component is an Insert part feature that keeps a full copy of the part you chose. Editing the source file later does not change the assembly. Each component stays its own body, also where it touches another component.

Mates are features too. They sit in the feature history after the components they position, so they undo, redo and rebuild like any other feature. The kernel solves the mates and moves every component that is not fixed.

The Assembly ribbon tab has two groups:

GroupCommands
ComponentsInsert part, Mate
ReviewBill of materials, Exploded view, Interference check

Each command opens the Outliner tab of the left panel on the matching section: Parts, Mates, Interference, BOM or Explode. When a part that already holds components is loaded, the ribbon switches to the Assembly tab by itself. The commands need an open part; Mate, Bill of materials, Exploded view and Interference check also need at least one component.

Insert a part

  1. Open or start the part that will hold the components. Choose Insert part on the Assembly tab.
  2. Under Sample part, pick one of the sample parts, or press Open a .ckpart file… to read a part from disk. A file that is not a part is refused with “That file is not a part file.”
  3. Set the Placement: X, Y and Z offsets in millimetres, and optionally Turn about X, Y or Z with an Angle in degrees. The default is no offset and no turn.
  4. Tick Fixed (does not move when mated) if this component should stay where it is. The first component of an assembly is usually fixed.
  5. Press Insert. The notice “Inserted <name>.” confirms it, and the component appears in the list.

Mates move components relative to each other. A component you leave unfixed can be moved by any mate that involves it; a fixed component never is.

Work with components

Every component is a row in the Parts list: its name, the part it came from, and a badge for the degrees of freedom it has left (“1 DOF remaining”, “fully defined”, “fixed”). Click a row to select the component’s faces in the model. The placement fields under a selected row change its X, Y, Z and turn; press Apply placement. Mates move the component again afterwards, so placement matters mostly for the starting position.

Buttons on a row:

ButtonWhat it does
Show / Hide (the dot)Hides the component in the view only. Not saved, and it does not change the model.
Suppress / UnsuppressLeaves the component out of the build. The component stays in the file.
Fix / FloatFixes the component in place, or lets mates move it again.
Gear icon (Edit this part)Opens the component’s own features in a tab. See below.
Pencil (Rename)Renames the component. Double-clicking the name does the same.
Cross (Delete component)Deletes the component together with the mates and component patterns that used its faces, in one undo step.

Mates

Choose Mate to open the Mates section, then New mate.

  1. Pick the Kind. The menu is grouped as Standard, Advanced and Mechanical, and each kind has a tooltip.
  2. Fill the references. Each reference slot has a Pick button: press it, then click a face in the model. Select faces in Face mode (the hint under the list says so). A round face gives its axis for kinds that need an axis, such as Concentric.
  3. Press Flip if the kind has it and you want the other orientation (the wording changes with the kind, see the table).
  4. Enter the value for kinds that have one (a distance, an angle, a ratio and so on) and, if you like, a Name.
  5. Press Preview to see the result without committing it (“Preview shown. Apply keeps it.”), then Apply. Cancel drops a preview.

References are faces. Edges are not accepted. Angles are in degrees, lengths in millimetres.

To change a mate, choose Edit on its row. Changing the kind replaces the mate. The Delete button removes it. Pressing Apply checks the draft first and tells you what is missing: “Pick every reference first.”, “Pick different faces.”, “Enter a number.” and so on.

Mate kinds

KindWhat you pickExtra fieldsFlip means
CoincidentTwo facesAligned or opposed
ParallelTwo facesAligned or opposed
ConcentricTwo round faces (axis)Aligned or opposed
DistanceTwo facesDistanceHas a Flip switch
AngleTwo facesAngleSupplementary angle (180 minus the angle)
PerpendicularTwo facesNo Flip
TangentA flat, cylindrical or spherical face and anotherThe other side of a flat face, or one round face inside the other
LockTwo facesNo Flip. Freezes the two components relative to each other as they are now.
SymmetricTwo faces and a mirror planeNo Flip
WidthThe two sides of a tab and the two sides of a slotNo Flip. Centres the tab in the slot.
LimitsTwo facesLimit (Distance or Angle), Minimum, MaximumNo Flip. Lets the faces move within a range.
HingeTwo round faces, optional stop facesDistance (stop offset, optional)No Flip. Shares an axis and leaves one rotation.
SlotA pin (round face), a slot wall, optional second wallHas a Flip switch
ScrewTwo round facesPitch, DriveLeft-hand thread
GearDriver and follower round facesRatio, DriveSame direction (default is opposite)
Rack and pinionPinion (round face) and rack (round or flat face)Pitch radius, Drive, Rack directionReverse

Five more kinds are listed but cannot be used yet: Profile centre, Path, Linear coupler, Cam and Universal joint. They show “kernel pending” in the menu and are disabled.

Drive and the test slider

Gear, Screw and Rack and pinion have a Drive field in degrees (it may exceed 360). Leave it empty and the coupling stays free. Under the field a Test drive slider previews the motion: every change runs the mate as a preview, Cancel drops it and Apply keeps the value. A Drive removes one degree of freedom from the assembly, because the coupling now has a fixed angle. Hinge has no Drive.

Degrees of freedom

The top of the Mates section reports what is still free:

  • The total (“N DOF remaining”) split into translational and rotational freedoms, and one line per component.
  • An Over-constrained banner when mates repeat or contradict each other. It lists the mates that add no constraint (“Redundant”) and the mates that conflict with earlier ones. Click a row to select that mate and its faces.
  • A “rolled back” note for each mate the kernel refused, with the reason: it cannot be satisfied together with other mates, the faces cannot be used for that kind, both components are fixed, both faces belong to one component, or a face it used no longer exists. A rolled-back mate leaves the components where the earlier mates put them.

Normally an edit that would break a mate is refused as a whole and the assembly stays as it was. The rolled-back notes mostly appear for files that were opened with such a mate already in them. In a very large assembly the kernel skips the translational and rotational split, and the panel says so.

Edit a component’s own features

To change a component itself, press the gear icon on its row, or Edit this part’s features in the component’s editor. The component’s part opens in a tab of its own, next to the assembly’s, with its full feature tree, sketches and editors. A bar over the viewport reads “Editing <part> (in <assembly>)” with Done and Cancel.

  • Done writes the edited part back into the component as one undo step in the assembly and closes the tab. Placement and mates stay, and the assembly rebuilds.
  • If a mate depended on something you removed, the assembly refuses the change, the part stays open and a message says so.
  • Cancel closes the tab and leaves the component unchanged.
  • Saving to a file is refused on that tab (“Finish editing the part first”). Close it with Done or Cancel first.

Only the edited component changes. Other instances of the same part are separate copies and keep their old geometry.

Bill of materials

Choose Bill of materials. The list has one line per distinct part: No., Part, Qty, Material, Mass each and Mass total, plus a Total row. Components of the same inserted part count as one line; copies made by a component pattern count too, suppressed components do not. A click on a row selects the bodies of those components.

Mass each is the volume of the part alone times the density of its material. If the material has no known density, the mass is left blank and a note says so. Save CSV writes bom.csv with the columns No.,Part,Qty,Material,Mass each (g),Mass total (g); its rows end with CR LF, and a text that starts with =, +, - or @ is written so that a spreadsheet shows it as text and never runs it as a formula. Copy text puts the same table on the clipboard as aligned plain text, ready to paste into an e-mail, and Save text writes it as bom.txt.

Exploded view

Choose Exploded view to spread the components apart for viewing. It is display only: measuring, mass, section and export use the assembled positions.

ControlWhat it does
SpreadHow far components move from the middle of the assembly.
DirectionAway from the middle, or along the X, Y or Z axis only.
Move a component along an axisPick a component, an axis and an offset in millimetres to adjust one component by hand.
ResetClears the spread, direction and manual offsets.

The arrangement is saved with the file. Hidden components are not part of it.

Interference check

Choose Interference check and press Check. The result lists pairs of components that share volume, with the shared volume. A pair the kernel could not compute shows its error code. A click on a pair selects its faces and frames them. The result goes out of date when the assembly changes (“Out of date: the assembly changed.”); press Check again. The Inspect drawer has the same check for the bodies of any part, see Measure and inspect.

Samples

Three sample assemblies are in the Library picker (titles starting “Assembly:”): a bolt in a block (coincident and concentric mates), a gear train (two gears on shafts with a gear mate of ratio 2; set a Drive on the gear mate to turn them) and a hinged door (a hinge with a stop and a limits mate of 0 to 110 degrees).

Not available

  • Replacing a part, or adding a new component inside the assembly; insert a part and mate it instead.
  • Dragging a component in the viewport in the exploded view; use the offset fields.
  • Mates on edges (faces only).
  • The five pending mate kinds above.

Next

Materials and appearance

This chapter covers how a part is made of a material, how it is coloured and finished on screen, the display styles and the Display menu, lighting and background, hiding things, and the Bodies list where each body gets its own colour, opacity and finish.

Two things are easy to confuse, so here is the rule up front:

  • The material is part of the file. It sets the density used for mass, and it sets the colour and finish of the part unless you override them.
  • A colour or finish you pick in the Display menu is a viewing choice kept in your browser, not in the part file. Colours set in the Bodies list are saved with the part.

The material

The first row of the feature tree reads “Material: steel” (or whatever the part uses), with a colour chip. Click it, press Enter or F2 on it, or use the pencil that shows when you point at it. The Material editor opens in the left panel, with OK and Cancel. Enter applies and Escape cancels.

  1. Type in the search box, or scroll the list. Materials are grouped as Steel, Aluminium, Copper alloys, Titanium, Cast iron, Plastics, Wood, Rubber, Glass, Concrete and Custom. Search matches a word of the name, the category, the standard, the grade or the region code (s355, a992, en 10025, au). Inside Steel the general steels come first, then the grades of the standards, grouped by region and standard.
  2. Click a material. The editor shows a swatch, its density, a default colour and, where usual, Young’s modulus, Poisson’s ratio and yield strength, and the mass of the current part at that density (“was …” shows the mass it has now). Steel grades from the standards also show ultimate strength, shear modulus, thermal expansion, the standard and grade, and the region, with a line saying whether the strengths were verified.
  3. Press OK to apply it.

The values are textbook figures that are good for estimating mass. They are not for certifying a design.

Woods and panels

The Wood category lists ten solid woods (birch, cedar, cherry, Douglas fir, eucalyptus, maple, oak, pine, teak and walnut) and seven panels (MDF, chipboard P5, OSB/3, and birch, eucalyptus, pine and spruce plywood). Each solid wood has its density at about 12% moisture and its stiffness along the grain from a named source (the species and a link are in the material’s note), and its own colour. A part with a solid wood material shows growth rings and fine streaks in a darker tone of that colour, running along the longest side of the part; the panels have no grain. The panels are marked unverified: their figures are typical manufacturer values until each is checked against its product standard.

Surface controls

The Display menu’s appearance section has a Surface group under the material list. Roughness, Metalness and Clear coat change how the part catches the light: a rough surface spreads the reflection, a metallic one tints it with the part’s colour, and a clear coat adds a thin glossy layer on top (a varnished wood, a painted panel). Each slider starts at what the chosen material gives, and a value you change is kept for the part, so choosing another material later does not undo it.

Tick Wood grain to draw growth rings on any part (a solid wood material has it already). Ring spacing is the distance between rings in millimetres, Grain contrast how dark they are (0 gives a plain surface), Grain colour the colour of the dark rings, and Grain direction the axis the grain runs along (by default the longest side of the part). Untick it to turn the grain off, even for a wood. Reset surface removes all of these changes. The settings are kept on this device, with the part’s colour and material, and are not saved in the part file.

Textures from Poly Haven

Under the Surface group, Choose a texture… opens a list of wood textures from the Poly Haven library (search by name; the thumbnail shows the look). Pick one and the part is drawn with it: the colour image and, when the texture has them, its roughness image and its normal map, projected onto the part from the three axes, so it works on any shape without texture coordinates. Texture size sets how large one tile of the image is in millimetres (it starts at the real size of the sheet the texture was photographed from), and Texture relief sets how strongly the texture’s normal map (its fine bumps and grooves, shown by the light) is drawn, from 0 (flat) to 1 (strong, the middle is the texture as photographed). Remove texture goes back to the colour and the grain. The author is credited under the texture. Poly Haven textures are public domain (CC0), so they may be used in any work.

Textures come from the internet, so they depend on Settings > General > Use online libraries, which is off until you turn it on (or press Allow online libraries in the list). With it off the app contacts nothing; with it on it contacts api.polyhaven.com, dl.polyhaven.org and cdn.polyhaven.com and sends only which texture you are looking at, never your part. Each downloaded texture (about 1.5 MB at 1K) is kept in the browser, up to 120 MB with the oldest removed first, so a part that uses it still shows it offline; Clear downloaded textures in the same Settings section empties the cache. A part opened on a computer that has not downloaded its texture shows its plain colour until online libraries are on. The texture choice is kept on this device with the part’s other appearance settings, not in the part file.

Steel grades from the standards

The Steel category holds fifteen grades from standards, with fy (yield), fu (ultimate), E, G, Poisson’s ratio, density and, where known, thermal expansion:

RegionGrades
EuropeEN 10025-2 S235, S275, S355; EN 10210 S355J2H (hot-finished); EN 10219 S355J2H (cold-formed)
United StatesASTM A36, A992, A572 Gr 50, A53 Gr B, A500 Gr B and Gr C (round and shaped each)
AustraliaAS/NZS 3679.1 grade 300 and 350

Strengths are minimum values in MPa (US figures are the ksi values converted: 36 ksi is 250 MPa). For thickness-dependent grades the figure is the thinnest band (S355: 355 MPa up to 16 mm); the note under the values says how it falls with thickness. The Australian yields (280 and 330 MPa) are conservative lower bounds, not a per-thickness table: the mill catalogue shows 280 to 320 MPa for 300PLUS and 340 to 360 MPa for grade 350 depending on flange or web thickness, so design yield depends on thickness.

A grade wears an unverified badge when a value rests on one secondary source or the editions of the standard disagree: ASTM A53 Gr B, ASTM A500 Gr C round and the two Australian grades. For A500 Gr C round the older editions give 46 ksi (315 MPa), which is the stored yield; the 2021 revision is reported to give 50 ksi (345 MPa) for all shapes, which the editor shows as “Yield strength, other edition”. Check the current edition of the standard before relying on either. US elastic constants (E 200 GPa, G 77.2 GPa) are the AISC 360 values and US thermal expansion is not given. Sources are listed in Frame stock data and sources.

Files that name a material by name keep working: “Mild steel”, “steel” and the other general entries are unchanged, and the new grades are looked up by their names (for example ASTM A992, EN 10025-2 S355) or ids.

Custom material… takes a name, a density and a colour. Custom materials are stored in your browser and listed under Custom with a remove button. A custom name cannot be the same as a built-in one. A file that names a custom material keeps the name when you open it on another computer, but there the material is unknown: Mass properties then asks for a density.

Use material colour (on by default) lets the material colour the part. Turn it off and bodies take the default colour.

Changing the material is one undo step. It does not appear as a row in the History log, but Ctrl+Z undoes it in order with your other edits. The material is saved in the file, so Save and autosave pick it up.

What the material changes on screen

The part is drawn in the colour and finish of its material: steel as a light cool grey with a satin metal look, brass warm and metallic, plastics glossy, rubber and gasket material matte, glass translucent. A colour you pick in Display > Appearance wins over the material colour. Choosing the default grey does not count as an override.

In an assembly each component carries its own material, so each is drawn in its own colour and finish. To override one component, select a face of it, then open the Display menu: the Appearance heading names the component (“Appearance of <name>”), and the change applies to that component only.

The Display menu

The Display button sits on the viewport. It holds, from the top:

SectionControls
StyleDisplay style (see below). For Ghost, an Opacity slider from 5 to 100 percent.
AppearanceEight colour swatches and a Material finish list: Default, Plastic, Brushed metal, Glass, Matte.
SceneFour lighting presets, a Light strength slider (0.3 to 2), a Reflections switch, Edge width (Thin, Medium, Bold), a Silhouette outline switch and the Background list (Theme, Light, Dark, Gradient).
AnalysisSurface analysis modes (zebra stripes, curvature, draft).
ShowSwitches for Edges, Sketches, Curves, Planes, Axes, Grid, Relations, Overall size, Threads and Design issues. While a sketch is open the sketch’s own show switches appear here too.

A Show all button appears when something is hidden. Layers you switch off in Show are only hidden from view; the model is not changed.

The View ribbon tab has the same style, lighting and background choices as commands, so they can be reached from the command search too.

Display styles

StyleShortcutWhat you see
ShadedAlt+1Lit faces, no edge lines.
Shaded with edgesAlt+2Lit faces and edge lines (default). The Edges layer controls the lines.
WireframeAlt+3Edge lines only; hidden edges are drawn faint. You can still pick faces.
Hidden lines removedAlt+4Flat white faces with black edges.
GhostAlt+5Translucent faces; set how transparent with the Opacity slider.

Picking and hover highlights work in every style. While you edit a sketch, the body is faded to a quarter of its opacity and comes back when the sketch closes.

Lighting and background

PresetLook
Studio (default)Soft highlights and reflections on metal. The highlights stay fixed to the screen as you turn the part.
FlatEven light, no reflections.
High contrastOne strong light, little fill.
TechnicalEvery face matte white with black edges and soft light, close to a drawing. Per-component colours are not shown.

Light strength scales every light. With Reflections off, metals lose their metal look, and the Flat and Technical presets never have it. The default background is the gradient, which follows the light or dark theme.

Under the presets, Choose an environment… replaces the built-in studio light with a real-world light environment (an HDRI) from the Poly Haven library, so metal and varnish reflect a room, a street or a sky instead of the studio softboxes. The list has thumbnails and a search, and Studio (built in) goes back to the default. Only the reflections and the image based light change, not the background. An environment has the same rules as a texture: it needs Settings > General > Use online libraries (off until you turn it on), only the 1K version (about 1.5 MB) is downloaded, it is kept in the same browser cache with the same 120 MB limit, and the author is credited under the choice. The Flat preset and the Reflections switch still turn the reflections off. The choice is kept on this device with the other display settings.

Edges and silhouette

Edge lines are drawn at a fixed pixel width (Thin by default) in a colour darker than the faces. The Silhouette outline (on by default) also outlines the rim of curved faces where no edge line lies. It is switched off in a section view, in Wireframe and Ghost, and for translucent bodies.

Hide and show

Press H to hide the body of the selected faces, or the selected sketch, plane or curve. Press Alt+H, or the Show all button, to show everything again. A hidden body cannot be picked. Hiding is for the session only and is not saved.

The eye on a row in the feature tree hides exactly what that feature made, in the view only. The row dims and shows a closed eye; click it again to restore. Nothing is rebuilt. Suppress is a separate button on the row and does rebuild the model.

The Bodies list

A part can hold several bodies. The Bodies tab of the left panel lists them, one row per body, ordered by the feature that made it. Each row shows an eye, a colour swatch, the name and the volume.

ControlWhat it does
Eye (or Space on a focused row)Hides or shows the body.
Row clickSelects the body. Shift or Ctrl adds to the selection. Clicking a face in the model selects its body row.
Double-click or F2Renames the body.
Isolate buttonHides every other body. Press it again to show all.
Show all / Hide othersShow everything, or keep only the selected bodies.
Copy, Delete, Join, Cut, IntersectEdit the bodies themselves. See Bodies and combining.

Below the list, the selected body has an Appearance group:

ControlWhat it does
ColourThe body’s colour.
Opacity5 to 100 percent. A body below 100 percent is drawn in a separate transparent pass.
FinishPart material (no override), Matte, Plastic, Chrome, Glass or Brushed metal.
Metallic, RoughnessFine control over the finish.
Clear coat0 to 100 percent: a thin glossy layer on top of this body only (a varnished or painted body next to a bare one).
Choose a texture…A Poly Haven texture on this body only, with its size, relief and the author’s credit, the same as the part’s texture under Textures from Poly Haven. It needs Use online libraries like any other texture.
Glass, Chrome, ResetPresets, and a button that removes the override (the clear coat and the texture too).

A body with a texture or a clear coat is drawn on its own, so a texture shows only on a body that is not see-through (a body below 100 percent opacity keeps its plain colour), and while a section view or a surface analysis (zebra, curvature, draft) is on, such a body is drawn with the colour and finish only. Textures and clear coats are set per body, not per face. Appearance set here is saved with the part and is not an undo step. Very clear bodies (below about a third opaque) are skipped by a click when something lies behind them, so you can pick what you see through the glass.

Limits

  • Appearance changes, hiding and the Display menu are not undo steps.
  • Per-face colours cannot be set in the Bodies list; scripts can set them (see Scripting).
  • Colour and finish are not written to STEP, STL or DXF exports. See Exporting.
  • A section view cuts opaque bodies only. Translucent bodies are not cut, and two translucent bodies that overlap are blended by the distance of their centres.
  • Zebra and curvature analysis colour opaque bodies only.
  • There are no cast shadows, ambient occlusion or textures.
  • Each browser keeps its own Display choices and custom materials.

Next

Saving and opening

This chapter covers making, opening and saving parts, the recent list, what happens to unsaved work, automatic backups, several parts open at once in tabs, compressed files, and keeping the built geometry inside a file.

A part is saved as a .ckpart file. It is plain text (JSON) that holds the recipe of the part, its feature history, so it stays small and opens in any version that understands the format. See File formats at a glance for what is inside.

The file controls

New, Open, Save, Export and Library are buttons at the left of the top bar. The rest of the file actions are in the More file actions menu next to Export.

ActionWhereShortcut
New partTop bar, first buttonCtrl+N (Cmd+N on a Mac)
OpenTop barCtrl+O
SaveTop barCtrl+S
Save asMore file actionsCtrl+Shift+S
Save geometry in fileMore file actions (a toggle)
Recover earlier versions…More file actions
Import STEP / STL / OBJ / GLB / 3MF / SolidWorks / SketchUpMore file actions
ExportTop barCtrl+E
LibraryTop bar

Some browsers reserve Ctrl+N and Ctrl+O for themselves; the buttons always work. The same actions are in the command search (press F). The name of the open part is shown in the top bar. Double-click it to rename the part. A dot after the name means there are changes since the last save.

New

New part opens a blank part named Part1, Part2 and so on. If the current tab is still blank, the new part uses it; otherwise it opens in a new tab and the part you were working on stays open in its own tab.

Open

Open shows the browser’s file picker. It accepts parts (.ckpart, .json, and compressed .gz parts), STEP (.step, .stp), SolidWorks (.sldprt), SketchUp (.skp), DXF (.dxf), SVG (.svg), FreeCAD (.FCStd) and SolidCraft (.solidcraft) files. The app decides by the extension. What each foreign format becomes is described in Importing.

You can also drag one file onto the window; a dashed overlay shows while you drag. Dropping more than one file at a time is refused (“Drop one file at a time.”). A DXF or an SVG opens into the sketch you are editing, or as a new sketch on the front plane. STL files cannot be imported.

Files saved by earlier versions of the app still open, and are written in the current format the next time you save.

Save and Save as

Save writes the part to the file it came from.

  • In browsers that can overwrite files (Chromium-based ones), the first Save asks where to put the file and later Saves overwrite that same file.
  • In other browsers Save downloads a file named after the part each time. Your browser decides where it goes.

Save as asks for a new file. In a browser with a file picker you get the picker. Otherwise a small dialog asks for the name; .ckpart is added for you and the dialog shows the name it will write. The dialog also has two boxes:

OptionWhat it does
Compress (.gz, about 10 times smaller)Writes name.ckpart.gz. See below. Shown only in the dialog (browsers without a file picker).
Keep the built geometry in the fileStores the finished model in the file so it opens at once. See below.

The name you give becomes the part name shown in the top bar, saved in the file and used by autosave. Cancelling a picker does nothing. A notice “Saved <file>” confirms a save, and a failure says why.

A saved file also holds a small preview picture of the part (used by the recent list) and the sheets of a drawing, exploded view and appearance of bodies if you made them. Display choices from the Display menu are not saved in the file.

Unsaved changes

The app asks before it throws changes away.

  • Closing a tab that has changes brings it up and asks Save, Don’t save or Cancel. Save only goes on once the save really happened.
  • Reloading or closing the browser window while any tab has changes shows the browser’s own “leave this page?” prompt.
  • Opening something does not discard the current part. It opens in a new tab (or in the current one when that is blank).

Autosave and restore

While a part has unsaved changes, the app copies it into your browser’s storage a moment after your last edit, and when you switch away from the page. If the page crashes or is closed, the next start offers Restore your last session? with three buttons:

  • Restore brings back each changed part in a tab of its own, marked as changed. The tab that was active is shown again.
  • Start new forgets the stored session.
  • Earlier versions… opens the list described below.

The dialog does not close on Escape, so a stray key cannot discard it. Save, Open, Library and New clear the stored session.

Imported meshes and STEP data are stored compressed (see Imported meshes and STEP data in the file), so a part with a scan still fits. Limits: autosave skips a part whose text is over about 3 MB, and a notice tells you to save to a file. When only the packed meshes are too big for the browser’s storage (about 2 MB of them), the backup leaves the meshes out, says so once, and keeps the rest; the STEP data of an imported solid is always kept. It also warns if the browser has no room or has autosave switched off. Undo history is not stored: a restored part starts with a clean history. Component tabs (see Assemblies and mates) are not stored.

Recover earlier versions

The app also keeps a rolling set of snapshots of the open part in the browser (the last ten, taken about every 30 seconds while you work, before each undo, before a large drop and before another part replaces this one). Choose Recover earlier versions… in More file actions, find the snapshot by time and feature count, and press Restore. The richest snapshot from the last day is always kept. Snapshots live only in this browser.

Recent files and samples

Library opens a searchable list of parts (the sample parts and the libraries you added) with a Recent section above it: the last eight samples and files you opened or saved, with their age and a preview.

When you save a part, a small picture of it (a PNG of about 20 KB or less) is written into the file as an optional thumbnail field, together with a hash of the part. That picture is what the Recent card shows. If the part has changed since, the next save draws it again; a picture that does not match the part is never shown. If the picture cannot be drawn (no solid, or it takes too long), the file is saved without one. A file with a damaged thumbnail field still opens normally.

Clicking a sample opens it as a new part. Clicking a recent file reopens it if the browser still has permission for it. That works for files that you saved through the picker. A file that you opened with the plain Open dialog is listed but the browser kept no access to it, and a notice asks you to use Open again. If the permission is refused or the file is gone, the notice says so.

Several parts in tabs

Parts open in tabs under the top bar. Each tab keeps its own history, selection, file, camera and unsaved-changes mark. The other tabs keep running quietly.

DoHow
New part in a new tabThe + button on the tab strip, or Ctrl+Alt+T
Switch tabsClick, or Ctrl+Tab / Ctrl+Shift+Tab
Jump to a tabCtrl+Alt+1 to 9 (9 is the last tab)
Close a tabThe cross on the tab, middle click, or Ctrl+Alt+W
ReorderDrag a tab
See all open partsThe down arrow at the end of the strip (also shown when there are more than seven)

Ctrl+Tab and Ctrl+W are reserved by browsers; in the installed app (see Install as an app and work offline) Ctrl+Tab works, and the Ctrl+Alt keys work everywhere. On a Mac use the Control key for these tab shortcuts.

You can have 32 tabs. Switching away from a sketch in progress finishes the sketch and keeps it; if it cannot be finished, it stays open and a notice says so. An open feature editor is closed when you switch. Closing the last tab leaves a blank part. The Drawing view closes when you switch tabs.

Imported meshes and STEP data in the file

A reference mesh (an STL or SketchUp import) and the STEP text of an imported solid are the heavy parts of a file, so they are stored packed:

  • Meshes are stored as one compressed block each: the vertices on a grid of at most one micron (finer for small models), written as differences between neighbours, the triangle corners as small numbers, the SketchUp colours as runs, then deflated. A 500,000 triangle scan is about 1.2 MB in the file, against about 12 MB for the raw numbers and about 24 MB for the same data as a JSON list of numbers. The rounding to a micron is the only loss: it is far below what a scan or a sketch resolves, and saving a mesh again does not move it further. A model with a value that cannot be put on a grid (not a number, or enormous) is stored exactly instead.
  • STEP text is stored deflated, about eight times smaller than the text.
  • Files written by earlier versions (meshes as plain base64, STEP text as plain text) open as they are and are packed the next time you save. A file saved by this version and opened in an older one loses its meshes and cannot rebuild the imported solid; nothing else is affected.
  • A mesh that is damaged or cut off in the file is left out with a notice naming it; the rest of the part opens. A damaged STEP block leaves the imported-solid feature with an error that says its data is missing.
  • Compression and decompression run in the browser’s own streams, and the rest in slices of a few milliseconds, so a large part does not freeze the page. The picking tree of a big mesh is built in slices too.

Compressed parts

A part is plain JSON and repeats itself a lot, so a file ending in .gz (for example bracket.ckpart.gz) is written compressed, roughly ten times smaller. Which control compresses depends on how the file is saved. In browsers without a file picker, Save as shows its own dialog: tick Compress there (a .gz you type in the name is stripped and the box decides). In browsers with a file picker (Chromium-based ones), Save as shows the browser’s picker instead and there is no Compress box; name the file with a .gz ending (or choose the compressed type in the picker) and the app compresses by the name the file ended up with. Plain downloads also compress when the name ends in .gz.

Programs that read .ckpart as text (scripts, other tools) need the file decompressed first.

Save the built geometry in the file

A large part takes a while to rebuild, and the app caches the finished view in the browser so the second open is instant. A file opened on another computer, or after the cache is cleared, would still rebuild. More file actions > Save geometry in file makes the file carry the finished view, so it shows the model and the tree about a second after you open it. The model still rebuilds behind it and replaces the view.

  • It is a cache, never an input. If you edit the file elsewhere, or open it in a different build of the app, the stored view is ignored and the part rebuilds normally. Deleting the field is always safe.
  • If the file carries a stored view that cannot be used, the app shows a short notice and rebuilds. The notice says which of four things happened: the part was edited after the view was stored, the view is from a different kernel build, the view has a format this version does not know, or it could not be read. A file with no stored view gives no notice.
  • Files written by an AI agent through the MCP export tool with cache: true carry the same stored view.
  • It makes files bigger. As a guide, a part with about 185,000 triangles adds about 3.4 MB of text to a recipe of about 2 MB. Combined with .gz it is smaller than without compression, but it does not compress as well as the recipe.
  • It is off by default. The choice is remembered, and a file that was opened with its view keeps it when saved.
  • Autosave never writes the view.

Next

File formats at a glance

This chapter lists every file type the app reads and writes, what each carries and what is lost, and then describes the part file itself.

What the app opens

All lengths are millimetres inside the app. Formats that carry other units are converted on the way in.

FormatExtensionHow to openYou getWhat is lost
CivilKit CAD part.ckpart, .json, .ckpart.gzOpen, dropThe full editable partNothing
STEP.step, .stpOpen, drop, More file actionsA part feature saved with the part (or a view-only solid, your choice in the import box)The history; colours, names, assembly structure
SolidWorks part.sldprtOpen, drop, More file actionsAn editable imported body (view-only if it cannot be built)The feature tree, sketches, configurations, annotations
SketchUp.skpOpen, drop, More file actionsA reference mesh saved with the part, with its colours (or a view-only surface model, your choice in the import box)Scenes, text, dimensions, curves as true arcs
STL.stlOpen, drop, More file actionsA reference mesh saved with the partColours, textures
OBJ.objOpen, drop (with its .mtl for colours), More file actionsA reference mesh saved with the part, with colours when the .mtl comes with itNormals, textures, smoothing groups, lines; objects are joined into one mesh
glTF binary.glbOpen, drop, More file actionsA reference mesh saved with the part, with its colours (metres and Y up converted)Textures, animation, vertex colours; compressed or multi-file glTF is refused
3MF.3mfOpen, drop, More file actionsA reference mesh saved with the part, with its colours and unitTextures, colour gradients, print supports; build items are joined into one mesh
FreeCAD.FCStdOpen, dropAn editable part for the features that mapFeatures that do not map; the rest of the document
SolidCraft.solidcraftOpen, dropAn editable part for the features that mapFeatures that do not map are kept as suppressed placeholders
DXF.dxfHome > Sketch group, or dropSketch geometry (lines, arcs, circles, splines, points)Text, hatches, dimensions, blocks, 3D entities
SVG.svgHome > Sketch group, or dropSketch geometry (paths, rectangles, circles, ellipses, lines, polygons)Text, images, fills, strokes, gradients, clip paths

DWG cannot be imported yet. “View only” means you can look at the body and turn the model, but it is not a feature, it is not saved with the part and the next edit replaces it. Importing has the details and limits of each.

What the app writes

FormatExtensionWhereCarriesWhat is lost
CivilKit CAD part.ckpart, .ckpart.gzSave, Save asThe recipe and the app’s own dataNothing
STEP.stepExportThe exact solidColours, history
STL (binary or ASCII).stlExportA triangle meshThe exact surfaces, colours, history
OBJ.objExportA triangle mesh, one object per bodyThe exact surfaces, history
3MF.3mfExportA triangle mesh for 3D printing, one object per body, with body coloursThe exact surfaces, history
glTF binary.glbExportA triangle mesh for viewers and the web, one node per bodyThe exact surfaces, history
DXF, sketch.dxfExportOne sketch as R12 2D geometryConstraints, dimensions
DXF, three views.dxfExportFront, top and right views of the edgesHidden lines, dimensions
Drawing.pdf, .svg, .dxfDrawing viewThe sheet as drawnThe link to the part
Bill of materials.csvAssembly > Bill of materialsThe tableNothing

Exporting describes each one and its options.

The part file

A part file is one JSON document in a text file, and is what Save writes. You can open it in any text editor, keep it in version control and diff it. Its main parts are:

FieldMeaning
format and versionTell the reader what it is looking at. The format string is ck-part.
nameThe part name shown in the top bar.
featuresThe ordered list of features: sketches, planes, extrudes, fillets and so on, with all their settings. The kernel replays them from first to last to build the model.
variablesThe equations and variables of the part.
materialThe name of the material, such as “Aluminium 6061”. Density and colour are looked up by name.

The file does not store the model’s faces. It stores how to rebuild them, which is why parametric edits work after you reopen a file, and why a file of a few kilobytes can describe a detailed part. For the complete field list, the feature types and how references to faces stay stable, see the kernel book chapter Overview of the part format.

Other data the app keeps in the same file when you use it:

  • A preview picture (a small PNG of the part in the isometric view), used for the recent list. It is refreshed when you save and is never read as part of the model.
  • The stored view if you chose Save geometry in file (see Saving and opening). It is a cache; removing it is always safe. The MCP export tool can also write it (cache: true), and the app tells you when it ignores one that does not match the file or this build.
  • Drawings, the exploded view of an assembly, the colours, opacity and finish of bodies and body names, an embedded script and the fonts used by text.
  • Configurations and variables that you defined.

Fields that the app does not know are left alone and written back, so a file edited elsewhere does not lose data.

Files from earlier versions

Files saved by earlier versions of the app still open. They are converted to the current format when read, and the next save writes the current format. A file that was made by a newer version still opens, with a notice that some features may be missing or wrong. See Versions and earlier files in the kernel book.

Compressed and plain

.ckpart.gz is the same file compressed with gzip. The app reads it without any extra step. A program that wants the text must decompress it first.

Units

A part has no unit setting. Everything is millimetres, in the file and in the interface, and this is also what Measure, Mass properties and the exports use.

Where the model comes from

The kernel does the geometry. Its own book covers the part format, the checks that decide whether a model is valid, and the import and export readers at a deeper level than this guide: start at the kernel book, and see Validation for what makes a solid valid.

Next

Importing

This chapter covers every kind of file the app can import: STEP, STL, OBJ, GLB and 3MF meshes, SolidWorks, SketchUp, FreeCAD, SolidCraft, DXF and SVG, plus how parts from samples and the library come in. For each, you will find how to import it, what you get, what is converted, how units and colours are treated, the import report and repair, and what to do when an import is slow or fails.

There are two very different results, so check which one you have before you plan to edit:

ResultFormatsWhat you can do
Editable featuresFreeCAD, SolidCraft, DXF and SVG (into a sketch), CivilKit CAD partsEdit the feature tree, change dimensions, add features. Saved with the part.
Imported solid featureSTEP (the default choice)The solid is the first feature of a new part: later features can cut, drill, fillet, mate and sketch on its faces. The STEP text is saved inside the part and the part rebuilds when it is opened.
Editable imported bodySolidWorksThe solid arrives as one imported body that later features can cut, drill, fillet and measure. It is saved with the part. When the kernel can rebuild the file’s feature history (sketches, extrudes, fillets and so on), the part opens with that history instead and you can edit it.
Reference meshSTL, OBJ, GLB, 3MF, SketchUp (the default choice)A mesh to look at and draw on: it is saved with the part, can be moved, turned, scaled and made see-through, and the 3D Sketch tool snaps onto its surface. A SketchUp, GLB or 3MF mesh keeps its colours and translucent materials, and an OBJ does when its material file comes with it. It is not a solid and not part of the feature history.
View-only bodySTEP and SketchUp when you choose “View only”Look at it, orbit and zoom. The body is not a feature, it is not saved with the part, and the next edit replaces the display.

STEP and SketchUp files ask which of the two you want in a small box (the choice is remembered per kind; the first option is the default). A view-only import opens as a new, empty part named after the file. The notice says so (“Imported bodies are view only and are not saved with the part.”). In the code, each Export entry is enabled only when the controller holds a built mesh from the part’s features, and an import only draws the body in the viewport without storing it there. So the Export entries should stay greyed out for a part that holds only an imported body. This follows from reading the code; it has not been checked in a running app.

How to import

  1. Choose Open in the top bar and pick the file, or drag the file onto the window. The app decides by the extension.
  2. Or open the More file actions menu and choose Import STEP / STL / OBJ / GLB / 3MF / SolidWorks / SketchUp, which only offers those kinds.

An import never replaces the part you are working on: it opens in a new tab, or in the current tab when that is still blank. A long import shows a progress overlay; for a slow one you can press its cancel button.

STEP

STEP (.step, .stp) is the best way to bring a solid from another CAD program.

  • You get, with the default choice Part feature, a new part named after the file whose first feature is the solid (an Imported STEP body row in the tree). The notice gives the face count. The STEP text is stored inside the part, compressed, so Save keeps it, the part rebuilds when you open the file, and the solid can be used in booleans, mates and sketches on its faces. If the part cannot be built from the text, the solid is shown view only and the notice says why. Choose View only in the box for the old behaviour: a body to look at that is not saved.
  • Units are read from the file and converted to millimetres, so an inch file arrives at the right size.
  • Converted: solids, faces with holes, planes, cylinders, cones, spheres, tori, spline and swept surfaces, and the curves bounding them. All solids in the file arrive in one body, at their own coordinates.
  • Repair: after reading, the importer closes small gaps and sews edges that do not quite meet, with a tolerance of 0.0001 mm.
  • Colours and names are ignored, and assembly structure is not read: parts placed by transforms in an assembly file are not positioned.
  • Limits: a file with only surfaces or open shells and no solid is refused (“noSolid”). Unusual entities are refused with a message that names the code (parse, noSolid, unsupported, badEntity, topology).

If STEP refuses a file, try exporting it again from the source program, choosing a solid (not surface) output, a standard application protocol and millimetres. The kernel book has the full list of what is read: STEP.

Recognise features (beta)

A STEP file is a plain solid: it has no history. Recognise features (beta) looks for the features a person would have modelled (holes, pockets, fillets, plates, a turned body on a plate) and rebuilds them as a new part with a real feature tree. After a STEP import a notice offers it; the same command is in the command search (Recognise features (beta)) for as long as that file is the one you imported last in this session.

  • Your imported part is not changed, and you can compare. The result opens as a new part, named name (features), next to the imported one. It holds two things: every recognised step in one From STEP folder, and the imported solid as Original (STEP) after it, a separate body that starts switched off. Switch its eye on to see the file’s solid beside the rebuild; switch the folder off to see only the file’s solid. Switch Original (STEP) off again before you add holes or cuts: two solids lying exactly on each other cannot both be cut, and the feature fails with the combine failed. (If you want it on while you edit, drag it to the end of the feature list.) Features you add are built on the rebuilt body, so they stop working when the folder is switched off.
  • Is it the same solid? Before it offers the new part, CadKit rebuilds it and compares the volume with the imported solid. Within 0.5 % it says the rebuild is the same solid, and within 2 % that it is close, and to check it; both can be opened as a new part. Beyond that it says how far off it is (it is 2.4 times the imported volume, or its volume is 40% smaller) and does not offer it as a new part, because most of the part is then wrong or missing. A rebuild that is not a valid solid is not offered either. Copy script is always available, so you can read or edit what was recognised. The dialog also lists what it left out, grouped (for example Plates: 4 not rebuilt yet).
  • What it does well today: a plain block with holes, pockets and corner fillets; a part whose outline is one profile extruded (a bracket); and a plate with a turned body on it, standing on the Y axis. What it does not: assemblies of many plates, sheet-metal frames and free-form shapes. Those come out as a starting point at best, and the dialog lists every recognised feature it did not rebuild, with the reason. Counterbores and countersinks are rebuilt as plain holes.
  • The recogniser is a separate download. The first time you use it the browser fetches it (about 2 MB compressed) and keeps it; nothing is downloaded until you ask. It runs on your computer: the STEP file is not sent anywhere. Recognition is by quiddity (Apache-2.0); the licence is on the Licences page.

Mesh files: STL, OBJ, GLB and 3MF (a model to sketch on)

STL (.stl, binary or text), OBJ (.obj), binary glTF (.glb) and 3MF (.3mf) are meshes of triangles, typically a 3D scan or a model from a mesh tool. CivilKit CAD keeps each as a reference mesh: you can look at it and draw on it, but it does not become a solid. The four go the same way; what differs is what each file carries (see the table below the steps).

  1. Drop the file on the window, or use Open or Import. Unlike the other formats, a mesh is added to the part you have open (it does not open a new tab), so it needs a part to be open. To bring an OBJ in with its colours, drop the .obj and its .mtl together.
  2. A dialog shows what the file holds: triangles, vertices, size, and whether the surface is closed. STL and OBJ files have no units, so pick the one the file was made in (millimetres, centimetres, metres or inches). A GLB (always metres) and a 3MF (it states its unit) are converted to millimetres for you and the dialog says so instead of asking. The size line updates as you choose, and a hint appears when the size looks wrong (a model under 2 mm across is usually a file in metres). Tick Move to the origin and sit on the ground to place it at the origin; otherwise it keeps the file’s own coordinates.
  3. The mesh appears shaded, the view frames it, and a row for it appears in the feature tree with an eye (show or hide) and a pencil. A mesh of up to about a million triangles stays responsive.

The Mesh panel (click the row or its pencil): name, shown, opacity (lower it to see your sketch through the surface), colour, triangle edges, position, rotation and scale, quarter turns about X, Y or Z, Move to the origin, Sit on the ground, and Delete mesh. Changes show at once and are one undo step when you press Done; Cancel puts everything back. A scan is often Y up or Z up in its file: use the quarter turn buttons to stand it upright.

Two ways to draw on it

  • Sketch on mesh: click a point on the surface. Then choose the plane of the sketch through that point: Surface normal (square to the surface there), or one of Front, Top, Right (parallel to the base planes). The ordinary sketch editor opens on that plane with the mesh still visible.
  • 3D Sketch on mesh (or the 3D Sketch tool with a mesh in the part): clicks that land on the mesh snap to its surface, so a spline you click across the head lies on it. Points, ends and other sketch points still snap first. The tick Draw on the imported mesh surface turns this off. Fit curves resamples the lines, splines and control splines of the sketch into many points and puts each on the surface (To the nearest surface point, or Along the work plane normal), so the curve follows the surface between your clicks. The result is an ordinary 3D sketch feature.
FileReadNot kept (the dialog and a notice say which applied)
STLTriangles, binary or textColours, textures
OBJVertices and faces (negative indices, v/vt/vn forms, polygons cut into triangles), colours from the .mtl (Kd, d or Tr) when it is dropped with the file, and the x y z r g b vertex colours some tools writeNormals, textures, smoothing groups, lines, free-form curves. Several objects or groups are joined into one mesh. Without the .mtl there are no colours, and a notice says so
GLBThe scene’s meshes with every node’s transform, triangle lists (indexed or not), base colours and alpha of the materials. Metres and Y up become millimetres and Z upTextures, colours per vertex, normals, animation and skinning (the model is shown at rest), lines and points. A GLB with Draco or meshopt compression, or with its data in a separate file, is refused with a message
3MFObjects, components and build items with their transforms, the model unit (converted to millimetres), colours from base materials and colour groups, models split over several filesTextures, colour gradients inside a triangle, print supports, slicer settings. Several build items are joined into one mesh

A file that holds several objects comes in as one mesh (one row in the tree) with its colours kept; the parts cannot be moved apart afterwards. OBJ has no up direction: a model that lies on its back is stood upright with the quarter turn buttons in the Mesh panel.

What is stored. The mesh travels in the .ckpart as welded vertices and triangle indices, packed and compressed (about 1.2 MB for a 500,000 triangle scan; see Imported meshes and STEP data in the file), with the vertices rounded to a grid of at most one micron. The browser’s automatic backup keeps a mesh up to about 2 MB packed and otherwise leaves it out and says so, so save to a file. Save as to a new name, dragging the saved file back in, and inserting the part from a library all keep the mesh; exporting a folder’s geometry or extracting a folder does not (those are bodies and features, not meshes). A mesh that is damaged in a file is left out with a notice and the rest of the part opens. The mesh is not sent to the kernel, is not counted in mass or volume, and is not in STL, STEP or other exports.

Not done: converting a mesh to a solid, remeshing or simplifying, mesh booleans, repairing holes (the dialog only reports them), colours or textures from an STL file, textures from any mesh file, importing the parts of a multi-part file as separate meshes, and constraints to mesh points.

SolidWorks parts

SolidWorks part files (.sldprt) are read directly.

  • You get the part with its feature history (sketches, extrudes, cuts, fillets, chamfers, holes, shells, patterns and revolves) when the kernel can rebuild it, and you can edit those features. A feature it cannot read back ends the history there, and the rest of the part is the file’s exact solid as an imported body. A part it cannot rebuild at all opens as that solid alone. More parts now rebuild their full history than before, including chamfers along a chain of edges, drafts (also on parts with several drafted faces), fillets that end at a neighbouring feature or go round a closed curve, and bosses whose profile is closed by a straight chord. In one set of eleven NIST test parts, eight rebuilt completely; the others still end in an imported remainder, so check the feature tree after opening. A part with a loft opens in about a second. The solid of the active configuration arrives as an editable imported body in a new part named after the file: the first feature of the tree is the body (written to the part as STEP by the kernel, so it is saved with the part). The notice says “Opened <file> (SolidWorks): N faces, as an editable body.” The body has the volume and the box of the solid SolidWorks itself writes to STEP. If the part cannot be built from the solid (the check of its volume fails), the solid is shown view-only as before, with the notice “Imported <file> (SolidWorks): N faces. Imported bodies are view only and are not saved with the part.”
  • Converted: planar, cylindrical, conical, spherical and toroidal faces and spline surfaces. Some blend and intersection curves are approximated, and the import fails if an approximation is off by more than 0.05 mm.
  • History folder: a SolidWorks history opens inside one SolidWorks history folder in the feature tree, with an eye toggle. Off shows exactly the file’s body; on shows the rebuilt history. A partial history shows the rebuilt features followed by an Imported remainder row. Features you add after the Imported body step refer to the file’s face names, so they may not survive switching the folder back on.
  • Units: SolidWorks stores metres; the importer scales to millimetres.
  • Not read: equations, configurations other than the active one, annotations and flat patterns. Sheet-metal parts arrive as the folded solid. Files with only sheet or wire bodies are refused.
  • Limits: files with more than 50,000 faces are refused. The oldest tested file is from SolidWorks 2011 and the newest from 2022; newer files are untested.

If a file fails, save it as STEP from SolidWorks and import that instead. More detail: SolidWorks.

SketchUp

SketchUp files (.skp) are surface models made of flat faces, not solids.

The picture shows a SketchUp file imported with the default Reference mesh choice, with the chair and table test file from the OpenSKP project (MIT).

  • You get, with the default choice Reference mesh, a mesh added to the open part (like an STL, so a part must be open) with each face in its SketchUp colour and translucent materials kept translucent. Everything an STL mesh does works: Sketch on mesh, 3D Sketch on mesh with Fit curves, opacity, move, turn and scale, show or hide, delete, and it is saved with the part. Choose View only for the old behaviour (a new part showing a body that is not saved). Texture images are not imported either way.
  • Units: SketchUp stores inches and the importer converts to millimetres.
  • Orientation: SketchUp is Z up and the app is Y up, so the model opens upright. The notice has a Flip orientation button that cycles through three views: upright, as in the file (Z up, so the model lies on its side here), and upside down. Rotate imported model in More file actions does the same while a SketchUp model is shown. For a mesh this sets its rotation (one undo step; the Mesh panel shows it), for a view-only body it imports the file again.
  • Hidden geometry is left out by default, and the notice says how many hidden faces were skipped, with a Show hidden geometry button (for a mesh it replaces the mesh, keeping where you put it). The box has an Include hidden geometry tick, and Import SketchUp with hidden geometry in More file actions opens it ticked.
  • Open surfaces: if the model is not closed, the notice warns (“SketchUp surface model: N open edges; solids operations may not apply”). A closed model has volume; an open one does not.
  • Not imported: scenes, cameras, text, dimensions, construction lines, true arcs (curves become many short flat faces), and styles other than face colours.
  • Limits: as a mesh there is no practical face limit (the limit is 5,000,000 faces and the mesh is stored compactly); as a view-only body, models over 50,000 faces are refused (“limit.faces”). A file with no faces, or with everything hidden, is refused (“body.empty”). Reading a very large file is the kernel’s work and takes seconds (a 39,000 face model took about 8 seconds on a busy machine); building and drawing the mesh afterwards is quick.

FreeCAD

A FreeCAD file (.FCStd) becomes an editable part.

  • You get a new part with the features that could be mapped. The notice says how many of the total mapped and shows the first warning, and counts the rest.
  • Which body: only one PartDesign body is imported, the one with the most features. A notice says if there were more.
  • Converted:
FreeCADBecomes
Sketches: lines, circles, arcs, ellipses, points, construction geometrySketch geometry. Points that meet are merged.
Coincident, horizontal, vertical, parallel, perpendicular, tangent, equal, radius, diameter, distance constraintsThe same constraints
Pad, Pocket (blind, symmetric, two lengths, through all, reversed)Extrude, add or cut
Revolution, Groove (about a sketch axis, a construction line or an origin axis)Revolve
Mirrored (about an origin plane)Mirror
LinearPattern, PolarPatternLinear and circular patterns
  • Not converted: point-on-object, symmetric, angle and block constraints and splines (counted in a warning; the shape is right but dragging it will not behave as it did in FreeCAD); tapered or custom-direction pads; “up to face/first/last” end conditions; Thickness, Draft, Hole, Boolean, Loft, Pipe, Helix, MultiTransform and clones; sketches on planes that are not parallel to a standard plane. Fillets and chamfers are left out in this version, and each is listed. Parameter expressions and spreadsheet links are dropped; the numbers they had are kept.
  • Units are millimetres, as in FreeCAD.
  • Colours are not imported.
  • Files with no PartDesign body (built in the Part workbench, or only imported shapes) import nothing and the notice says why. Export STEP from FreeCAD and import that instead.

SolidCraft

A SolidCraft file (.solidcraft) becomes an editable part.

  • You get a new, unsaved part named after the file, with one feature for each feature that could be converted. A progress overlay shows “Importing <file>: feature N of M” and has a cancel button, because a large file can take minutes.
  • Orientation: SolidCraft is Z up and the app is Y up. The importer turns the model so that it stands the right way up and keeps its shape. A file converted from a SolidWorks part (its original solid names a .sldprt) is already Y up, like the app, and is not turned.
  • Converted: sketches on planes and faces with their geometry (lines, arcs, circles, ellipses, splines) and constraints (including parallel, perpendicular, equal, fixed points and point-to-line distances); extrudes (new body, join, cut, through all; symmetric, two-sided and tapered; starting or stopping at a face; regions picked by their outlines); surface extrudes and the thicken of one (a plain distance, one or both ways; a thicken that makes a new body or joins); boxes, cylinders, spheres and tori; fillets and chamfers; shells; revolves about a line of the sketch, a line in space or the sketch axis (also symmetric); lofts, including to a point and along guide rails; mirrors of features and of whole bodies; sweeps along a spline or along lines and arcs (with a twist); coils; circular patterns (of features about a coordinate axis through the origin, of bodies about any axis) and rectangular patterns; holes, also up to a face; sheet-metal base flanges (as a plate of the sheet thickness); scale; moving and copying bodies; combining and removing bodies; text; and plastic features such as bosses, rests, snap fits and lips. Named parameters arrive as the part’s variables (see below). Expressions may use + - * / ^, parentheses, pi, the functions sin, cos, tan, asin, acos, atan, atan2, sqrt, abs, min, max, floor, ceil, round, trunc, exp, ln, log10, hypot, pow and mod (angles in degrees), and the units mm, cm, m, in, ft, deg and rad.
  • Assemblies: each component becomes a part of its own, inserted once per occurrence and placed by its transform. A component placed inside another one (a sub-assembly) is inserted into the part of that component, so it moves with it. A placement the file hides has its bodies hidden here too (in every copy of the component that holds it). A revolute joint between two circles becomes a hinge mate. Other joints are reported as skipped. Timeline folders of the file become tree folders.
  • Parameters: the named parameters of the file become the part’s variables, so you can change one and the part follows. A field written as a name or an expression over them (an extrude depth, a hole or sphere size, a fillet radius, a chamfer or shell thickness, a revolve angle, a sweep twist, a pattern spacing, a cylinder height) stays an expression, and so does a sketch dimension that names a parameter. The expressions may use + - * / ^, pi, and the functions sqrt, sin, cos, tan, abs, min, max, pow, mod, hypot, atan2, asin, acos, atan, round, floor, ceil, trunc, exp, ln and log10. What the part cannot hold (a parameter whose name it cannot take, such as sin or mm) is kept as the number it evaluates to, and the row of that feature says so. Other fields, such as a box size or a position, are plain numbers.
  • Colours: body colours and opacity, metallic and roughness, and hidden bodies are carried over. Per-face colours and hidden joints are not.
  • The stored solid of a file converted from another CAD system (SolidWorks, Fusion 360 and others) is kept as an imported body. The importer reads it through the kernel first: a converter that restates the geometry can turn some faces the wrong way, and then the body is healed (the kernel’s own STEP of it is used). When the file also builds a body from sketches and operations, the importer rebuilds it and compares its volume with the stored solid; if they differ by more than 0.5%, the stored solid is the body, the operations that build bodies are shown as skipped with both volumes, and the sketches stay.
  • What cannot be converted stays as a suppressed placeholder row in the tree that shows the raw feature type, so nothing is lost silently. Features that depend on it are reported too. The notice says how many converted, names the first problem, and counts the rest. The geometry is then partial.
  • Refused as a whole: a file that is not a valid SolidCraft file, has an unknown format version, or uses units other than millimetres. The part you had open is untouched.
  • Known gaps: sheet metal other than base and contour flanges, joint limits, patterns along a path of non-round seeds, circular patterns of features about an axis that is not a coordinate axis through the origin, sweeps that keep the profile at a fixed angle or scale it, surface features other than the surface extrude and its thicken, conic curves in sketches, per-face colours, and modelled threads. A tapered extrude that is also symmetric, two-sided or stops at a face is reported, as is an end offset from a face. A thicken is made on the front side of its surface, because the file’s own side is not read: the result lists a note, and Back in the editor flips it.

A .solidcraft file is either a zip archive or a bare JSON document. Both are read.

DXF

A DXF file (.dxf) brings 2D geometry into a sketch. It does not make a part.

  • Into the sketch you are editing: while a sketch is open, choose Import DXF in the Import group of the sketch ribbon, or drop the file onto the window.
  • As a new sketch: choose New sketch from DXF, in the new-sketch menu of the Home tab. The sketch goes on the selected face or plane, or on the front plane when nothing is selected. Dropping a DXF with no sketch open does the same.
  • Read: lines, circles, arcs, polylines (bulges become arcs, a closed flag closes the outline), splines and points. Entities on a layer named CONSTRUCTION become construction geometry.
  • Units come from the file’s drawing units and are converted (inches, feet, centimetres, metres and others). Unitless or millimetre drawings are used as drawn. An unknown unit code is read as millimetres, with a notice.
  • Not read, and listed in a notice: blocks, text, hatches, dimensions, ellipses and 3D entities.
  • Connected outlines: end points closer than 0.000001 mm are merged, so outlines close. No constraints are added.
  • Limits: more than 20,000 entities, coordinates further than 1,000,000 mm from the origin, binary DXF and DWG are refused with a message. The origin is kept as drawn (the drawing is not re-centred), so move a far-away drawing to the origin first.

SVG

An SVG file (.svg) brings 2D drawing geometry into a sketch, the same way a DXF does. It does not make a part.

  • Into the sketch you are editing: while a sketch is open, choose Import SVG in the Import group of the sketch ribbon, or drop the file onto the window.
  • As a new sketch: choose New sketch from SVG, in the new-sketch menu of the Home tab. The sketch goes on the selected face or plane, or on the front plane when nothing is selected. Dropping an SVG with no sketch open does the same.
  • Read: paths (lines, arcs and curves, written absolute or relative), rectangles (also with rounded corners), circles, ellipses, lines, polylines and polygons, inside groups and with any transform (move, scale, rotate, skew). A shape that is defined once and reused with use is placed wherever it is used.
  • How curves arrive: straight lines stay lines and circular arcs stay arcs, circles stay circles and ellipses stay ellipses, also after the drawing is rotated or mirrored. Bezier curves become splines that follow the curve exactly; an elliptical arc becomes a short chain of splines. A closed outline (a path ending in Z, a rectangle, a circle) closes in the sketch, so you can extrude it, and an outline inside another one cuts a hole.
  • Size: the file’s width and height in millimetres, centimetres, inches or points, together with its viewBox, set the size. SVG’s Y axis points down and the sketch’s points up, so the drawing is turned upright and its lower left corner is at the sketch origin. A file with no size in those units is read at 96 pixels to the inch (1 px = 0.2646 mm) and a notice tells you; check the dimensions of the result.
  • Not read, and listed in a notice: text (convert it to outlines in your drawing program first), images, scripts and other elements. Fills, strokes, gradients and styles are ignored. Shapes that use a clip path, mask or filter are imported whole, and the notice counts them. Shapes drawn twice on top of each other are imported once.
  • Safety: the file is only read as drawing data. Scripts are never run and nothing is fetched from other addresses; a file that declares entities is refused.
  • Limits: more than 20,000 entities, a file over 10 MB, and coordinates further than 1,000,000 mm from the origin are refused with a message. No constraints are added, and the origin is kept as drawn.

Parts from samples and the library

Library (top bar) opens a sample part as a new part, fully editable. Parts from a library, and the Catalog, are added to the part you have open as ordinary features in one undo step; they are not imports of a file. See The Library.

To use another saved part inside an assembly, see Assemblies and mates.

The import report and repair

An import that brings in every part as a solid has nothing to report. When it does not, a notice says what became of the parts (“2 of 3 parts came in as solids. 1 came in as surface bodies of the faces that could be read and need repair before they can be modelled on.”) and offers Import report. The same report is behind the Diagnostics tab of the drawer (press \, choose Diagnostics): the import step gets a warning that says how many parts came in as surface bodies, with Import report and Repair buttons.

  1. Press Import report in the notice or in the Diagnostics warning.
  2. Read the summary, then one row per part of the file: Solid (42 faces), Surface body: 31 of 42 faces, needs repair, or Not imported: none of its 60 faces could be read. Under a part that is not a solid, each reason is the kernel’s own sentence with its code and the faces concerned (six faces are named, then “and n more”).
  3. Press Repair to fix what can be fixed, or Close.

Repair adds one undoable repair step after the import (listed in History as Repair): it rebuilds the faces that could not be read on their own surface, sews small gaps and fills flat holes. A notice then says how it went: “repaired into a solid (3 faces rebuilt, 1 gap sewn, 2 holes filled)”, “still a surface body after repair (…)”, or “not repaired: …”. A repair the kernel refuses is not added to the history and the notice gives its reason. Undo removes a repair like any other step.

A file that came in view only is repaired the other way round: Repair first makes it an editable part (the solid as imported is kept inside it) and then adds the repair step. The report says so before you press the button. This applies to STEP, SolidWorks and SketchUp files that came in as a view-only body.

Common problems

SymptomFix
No Import report after an importEvery part came in as a solid, so there is nothing to report
A part says “Not imported”None of its faces could be read. Fix the file in the source program and import it again
Repair says “not repaired”The kernel’s reason follows the colon. The step is not added, so nothing has changed
Repair left a surface bodyThe remaining faces are listed in the notice. Repair what is left, or rebuild those faces yourself on top of the import
The report is goneOpen it again from the Diagnostics tab of the drawer

When an import is slow or fails

  • Wait for the overlay. A large STEP or SolidWorks file can take seconds and a large SolidCraft file minutes. A busy overlay with a cancel button is shown, and nothing else is changed until it ends.
  • A SolidCraft import says where the time went. The notice after it reads like “Imported name in 3.2 s: read 0.4, kernel 2.5 (310 questions), mapping 0.3, rebuild 0.0”: the time to read the file, the kernel’s time and the number of questions put to it, the time to map the features, and the rebuild. A slow file shows which step to blame.
  • A notice names the cause. “Could not import <file>: …” gives the reason or the error code. Read the notice before trying again; the Console tab of the drawer keeps recent notices.
  • Nothing to import. STEP with no solid, SketchUp with no visible faces and FreeCAD with no PartDesign body are refused. Check the source model has a solid and that nothing is hidden.
  • Too large. Over 50,000 faces for SolidWorks and SketchUp. Simplify the model in the source program or split it.
  • Wrong size. Imports apply the file’s units. If the part is 25.4 times too big or small, the units in the source file were wrong; fix them there.
  • Gaps or open edges on a STEP or SketchUp import mean the surface is not closed. Fix it in the source program, or run it through STEP export. When parts come in as surface bodies rather than solids, the Import report lists them and Repair tries to rebuild them: see The import report and repair.
  • Imported but a feature is missing (FreeCAD, SolidCraft): look at the notice and at the tree. Placeholder rows are suppressed; the rest is real. You can rebuild the missing features yourself on top of what came in.
  • Still stuck? Troubleshooting has more.

Next

Exporting

This chapter covers every way to get a model out of the app: STEP, STL, OBJ, 3MF, glTF (GLB), DXF, drawings as PDF, SVG and DXF, the bill of materials as CSV, and the part file itself.

All exports use millimetres. Files go through the browser: depending on the browser they are saved straight to your downloads folder or you are asked where to put them. A notice confirms each export and warns about problems.

The Export menu

Choose the Export button in the top bar (or press Ctrl+E) to open the list of formats. Each entry is also a command in the command search (press F), so you can type “export” to find them.

Menu entryFileNeeds
Export STL (binary)<part>.stlA solid on screen
Export STL (ASCII)<part>.stlA solid on screen
Export OBJ<part>.objA solid on screen
Export 3MF (3D printing)<part>.3mfA solid on screen
Export glTF (GLB)<part>.glbA solid on screen
Export STEP<part>.stepA solid on screen
Export sketch as DXF<part>-<sketch>.dxfA sketch being edited, or selected in the feature tree
Export 3 views as DXF<part>-views.dxfA solid on screen

An entry that cannot run is greyed out. The file name starts with the part name; characters that file systems do not allow are replaced with an underscore. If there is nothing to export you get a notice: “There is no solid to export yet” or “Open a sketch or select one in the feature tree to export it”.

Before the export runs, the app waits for the model to finish rebuilding, so a file is never made from a stored preview.

What is exported is the model as built: hiding a body or a component, changing the display style, the exploded view and section views do not change the file. Colours, finishes and materials are not written to any of these formats.

STEP

Use STEP to hand an exact solid to another CAD program. Export STEP writes the kernel’s exact surfaces, not triangles. It can take a moment on a large part, with the busy overlay showing. The exported file imports back to the same volume. STEP carries no colours or feature history.

STL and OBJ

Use STL for 3D printing and slicers, and OBJ for rendering programs.

  • Both are triangle meshes made from the same triangles the viewport shows.
  • STL (binary) is smaller and is the usual choice. STL (ASCII) is readable text. The solid name inside the file is the part name.
  • OBJ has welded vertices and counter-clockwise faces, one object.
  • After writing, the app checks that the mesh is watertight. The file is still written, but if the surface has open edges, non-manifold edges or flipped faces you get a warning (“… is not watertight … a slicer may need to repair it”). The note on the number of triangles tells you the size of the mesh.

3MF and glTF (GLB)

Use 3MF for 3D printing programs that read colours and several bodies, and GLB for web viewers, game engines and AR.

  • Both write one object per body, named as in the Bodies list, with the body’s colour (and opacity) when it has one. 3MF also uses the same triangles as STL; GLB carries the viewport’s smooth normals.
  • 3MF is a zip file, in millimetres with Z up, as the model is. The watertight check of STL and OBJ applies.
  • GLB is a single binary glTF 2.0 file. glTF is in metres with Y up, so the part is scaled by 0.001 and turned so that the model’s Z axis points up the file’s Y axis (a 10 mm cube is 0.01 m). Metallic and roughness are written when you set them on the body; otherwise the material is a plain matt one.
  • Only visible bodies and the mesh quality and chord boxes of the Export menu apply to both.

Cosmetic knurls in exports

A cosmetic knurl is only drawn in the open part. STEP, STL, OBJ and the folder exports below still include it: the app copies the part on the side, cuts the knurl into the copy as real grooves (the same cuts the Knurl wizard makes with Cosmetic off) and writes the copy. Your part is not changed: the knurl stays cosmetic and nothing is added to the history or the undo list. The notice after the export says “Included N cosmetic knurl(s) as real cuts”.

Choose how this works in Settings > General > Export > Include cosmetic knurls in exports, kept on this device:

  • On (the default) cuts them for every export.
  • Ask each time shows a small dialog: Include the knurls, Export without or Cancel. Tick Do not ask again to keep the answer as the setting.
  • Off writes the plain solid and warns that the knurls are not in the file, with a button that converts them to real cuts in the part.

Straight grooves cut in about a second. Diamond and pyramid knurls with round grooves, or dense ones, can take a minute or more (a pyramid of 90 V grooves took about 40 seconds on the test machine): a hint says so first, the busy overlay says “Cutting knurl grooves for the export…” and Cancel stops it. If the cut fails or takes more than 120 seconds, nothing is written until you choose: the message gives the reason and offers Export without the knurl or Cancel. One case keeps the plain solid and the warning: STL or OBJ with some bodies hidden. An STL or OBJ with a chosen mesh tolerance meshes the knurled copy at the standard tolerance and says so. Drawings and the DXF with three views are made from the open part, so they still show the plain cylinder. Mass properties are not changed. Exporting again is instant: a successful cut is kept, so exporting the same part again with the same knurls (also as another file type of the same kind: STEP again, or STL and OBJ) reuses it and the notice says so; changing the part, the knurl or the kernel build cuts again. The folder exports cut each time.

DXF from a sketch

Export sketch as DXF writes the sketch you are editing, or the sketch selected in the feature tree. The file is DXF R12 (ASCII), which most CAD, laser and CNC programs read.

  • Lines, circles, arcs and points are written exactly. Ellipses and splines are written as short line segments, because R12 has no spline or ellipse. Some entities that cannot be written are counted in a warning.
  • Construction geometry goes on a layer called CONSTRUCTION with a dashed line type. Everything else is on layer 0.
  • The units are marked as millimetres. A sketch with no geometry is refused.

DXF with three views

Export 3 views as DXF writes the edges of the solid as three views: front, top above it and right beside it (third-angle projection). Edges seen end-on collapse to a line and edges that land on top of each other are written once. Hidden lines are not drawn, and there are no dimensions. For a proper drawing with hidden lines, sections and dimensions use the drawing view below.

Drawings: PDF, SVG, DXF and print

In the Drawing view the toolbar has PDF, SVG, DXF and Print buttons. They are described in Drawings. In short: PDF is one vector page at the sheet size, SVG is the sheet in millimetres, DXF has layers for visible, hidden, centre, thin, hatch, dimension, text and border lines (arrowheads are left out), and Print opens your browser’s print dialog, where “Save as PDF” also works. The file name comes from the title in the title block, or the part name. A sheet with no views cannot be exported (“Add views first”).

Bill of materials

In the Assembly panel, Bill of materials > Save CSV writes bom.csv. See Assemblies and mates.

The part file

Save and Save as write the editable part, .ckpart, optionally compressed to .ckpart.gz. That is the way to keep or share a model you want others to edit, and the only export that preserves the feature history. See Saving and opening.

One folder as a file

A folder of the feature tree can be taken out of a model on its own. Right-click the folder.

ChoiceResult
Export folder geometry as STEP<part> - <folder>.step, the exact solids of the folder
Export folder geometry as STL<part> - <folder>.stl, binary, the same checks as a normal STL
Export folder geometry as part file (frozen)<part> - <folder>.ckpart: a part whose one feature is the imported solid, so it opens, measures and can be cut or drilled but has no history
Extract folder as a parta new document with the folder’s features and the variables they use; nothing is written until you save it

What is in the file. The bodies the folder’s features made or changed (with the cosmetic knurls whose cylinder is on one of them, see above), as the model builds today. A body that a feature outside the folder also touched comes out whole, with those changes, and a notice says how many bodies that is. Hidden bodies are included, because you asked for this folder. The open model is not changed.

Refused, with a hint. A rolled-back model (“roll forward first”), a folder that holds only sketches, planes or axes, a folder whose solid features are all suppressed, and a folder whose features left no body in the result (a failed feature, or bodies a later feature deleted).

Extract as a part needs the folder to stand on its own. It is refused, naming exactly what it found, when a feature of the folder uses a feature outside it (a sketch from another folder), a face of one (F2.C1: face names are not stable in a new document) or a body made outside it. The new part is then built on the side and its volume compared with the folder’s bodies; a folder that cuts geometry it does not name (a “through all” cut into a body made elsewhere) is refused with both volumes instead of opening an empty or different part. The extract keeps the feature numbers, copies the material and the variables the folder uses (with their values), and leaves behind colours, body names, configurations and the stored view.

What is not in the Export menu

  • GLB (glTF). Not offered in the app. The MCP server can write a GLB; see Agents and the MCP server.
  • Exporting a few features that are not a folder. Group them into a folder first; see the next section.
  • STL/OBJ import. The app can export meshes but cannot read them.

Troubleshooting

  • The Export button or an entry is greyed out. There is no solid on screen. A part that only holds a view-only import (see Importing) has no mesh built from features, which is what the entries test for, so they should be greyed out. And a sketch export needs an open or selected sketch.
  • The slicer says the STL is not watertight. Read the warning for the count of open edges. A model with open surfaces (a surface body that was never thickened or knitted) is not a solid.
  • A DXF opens at a strange size. The sketch is in millimetres; check the unit setting in the program that opens it.
  • STEP fails or the file is empty. Check Diagnostics for feature errors first; see Checks and diagnostics.

Next

Drawings

This chapter covers the drawing view: making a sheet of views of your part or assembly, adding dimensions, notes, balloons and a title block, and exporting the sheet as PDF, SVG or DXF.

A drawing belongs to the part. It is saved in the part file, and when the part changes the views are projected again, so the sheet follows the model.

Open the drawing view

Press Drawing in the Part / Drawing switch in the top bar. The sheet appears over the viewport. The switch needs an open part, and a part with no body says “Nothing to draw: the part has no body.” Back to part (top left of the drawing toolbar) or Part in the switch returns to the model. The Drawing view closes when you switch to another document tab.

The sheet

The panel on the right edits the sheet:

SettingChoicesDefault
SizeA4, A3, A2, A1, A0, ANSI A, B, C, D, EA3
OrientationLandscape, PortraitLandscape
Scale10:1, 5:1, 4:1, 2:1, 1:1, 1:2, 1:4, 1:5, 1:10, 1:20, 1:50, 1:1001:1
Unitsmm, in (for dimension text; the model is in millimetres)mm
ProjectionThird angle, First angleThird angle

The sheet scale applies to every view that does not have its own scale. In third-angle projection the top view sits above the front view and the right view to its right; first angle swaps the sides. A change of projection affects views you add afterwards, not the ones already placed.

The Title block at the bottom right has Title, Part number, Material, Author, Date, Revision, Mass and Company, plus the sheet scale and number. Title and Material start from the part (its name and its material), and the mass is the part’s volume times the material density, kept up to date while the field still holds the computed value. Type over any field to set it yourself. From the part puts the computed values back.

Make views

The toolbar groups the view tools first.

ToolWhat it does
Standard viewsFront, top, right and isometric views at the largest standard scale that fits the sheet, leaving room for the title block and the bill of materials. Replaces the views already on the sheet, and adds overall dimensions, diameters and hole callouts to the front view.
Add viewChoose Front, Back, Left, Right, Top, Bottom or Isometric from the list, then press Add view.
Projected viewClick a view, then click on the side where the new view should go. It stays aligned with the view it came from.
Section viewClick a view to place a cut line (hold Shift for a horizontal line). The cut part is hatched, the parent shows the cut line with arrows and a letter, and the new view is labelled SECTION A-A. If the line misses the part you get a notice.
Detail viewDrag a circle on a view. That area is shown larger (twice the parent’s scale by default), labelled DETAIL B, and cut at the circle.
Auxiliary viewClick an inclined straight edge of a view. A view looking square at that edge is made.

Views appear one at a time as the kernel projects them, with “Projecting views…” in the status line. Each view is cached, so moving, scaling or switching lines does not recompute it.

Select, move and edit views

Use Select (the default) to click a view and drag it. Projected and section views move only along the axis they share with their parent so they stay aligned; moving a parent carries the views made from it. Dragging empty space pans the sheet, the mouse wheel zooms at the pointer, and a right or middle button drag also pans. Fit sheet resets the camera.

With a view selected, the panel edits:

SettingWhat it does
LabelThe text under the view. The Label box shows or hides it.
ScaleThe view’s own scale, or the sheet’s.
Hidden linesShows hidden edges as dashed lines.
Tangent edgesShows the lines where smooth faces meet.
Centre lines and marksDraws centre lines on cylinders seen from the side and centre marks on round holes. They can be picked, selected and dimensioned.
Align to parentSnaps a projected or section view back into line.

Delete (or the Delete key) removes the selected view together with the views made from it and their dimensions.

Dimensions

Choose Dimension (or press D), then click an edge or a centre line in a view.

  • A straight edge gives its length.
  • A full circle gives a diameter; hold Shift on the pick to get a radius instead. An arc gives a radius.
  • Click two edges for a distance (parallel edges), an angle (edges that meet), a centre distance (two circles) or the distance from a circle centre to a line. Press Enter to finish a one-edge dimension; a second click completes a two-edge one.
  • Centre lines and centre marks work as references: click two parallel centre lines (for example the axes of two shafts) for the distance between them, a centre line and an edge for the distance from the axis to the edge, two centre marks for the distance between the hole centres, or two centre lines that meet for the angle. The dimension line is placed outside the view, beyond any dimension already there. Clicking a centre line with the Select tool selects just that line, and dragging it still moves its view.
  • Drag a dimension to move its line, or the leader of a round one.
  • In the panel, edit the text. Use <> for the measured value, for example <> +0.1 / -0 or 4 HOLES <>. Leave it empty to show the measured value. A radius or diameter has a toggle to switch between the two.

A dimension remembers the two faces of the edge it was made on (for a centre line, of both silhouette edges of the cylinder), so it finds the edge again after the model changes. If an edge disappears, the dimension stays where it was and the status line says how many were lost.

Auto dimension adds overall width and height, one diameter per hole position, and the hole callouts below, for the selected view (or all views except the isometric if none is selected).

Hole and thread callouts

A circle that belongs to a Hole or Thread feature gets that feature’s text: for example M10x1.5 ↧ 30 for a threaded hole with its depth, Ø6.5 THRU, or M5 CLR THRU, with CSK or C'BORE for countersunk and counterbored holes. The text is computed from the feature, so it changes when the feature changes.

Notes, balloons and symbols

ToolWhat it does
NoteClick on the sheet for a text note. Shift+click on a view for a note with a leader to that point. Edit the text (several lines) in the panel.
BalloonClick on a view for a numbered balloon with a leader. The Number field in the panel renumbers it.
Auto balloonsAssemblies only. Adds a balloon for each bill-of-materials item to the selected view (front by default), attached to a visible edge of the item.
Surface finishClick on a surface for a surface finish symbol with a leader. The panel edits the roughness; the default is Ra 1.6.
GD&T frameClick for a feature control frame. Type the cells separated by a vertical bar, for example POS|0.1|A. Plain ASCII characters, no special tolerance symbols.

For an assembly, a bill of materials table (part, quantity, material and mass, the same as the Assembly panel’s list) is drawn above the title block. Untick Show table in the panel to hide it.

Undo and delete

Ctrl+Z and Ctrl+Y (or the Undo and Redo buttons) step through the changes you made to the sheet. The part’s own history is not touched. Typing in a field counts as one step. Changes that the part causes (a new mass, regenerated dimensions) are saved but are not steps. Escape drops the current tool, then clears the selection.

Export and print

The toolbar ends with PDF, SVG, DXF and Print. All four come from the same drawing, so they agree.

OutputDetails
PDFOne page at the sheet size with vector lines, dashes, filled arrowheads and Helvetica text.
SVGThe sheet in millimetres.
DXFDXF R2000 (AC1015) ASCII in millimetres, y up. Lines are written as LWPOLYLINE, plus circles, arcs and text. One layer per line style: BORDER, VISIBLE, HIDDEN, THIN, CENTER, DIM, TEXT and HATCH, with HIDDEN and CENTER line types. Arrowheads are left out.
PrintOpens the browser’s print dialog at the sheet size. Choose “Save as PDF” there if you prefer.

The file is named from the title block’s Title, or the part name when it is empty. Add at least one view first. The status line shows “Saved <name>” after an export.

Speed

Hidden-line projection is the slow step. A plate takes a fraction of a second per view. A complex part with many curved faces takes longer, and the isometric view is usually the slowest. Views are cached by the version of the part and the view definition, so leaving and re-entering the Drawing view, and moving or scaling views, does not repeat the work.

Limits

  • One sheet per part. There are no revision tables, ordinate or chain dimensions, break lines, weld symbols or sheet templates; the title block layout is fixed and the border margin is 10 mm.
  • Tolerances are typed text only. GD&T frames have no characteristic symbols and datum triangles.
  • Hidden lines come from the kernel and are sometimes split into more pieces than needed on curved edges. Section view of a torus can fail.
  • Views you added before changing the projection keep their sides.
  • New views are placed in a free spot by a simple search, so overlaps can happen. Drag them apart.
  • Zoom is by mouse wheel only.

Next

Measure and inspect

This chapter covers the tools that look at a part without changing it: mass properties, measuring distances and angles, section views, interference between bodies, and surface analysis. None of them edits the document, and every result is a read-only query of the part as it is on screen.

Where the tools are

The Evaluate ribbon tab has them. Mass properties, Measure, Interference check and Section view open the Inspect tab of the bottom drawer, which holds one card for each. You can also open the drawer with the backslash key (\) and choose Inspect, or find any of them in the command search (press F).

ToolCommandKey
MeasureMeasureM
Mass propertiesMass properties
Section viewSection view
Interference checkInterference check
Zebra stripesZebra stripesAlt+Z
Gaussian curvature, Mean curvaturethe same names
Draft analysisDraft analysisAlt+D
Curvature combCurvature combAlt+C

The commands need a solid on screen. There is no separate probe tool: to read a position, pick a corner with Measure. The size of what you have selected appears in a small card in the corner of the view (a lone corner has a position, not a size, so it shows no card): see The quick readout.

Mass properties

Open the Inspect tab and the mass card computes at once, or press Compute. It shows:

  • Volume (mm³), surface area (mm²) and mass,
  • the centre of mass, the bounding box and its size,
  • the principal moments of inertia (g·mm²).

Mass depends on the Density field (g/cm³). It starts from the part’s material (steel is 7.85, aluminium 2.70 and so on). A note under the field says which material it took the density from. If the part has no material, or one whose density is not known, the field starts at 1 and the note asks you to set a density. You can type any value, and the mass and moments follow at once. To change the material itself see Materials and appearance.

Settings > General > Mass display chooses how a mass is shown: automatic (grams below one kilogram, kilograms above), grams, kilograms, pounds or ounces, with 3 to 6 significant digits. It applies wherever a mass appears (this card, the material editor, the bill of materials and drawing tables). The values are the same; only the unit and the digits change, and it is kept on this device.

A part made of several solid bodies lists volume and mass per body in a table. Surface bodies have no volume; they are left out of the mass, and a note says so.

Once you have a result it stays current: after an edit the card shows “Out of date: the part changed.” and recomputes. Copy puts the numbers on the clipboard as tab-separated lines for pasting into a spreadsheet.

Measure

  1. Press M, or choose Start measuring in the Measure card. The drawer opens on the Inspect tab.
  2. Pick one or two items in the model. The usual selection modes work: Q for faces, E for edges, V for corners.
  3. Read the result in the card. A red leader with the value is drawn in the view too.

Picks add up instead of replacing each other. A third pick keeps the last two. Clear picks empties the list, and Copy puts the results on the clipboard. M again, or Stop measuring, ends the tool.

You pickYou get
A cornerIts position
An edgeLength. A circular edge also gives radius, diameter and centre.
A faceArea and surface kind. A cylinder, cone, sphere or torus also gives radius, diameter and centre.
Two cornersMinimum distance and the offset along each axis
A corner and an edgeMinimum distance
A corner and a faceMinimum distance, and the distance along the normal for a flat face
Two edgesMinimum distance. Two straight edges also give the angle (0 to 90 degrees); two circles give the centre distance.
A face with a face or an edgeMinimum distance, normal distance and the angle between them, from the exact surface

Distances that involve corners and edges are taken from the lines drawn on screen, so on a curved edge they are as fine as the display. Anything with a face uses the exact surface. If a pair cannot be measured the card says “No measurement for this pair.”

The quick readout

A small card in the corner of the view shows the size of the selection as you make it. It needs no tool and no drawer: pick something with the usual selection modes and the card is there. It shows only the value lines, with no visible heading.

You pickThe card shows
One straight edgeLength
One circular edgeDiameter, radius and circumference. A curved edge shows its length instead
One faceArea. A round face also gives its radius and diameter
Two itemsThe minimum distance between them, and the angle when there is one (two straight edges or two circular edges; two corners give the distance alone)
Three or moreHow many items are selected

The numbers are in the units of the rest of the app (millimetres and degrees) and follow the selection as you add and remove picks. On a phone or a tablet the card sits at the top left of the view instead of the bottom right.

It is hidden while a sketch is open and while the Measure tool is running: Measure draws its own leader with the value in the view, and its card in the drawer holds the full result.

Common problems

SymptomFix
The card is not thereNothing is selected, a sketch is open, or Measure is running. Pick something with Measure stopped
The card and the selection list overlapThey share the bottom-right corner, and the card is drawn over the list. Collapse the list with its arrow button
It shows a count instead of a sizeIt gives sizes for one or two items; with three or more it shows the selection summary: the count with the total area or length, for example “3 edges, 60 mm”
A curved edge shows no diameterA curve that is not a circle has no diameter: the card shows its length

Section view

A section cuts the part open so you can see inside. It is a view only: it does not change the model, and Measure, Mass properties and exports do not use it.

  1. In the Section card choose Front, Top or Right. The plane starts through the middle of the part. To cut on a face, select one flat face first and choose Selected face; the plane starts on that face. If you have not selected a flat face you get a notice.
  2. Drag the Offset slider, or type a number in millimetres, to move the plane along its normal.
  3. Tick Flip side to keep the other half.
  4. Choose Off to remove the cut. The Section view command on the ribbon turns the last section on or off.

The cut face is filled so the section looks solid. Selection, hover colours and design-issue colours are not clipped. The section stays while you rebuild the part or switch drawer tabs.

Interference check

Interference finds bodies of one part that share volume. Press Check in the Interference card. If the part has only one solid, the card says “Needs two or more solid bodies”. Otherwise it lists each pair that overlaps with the shared volume, or says “No interference between N bodies”. Click a pair to select the faces involved and frame them. The result goes out of date when the part changes, and you must press Check again.

For components in an assembly, the Assembly tab has its own Interference check that names the pairs by component. See Assemblies and mates. Note that bodies made by overlapping features in one part are merged by the kernel, so this check mainly finds overlaps between separate bodies you have kept apart.

Surface analysis

These tools colour the model to show how smooth the surfaces are. Turn one on in the Surface analysis group of the Evaluate tab, or in the Analysis section of the Display menu, which also has the settings. A colour legend appears over the view.

ModeWhat it shows
Zebra stripesStripes reflected in the surface. A break in a stripe is a break in tangency; a kink in a stripe is a break in curvature. A Stripe density slider changes the spacing.
Gaussian curvatureRed for dome-like, blue for saddle-like, white for flat or rolled areas.
Mean curvatureRed where the surface bulges out, blue where it dips in.
Draft analysisFaces coloured by the angle to a pull direction (X, Y or Z) with a Least draft setting in degrees: green has draft, red has none, blue faces the other way.
Curvature combTeeth along edges and sketch curves as long as the curvature there. Smooth teeth mean a smooth curve. A Comb size slider scales it.

Analysis colours opaque bodies only. For manufacturing checks that report numbers instead of colours, see Design checks.

Limits

  • Everything is in millimetres, grams and g/cm³. There is no unit switch.
  • Mass uses one density for the whole part. A part has one material; per-body materials are not available.
  • A pair of corners and edges is measured on the display lines, not the exact geometry.
  • A view-only import (see Importing) is only drawn in the viewport. The inspect tools test for a solid built from the part’s features, so they should treat a part holding only an import as having no solid. This comes from reading the code, not from running it.

Next

Checks and diagnostics

This chapter explains how the app tells you that something is wrong with the model: the status bar, the red rows in the feature tree, the Diagnostics card, and the card in a feature editor that stops a change that would break the model. It also shows how to read the messages and what to try. The Check tab, which tests a part against manufacturing rules, is covered in Design checks.

Why a model breaks

A part is a list of features that are rebuilt from first to last. When you change one feature, everything after it is rebuilt too. If one feature can no longer be built, the features that depend on it fail as well, so one problem can look like twenty. The app sorts these for you: it finds the cause (the first failure that stands on its own) and shows the rest as consequences that only follow from it. Fix the cause and the consequences normally go away.

An edit that would break the model is refused. The kernel rebuilds the candidate first, and if any feature fails the document stays exactly as it was. A broken model can still reach you by opening a file that already has failing features.

The status bar

The bar at the bottom of the window reports on the whole part:

ItemMeaning
Ready / BusyWhether the kernel is working. A busy overlay with a cancel button shows during long rebuilds.
NoticeThe latest message, such as a refused edit or a finished export. It stays for a few seconds. The Console tab of the drawer keeps the whole list.
Features, Faces, TrianglesSize of the model.
Cached viewShown while a stored view is on screen and the model rebuilds behind it. Edits wait for the rebuild.
Design check chipThe last design check result, for example “FDM 3D printing: 2 errors, 5 warnings”. Click it to open the Check tab. It is dimmed when the part has changed since.
Last rebuildHow long the last rebuild took.
ErrorsThe number of causes. When some features fail only because of an earlier one, it adds “(+N blocked)”. It is red when anything fails.

The button at the right end opens and closes the drawer, which you can also toggle with the backslash key (\).

The feature tree

A feature that fails is shown in red, with the reason underneath. Features that only fail because of an earlier one are muted and carry a blocked by F14 chip instead of red text. Click the chip to select the cause. The tree header badge counts causes only.

An amber ! on a row is a warning: the feature still works, but the kernel noticed something. Point at it to read the hint.

The Diagnostics tab

Open the drawer and choose Diagnostics. When the model has errors, the card shows:

  1. A summary sentence such as “The edit broke the model at F14 Trim barrel and handle: the surfaces do not cut each other. 16 later features could not be built because of it.”
  2. The cause: the feature and the error code.
  3. What to try: plain advice for that error (see the table below).
  4. Buttons:
ButtonWhat it does
Undo this changeUndoes the last edit. Shown when there is history to undo.
Select F14Selects the cause in the tree and frames it.
Show N consequencesFolds open the list of dependent errors, each of which selects its feature. “Hide consequences” folds it again.
Copy all errorsCopies the raw error list, handy for a bug report.

If two unrelated features fail, they are two separate causes, and the second is listed under the first.

When the kernel refused an edit that you just made, the card describes that edit and says “This edit was not applied; your model is unchanged.” The toast and the History entry carry the same one-line summary.

In a feature editor

While an editor is open, the live preview is checked as you type. If the preview has a problem the saved model did not have, the editor shows a short card under the fields with the sentence, the advice, Cancel edit, Select F14, a folded list of consequences and Copy all errors. The Confirm button is greyed with the tooltip “This change breaks the model (F14). Cancel or adjust.” Hold Shift while you press Confirm to try the edit anyway: the kernel still refuses it if it breaks, so Shift cannot put a broken model into the file, it only shows you the refusal. The Gear, Thread and Hole editors show just the one-line summary as a hint.

What to try

The advice shown for common errors:

Message (cause)What to try
The surfaces do not cut each otherMake a smaller change, or move the trimming tool so it crosses the surface again.
It removes nothing / it cuts nothingThe cut or tool no longer touches the body. Move the profile so it overlaps the body, or flip the direction.
A face or edge it uses no longer existsA feature was built on a face or edge that has gone. Pick it again, or undo the change that removed it.
The combine failedMake sure the two bodies overlap in a volume, not only along a face, or nudge one by a small amount.
The fill boundary is not validThe edges around the hole no longer form one closed loop. Make a smaller change, or pick the edges again.
The rounding failed (fillet or chamfer)Use a smaller radius, round fewer edges at once, change the order, or round last. With Tangent chain on, the rounding runs around corners.
The wall is thicker than the part allows (shell)Use a thinner wall.
The shell could not be madeTry a smaller thickness or open a different face.
The sketch is not a closed outlineClose the gaps in the sketch. See When a sketch will not solve.
The sweep failedMake sure the profile sits at the start of the path and the path has no sharp kinks.
The loft failed, or makes an invalid solidUse profiles with the same number of segments, in the same order, along one direction; put a point profile first or last; no two profiles should cross.
The profile crosses the axis (revolve)Move the profile to one side of the axis.
Anything elseUndo the last change, or adjust the values until the feature builds again.

A rounding that is wider than the faces beside it, or a radius too large for the edges, has its own message with the same advice.

Reading the kernel’s own detail

The code shown next to the cause, such as booleanFailed or missingReference, is the kernel’s error code. The kernel book explains what each means, and what the kernel checks when it decides that a solid is valid: Validation and Feature errors and diagnostics.

A short example

You lower the angle of a surface and the status bar turns red: “Errors 1 (+16 blocked)”. The edit is refused, so the model is unchanged and the Diagnostics tab shows the cause with “This edit was not applied”. Read the sentence, follow “What to try”, press Select F14 to see the feature, and set a value that works. If you opened a file that is already broken, use Undo this change or fix the cause.

Next

Design checks

Design checks test a part against manufacturing rules for 3D printing, 3-axis CNC milling or injection moulding, and show you where it breaks them. This chapter covers the rules, how to run a check, how to read the results, and how to change the limits or make a rule stop edits that make things worse.

A check never changes your model, and nothing runs on its own unless you switch on Check after every edit or set a rule to Block. The rules are a first set of useful tests, not a certification of manufacturability.

Run a check

  1. Open the drawer (backslash key, or the drawer button at the right of the status bar) and choose the Check tab.
  2. Pick a Profile: FDM 3D printing, CNC milling, 3 axis, or Injection moulding.
  3. Press Run check.

The list groups the issues by severity with counts: Errors, Warnings and Notes. Each row shows the rule, a sentence with the numbers, and “measured / limit” with the unit. “No issues found.” means every rule passed.

  • Click a row to select the faces (or edges) it names and frame them in the view. Point at a row to light them up.
  • Show on part (also the Design issues switch in the Display menu, off by default) tints the faces named by the issues: red for errors, amber for warnings, blue for notes.
  • The status bar shows the result, for example “FDM 3D printing: 2 errors, 5 warnings”. Click it to open the tab. Before your first check there is no chip.
  • When you change the part, the result greys out with “Out of date: the part changed after this check. Run it again.”, the tint disappears and rows stop being clickable until you run it again.

Each rule reports at most 100 issues. If there are more, a line says how many were left out.

The rules

The rules come from the kernel. These are the rules and default limits of this version.

FDM 3D printing

RuleWhat it checksDefault limits
WatertightThe body is one closed shell with no open or non-manifold edges and no inside-out solids. Exact.
Single solidThe part is one solid; several solids print as separate pieces. Exact.At most 1 solid
Minimum wall thicknessWall thickness, found by casting rays inward from points on the surface. Sampled, so a very thin sliver can be missed.1.2 mm
OverhangDownward faces steeper than a limit, measured from vertical (0 is a wall, 90 a flat ceiling), against the build direction. Faces on the build plate are ignored.45 degrees, build direction up (0, 1, 0), ignore patches under 0.5 mm²
Bridge spanFlat downward faces above the plate, reported by their narrowest width.10 mm, face counts as flat within 10 degrees
Minimum feature sizeHole and pin diameters (exact) and gaps between facing walls (sampled).0.8 mm diameter, 0.8 mm gap
Build plate contactThe flat area touching the build plate.At least 20 mm²

CNC milling, 3 axis

The profile assumes a single setup with the tool approaching from +Z.

RuleWhat it checksDefault limits
WatertightAs above.
Minimum internal radiusVertical internal corners smaller than the cutter radius. Sharp inside edges count as radius 0; drilled holes are not corners.1 mm, tool axis (0, 0, 1)
Minimum wall thicknessAs above.1 mm
Undercut / tool accessFaces the tool cannot reach: facing away from it, or hidden under another part of the body.Direction (0, 0, 1), ignore patches under 0.5 mm²

Injection moulding

The profile assumes a two-part mould pulled along +Z.

RuleWhat it checksDefault limits
WatertightAs above.
Draft angleThe angle of each wall against the pull direction. A face is flagged when at least half of its area is under the limit.1 degree, pull (0, 0, 1), ignore faces under 0.5 mm²
Uniform wall thicknessWall thickness compared with the part’s median. Sampled.Within 0.25 (25 percent) of the median
Minimum wall thicknessAs above.0.8 mm
Undercut (two-part mould)Faces that neither mould half can form: hidden under other material both looking along the pull direction and against it. The wall of a hole drilled across the pull, or a slot open to the side, is one. A face only one half can see is fine, that half forms it. Sampled.Pull (0, 0, 1) and its opposite, ignore patches under 0.5 mm²

Not covered yet: sheet-metal rules, rules of your own, draft direction signs and parting lines, tool reach and stock, support volume, and a suggestion for the best build orientation.

How exact the rules are

  • Exact from the model: hole and pin diameters, concave cylinder radii and sharp inside edges parallel to the tool axis, watertightness and the solid count.
  • Based on the display triangles: overhang, bridge, plate contact, draft and the facing-away half of undercut. These are exact for flat faces; for curved faces they are measured per triangle with an error of about 0.04 percent of the part’s diagonal.
  • Sampled: minimum wall, the gap half of minimum feature, the hidden half of undercut and uniform wall. A feature thinner than the sample spacing can be missed, and thickness is the straight distance along the surface normal.

The printing rules start with the build direction along the model’s +Y axis (0, 1, 0), while the CNC and moulding rules start along +Z (0, 0, 1). These are model directions, not camera directions. Set the direction vector to the way you will actually print, machine or mould the part, or the results will be wrong for you.

Rule modes and limits

Open Rules and limits to see every rule of the profile. Each has a mode and its limits.

ModeEffect
OffThe rule is not checked.
InfoProblems are listed as notes.
WarnProblems are listed as warnings.
BlockProblems are listed as errors, and edits that make them worse are rejected (see below).

Rules start as Warn (a few rules in a profile start as Info), so nothing blocks an edit until you choose Block. Limits are number fields with their unit; the build or tool direction is three fields for x, y and z. A limit is kept within the range the rule allows. Reset to profile puts every rule back to the starting mode and limits. Your settings are kept per profile in this browser, together with the profile you last used and the state of Check after every edit. They are not saved in the part file.

Check after every edit

Tick Check after every edit and the active profile runs about 0.4 seconds after you finish each edit, never two at once; the chip and the tab update. It is off by default. A check on a large part can take a while, and the status shows the busy overlay with a cancel button while it runs.

Block: stop edits that make things worse

When a rule is set to Block, the app compares the check before and after each committed feature edit (Confirm in an editor, tree commands, delete, redo). If a Block rule now has more issues than before, on faces or edges that were not flagged before, the edit is rejected: it is undone, no history entry is added, and a message names the rule and the numbers, for example:

Edit rejected, it would break a Block rule: Overhang: 62 degrees on F5.S.e2, limit 45

Things to know:

  • Violations that were already there never block, so a part that is not perfect yet can still be edited.
  • Sketch confirmations and previews are never blocked, only committed feature edits.
  • If the check itself fails or is cancelled, the edit is kept.
  • The comparison uses the last check of the current state, or one the app makes just before the edit.

Next

The Library

This chapter covers the Library picker in the top bar (the bundled sample parts and the libraries you added, in one list), the Libraries tab of the Catalog (parts you can drop into a model), how to add libraries of your own, and how licences and thumbnails work.

The Library picker

The Library button in the top bar is the place to open a whole part. It lists the bundled samples and the parts of every library you added, grouped by library. Samples are complete example parts that ship with the app: use them to see how a feature is built or as a starting point.

  1. Click the Library button in the top bar (the icon right of the file menu), or press F to open command search and type “library”.
  2. Narrow the list with the filter bar above it (search, category, tags). The same bar is in the Catalog’s Libraries tab.
  3. Click a part. It opens as a new document (click the card itself; this stays the default). If the current document has unsaved changes, the app asks first what to do with them. A part from a library whose licence you have not confirmed yet asks for that confirmation first (see Licences).

To put a part into the document you already have open, press Insert into this part under its card instead. The Library closes and the part is armed exactly as if you had clicked it in the Catalog’s Libraries tab: move over the model, click a face or plane to place it there (the Placement options and Esc work as in the Catalog), and the whole insertion is one undo step. The button is greyed out when no document is open. A part from a library whose licence you have not confirmed yet asks for that confirmation first.

When the filter box is empty, the dialog also lists your recent files and samples above the list, newest first, each with a picture. A file you saved from the app carries a small picture of itself, so its card shows the part instead of a placeholder. Press Esc or Close to leave the dialog.

A sample is an ordinary part. Edit it, save it under a new name with Save as, and the sample itself is never changed.

Manage libraries

Manage libraries (in the Library picker, and in the Catalog’s Libraries tab) lists every library with its part count and licence. For each one you can:

  • Disable or Enable it. A disabled library stays in the list but its parts are hidden from the Library picker and from the Catalog.
  • Refresh it (an added library): fetch its list again.
  • Remove it (an added library): drop it and the files kept for it on this device.

+ Add library in the same place adds a library from a github:owner/repo address, an https address or a folder, with a preview and the licence confirmation before anything is added.

The two places overlap. The Library picker opens a part as a new document, or hands it to the same placement as the Catalog (Insert into this part). The Catalog’s Libraries tab adds a part to the document you have open: drag a card onto a face or plane, or click it and then a face.

The Catalog and its two tabs

Parts you drop into a model live in the Catalog panel. Open it with the Catalog command (key Shift+K; ribbon: Home tab, Create group), or open the Catalog tab of the side panel. The Catalog needs an open document; with none, it says “Open a part to use the catalog.”

The Catalog has two tabs:

  • Primitives: plain shapes (block, cylinder, hole and so on) that you drop onto faces. See Catalog parts.
  • Libraries: one searchable list of parametric parts, bundled samples, and the libraries you have added (the same libraries as the Library picker).

Each library entry is a card with a picture, a name and a mark:

MarkMeaning
IncludedShips with the app: the parametric catalog parts and the bundled samples.
Add-onComes from a library you added.

Add-on cards also show a cloud icon while the part is not stored on your device, and Installed once it is.

Finding a part

The search box, the category list and the tag chips are the same in the Library picker and in the Libraries tab (see The filter bar). The chips All, Included and Add-ons (Libraries tab) limit the list by origin. The list shows 60 cards at a time; choose Show more for the next page.

The filter bar

One bar, two places: above the list in the Library picker and at the top of the Catalog’s Libraries tab.

  • Search. Type words; every word must appear in the part’s title, id, category (the category as the library wrote it, and its group name such as “Pipe & fluid”), tags or, for samples, description. The text in the box is kept when you close and reopen the picker.
  • Category. The menu lists the categories with the number of parts in each, for what the other filters leave (so choosing a tag updates the counts). The bundled samples use twelve groups: Fasteners, Power transmission, Motors & electronics, Pipe & fluid, Fans & impellers, Mechanisms, Brackets & structure, Enclosures, Sheet metal, Consumer products, 3D printing and Marine. A library’s own category (say “tubing & pipe” or “fasteners”) is shown as the library wrote it, and is also filed under the matching group above when its name matches one of a small set of known words (case, “&” versus “and” and plurals do not matter). A category the app does not recognise stays as it is. A category with fewer than three parts folds into Other in the menu; those parts keep their own category and search still finds them by it.
  • Tags. Under the menu, the tags of the parts now shown appear as chips with a count. Click a chip to require that tag; click several and a part must have all of them. Twelve chips show at first; More tags shows the rest. Clear filters appears as soon as something is set and clears the search, the category and the tags.
  • Remembered. The last category and tags are remembered on this device, separately for the picker and for the Libraries tab. If the browser blocks storage the bar simply starts clean each time. A remembered category or tag that no library offers any more is ignored.
  • Make one with a wizard. With Fasteners chosen (or the tag bearing selected), a link above the chips opens the wizard that builds that kind of part, the Screw wizard or the Bearing wizard. It needs an open document, like the wizards themselves.

Putting a part in your model

There are two ways to bring a library part into the open document, and they differ in where the part ends up.

Drag it where you want it

Drag a card onto the model. A translucent preview follows the pointer and shows the real result. Release to drop it; release off the canvas or press Esc to cancel and nothing is written.

You can also click a card, then click a face. Hold Alt to turn snapping off.

Where it lands:

  • On a face, the part stands on that face, with its own up direction along the face normal. The drop point becomes the part’s origin.
  • On a datum plane, a plane row in the feature tree, or empty ground, it goes onto that plane at the pointer. The first body goes on the ground plane.
  • The Placement row applies in part. Direction: Down hangs the part below the plane (ground and plane drops only). Rotate turns the part about the plane normal when you drop it on a plane or the ground. On a face, Rotate has no effect because it would turn the body the part stands on; the app tells you the part keeps its orientation. Mirror is not applied to library parts.

The drop is one undo step. The part’s variables are given a unique prefix so they do not collide with yours, and its feature ids are renumbered.

If the part is not stored on your device, the app fetches it first, shows a “Fetching…” spinner, and checks it. If the fetch fails you get an error message and nothing changes.

Insert at the part’s own origin

Click a card to select it. The detail panel shows the library, licence, category, tags and size, with links to the part and library pages, and four buttons:

ButtonWhat it does
InsertAdds the part to the open document at its own origin, as one undo step. Disabled when no document is open.
Open as new documentOpens the part as a new document, with its provenance recorded.
DownloadSaves the part as a .ckpart file on your computer.
InstallKeeps the part on this device so it works offline. Shown only for add-on parts that are not installed yet.

Use Insert when you want the part exactly where it was designed. Use a drag when you want to choose the place.

Inserting versus opening

Insert or dropOpen as new document
ResultThe part’s features join the open documentA new document holding only the part
UndoOne stepNot applicable
VariablesPrefixed, so they never collideKept as they are
Appearance (colours, body names, saved view)Not carried overKept

Both record where the part came from. The Libraries tab lists, under “Parts from libraries in this document”, each inserted part with its library and licence. An inserted part that you undo drops out of the list.

When a part stays at its origin

The app moves a dropped part only when it can do so safely. In these cases it leaves the part at its own origin and tells you why:

  • The target face is curved.
  • The part is drawn on several different standard planes, or on planes derived in ways other than an offset.
  • The part uses fixed directions of the document, such as a pattern along a world axis.
  • The part is an assembly (it holds inserted components and mates).
  • You dropped it on a plane feature and the part refers to edges.

If you need a different orientation on a face, drop or insert the part and then move it with the move / rotate ball.

Adding a library

You can add a library from a GitHub repository, a web address, or a folder on your computer. A library is data only: part files and a list. Nothing downloaded from a library is ever run.

  1. On the Libraries tab, or under Manage libraries in the Library picker, choose + Add library.
  2. Enter one of:
    • github:owner/repo, optionally with @branch-or-tag (for example github:owner/repo@v1.0).
    • The https address of a library.json file.
    • Pick a folder… and choose a folder that holds a library.json and the part files it lists.
  3. Choose Fetch. The dialog shows the library name, the number of parts, its licence, and how many parts have no picture.
  4. If the licence needs confirmation, tick I understand this licence applies to parts taken from this library.
  5. Choose Add library.

Notes:

  • Only https addresses are accepted. Addresses that redirect to a non-HTTPS address are refused.
  • GitHub libraries are read from the repository’s public files. Private repositories are not supported.
  • A branch can move. Give a tag or a commit when you want a fixed version. Each part’s checksum is checked either way, and a part that does not match its listed checksum or size is refused.
  • A folder library is remembered only through the copy saved when you added it. To refresh it, add the folder again.

Managing libraries

Expand Manage libraries under the list. Each library has a row with its mark, part count, licence and a link to its page. For add-on libraries:

  • Refresh fetches the list again.
  • Remove library removes it and its saved files from this device.

Without a network, the saved list and the parts you installed keep working, and an offline badge appears on the library.

Installing for offline use

Choose Install on a card (it appears on hover) or in the detail panel. The part is downloaded, verified and kept on your device (in the browser’s storage). Dropping or inserting a part also saves it. See Install as an app and work offline.

Licences

Every library, and optionally each part, states a licence. The app compares it with a list of permissive licences (MIT, BSD, 0BSD, Apache-2.0, ISC, CC0, CC-BY, OFL, Unlicense, Zlib and combinations of only these).

For any other licence, or none at all, the app asks you once per library and licence to confirm before you use a part: “parts taken from this library may carry its terms.” Your choice is remembered on this device and is never written into documents. This is a notice, not legal advice. Check a library’s terms yourself before you use its parts in a product. The bundled samples are never asked about.

Thumbnails

Each card has a picture:

  • The parametric catalog parts and the bundled samples have pictures prepared in advance.
  • Add-on parts use the picture the library lists. When it lists none, a part file saved by this app carries its own picture (its thumbnail field) and that is used once the part is on your device, as long as it still matches the part.
  • A part with no picture gets one drawn on your device once it is installed, in the background when the browser is idle. Until then, and for parts that are not installed, the card shows a placeholder with its category icon.

A library without pictures still works. It only looks plainer.

Limits

  • Mirror does not apply to library parts, and Rotate and Direction apply only to drops on a plane or the ground, not on a face.
  • A part drawn on several planes, or tied to fixed world directions, cannot be moved when dropped. It lands at its own origin.
  • Appearance is not carried into the document on Insert. Open the part as a new document to keep it.
  • There is no download progress bar; a spinner shows while a part is fetched.
  • No GitHub token support, so no private repositories.
  • Parts that cannot be fetched while offline give “This part is not saved on this device and there is no network.”

Next

Parametric wizards

This chapter covers the commands that build a whole part from a few parameters: gears (spur, ring, helical, herringbone and rack), propellers (airfoil and marine), turbo impellers, ball bearings, screws, washers, nuts, standoffs, heat-set inserts, springs, a two-part case, grid trays and bins, knurls, and corner holes on a plate. Each one produces ordinary features that you can inspect and edit afterwards.

All of these are about geometry only. The app does not calculate strength, lubrication, or aerodynamic or hydrodynamic performance.

What the wizards have in common

  • They live on the Features tab, Create group. The Gear button is a family: Gear (default, shortcut Shift+Y), Gear pair, Propeller, Impeller, Knurl, Screw, Washer, Nut, Standoff, Heat-set insert, Spring, Case, Tray and Bearing share one ribbon button, and the button shows the one you used last. You can also search for them with command search (F).
  • You need an open document. The commands are greyed out without one.
  • A live preview shows in the viewport while you change values.
  • A readout and checks show the derived numbers. Errors stop the build. Warnings do not.
  • The settings are stored on the part, so you can reopen the wizard later and change them. The features are regenerated from the settings, keeping their ids, so later features that refer to them keep working.

Whether a wizard’s result moves when you edit the part it sits on depends on the wizard. A bearing added from a selected flat face stays on that face (see Bearings), and a knurl cut into a cylinder keeps its distance from the cylinder’s end face (see Knurl). The other wizards (Gear, Propeller, Impeller, Screw, Washer, Nut, Standoff, Heat-set insert, Spring) are built at the numbers you gave.

Parts built by a wizard are not locked. You can add fillets, cuts and patterns on top. What you cannot do is edit the generated profile sketch by hand while it is still tied to its wizard (see each section).

Gears

Gear builds a parametric gear from a true involute tooth profile. Gear pair builds two meshing gears at the right centre distance. Both are one undo step, and the Gear editor opens on the result with a live preview. Press Enter or the tick to keep it, or Esc or the cross to cancel.

Where the gear goes

  • With one face selected, the gear is built on that face.
  • With a plane feature selected in the tree, it is built on that plane.
  • Otherwise it is built on the Top plane.

A new gear starts as a spur gear: module 2, 20 teeth, 20 degree pressure angle, face width 10, bore 8, no hub. Gear pair starts with the same gear plus a 40-tooth mate with a 10 mm bore and a backlash of 0.06 of the module.

Gear types

TypeWhat you get
SpurExternal straight-toothed gear.
RingInternal gear: a rim with the teeth cut on the inside. No keyway or hub. Root fillet is not applied.
HelicalExternal gear whose teeth twist, built as a real twisted extrude. Has helix angle and hand.
HerringboneDouble-helical gear: two opposed helices, with an optional groove between them.
RackA straight rack of the given number of teeth. No bore, hub or mate.

Bevel and worm gears are not built by the Gear command. The sample list includes a bevel gear and a worm screw that were modelled by hand.

Parameters

ParameterWhat it doesDefaultRange and notes
SizingChoose Module or Diametral pitch.ModuleDiametral pitch converts as module = 25.4 / pitch.
ModuleTooth size in mm.20.1 or more.
Diametral pitchTeeth per inch, when sizing is by pitch.12.70.5 or more.
TeethNumber of teeth.206 or more. For a rack it is the number of teeth along it, 1 or more.
Pressure angleFlank angle.20 deg10 to 30.
Face widthThickness of the gear. For a herringbone, the total.10 mm0.1 or more.
Helix angleTooth twist (helical and herringbone).15 deg1 to 45. A herringbone starts at 30 and warns outside 15 to 45.
HandHelical: Right or Left. Herringbone: Apex leading or Apex trailing.RightA mating gear takes the opposite hand.
Centre grooveHerringbone: width of the groove between the two chevrons. 0 means none.About 3 x module when you switch to herringboneThe groove leaves a web at the root, so the two halves stay joined.
Rim thicknessRing gear: radial thickness beyond the tooth roots.0, meaning 2.5 x module0 or more.
Bore diameterShaft hole through the gear.8 mm0 means no bore.
KeywayCuts a keyway in the bore.OffNeeds a bore.
Key width and depthKeyway size.0, meaning “by shaft size”The default follows the common DIN 6885 table for the bore size. Type your own values to override.
Hub diameter and lengthOptional boss on the gear.0 (no hub)Length is measured from the front face. For a herringbone, the hub is centred on the mid plane.
AddendumTooth height above the pitch circle, as a multiple of the module.10.2 or more.
DedendumTooth depth below the pitch circle, as a multiple of the module.1.250.2 or more.
Root filletRadius at the tooth root, as a multiple of the module.0.30 to 0.6. 0 gives a sharp root.
Profile shiftShifts the cutter. Positive thickens the tooth and raises the tip.0-1 to 1.5.
BacklashTooth thickness removed at the pitch circle by this gear, in mm.00 or more.

Helical and herringbone gears use the module and pressure angle as normal values; the app converts them to the profile in the plane of rotation.

Adding a mating gear

For spur, helical and herringbone gears, tick Add a mating gear in the Mating gear section. It takes the module, pressure angle, width, profile shift and backlash from the first gear and has its own tooth count, bore and hub. The editor shows the centre distance and the gear ratio.

Ticking the box starts the mate at twice the teeth and, if the backlash was 0, sets it to 0.06 of the module so the flanks do not touch. The two gears are separate solids in one part, not an assembly.

The readout and its warnings

The Readout section shows the pitch, outside, root and base diameters (a rack shows circular pitch and length), the contact ratio, and the minimum number of teeth that avoids undercut.

The contact ratio is measured against the mating gear. With no mate, it uses a gear with the same number of teeth. A value of 1.2 or more runs smoothly. For helical and herringbone gears the total includes overlap.

WarningWhat to do
Fewer teeth than the minimum for no undercut (18 at 20 degrees and a standard addendum)Add teeth, or press Use shift to apply the profile shift that avoids undercut.
Teeth come to a pointRaise the module or tooth count, or lower the addendum or profile shift.
Tip lowered to keep a landSame remedy as above.
Teeth touch at the rootReduce backlash, profile shift or dedendum.
Ring tip circle below base circleThe ring’s teeth were shortened. Change the tooth count or the shift.
Herringbone helix angle outside 15 to 45Choose an angle in that range.
Half the face width twists more than a quarter turnLower the helix angle or the face width.
Groove at least as wide as the faceLower the groove or widen the face.

What is built

Gear parts are made of ordinary features: a profile sketch (the closed tooth outline), an extrude for the body, and optionally a hub, a groove (herringbone), a bore and a keyway. A pair repeats these for the second gear. A helical gear uses the extrude’s twist. A herringbone uses two extrudes with opposite twist, up and down from the mid plane.

Editing a gear afterwards

Double-click any feature the gear made in the feature tree, and the Gear editor opens on the settings. The features are regenerated with the same ids. You cannot edit the profile sketch by hand while it belongs to the gear. To take it over, delete the gear’s settings by editing the part file, or rebuild the shape from a copy of the sketch.

Large gears take time to rebuild. Cost grows roughly in line with the tooth count, and a herringbone costs about twice a helical gear of the same size. The preview waits until you stop typing before it rebuilds.

Propellers

The Propeller command opens a three-step wizard in the Editor tab of the left panel: Size, Blade and Review. You can also start it from the Catalog: Primitives tab, Generators, Propeller.

On the Size step, Family selects what kind of propeller you make. You choose the family for a new propeller only. An existing propeller reopens in the family that made it.

FamilyUse it for
AirfoilFans, drones and aircraft: airfoil sections lofted into a blade.
MarineBoat propellers: the blade face lies on a helicoid, with the thickness on the back.

On the Review step, Create adds the propeller as one undo step. When you reopen a built propeller, the button says Apply and regenerates it.

The shaft axis is Z, the thrust is toward +Z, and the first blade lies along +X.

Airfoil propeller

Presets on the Size step: Drone 5 inch, Desk fan and RC plane. Custom is the default.

Size step

ParameterWhat it doesDefaultRange
DiameterTip diameter.120 mm10 mm or more.
Hub diameterCentral boss.24 mmAbove 0 and at most 60 % of the diameter.
Hub lengthHub length along the shaft.20 mmAbove 0.
Bore diameterShaft hole. 0 means none.6 mmLeaves at least 1 mm of hub wall, and stays inside the blade roots.
BladesNumber of blades.32 to 8.
RotationCounter-clockwise or Clockwise, seen from the thrust side (+Z).Counter-clockwise

Blade step

ParameterWhat it doesDefaultRange
TwistHow the blade angle varies along the span: Pitch (constant pitch), Pitch angle (the same law set by an angle), or Linear (straight line from root angle to tip angle).Pitch
PitchDistance advanced per revolution.90 mm/revAbove 0.
Angle at reference, Reference radiusPitch angle and where it is measured, as a fraction of the tip radius.20 deg at 0.75Angle up to 80 deg. Radius 0.25 to 1.
Root angle, Tip angleLinear twist ends.55 and 12 degUp to 80 deg.
Root, mid and tip chordBlade width along the span. Drag the three points on the Chord curve graph, or type values.18, 20, 9 mmAt least 1 mm.
Thickness at root, mid and tipThickness as a fraction of the chord, on the Thickness curve.0.14, 0.10, 0.060.02 to 0.4.
Shape exponentMoves the mid value toward the root (below 1) or the tip (above 1). One for chord, one for thickness.10.2 to 5.
AirfoilNACA 4-digit, Circular arc, or Flat plate.NACA 4-digit
CamberSection curvature as a fraction of the chord.0.040 to 0.12.
Camber positionNACA 4-digit only.0.40.1 to 0.9.
PivotChordwise point the sections turn about. 0 is the leading edge.0.40 to 1.
RakeBackward sweep out of the plane of rotation.0 deg-45 to 45.
SkewSideways offset of the tip toward the trailing side.0 mmWithin half the radius.
Root embedWhere the blade starts inside the hub, as a fraction of the hub radius.0.60.3 to 0.9.
SectionsAirfoil sections the blade passes through. More follows the twist more closely and builds more slowly.75 to 12.

Drag a point on a graph up or down, or focus a point and use the arrow keys (hold Shift for bigger steps).

Review step

The readout gives the diameter, blade count, pitch, pitch-to-diameter ratio, section angles at the root, at 0.7 R and at the tip, and the blade area ratio. Checks list errors (these disable Create) and warnings, for example blades that overlap at the hub, a root deeper than the hub, or a tip too thin to print.

What is built, and how to edit it

The hub is a circle extruded on the mid plane. Each blade section is a sketch of two splines on its own plane. The blade is a loft through the sections, joined to the hub, repeated as a circular pattern, and a bore is cut.

Hub diameter, hub length, bore and blade count are named variables (prop_hub_d, prop_hub_len, prop_bore_d, prop_blades). Edit them in the Variables panel to rebuild just the hub and bore. The blade shape itself is part of the generated sketches, so change it in the wizard. If you change the hub radius in Variables so the blade roots poke out, change the hub in the wizard instead; it moves the roots with it.

Double-click any propeller feature to reopen the wizard.

Marine propeller

Choose Marine under Family on the Size step. The wizard has the same three steps. Presets: Outboard, 3 blades, Inboard, 4 blades, Quiet, 5 blades skewed.

Size step

ParameterWhat it doesDefaultRange
DiameterTip diameter.250 mmAbove 0.
Hub diameterCentral boss.50 mmAbove 0 and below 60 % of the diameter.
Hub lengthHub length.110 mmLong enough to hold the blade roots. The review tells you how long if it is too short.
Bore diameterShaft hole.20 mmMust leave a wall (under 90 % of the hub).
BladesNumber of blades.32 to 6.
RotationRight-hand or Left-hand. Left is the mirror of right.Right-hand

Blade step

ParameterWhat it doesDefaultRange
Pitch / diameterPitch at the tip divided by the diameter.10.4 to 2.
Progressive pitchHow much the pitch changes from tip to root. Positive means more pitch at the hub.0-0.15 to 0.5.
RakeThe blade leans aft by this angle. Negative leans it forward.0 deg-20 to 30.
Expanded area ratioTotal developed blade area over disc area. Sets the widest chord.0.50.25 to 1.2.
Widest chord atWhere the blade is widest, from the hub (0) to the tip (1).0.450.05 to 0.95.
Root chord, Tip chordWidths at the ends, as a fraction of the widest chord.0.55, 0.30.05 to 1.
Tip skewSweep back of the mid-chord line at the tip.15 deg-45 to 45. A warning above 45.
Thickness at the root, at the tip (t / D)Blade thickness as a fraction of the diameter, normal to the face. All of it is on the back.0.035, 0.0050.005 to 0.08 at the root, 0.001 to 0.04 at the tip.
Thickest atWhere along the chord the foil is thickest.0.450.2 to 0.7.
Edge thicknessEdge thickness as a fraction of the maximum. The edge is never thinner than 0.3 mm.0.060.02 to 0.5.
Tip roundingOuter share of the span over which the tip closes to a round end. 0 keeps a square tip.0.150 to 0.4.
Root embedWhere the blade starts inside the hub.0.850.35 to 0.95.
Section spacingAngle between the helicoid sections. Finer follows the outline better.3 deg3 to 10.

Marine: what to expect

  • The blade is one loft through closed sections in planes through the shaft, joined to the hub, patterned, and bored. Hub diameter, bore and blade count are plain numbers, not document variables.
  • With rake and progressive pitch at 0, the face is a true constant-pitch helicoid.
  • Joining the blade to the hub is the touchy step. If the preview fails, the wizard retries with section spacings of 7, 6, 4 and 3 degrees and tells you which one built (“The hub fuse failed at … degrees; built with a section spacing of …”). If nothing builds, try a pitch/diameter above 0.8 or a coarser spacing by hand.
  • A warning tells you when the pitch at the hub is 0.8 D or lower, because those are the cases most likely to need a retry.
  • Editing a marine propeller usually changes the section count, so Apply removes the old features and adds new ones, and takes two undo steps. An edit that keeps the section count replaces them in place, in one step.
  • A rake of about 25 degrees or more can leave a few small gaps in the display mesh. The solid is still valid, but the Check panel may list them.

Turbo impellers

The Impeller command builds an open radial compressor wheel: a shaped hub, back-swept main blades, shorter splitter blades between them, and a shaft bore. The wizard has three steps: Hub, Blade and Review, opened in the Editor tab of the left panel. Presets: Compressor, 7 + 7 blades (the default), Small compressor, 5 + 5 blades, Wide, 9 + 9 blades, more wrap.

Hub step

ParameterWhat it doesDefaultRange
Exducer diameterHub diameter at the back face (the wheel exit).45 mmAbove 0.
Inducer diameterHub diameter at the nose plane (the inlet).20 mmAbove 0 and below the exducer diameter.
Hub lengthAxial length from the nose to the back face.16 mmAbove 0.
Bore diameterShaft bore. 0 means none.8 mmMust leave a wall in the hub.
Main bladesFull-length blades.73 to 12.
Splitter bladesShort blades between the main ones.70 up to the main blade count.

Blade step

ParameterWhat it doesDefaultRange
Total wrapHow far each blade winds around the axis.75 deg20 to 160 (a warning above 120).
Blade thickness at the hubTangential thickness where the blade meets the hub.2.5 mmAbove 0 (the field minimum is 0.3).
Blade thickness at the tipTangential thickness at the shroud end.0.8 mmAt least 0.2 mm. A warning below 0.5 mm.
Splitter startWhere splitters begin along the flow path (0 is the nose, 1 the back face).0.450.15 to 0.85.
Section line, axial and radialReach of the hub-to-shroud line each blade section follows.0.6 and 2.2 mmAbove 0 in both.
Root embedHow far the blade roots sit below the hub surface, so the join holds.1.0 mm0.3 to 3.
Sections per bladeSections the blade passes through.128 to 24 (10 to 16 is the suggested range).

The review step reports the radii, blade counts, wrap, section line length and tip pitch, and lists errors and warnings. If a preview fails, the wizard retries with 12, 10 and then 14 sections and tells you which count built.

Limits and editing

  • There is one meridional blade shape. There is no leading-edge sweep, no changing wrap along the span, and no shroud surface. The hub contour’s knee is fixed at 75 % of the length.
  • Blades are joined to the hub without a root fillet.
  • Reopen the wizard by clicking any feature the impeller made.

Bearings

Bearing adds a ball bearing as ordinary features: an inner ring, an outer ring and, for an open bearing, the balls. Start it from Features > Create, command search, or the Catalog: Primitives tab, Generators, Bearing. The live preview shows the bearing before Add bearing keeps it as one undo step.

The Size list holds the nominal ISO 15 dimensions (bore x outer diameter x width) of the miniature 6xx series (602 to 629), the MR miniature series (MR52 to MR149), the 60xx, 62xx and 63xx series (bores 10 to 60 mm) and some inch sizes (R2 with its 1/8 inch bore, R3, R4, R6, R8, R10, R12). Type in Search to narrow the list: 620 lists 6200 to 6209, 8x22 finds the 608, and a whole designation such as 6204-2RS or MR63ZZ picks that size and its sides. Typing a bore, outer diameter or width by hand makes it a custom size.

ParameterWhat it doesDefault
SidesOpen shows the balls, Shielded (2Z) is a flat disc on each face, Sealed (2RS) is a thicker seal with a sloping lip.Shielded
ChamferChamfer on all four corners of each ring. 0 leaves them sharp.By size (0.1 mm for the smallest, 0.3 mm for a 608, 1 mm for a 6204 or larger)
Balls, Ball diameterOpen bearings only.The diameter is just under the gap between the races, the count about 1.6 ball diameters of pitch
First face centre, ExtendsWhere the first face sits and which way the bearing runs from it.Origin, up (+Z)

Each ring and each ball is its own body (named, for example, Bearing 608 inner ring), and a shield or seal belongs to the outer ring. Each ring has a ball groove (a circular arc about the ball centre circle, radius 0.52 ball diameters and 0.27 deep, so the balls sit in it); a bearing too small for one gets plain races. There is no cage, and the ring, groove, ball and shield sizes follow rules of thumb rather than a maker’s catalogue. Use it for assemblies, fit checks and looks, not for load ratings.

Housing seat

The Housing seat read-out gives the pocket for the outer ring: its diameter with the fit allowance, and the bearing width as the depth. Fit chooses H7 housing (cut at the middle of the +IT7 / 0 zone of ISO 286), Nominal (press fit) (the outer diameter itself) or 0.2 mm clearance (for a printed pocket). Select a flat face before you open Bearing and the bearing is placed on that face, running into the body; tick Cut this pocket in the picked face and the pocket is cut first, then the bearing is added in it.

Following the face

A bearing added from a selected flat face stays on that face. Put a bearing at each end of a 30 mm shaft, then change the shaft length to 20 mm in the extrude: the bearing and its pocket at the far end move with the end face, and changing the length back moves them back. The same holds for a plate that gets thicker or thinner. The face must be flat and face along the X, Y or Z axis, and the bearing keeps its distance from the face’s own origin, so it follows the face along its normal but not when you move the shaft sideways in its sketch.

What does not follow: a bearing placed by typing its numbers without a selected face, one whose first face centre or direction you changed by hand (only sliding it across the face keeps it attached), one on a tilted face, and bearings made in an earlier version, which stay at the position they were made at. Delete such a bearing and add it again from the face to attach it. If an edit leaves a seat that no longer touches the part, the failure card says so and suggests this.

In the Script tab: part('Housing').bearing({ designation: '608', seal: '2RS', origin: [0, 0, 10], axis: [0, 0, -1], seat: true }); add onFace: 'F2.C1' (the face the bearing sits on) to build it from the face as the wizard does. The Bearings example shows a row of them.

Screws

Screw adds a screw or bolt as ordinary features: one body for the head and shank, then cuts for the drive. Start it from Features > Create, command search, or the Catalog: Primitives tab, Generators, Screw. The preview shows the screw as you change the fields; Add screw keeps it as one undo step, and Escape or the cross cancels. It needs an open document, but no solid: the screw is placed at the numbers you give.

FieldWhat it doesDefault
SizeThe metric size from the list, M2 to M16.M3
LengthThe shank, in millimetres, from the underside of the head to the tip (a countersunk screw: from its flat top).8 mm
HeadPan, Button (dome), Countersunk, Cheese (cylindrical) or External hex. Picking a head sets the drive to the usual one for it.Pan
DriveCross (approximate), Hex socket, Slotted, Torx (approximate) or None. Not shown for an external hex head: that one is turned from outside.Cross
Bearing face centre X, Y, ZWhere the screw sits: the centre of the underside of the head (a countersunk screw: of its flat top), in millimetres.0, 0, 0
Shank pointsWhich way the shank points: Down (-Z), Up (+Z), -X, +X, -Y or +Y.Down (-Z)

Cross and Torx are approximations: the cross is two tapered arms with a blunt tip rather than real Phillips wings, and the Torx is a star that looks the part. They are good for looks, fit checks and mass, not for toleranced drives.

The screw is its own body and does not merge with what it touches; it is listed as Screw in the Bodies panel. Not every size has every head: the table follows the standards, so M12 and M16 have button, countersunk and hex heads only, and a head the size has no row for is refused with the kernel’s message.

There is no thread option: a helical thread on a shank does not build yet. Add one afterwards with Home > Create > Thread on the shank, as for any cylinder (see Holes and threads).

The wizard always starts from the defaults: it does not reopen from the tree. To change a screw, delete the features it made in the Screw folder and add it again.

In the Script tab: screw({ size: 'M5', length: 12, head: 'countersunk', origin: [0, 0, 10], axis: [0, 0, -1] }).

Common problems

SymptomFix
The length is refusedIt must be more than 0, and a countersunk screw’s length includes its head, so it must exceed the head height
A hex head shows no Drive rowA hex head takes no drive: it is turned from outside
“size M12 has no pan head in the table”Not every size has every head. Pick one the size has: M12 and M16 take button, countersunk and hex
The screw sits in the wrong placeThe bearing face centre is the middle of the face it sits on. Check it, and which way the shank points
You want a thread on the shankNot in the wizard: add it with Home > Create > Thread afterwards

Washers

Washer adds a flat or a spring (split) washer as ordinary features: one sketch and one extrude, a separate body, all in one tree folder named Washer (the next one Washer 2). Start it from Features > Create, command search, or the Catalog: Primitives tab, Generators, Washer. The preview shows the washer as you change the fields; Add washer keeps it as one undo step, and Escape or the cross cancels. It needs an open document, but no solid.

FieldWhat it doesDefault
KindFlat, or Spring (split).Flat
Standard / CustomStandard shows a list of sizes with a filter box above it: type M8, 8 or 7089 (every word you type must appear in the row), click a row, or press Enter when one row is left. Picking a row fills the three diameters and the thickness. Custom hides the list. Editing any of the numbers switches to Custom by itself.Standard, M8
Inner diameter, Outer diameter, ThicknessThe size in millimetres.8.4, 16, 1.6
Gap widthSpring only: the width of the split, across it.The thickness
First face centre X, Y, ZThe centre of the washer’s first side, in millimetres. Give a screw the same position and axis and the washer lies under its head.0, 0, 0
Thickness runsWhich way the thickness extends from that side: Down (-Z), Up (+Z), -X, +X, -Y or +Y.Down (-Z)

Washer on a hole

Click Washer on a hole in the wizard, then click the wall of a hole on the part (or its circular edge: press E for edge picking). The wizard reads the hole’s diameter and axis and the flat face it opens on, takes the standard size whose medium clearance hole (ISO 273) the hole contains (a 6.6 mm hole gives M6, 9 mm gives M8, 11 mm gives M10), and places the washer coaxial with the hole, touching that face, in the usual Washer folder. If the hole is smaller than the smallest clearance hole of the standard, the nearest size is used and the panel says so. You can still pick another size, change the kind (the spring washer reads the same hole), choose Custom, and set an Offset from the face to lift the washer off the seat. In a through hole the washer sits on the end you picked, or the upper one; Seat on the other end switches. In a blind hole it sits on the open end, and in a counterbored hole on the counterbore floor. A countersunk or chamfered hole, a hole that is not along the X, Y or Z axis, and a face that is not a hole are refused with a message instead of a guess. Editing the position fields by hand leaves the hole. A screw, washer and nut stack on a hole is not part of this: add the screw separately.

The standard lists are ISO 7089 (normal series, M1.6 to M64; DIN 125 form A has the same sizes), ISO 7093-1 (large series, M3 to M36; DIN 9021 has the same sizes over this range) for flat washers, and DIN 127 B (spring lock washer, M2 to M36) for spring washers: each row shows M8 - 8.4 x 16 x 1.6 (ISO 7089), inner x outer x thickness. A size the tables could not confirm is left out: use Custom.

The spring washer is a flat split ring. The lift (the helical twist of a real one) is not modelled, and the gap is cut square.

The wizard always starts from the defaults: it does not reopen from the tree. To change a washer, delete the features it made in the Washer folder and add it again.

In the Script tab: washer({ inner: 8.4, outer: 16, thickness: 1.6, origin: [0, 0, 4], axis: [0, 0, 1] }), or kind: 'spring', gap: 2 for the split ring.

Common problems

SymptomFix
The list shows “No standard size matches”Clear the filter, or switch to Custom and type the size
The outer diameter is refusedIt must be larger than the inner diameter
The gap is refusedIt must be more than 0 and smaller than the hole

Nuts

Nut adds a hexagon nut as ordinary features: a hexagonal prism as a separate body, the bore cut through it, and a revolve cut that chamfers the corners at 30 degrees on both faces. Start it from Features > Create, command search, or the Catalog: Primitives tab, Generators, Nut. The preview shows the nut as you change the fields; Add nut keeps it as one undo step, and Escape or the cross cancels. Everything goes into one tree folder named Nut (the next one Nut 2), and the body has the same name.

FieldWhat it doesDefault
TypeRegular (ISO 4032), Thin (ISO 4035) or Style 2 (ISO 4033). Style 2 has no sizes below M5: picking it with a smaller size moves to M5.Regular
SizeM2, M2.5, M3, M4, M5, M6, M8, M10, M12, M14 or M16: the metric coarse sizes of the kernel’s thread table that the standard lists.M8
Chamfer the cornersA 30 degree chamfer on both faces, starting from a bearing-face circle of 0.9 times the width across flats. Off leaves a plain prism.On
ThreadPlain bore (a bore at the minor diameter, no thread feature), Cosmetic thread (a bore at the tap drill with a cosmetic thread: it shows in the thread list and drawings) or Modelled thread (the real helical groove).Plain bore
Print clearanceModelled thread only: millimetres, positive for a looser nut thread (the major and minor diameters grow by twice this), negative for a tighter one; up to 1 mm either way.0
First face centre X, Y, ZThe centre of the nut’s first face, in millimetres. Give a screw or a washer the same position and axis and the nut stacks on it.0, 0, 0
Thickness extendsWhich way the thickness runs from that face: Down (-Z), Up (+Z), -X, +X, -Y or +Y.Down (-Z)

The panel shows the width across flats, the width across corners, the thickness and the bore of the size. Those come from the maximum dimensions of ISO 4032, 4035 and 4033, entered from the standards’ public tables and not yet checked against the standard text: the panel says so, and marks the rows that are less certain than the rest (M14, and the thin M2 and M2.5). Compare them with the nut you buy before you rely on a value.

A modelled thread is slow to preview and can fall back to a cosmetic one if the kernel cannot cut it (the thread list says so). A large print clearance on a fine pitch is the usual cause: in testing an M5 nut took 0.1 mm, but 0.2 mm made the kernel fall back to a cosmetic thread. The nut is its own body and does not merge with the screw it sits on. The washer face and the bore countersink of real nuts are not modelled, nor are nyloc rings, flanges and wings.

In the Script tab: nut({ size: 'M5', type: 'thin', thread: 'modeled', clearance: 0.1, origin: [0, 0, 6], axis: [0, 0, 1] }).

Standoffs

Standoff adds a round or hexagonal spacer, female-female or male-female, with its threads, as a separate body in one Standoff folder. It is on the same buttons as the Nut wizard.

FieldWhat it doesDefault
SizeM2, M2.5, M3, M4, M5 or M6. Picking a size fills the outside size and the thread length with the usual values for it.M3
ShapeRound or Hex.Round
EndsFemale - female (a threaded bore in each end) or Male - female (a bore in the first end and a stud on the far one).Female - female
LengthThe length of the body, end to end. A male stud adds to it, and the panel shows the overall length.15 mm
Outside diameter / Width across flatsThe outside size, according to the shape.6 mm (round), 5.5 mm (hex)
Thread lengthThe depth of each female thread and the length of the male stud.6 mm
Thread, Print clearanceAs for the nut. On a stud a positive clearance makes the stud thinner.Plain bore
First end centre X, Y, Z, Standoff extendsWhere the first end sits and which way the standoff extends from it.0, 0, 0, Up (+Z)

The wizard checks what it can without the kernel: the threads must not meet (twice the thread length less than the length for female-female, the thread length less than the length for male-female), and the wall must be at least 0.5 mm, so the outside size is at least the nominal diameter plus 1 mm. A problem blocks Add standoff and says what to change. The outside sizes are typical catalogue values, not a standard: round standoffs of one thread size are sold in several diameters, so enter the one you buy. The ends are square (no chamfers) and the stud is a plain cylinder at the nominal diameter.

In the Script tab: standoff({ size: 'M3', length: 12, kind: 'hex', ends: 'male-female', threadLength: 6, origin: [20, 10, 1.6] }).

Heat-set inserts

Heat-set insert adds the knurled brass insert that is pressed into a printed part with a soldering iron, and, if you ask, the hole for it. The insert is one revolve as a separate body in a Heat-set insert folder: a ring with the bore of the thread and a few groove rings round the outside that stand for the knurl.

FieldWhat it doesDefault
SizeM2, M2.5, M3, M4, M5 or M6. Picking a size fills the next five fields.M3
Outside diameter, LengthThe insert’s size over the knurl and end to end.4.6, 5.7 mm
Hole diameter, Hole depthThe recommended hole in the plastic: a little smaller than the insert, and deeper than it is long to leave room for the displaced plastic.4, 7 mm
Groove ringsThe number of rings round the outside, 0 to 8.3
Thread, Print clearanceAs for the nut.Plain bore
Also cut the holeCuts the recommended hole at the mouth, before the insert is added. Cut it into then lists the bodies of the document: Every body it reaches (the default) or one of them by name.Off
Hole mouth centre X, Y, Z, Insert goesThe centre of the face the insert is pressed into, and the direction it goes in. The insert lies flush with that face.0, 0, 0, Down (-Z)

The values are typical catalogue dimensions, the middle of the ranges that manufacturers publish (for M3: 4.0 to 4.6 mm outside, 4 to 5.7 mm long, a 3.8 to 4.2 mm hole), and not a manufacturer’s drawing: the panel marks them unverified, and the sheet of the insert you buy comes first. The insert is bigger than the hole by the press fit, 0.3 mm on each side for M3. The two bodies overlap by that amount, as they do in reality once the plastic has flowed round the knurl, so an interference check on the pair reports it. To leave out the overlap, set the hole diameter to the outside diameter.

In the Script tab: heatSetInsert({ size: 'M3', hole: true, origin: [0, 0, 12], axis: [0, 0, -1] }) (hole: 'Block' cuts only the body made with that name).

These three wizards always start from the defaults and do not reopen from the tree. To change one, delete the features in its folder and add it again.

Common problems

SymptomFix
“There is no M4 nut in ISO 4033”Style 2 starts at M5: pick Regular or Thin, or a larger size
The two threads would meetThe standoff is too short for two threads: shorten them, lengthen it, or use Male - female
The wall would be under 0.5 mmThe outside size is too small for the thread: use at least the nominal diameter plus 1 mm
The hole is refusedIt must be no larger than the insert’s outside diameter, and at least as deep as the insert is long
A modelled thread comes out cosmeticThe kernel could not cut the groove: lower the print clearance, or use a cosmetic thread

Springs

Spring adds a coil spring as ordinary features: one wire swept along a helix, as a separate body in one tree folder named Spring (the next one Spring 2). Start it from Features > Create, command search, or the Catalog. The preview shows the spring as you change the fields; Add spring keeps it as one undo step, and Escape or the cross cancels. The wizard shows the geometry it derives (the pitch, the gap between turns, the mean diameter and the length of wire for a compression spring; the overall length for an extension spring; the angle between the legs for a torsion spring) and refuses values that would make the turns touch.

FieldWhat it doesDefault
TypeCompression, Extension (hooks) or Torsion (legs).Compression
Outer diameterThe outside diameter of the coil, measured over the wire. An extension spring needs more than three times the wire diameter, for the hook bends.
Wire diameterThe diameter of the wire.
Free lengthCompression only: the length with no load, end to end, wire included.
TurnsHow many times the wire goes round; fractions are fine. For an extension spring it counts the tight body between the hooks; for a torsion spring the fraction after the whole turns sets the angle between the legs.
WindingRight hand or Left hand.Right hand
Far end outer diameterCompression only: a value different from the outer diameter makes the coil a cone.The outer diameter
Pitch ratio, far end : first endCompression only: 1 is an even pitch, below 1 the turns close up towards the far end (a progressive suspension spring), above 1 they open.1
EndsCompression only: Plain (the wire just stops), Closed (tight turns that touch at each end) or Closed and ground (closed turns with both ends ground flat, so the spring is exactly the free length).Plain
Closed turns per endClosed and ground ends only: how many turns at each end touch the next. They count in the turns above, so the body has the turns less twice this many.1
First leg length, Second leg lengthTorsion only: the length of each straight leg, which leaves the coil tangent to its end.
First end centre X, Y, ZWhere the spring starts: the centre of its first end (the lowest point of the lower hook for an extension spring).0, 0, 0
Spring extendsThe direction from that end: Up (+Z), Down (-Z), +X, -X, +Y or -Y.Up (+Z)

An extension spring is a tight coil of touching turns with a machine hook, an open loop centred on the axis, at each end; a fraction of a turn turns the two hooks against each other. A torsion spring is a close-wound coil with a straight leg at each end. Closed and ground takes a quarter of the wire diameter off each end. Closed and ground springs, cones, progressive, extension and torsion springs are wound along a curve and take a few seconds to preview, longer with many turns.

A spring is its own body and does not merge with the part it sits in. Only the geometry is made: the app does not work out the spring rate or the stress, and an extension spring has the machine hook only, no other end types.

In the Script tab: spring({ outer: 12, wire: 1, length: 30, coils: 8, ends: 'ground', closedTurns: 1 }), with topOuter for a cone and progression for a progressive pitch; extensionSpring({ outer: 10, wire: 1, coils: 12 }); and torsionSpring({ outer: 10, wire: 1, coils: 4.25, leg1: 15, leg2: 15 }). All three take hand, origin and axis.

Make a tray or bin

Tray makes a tray or bin on a grid with Gridfinity-style sizes: one grid unit is 42 mm, one height unit 7 mm, and every outside size is 0.5 mm under whole units so neighbours fit. It is one body in a tree folder named Tray: a block of the size you give, with a cavity along its length whose lower edges are rounded by the scoop radius, so small things slide to the front and into the hand. The cavity is open at both ends, so trays can run on, unless you close the ends with a wall. Start it from Features > Create, command search, or the Catalog.

FieldWhat it doesDefault
MakeTray or bin, or Baseplate: a plate with a pocket for every grid cell that a tray’s foot seats in. A baseplate has whole or half units, no tolerance (plates butt), and only these fields: size, plate thickness (default 1.2 mm under the 4.75 mm pockets), pocket clearance (default 0.1 mm all round, which leaves a 0.3 mm ridge between pockets), Split to fit the bed (on: a plate longer than the printer bed is cut into the fewest equal pieces, in whole or half units, that each fit it, one body each named Baseplate 1-1, 2-1, … with square corners; off: one piece and a warning), corner radius, the drawer and printer fields. In the Script tab: gridBaseplate({ widthUnits: 3, lengthUnits: 4 }).Tray or bin
Width, Length, HeightThe size in grid units (whole or half units across and along) and in height units.1, 4, 4
Scoop radiusThe rounding of the lower edges of the cavity. A small radius gives an almost flat bottom, 0 a square one. At most half the inside width and at most the depth of the cavity.8 mm
End wallsNone (an open tray), Front, Back or Both (a bin).None
Wall thickness, Floor thicknessThe side and end walls, and the material under the lowest point of the scoop. At least 0.4 mm.1.2 mm, 1.2 mm
Corner radiusRounds the four vertical outside corners.3.75 mm
Gridfinity footThe stepped base under every grid cell (a 0.8 mm chamfer, 1.8 mm straight, a 2.15 mm chamfer: 4.75 mm in all, inside the height), so the tray seats in a Gridfinity baseplate. The floor is then measured above the foot, so the cavity is 4.75 mm shallower and the scoop must fit in what is left. Needs a corner radius of at least 3.1 mm.On
Magnet holesFour 6 x 2 mm holes, 26 mm apart, in the underside of every whole grid unit. The floor must be at least 2.8 mm (the foot counts toward that).Off
Drawer width, depth, heightThe inside size of your drawer in mm (0 = skip). The panel shows how many units it takes across and along, the height in units, and the space left over; Fill the drawer length sets the length (and the height) to it. A part of n units is n x 42 - 0.5 mm, so a 480 mm drawer takes 11 units and leaves 18.5 mm. Tick half units to fill more of it.Not given
Printer, BedBambu X1 Carbon (256 mm), Creality K1 Max (300 mm) or Custom. The panel warns when the longest side is longer than the bed.256 mm
Grid unit, Height unit, ToleranceThe sizes of the grid, so other grids work too.42, 7, 0.5 mm
Name, Bottom face centre X, Y, ZThe body name and where the tray stands; it rises along +Z.Tray, 0, 0, 0

Checks in plain words block the preview and Add tray until the numbers work: a half unit that is not a half, a wall under 0.4 mm, a scoop that is wider than the cavity or deeper than it, a floor too thin for the magnet holes. The tray is its own body and leaves the bodies already in the document alone.

Not included yet: a stacking flange, dividers and labels, several narrow trays in one module, and splitting a tray longer than the bed into pieces that join.

In the Script tab: gridTray({ widthUnits: 1, lengthUnits: 4, heightUnits: 4, scoopRadius: 8 }) (also foot, endWalls, magnets, wall, floor, cornerRadius, pitch, unitHeight, tolerance, name, origin). The wizard and the helper build the same features.

Make a case

Case makes a closed box with a lipped lid in one step: the outside size, the wall, where the lid starts and the lip, and you get two bodies, a base and a lid, in one tree folder named Case (the next one Case 2). It does what takes several steps by hand and needs no selected face, which the Shell command does: two cups, each an outline extruded as its own body and shelled open on one face, a ring-shaped tongue on the rim of one and a matching groove in the rim of the other, and the lid placed on top of the base. Start it from Features > Create, command search, or the Catalog. The preview shows the base and the lid as you change the fields; Add case keeps them as one undo step, and Escape or the cross cancels.

FieldWhat it doesDefault
Width, Depth, HeightThe outside size of the closed case, lid included, in mm.80, 50, 30
Wall thicknessThe thickness of every wall, the floor and the top. At least 0.4 mm, and two walls must be thinner than the smallest outside size.2
Round the edgesWhich outside edges are rounded: Off, Side edges (the four vertical edges), Top edges (the outer edges of the lid top and of the base bottom, never the seam where the halves meet and never the inside) or Side and top edges. A radius field appears for each edge that is on.Off
Side edge radiusThe radius of the four vertical edges, on the outside. It must be more than the wall, so the inside corner does not collapse, and at most half the width or depth.5
Top edge radiusThe radius of the round on the top of the lid and on the bottom of the base. With both on, the round follows the rounded outline, so it can be at most the side edge radius. It is also limited to about 2.2 times the wall (a bigger round would leave under half a wall at the round) and to less than the height of the shorter half less the groove.2
Lid heightHow tall the lid is: the case is cut this far below its top, so the cut is at height - lid height above the bottom. It starts at a quarter of the height (at least three walls) and follows the height until you type a value.A quarter of the height
Tongue heightHow far the tongue stands out of its half. The groove is this plus the clearance deep. Follows the wall (0.75 of it) until you type a value.1.5
Tongue widthThe width of the tongue as a fraction of the wall, centred in the wall.0.5
ClearanceThe gap between tongue and groove on each side and at the top, in mm. 0.2 suits an FDM printer.0.2
Tongue onLid (the tongue stands out of the lid and the groove is in the base) or Base.Lid
Name of the base, Name of the lidThe names of the two bodies.Base, Lid
Bottom face centre X, Y, ZWhere the case stands: the centre of its bottom face. It rises along +Y from there: the floor is on the Top plane and the lid on top.0, 0, 0

The panel shows the heights of the two halves, where the cut is and the tongue and groove sizes. Checks in plain words block the preview and Add case until the numbers work: a wall under 0.4 mm, a side edge radius that is not more than the wall, a top edge radius above any of the limits in the table, a lid or a base not taller than the wall, a groove that would leave less than a wall under it, a tongue and its clearance on both sides as wide as the wall, or two halves with the same name.

With the defaults and a lid height of 15 mm, the case is the one built in Cases and moulds: two valid bodies of 28 882.24 mm³ together. The case is its own pair of bodies and leaves the bodies already in the document alone, including an earlier case closed at the same height. The tongue is centred in the wall, with the clearance on both sides and above it: the nearest the two halves come to each other, apart from where the rims rest on each other, is the clearance (checked with Evaluate > Overlap and the clearance measurement).

The top edges are rounded after each cup is shelled, so the outside gets the round and the inside stays square: where the radius is bigger than the wall, the wall at the round is thinner than the wall (it is wall x 1.41 - 0.41 x radius thick there, 1.17 mm for a 4 mm round on a 2 mm wall). The tongue and groove are on the seam rim and are not touched, so the fit keeps its clearance.

What it does not make: screw bosses, a seal groove, snap fits, vents or a label recess. Add those afterwards with the ordinary features, cutting into the base or the lid by name.

In the Script tab: caseBox({ width: 80, depth: 50, height: 30, wall: 2, lidHeight: 15, tongueHeight: 1.5, tongueWidth: 1, clearance: 0.2 }) (also radius for the side edges and topRadius for the top edges, each 0 = sharp, tongueOn: 'lid' | 'base', names, origin; axis: 'y' (the default: the case stands on the Top plane and rises along +Y, the app’s up axis) or axis: 'z' (the old orientation: lying on the Front plane, rising along +Z); joint: 'lipJoint' builds one shelled box and splits it with the lip joint instead, in a part with no other body). The wizard and the helper build the same features.

Adding a bolt to a hole

Add fastener to hole puts a bolt in a hole you point at, with a washer and a nut if you want them. The size, the head and the length come from the hole, so for the usual case there is nothing to type.

  1. Select the cylindrical wall of a hole (click it in face mode), or several holes, then right-click and choose Add fastener to hole. The same command is on the Features tab, Create group, and in command search; it is greyed out until a hole wall is selected. In the feature tree, right-click a Hole feature, or a pattern of holes, and choose Add fastener to hole.
  2. The Fasten this hole panel opens with the fasteners already previewed in the viewport. Change what you want:
    • Bolt: Hex head bolt (ISO 4017), Socket cap screw (ISO 4762), Button head (ISO 7380) or Countersunk (ISO 10642). It starts from the mouth of the hole: a plain hole takes a hex bolt, a counterbore a socket cap screw and a countersink a countersunk screw. The panel says which rule applied.
    • Size: the nearest metric size to the bore, M2 to M16. A 5.5 mm bore is M5 clearance, a 4.2 mm bore is M5 tapped; the line under the field says which it matched and the table value it was compared with. When the bore is more than 0.3 mm from every table value the line says nearest, not matched.
    • Length: the material along the hole axis from the bearing face to where the hole leaves, plus what you stack on it (the washers and the nut), rounded up to the next standard length (6, 8, 10, 12, 16, 20, 25, 30, 35, 40, 45, 50 … 200 mm). Type your own and Auto brings the standard one back. A blind hole takes the longest standard length that fits its depth.
    • Washer: none, under the head, or under the head and under the nut (ISO 7089 flat washers).
    • Nut: a hex nut (ISO 4032) on the far side of a through hole, sitting on the face the hole leaves by (or on the floor of a pocket the hole widens into there).
    • Head on the other end: shown for a plain through hole, which opens on both sides.
    • Holes: the other holes to fasten in the same step. N more identical holes on this plane counts the holes with the same diameter, type (plain, counterbored, countersunk) and depth that open on the same plane, however they were made (a Hole feature, a pattern of it, a cut); it is on by default when there are any. Other selected holes, and the other holes of the pattern a hole belongs to, have boxes of their own and get their own size and length.
  3. Add fasteners (or Enter) adds everything as one undo step; Escape cancels.

Each fastener is its own body in one tree folder named Fasteners: Bolt, Washer, Washer (nut) and Nut, numbered (Bolt 1, Bolt 2 …) when there are several holes. They sit on the hole axis with the head outside and the shank pointing into the part, and none of them cuts or fuses with the part, so the hole stays as it was. A hex head is built as a second body and united with the shank by name, which keeps it from fusing with the plate it sits on.

What it cannot do

  • It reads plain, counterbored and countersunk holes whose walls are cylinders and cones about one axis. A hole modelled with a real thread (a helical groove) is not matched by its thread pitch: only its bore diameter is read, so the size is the nearest one by diameter. A hole that is not a hole (a boss, a slot) is refused with a message.
  • A blind hole gets no nut: it has no far side. A tapped hole (a bore at the tap drill) gets no nut either, because the bolt holds by its thread; the panel says why.
  • A countersunk mouth takes no washer, and a washer or a head wider than a counterbore is refused with the two sizes.
  • The socket cap screw and the button head use the shapes of the Screw wizard: cap screws above M10 (and the cap head’s exact ISO 4762 height) are not in its table, so those choices say so. The bolt is plain: no thread is drawn on its shank.
  • The bolt is not tied to the hole. If you move the hole or change its diameter afterwards, delete the Fasteners folder and add them again.

Corner holes

Corner holes put mounting holes on a plate in one step, instead of placing each point by hand.

  1. Select the plate’s flat face and start Hole (Shift+H). The Point tool is active as usual, and a Corner holes card appears at the top right of the canvas.
  2. Choose Place holes. By default this puts a hole in each of the four corners, 10 mm in from both edges.
  3. Confirm the sketch with the tick, as for any hole. The Hole editor opens for the size, kind, fit and depth.

FieldWhat it doesDefault
InsetDistance from both edges to each hole centre.10 mm
Match corner filletShown when the plate has equal rounded corners. The inset follows the fillet radius, so each hole is concentric with its corner.Off
Holes along X, Holes along YHoles on each row and column, corners included. 2 and 2 is the four corners. 3 adds a hole in the middle of each side. Holes lie on the edge of the grid, never in the interior.2 and 2

The card shows the hole count and the plate size. Pressing Enter in a count field also places the holes. Placing again replaces the earlier corner points. Points you added by hand with the Point tool stay.

Nothing is placed, and the button is disabled, when the inset is 0 or negative, the inset is half the plate or more, a count is below 2 or not a whole number, or the plate has no size. A warning appears, and the holes are still placed, when less than 1 mm of material would be left between a hole and the edge.

To change them later, double-click the hole in the feature tree. The same card appears above the Hole editor, with the button Update holes. It re-places the points against the face as it is now (so a plate that changed size is followed) in one undo step. Hole size, kind, fit and depth are left alone. If you moved or dimensioned the points by hand, Update holes puts them back on the grid.

Limits: the exact plate outline is used only for a flat face that is a rectangle, with or without equal rounded corners. Any other outline uses its bounding box and says so. The inset is a plain number, not an expression. A hole sketch on a plane that is not a body face (a standard or datum plane) has no card. Use the Point tool there.

See Holes and threads for the hole settings themselves.

Knurl

The Knurl wizard puts a straight, diamond or pyramid pattern of grooves on a cylindrical face. Select a cylindrical face on the outside of a body, then choose Knurl from the Create group. You can also open Knurl first: the panel says “Click a round face of the part” and waits, the Knurl button stays dimmed, and clicking a round face in the viewport fills in the cylinder. If you click a face that cannot be knurled (a flat face, a tilted cylinder or the wall of a hole), the panel says why and keeps waiting. Escape or Cancel closes it. Set the pattern, the groove shape, the number of grooves, their depth, the helix angle (diamond) and the band along the axis; the viewport previews the result as you type.

Cosmetic (instant) is ticked when the wizard opens. In that mode the grooves are only drawn: they appear at once however many you ask for, but the body stays a plain cylinder, so the mass and the Bodies list do not include them. Exported files (STEP, STL, OBJ and a folder export) do: the export cuts the grooves as real ones in a copy of the part and writes the copy, so the open part stays as it is (see Exporting). A cosmetic knurl has a row under Origin in the feature tree (“Knurl 1 (display only): 30 grooves”); click it to reopen the wizard and change it. The export notice says how many knurls it included. If you turn that off in Settings, the app instead tells you they are not in the file and offers to convert them to real cuts.

A cosmetic knurl is kept in the part file: Save writes it and opening the file brings it back, with its row. It is not a feature, so it is not in the history, and a part built by a script loses it when the script is run again; changing a variable of such a part does not rerun the script while a cosmetic knurl is present, and says so. If you need the grooves in the part itself (in its mass, or for a program that opens the part file rather than an export), untick Cosmetic so they are part of the solid.

Untick Cosmetic to make a real cut. The grooves are then cut into the solid as ordinary features, in one “Knurl” folder, so mass and exports include them. Diamond and pyramid cuts take several seconds to build, and the preview waits until you stop typing. The wizard keeps your choice when you change the pattern.

Following the end face

A cut knurl keeps its distance from the end of the cylinder. Knurl a 30 mm shaft with a band that ends 5 mm from its far end, then change the length of the shaft in the extrude to 20 mm or 40 mm: the band moves with that end and stays 5 mm from it, and changing the length back puts it back. The band is measured from whichever flat end face of the cylinder is nearer to it (for a band across the whole cylinder, the end that the extrude moves), so a band near the fixed end stays where it is. This holds for straight grooves, and for diamond and pyramid when Build is Cut grooves.

What does not follow: a Cosmetic knurl (a display record at fixed positions), a diamond or pyramid built as Faceted (the wizard says so under the options), a cylinder whose ends are not flat faces (a chamfer, a fillet or a cone at the end), and knurls made in an earlier version. They keep the numbers they were made with. If a change then leaves a band past the end of the part, the failure card says the knurl band no longer touches the part and suggests undoing the change or setting the band again. If the part becomes shorter than the band reaches, shorten the band.

In the Script tab: knurl({ radius: 10, from: 15, to: 25, count: 24, depth: 0.5, onFace: { face: 'F2.C1', at: 30 } }) builds the cut grooves from the end face F2.C1, which lies at 30 along the axis; from and to then say where the band is now. For diamond and pyramid add method: 'boolean'.

Samples

The Library picker lists ready-made examples to open and study: Spur gear, Gear pair, Herringbone pair, Marine propeller, Turbo impeller, and a plate with rounded corners and four corner holes. Samples made by these wizards reopen in the same editor. Hand-modelled samples (a bevel gear, helical gear, a four-blade propeller) do not.

Next

Catalog parts

The Catalog holds ready-made shapes that you drop onto your model: plain primitives (blocks, holes, pockets) and parametric parts (cuboids, tubes, tori, edge rounders and more). This chapter covers how to place one, what its parameters mean, and how to edit the result.

Dropping a catalog item does not paste a mesh. It adds real sketches and features (extrudes, lofts, revolves, fillets) to your part, so you keep editing it in the feature tree, in the Variables panel and with the size box, like anything you modelled by hand.

Open the Catalog

Run the Catalog command: key Shift+K, ribbon Home tab, Create group (it shares a button with Variables and Script). The Catalog tab of the left panel opens. It needs an open document.

It has two tabs:

  • Primitives: six ready shapes that add material and eight that remove it, plus a Generators block with the Propeller wizard (see Parametric wizards).
  • Libraries: one searchable list that holds the parametric parts described below, the bundled samples and any libraries you added. See The library and samples.

Placing a catalog item

You can drag or click.

Drag

  1. Press on a card and move over the model. A label follows the pointer, naming the shape, the face under it and any snap. The part turns translucent and shows the real result, rebuilt as you move.
  2. Release over the model to drop it. Release anywhere else, or press Esc, to cancel. Nothing is written until you drop.

Click to place

  1. Click a card. It stays highlighted.
  2. Move over a face and click. Press Esc or click the card again to put it down.

While you place:

KeyEffect
RRotate 90 degrees.
FFlip to the other side.
AltTurn snapping off.
EscCancel.

Snapping applies on flat faces. Within 14 screen pixels the shape snaps to a corner, a circle centre (a hole rim), an edge midpoint or a face centre. The label names which.

One drop is one undo step.

Where it goes

  • On a face: the shape sits flat on the face under the pointer. Primitives work on curved faces too: they get a tangent plane at the picked point. Parametric parts need a flat face. On a curved face you get “Parts library shapes need a flat face”.
  • On a plane: drop on a reference plane drawn in the viewport, on its row in the feature tree, or on a plane feature. A face under the pointer wins over a plane.
  • On empty space: with no body yet, the shape becomes the first body on the ground plane (Top for Y up, Front for Z up). Once a body exists, empty space is not a target.
  • Cuts and edge rounders need a body. Their cards are dimmed until there is one, and dropping gives “Nothing to cut yet: drop a block first”.

The Placement row

The Placement row sets how the next shape stands. It is always visible on the Primitives tab and in a collapsed Placement section on the Libraries tab.

ControlWhat it does
Place onGround (the default, named for your up axis), Front, Top or Right. A plane you hover or drop on overrides it.
DirectionUp (away from the plane) or Down (flipped).
Rotate0, 90, 180 or 270 degrees.
Sphere wall (mm)Wall thickness of the next Sphere primitive. 0 makes a solid sphere, a larger value makes it hollow.
MirrorMirrors the shape.

On a face the shape has its own frame, so Rotate, Mirror and Direction do not apply there.

Primitives

Adds materialRemoves material
Block, Cylinder, Sphere, Cone, Boss, SlotPocket, Round pocket, Dimple, Cone cut, Slot cut, Hole, Counterbore, Countersink

Sizes are picked for you: 40 % of the smaller side of the face, rounded to a neat number (30 mm for the first body). Adding shapes are as tall as they are wide. Cutting shapes go half as deep, never more than half the part’s thickness. Holes go through the part, with an ISO size matched to the face.

ShapeWhat it makes
Block, PocketA sketched rectangle, extruded or cut.
Cylinder, Boss, Round pocketA sketched circle, extruded or cut.
Cone, Cone cutA circle extruded with a draft that tapers the radius to a fifth.
Slot, Slot cutA rounded-bar sketch, extruded or cut.
Sphere, DimpleThe first body gets a whole sphere. On a part, a hemisphere that sits on the face.
Hole, Counterbore, CountersinkA point sketch and a through hole.

A sphere on a face is a hemisphere on purpose. A whole sphere fused to a flat face does not mesh correctly in the current kernel.

After a drop, the shape is selected and shows its size box: drag a handle to resize, or drag the centre pad to move it. Hold Alt to skip snapping while you move.

Parametric parts

On the Libraries tab, the cards marked Included in the library named BOSL2-based parts are parametric. The app builds each one as exact geometry (cylinders, cones, spheres and tori are true surfaces, not polygon meshes). The detail panel names the source and licence of each part.

Use the Category menu to filter: Blocks, Cylinders, Round, Profiles, Edge masks. The search understands everyday words: “pipe” finds Tube, “hexagon” finds Regular prism, “ramp” finds Wedge, “donut” finds Torus, and “printable hole” finds Teardrop. Matches from this set appear first.

Setting parameters

Click a card to select it. A form opens under the list with one field per parameter, each with its unit. A * next to a label means the value becomes a document variable. Reset returns the form to its defaults.

If a combination is not valid, the form says “Check the values:” with the reason, and the card cannot be placed until you fix it.

Then drag the card or click it and then a face. While you drag, the real features are previewed using the form values. The drop commits them, with any variables, as one undo step.

Under the form, a Script section shows the exact script that will be added. It is the same text that runs. See Scripting.

Parameters shared by many parts

ParameterChoices or rangeMeaning
OperationAdd material (default) or Cut into the partAvailable on Cuboid, Cylinder / cone, Tube, Rectangular tube, Pie slice and Regular prism. A cut goes into the part from the picked face and needs a body.
OriginBottom on the face (default) or CentredBottom puts the base on the face. Centred puts half the shape into the part.
Rounding radius and Chamfer0 up to the limit for the shapeRound or chamfer edges. Only one of the two can be non-zero. A cut cannot be rounded or chamfered.

The parts

PartCategoryParameters (default, range)Notes
CuboidBlocksLength X 40 (1-200), Width Y 30 (1-200), Height Z 20 (1-200), Rounding 0 (0-50), Chamfer 0 (0-50), Origin, OperationRounding or chamfer applies to all twelve edges and must be under half the smallest side.
PrismoidBlocksBase X 40, Base Y 30, Top X 20, Top Y 15, Height 25, Top shift X 0, Top shift Y 0A rectangle-to-rectangle taper. No rounding or chamfer. Add only.
WedgeBlocksLength X 30, Width Y 20, Height Z 15A right-triangle prism. Add only.
Rectangular tubeBlocksHeight 30, Length X 30, Width Y 20, Wall 3 (0.2-40), Origin, OperationThe wall must be less than half the smaller side.
Cylinder / coneCylindersHeight 30, Base diameter 20, Top diameter 20 (0.5-200), Rounding, Chamfer, Origin, OperationEqual diameters give a cylinder. Different diameters give a cone. Only a cylinder can be a cut.
TubeCylindersHeight 30, Outer diameter 30, Inner diameter 22, Origin, OperationThe inner diameter must be at least 0.2 mm smaller than the outer.
Pie sliceCylindersHeight 10, Diameter 40, Angle 60 (5-350), Origin, OperationA sector of a cylinder, with its apex at the origin.
Regular prismCylindersSides 6 (3-24), Height 20, Radius 15 (to the corners), Flat at start off, Rounding, Chamfer, Origin, OperationHexagon, octagon and so on. A corner points along +X unless Flat at start is ticked.
SphereRoundDiameter 30, OriginAn exact sphere.
TorusRoundMajor radius 15, Minor radius 4, OriginThe minor radius must be smaller than the major.
TeardropProfilesLength 20, Radius 5, Angle 45 (20-80), Cap height 0A circle plus a pointed cap, extruded in both directions. Cap height 0 gives a pointed tip. See the note below.
OnionProfilesRadius 15, Angle 45, Cap height 0A sphere with a conical hat.
Round face edgesEdge masksRadius 3 (0.5-8)Rounds every edge of the face you pick. Needs a body.
Chamfer face edgesEdge masksChamfer leg 3 (0.5-8)Chamfers every edge of the face you pick. Needs a body.

Lengths and diameters are in millimetres. A cap height above 0 must be at least the circle’s tangent height, or the form reports it.

The Teardrop form’s note suggests using it as a cut for a printable horizontal hole. The part itself adds material only: it has no Operation choice, so it cannot be used as a cut at present.

What gets created and how to edit it

Take a Cuboid with a Rounding of 3 dropped on a face. The app adds a variables block, a sketch of the rectangle on the face, an extrude, and a fillet. The rounding and height are variables with a unique prefix, such as cuboid1_, cuboid2_ for the next drop.

  • Variables link only to feature parameters: extrude depth, fillet radius, chamfer distance and loft offsets. Change them in the Variables tab and the part regenerates.
  • Sizes drawn into a sketch (a width, a diameter, an angle) are plain numbers in the sketch. Change them by editing the sketch, with the size box, or in the script. Editing a variable does not change them.
  • On a face, fillets and chamfers leave the footprint edges alone, so a rounded boss merges with the face instead of filleting the junction.
  • Spheres, tori, onions and rounded cones are revolved shapes. On a face the app adds a hidden helper sketch and a perpendicular plane, which are listed in the tree but hidden in the view.
  • On the ground, the base sits on the plane and the shape rises away from it.

Limits

  • Parametric parts need a flat face. Primitives handle curved faces; parametric parts do not.
  • Edge rounders act on every edge of the picked face. You cannot pick a subset of edges. For that, use Fillet or Chamfer.
  • Only two anchors are offered, bottom and centre. There are no spin, orient or named anchors. Rotate the part, or place it on another face.
  • A cuboid chamfer leaves the corner where three chamfers meet as the kernel builds it, with no extra trimming cut.
  • Some options are not offered: choosing a subset of edges on a cuboid, rounding or chamfering a prismoid, rounding a tube, and mesh-style spheres.
  • Cut mode is not available for Prismoid, Wedge, Sphere, Torus, Teardrop or Onion.
  • Curves are exact, so there is no facet-count setting.
  • Rotate and Mirror in the Placement row do not apply to revolved shapes.

Credits

The parametric parts are based on BOSL2 (the Belfry OpenSCAD Library, version 2) by Revar Desmera and contributors. The app re-expresses the shape definitions and parameter meanings of a set of BOSL2 modules as feature scripts for its own geometry kernel; no OpenSCAD code is copied or run. The library is named BOSL2-based parts because it follows BOSL2’s shapes and parameters but is not BOSL2 itself, and BOSL2’s authors do not endorse this app.

BOSL2 is used under the BSD 2-Clause licence:

Copyright (c) 2017-2019, Revar Desmera. All rights reserved. Redistribution and use in source and binary forms, with or without modification, are permitted provided that the copyright notice, the list of conditions and the disclaimer are retained. The software is provided “as is”, without warranty. The full licence text is in the app’s licences page and in THIRD_PARTY.md.

The library row and each part’s detail panel in the Libraries tab repeat this credit.

Next

Scripting

A short JavaScript script can build a part for you: you describe sketches and features in code, press Run, and the app creates a normal feature tree that you can edit like any other part. This chapter covers where to write a script, what it can create, a complete example, and the limits.

Scripts are useful for parts with many repeated or computed features, for parameter studies, and for building something the same way every time.

Write and run a script

  1. Run the Script command (ribbon Home tab, Create group, on the button it shares with Catalog and Variables). The Script tab opens in the left panel.
  2. Write your script in the code box, or pick one from the Examples list. Examples include a bracket, a flanged cylinder and a thin-walled box.
  3. Choose Run, or press Ctrl/Cmd+Enter in the code box.

What happens when you run:

  • A script always builds a new untitled part. If the part that is open has unsaved changes, the app asks what to do with them first.
  • A progress bar shows “Building n / total” and the time. Cancel stops the run and leaves your open part untouched.
  • When the run finishes, the status says “Script ran: n features”. Warnings appear as notices.
  • The script text is saved in the document, so reopening the file shows it in the Script tab again.

Other buttons in the Script tab:

ButtonWhat it does
OpenLoads a script from a .js, .ts or .txt file into the box.
SaveDownloads the script as a file.
FormatTidies the indentation (Shift+Alt+F). It never changes what the script builds.

A run that fails shows a red banner above the code box with the message and the line number (“Line N: message”). The banner stays until the next Run, the failing line is tinted in the box, and clicking the message selects that line. Opening the Script tab puts the cursor in the box, and the cursor returns there after a run, so what you type never reaches the viewport’s single-key shortcuts. A clean run shows a green line with the number of features built, and under it one row per expect... check: a tick and what was checked, or a cross and the failure (which is also in the banner). Clicking a row selects its line. If the script cannot start at all (a syntax error, a name clash such as const plane = ...), nothing is replaced and the part that was open stays as it was.

Some names belong to the script itself and cannot be used for your own variables: at, bearing, edges, expr, face, faces, group, part, plane, screw, through and variables. Declaring one (const plane = ...) stops the run with a message that names the line and suggests a new name.

Editing variables afterwards

If your script declares variables, they appear in the Variables tab. When you change one there and you have not edited the model by hand since the run, the app reruns the script with your values and rebuilds the part. If you have changed the model by hand, the app does not rerun and tells you: press Run to rebuild from the script, which replaces those changes.

A complete example

This script builds a 60 x 40 x 12 plate with two 8 mm holes and rounded vertical edges.

// plate with two holes and rounded edges
const { w, h } = variables({ w: 60, h: 40, t: 12 });
part('Bracket')
  .sketch('front', (s) => s.rect(w, h))
  .extrude(expr('t'))
  .hole(face('>Z'), [-15, 0], { diameter: 8 })
  .hole(face('>Z'), [15, 0], { diameter: 8 })
  .fillet(edges('|Z'), 4);

What each line does:

  • variables({...}) declares named values. They become document variables, editable in the Variables tab. It returns their numbers, so you can use w and h in the code.
  • part('Bracket') starts the part. The name becomes the document name. Every script builds one part. If you write several part(...) calls, the last one wins.
  • .sketch('front', ...) adds a sketch on the front plane. The function receives a sketch builder s.
  • .extrude(expr('t')) extrudes the sketch. expr('t') keeps the depth linked to the variable t.
  • .hole(face('>Z'), [x, y], {...}) drills a hole in the face that points furthest toward +Z, at that position on the face.
  • .fillet(edges('|Z'), 4) rounds the edges that run parallel to Z with a 4 mm radius.

A script must start with part(...). A script that builds no part gives “the script builds no part: start with part(“Name”)“.

What a script can create

Each part method adds one feature, in order.

Sketches

part.sketch(plane, fn, name?) takes a plane: 'front', 'top' or 'right', a face selector such as face('>Z'), or an offset plane made with at('front', 10).

Sketch builder methods:

MethodDraws
rect(w, h, [cx, cy])A rectangle, centred at [cx, cy].
rrect(w, h, r, [cx, cy])A rectangle with rounded corners.
circle(radius, [cx, cy])A circle (the argument is the radius).
polygon(points), polyline(points), line(a, b)A closed polygon, an open chain, a single line.
arc(centre, start, end), arc3(a, mid, b)An arc, counter-clockwise from start to end, or through three points.
spline(points, {closed}), cvspline(points, {closed, degree})An interpolating or control-point spline.
curve(fn, {from, to, count, closed}) (short names t0, t1, n)A spline through a JavaScript function t => [x, y] sampled count times (default 48). With closed: true it is a loop that does not repeat the end point.
polar(fn, {count, closed, center}) (n for count)A polar curve: fn(angle) returns the radius, the angle is in radians, a full turn by default (96 points, closed). Waves, cams, petals, rounded stars.
point([x, y]), points(list)Point entities, which holes use.
polarPoints(centre, radius, n, startAngle), grid(origin, [dx, dy], [nx, ny])Points on a circle or grid.
axis(), axisAt(from, to)A construction line used as a revolve axis.
text(string, at, options)Letters as closed profiles. See Text.

For example, a wavy disc outline and a closed section for a loft:

// radius 30 with 12 waves, 3 mm deep
part('Wavy').sketch('front', (s) => s.polar((a) => 30 + 1.5 * Math.cos(12 * a), { count: 120 })).extrude(5);

// a closed spline as a loft section, at two sizes
const wave = (r) => (s) => s.polar((a) => r * (1 - 0.1 * (1 - Math.cos(8 * a)) / 2), { count: 96 });
part('Taper').loft([{ on: at('top', 0), draw: wave(30) }, { on: at('top', 20), draw: wave(18) }], { newBody: 'Taper' });

The function is sampled when the script runs and the points are stored. To keep the curve as a formula the kernel refits (and that follows variables without rerunning), use equation({ x, y, t }) instead; its formulas are text and use degrees. A polar curve takes radians, like JavaScript’s Math.sin. (polar(count, draw) with a number first is the polar pattern, which repeats a drawing round a centre.)

Sketch planes use these axes:

PlaneSketch x is worldSketch y is worldExtrudes toward
'front'+X+Y+Z
'top'+X-Z+Y
'right'-Z+Y+X

A sketch on a face has its normal pointing out of the body.

Features

CallFeature
.extrude(depth, {direction, mid, flip, draft, thin})Extrude (add) the last sketch.
.cut(depth or through(), {direction})Extrude (cut). With the default direction: 'auto' the script tries into the part, and flips once if that cuts nothing, adding a warning. State the direction yourself to skip the retry.
.revolve(angle = 360, {op, thin, axis})Revolve about the sketch’s axis line.
.thin(t)Makes the previous extrude or revolve thin-walled.
.hole(face, [x, y], {diameter, depth, kind, ...})A hole. kind can be 'cbore', 'csk' or 'tapped'. Through unless depth is given.
.holes.points / .polar / .grid(...)One hole feature at many points.
.fillet(edges, radius), .chamfer(edges, distance)Edge rounding. Different radii become one fillet per radius.
.shell(face or faces, t)Hollow out, opening the given faces.
.linearPattern({count, spacing, direction}), .circularPattern({count, axis, angle}), .pathPattern({path, count, spacing})Patterns of the last feature, or of seeds you name. A linear pattern’s direction is 'x', 'y', 'z', any vector such as [1, 1, 0] (oblique is fine) or a straight edge; a circular pattern’s axis is 'x', 'y', 'z', [ox, oy, oz, dx, dy, dz], { point, dir } or a straight edge, so a bolt circle can turn about any point. A linear pattern can use totalLength or to (a plane, face or point the last copy reaches) instead of spacing, and a second direction. A path pattern follows an open sketch.
.workplane(base, offset)A reference plane.
.loft(sections), .sweep(profile, path, {guides, guideMode}), .mirror(plane), .rib(thickness, {fillet, draft, side, target})Loft, sweep, mirror and rib. A rib can round its free edge (fillet), taper its sides (draft, degrees), put all its thickness on one side of the sketch plane (side: 'left' or 'right') and grow to named bodies only (target). A sweep path can be a helix ({ curve: handle }), and one or two guide curves make it taper or flare.
.draft(faces, angle, {neutral}), .moveFace(faces, {distance}), .pressPull(faces, {distance, taper})Taper walls about a neutral plane; push or pull faces; continue a flat face straight with an optional draft or scale taper.
.lip(rim, edges, {width, height}), .groove(...)A raised band on a rim, and the groove it fits.
.scale(factor, {about}), .moveBody(bodies, {translate, rotate, copy, mirror})Scale bodies; move, rotate or copy them, also as a mirror image.
.split(plane, {names}), .split(target, tools), .deleteBody(bodies), .deleteFace(faces)Split a body at a plane (a face, a standard plane or an offset plane) into two named bodies, or by tool bodies; remove bodies, or remove faces (the solid becomes a sheet; nothing is healed).
.lipJoint(plane, {height, width, clearance, tongue, names})Split a shelled body at a plane and give the cut a centred tongue on one half and a matching groove, wider and deeper by clearance, on the other. See Cases and moulds.
.sphere(radius, {centre, op}), .helix({radius, pitch, revolutions}), .axis(...)A ball, a helix curve, and a reference axis.
.gear({module, teeth, thickness, ...})The gear generator.
.screw(...), .washer(...), .nut({size, type}), .standoff({size, length, kind, ends}), .heatSetInsert({size, hole}), .bearing(...)The fastener and bearing wizards, each as its own body placed by origin and axis. See Parametric wizards.
.spring(...), .extensionSpring(...), .torsionSpring(...)The Spring wizard’s three types, each as its own body.
.thread(...)A cosmetic or modelled thread on a hole or cylinder.
.surfaceExtrude, .surfacePlanar, .surfaceLoft, .thicken, .knitSurface bodies.
.insertPart(doc, {...}), .mate({...})Assemblies inside the part.
.appearance({...}), .bodyName(handle, name)Colour, opacity, finish and body names. They add no feature and no history step.
.feature(json), .sketchFeature(on, {...})Raw features, for anything without a helper.

Values are numbers or expr('w*2'), an expression over your variables stored in the feature. Inside a sketch, an expr contributes its current number only, so a sketch size does not follow later edits to a variable.

Choosing faces and edges

Selectors are resolved when the script runs, against the body as it is just before that step.

  • face('>Z') is the face pointing along that axis that lies furthest along it. Other forms: '<X', '>Y' and so on, or a persistent name such as 'F3.C1'. Rule objects such as face({ normal: [0,0,1], areaGreater: 100 }) combine tests. A selector for one face must match exactly one, or the run stops with “Line N: face(…) matches 6 faces”.
  • faces(...) matches several. Use .largest(), .smallest() and .nth(i) to pick one.
  • edges('|Z') is edges parallel to Z. edges('all'), '>X', and rule objects such as edges({ onFace: face('>Z') }) also work.
  • Order and group by position. edges(...) and faces(...) take .sortBy(key) and .groupBy(key), so a selection can say where something is instead of relying on a generated name. A key is '>Z' (highest first), 'Z' or '<Z' (lowest first), likewise X and Y, a direction such as [1, 1, 0], or { along: edges(...) } (the distance along a straight rail edge). After .sortBy, .nth(i), .first(n) and .last(n) count in that order (a negative i counts from the end): edges('|X').sortBy('>Z').first(2) is the two highest edges running along X. .groupBy(key, { tol }) collects the ones at the same position (within tol mm, 0.001 by default) and .first(), .last(), .nth(i) or .at(height) chooses a group: edges('all').groupBy('Z').at(12) is every edge at height 12. Ties are broken by x, y, z, so the pick is the same after the model rebuilds.
  • A face selector that resolves to the furthest of several same-facing faces gives a warning that names the candidates. Restrict it with a face name or {of: handle}.
  • const h = part.handle() captures the feature just recorded, for {of: h} and for patterns.

Reading results back

A script can check what it built.

const p = part('Plate').sketch('front', (s) => s.rect(60, 40)).extrude(10);
const v = await p.volume();                        // mm3
p.expectVolume(60 * 40 * 10).expectValid().expectBBox({ size: [60, 40, 10] });

await reads: volume(), area(), bbox(), centreOfMass(), inertia(density) (mass, first moments, inertia tensor about the centre of mass and the origin, principal moments and axes; density in g/cm³), faceCount(), edgeCount(), isValid(), issues(), faces(), edges(). Assertions check the result without await; a failed one adds a “Line N: expected volume 25000, got 24000 (tolerance 1e-6 relative)” style error and the run continues:

AssertionChecksTolerance
expectVolume(v, {tolerance, abs, body})The exact volume in mm³.Relative, default 0.001 (0.1 %); abs in mm³ instead.
expectBBox({min, max, size}, {tolerance, body})The bounding box, in mm, for the keys you give. It is the display box, not the control polygon of a spline or loft, and can fall short of curved faces by a few thousandths of a mm (more for small round bodies).Absolute in mm, default 0.001.
expectMinFaceArea(a, {body})No face smaller than a mm², so no slivers; the message names the smallest face.None: a is the limit.
expectValid(), expectFaceCount(n)The validity check, the number of faces.None.

All of them read every body together; give { body: 'Name' } (a body made with newBody) to check one body. Volumes of lofted and swept bodies are best checked to about 0.5 %: expectVolume(78968, { tolerance: 0.005 }).

Each read rebuilds everything recorded so far, so read once after a group of features, never inside a loop that adds features.

Limits

  • Size: a script is limited to 40,000 characters and 2,000 steps. A for or while loop stops after 100,000 turns (“loop limit exceeded”).
  • Safety: the script runs with only the API names in scope. Browser functions such as fetch, window and timers are blocked. This prevents accidents but is not a security boundary. Do not run scripts from people you do not trust.
  • No sketch constraints: sketches made by a script are plain geometry without constraints.
  • No separate assemblies: an assembly is insertPart plus mate features inside one part.
  • Not covered by helpers: closed (ring) lofts, sweep with a kept normal, and surface features such as fill, trimSurface, extend and projectCurve. Use .feature({ type: ... }) for kernel features that have no helper. dome is not built in the kernel.
  • Patterns take any direction or axis: a linear pattern’s direction can be a vector at any angle or a straight edge, and a circular pattern’s axis a point and a direction ({ point: [40, 0, 0], dir: [0, 0, 1] }) or an edge. .holes.polar still makes a bolt circle of holes in one feature.
  • Chamfers: a chamfer with two distances, or with distance and angle, is reported as unsupported by the kernel today. Cut the bevel instead.
  • Line numbers come from the browser. In browsers other than Chrome and Edge, an error may show line 0.
  • Fonts: a script can use the built-in fonts gauge and engrave and a short list of library fonts by id. Fonts picked in the editor cannot be named from a script.
  • Running creates a new part. A script run in the Script tab cannot modify the part you have open. An agent linked in Settings can run a script on the open part, as one undo step (see Agents and the MCP server).

Next

Agents and the MCP server

CivilKit CAD includes a local server that lets an AI coding assistant build and check parts by writing scripts. It speaks the Model Context Protocol (MCP), so any MCP client can use it: Claude Code, Cursor, Claude Desktop, Codex and others. This chapter takes you from nothing to a first successful tool call, then lists every tool, error code, flag and limit.

What it is, and what it is not

  • It is a separate program that runs on your computer, started from a checkout of the CivilKit CAD application repository. It is not a panel inside the browser app, but the app’s Chat panel uses it to run your Claude Code (see Chat: ask for a change in words).
  • It has its own document and its own copy of the geometry kernel. By default it does not read the part you have open in the browser, and the browser does not show what the agent builds. You can link the two on purpose with the agent link (see Linking the open app): then the agent can read, take pictures of and, if you allow it, add to the part you have open. It is off until you turn it on.
  • No tool or resource can load an existing part into the server. The agent starts from an empty document and builds everything with scripts, so none of your hand edits are involved or preserved.
  • Everything on one machine shares one open document: there is one background process, one daemon.json and one port. Two assistants, or two projects, that use the server at the same time overwrite each other’s work.
  • Work moves between the two by file. The agent calls export to write a .ckpart file (or STEP, STL, GLB), and you open it in the app with Open (see Saving and opening).
  • The assistant brings its own model and key. The server never reads or stores a key.
  • It uses the same script language as the Script tab (see Scripting). A part an agent builds is an ordinary feature tree.

If you only use the web app, you do not need this chapter.

Before you start

You need three things.

  1. Node 22.

  2. Two source trees, side by side. The launcher runs TypeScript through the application repository’s own vite-node, and its settings (vite.config.ts) point the @ck/* imports at the kernel’s packages. So you need both:

    • the application repository (it contains apps/cad and packages/mcp), and

    • the kernel repository, checked out in the same parent folder and named kernel, like this:

      work/
        app/       the application repository
        kernel/    the kernel repository
      

      If the kernel checkout has another name or place, set the environment variable CK_REBUILD to its absolute path (in the client configuration, next to CK_WASM).

    Then run npm install in the application repository:

    cd work/app
    npm install
    
  3. The kernel binary (ck_wasm.wasm). It is not stored in the repository. Get it in one of two ways:

    • Download the one the published app uses. The site serves it at /cad/kernel/ck_wasm.wasm:

      curl -o ck_wasm.wasm https://civilkit.io/cad/kernel/ck_wasm.wasm
      

      This build loads in the launcher and runs scripts.

    • Or build it from the kernel repository with cargo build -p ck-wasm --target wasm32-unknown-unknown --profile fast. See the kernel guide.

Then tell the server where the binary is, in one of two ways:

  • Set the environment variable CK_WASM to its absolute path (the client configurations below do this), or pass --wasm PATH.
  • Or copy it to apps/cad/public/kernel/ck_wasm.wasm inside the checkout, which is the default place the server looks.

In the commands below, replace <checkout> with the absolute path of the application repository and <wasm> with the absolute path of the .wasm file.

Connect a client

Claude Code

claude mcp add ck-cad -e CK_WASM=<wasm> -- node <checkout>/packages/mcp/bin/ck-mcp.mjs

To share the setup with a project instead, put this in a .mcp.json file at the project root:

{
  "mcpServers": {
    "ck-cad": {
      "command": "node",
      "args": ["<checkout>/packages/mcp/bin/ck-mcp.mjs"],
      "env": { "CK_WASM": "<wasm>" }
    }
  }
}

Cursor

Put the same JSON in .cursor/mcp.json in a project, or in ~/.cursor/mcp.json to use it everywhere. Restart Cursor or reload its MCP settings.

Claude Desktop

Add the same mcpServers entry to claude_desktop_config.json, merging it with anything already there:

SystemFile
macOS~/Library/Application Support/Claude/claude_desktop_config.json
Windows%APPDATA%\Claude\claude_desktop_config.json

Restart Claude Desktop after editing. Use the absolute path of node as command (for example the output of which node on macOS), because desktop apps often do not see the PATH of your shell.

Codex

Append this to ~/.codex/config.toml:

[mcp_servers.ck-cad]
command = "node"
args = ["<checkout>/packages/mcp/bin/ck-mcp.mjs"]
env = { CK_WASM = "<wasm>" }

On Windows, write paths with forward slashes or doubled backslashes in JSON and TOML.

Check that it works

  1. List the servers. In Claude Code, run claude mcp list. ck-cad should be listed and connected.

  2. Check the background process. The first tool call starts a shared background process, which can take a few seconds (the launcher waits up to 40 seconds). Then run:

    node <checkout>/packages/mcp/bin/ck-mcp.mjs --status
    

    It prints JSON such as {"running":true,"port":53124,"pid":4242}. It prints {"running":false} when no process is running, which is normal before the first call or after it has idled out. --stop stops it.

  3. Make a first call. Ask your assistant: “Use ck-cad to build an 80 by 50 plate, 12 mm thick, and report its volume.” The assistant calls run_script. If you want to see the protocol itself, this is what a client sends and what the server answers. You can try it without any client: put the lines below in a file msgs.jsonl and run

    CK_WASM=<wasm> node <checkout>/packages/mcp/bin/ck-mcp.mjs --stdio-direct < msgs.jsonl
    

    The replies print one per line. The process exits when its input ends.

A first call, as JSON-RPC

The messages below are one per line. A client sends initialize, then notifications/initialized, then calls.

{"jsonrpc":"2.0","id":1,"method":"initialize","params":{"protocolVersion":"2024-11-05","capabilities":{},"clientInfo":{"name":"test","version":"1"}}}
{"jsonrpc":"2.0","method":"notifications/initialized"}
{"jsonrpc":"2.0","id":3,"method":"tools/call","params":{"name":"run_script","arguments":{"mode":"new","code":"part('Plate').sketch('front', (s) => s.rect(80, 50)).extrude(12)"}}}

The reply to run_script has two text blocks. The first is a one-line summary, and the second is the JSON result (shortened here):

script#1 (new) built 2 features, volume 48000
{ "ok": true, "run": "script#1", "mode": "new", "errors": [], "warnings": [],
  "created": ["F1", "F2"], "removed": [], "regenMs": 21, "featureCount": 2, "solids": 1,
  "volume": 48000, "area": 11120, "centerOfMass": [0, 0, 6],
  "bbox": { "min": [-40, -25, 0], "max": [40, 25, 12], "size": [80, 50, 12] },
  "faceCount": 6, "edgeCount": 12, "validity": { "ok": true, "issues": [] } }

The volume is 80 x 50 x 12 = 48000, as it should be. Now facts (no arguments) and tree:

{"jsonrpc":"2.0","id":4,"method":"tools/call","params":{"name":"facts","arguments":{}}}
{"jsonrpc":"2.0","id":5,"method":"tools/call","params":{"name":"tree","arguments":{}}}

facts returns featureCount, solids, volume (48000), area (11120), centerOfMass, bbox, faceCount (6), edgeCount (12), and validity (ok: true). tree returns:

{ "name": "Plate", "featureCount": 2, "handMade": 0,
  "features": [
    { "index": 0, "id": "F1", "type": "sketch", "name": null, "origin": "script#1",
      "params": { "plane": { "kind": "std", "id": "front" }, "points": "5 items", "entities": "4 items", "constraints": "0 items" } },
    { "index": 1, "id": "F2", "type": "extrude", "name": null, "origin": "script#1",
      "params": { "op": "add", "sketch": "F1", "end": "blind", "depth": 12 } } ],
  "errorCount": 0 }

To keep the part, call export with format: "ckpart" and a path, then open the file in the app.

The tools

An agent changes the model with one tool, run_script. Everything else reads, proves, shows or documents. The measuring tools (measure, clearance, interference, thickness, draft, dfm) answer what the kernel can compute exactly, so an agent can check its own work instead of estimating: they never change the model, name the bodies and faces they talk about, and give a verdict. Touching solids merge into one body unless the feature has newBody: true, so make parts that must stay separate with it before asking about clearance or interference. Tool calls run one at a time. Every input is checked against its schema, and unknown fields are refused.

ToolArgumentsWhat it returns
run_scriptcode (required, up to 40,000 characters), mode (required: new or attach), name? (part name for new), replace? (last, all or none; attach only, default last)The result shown above: ok, run, mode, errors, warnings, created and removed feature ids, regenMs, and a summary of the part.
treenoneThe feature list in order: id, type, name, origin (script#N) and key parameters, with any errors and hints.
findquery (required)Features, face names and edge names that match the text.
inspectid (required)One feature in full, the faces and edges it created, what depends on it, and its error if any.
factsexpect?: list of checks such as [{"kind":"volume","value":1200,"tol":0.01},{"kind":"valid"}]Mass properties, bounding box, counts and validity, plus a pass or fail per check.
probepoints?: list of [x,y,z]; rays?: list of {origin, dir}Per point: inside, outside or boundary, with the signed distance and nearest face. Per ray: the hits with face names.
sectionplane (required: {origin?, normal}), detail? (boolean)The exact cross-section loops, their areas and the plane frame. detail: true adds the polyline points.
sectionsaxis (required: x, y or z), n? (1 to 200), positions?Areas of several slices and the volume they add up to, compared with the exact volume.
bodiesnoneOne row per body: name, creating feature, volume, bounding box, colour. The names and numbers it shows are what the measuring tools take.
measurea, b (required: a body name or number, a face, edge or vertex name, or a point [x,y,z]), samples?The minimum distance between the two, the closest point on each with the face or edge it lies on, the offset between them, and whether they touch. For two faces it adds the angle between them.
clearancea?, b? (default: the two bodies when there are exactly two), required? (mm), within?, limit?The gap between two bodies with the closest points and the closest face pairs, and a verdict: clear or contact, and pass or fail against required with the shortfall.
interferencea?, b? (bodies)Every pair of bodies that share volume: the overlap volume in mm³, its centre and box, and the share of the smaller body that is inside the other. A pair the kernel could not compute is reported as incomplete, not as clear.
thicknessmin? (mm), body?, top?, method? (ray or sphere), samples?The thinnest wall with where it is (the point and the two faces), the mean, the thinnest few places, and pass or fail against min with the places under it.
draftpull? ([x,y,z] or +Z … -X; default +Z), min? (degrees; default 1), faces?, body?The draft angle of each face against the pull direction, the class of each (ok, vertical, undercut, parting), the walls under min worst first, and the count per class.
dfmprocess (required: injection, cnc or printing), direction?, params? (per-rule limits), rules?, maxIssues?The design checks of the Check tab for that process: each issue with its rule, severity, faces, the measured value against the limit, and a point. For injection it includes Undercut (two-part mould): faces that neither mould half can form. The limits used are listed in the result.
snapshotview?, up?, size? (64 to 2048), style?, projection? (ortho or perspective), section?, sheet?, highlight?, markers?, frame?, annotate?, background?A PNG image plus a short text summary (view, size, bytes).
checkpointname (required)Saves the whole document under a name. At most 20 are kept in memory; the oldest goes.
restorename (required)Replaces the document with a checkpoint. Notes are not restored. It can be undone.
checkpointsnoneLists the saved checkpoints.
notestext?, append?Reads the scratch notes, or replaces them with text, or adds to them with append: true. Notes survive restore and undo.
list_methodsquery?Searches the registered script methods. With no query it returns the guide, all methods with signatures, and the recipes.
docsnames (required, 1 to 30)Full entries (signature, summary, example) for methods, or the code of recipes by id. Unknown names are reported as unknown.
undo, redononeStep through the document history (50 states).
ask_userquestion (required), options?A “needs user input” result. MCP has no screen of its own, so the agent should ask in its reply.
exportformat (required: step, stl, glb or ckpart), path?Writes the file and returns the path and size. Without path, it writes ./<part name>.<extension> in the server’s working directory. The server is one shared process per machine, so that is the folder of whichever client started it first, not necessarily where you are working. Always pass an absolute path.

Attach mode

In attach mode the script’s features are added to the features already in the server’s document, which can only come from earlier scripts, since nothing can load your own part. Each feature a script makes carries an origin mark such as script#2. By default a re-run first removes the features of the previous script run, so a corrected script does not duplicate its output; replace: "all" removes every script’s features and replace: "none" only adds. If a later feature depends on one that would be replaced, the run is refused and names it. tree reports handMade, which is always 0 here. Runs are all-or-nothing: a script with an error leaves the document as it was.

What list_methods and docs cover

The registry behind list_methods and docs is a small core set of about thirty entries: part, variables, expr, face, edges, at, through, sketch, extrude, cut, revolve, thin, hole, holes.*, fillet, chamfer, shell, linearPattern, circularPattern and the basic sketch builder methods. The script language itself has many more methods, such as loft, sweep, mirror, gear, thread, surfaces and assemblies (see Scripting). These work in run_script, but the registry does not describe them: list_methods {"query":"loft"} returns no methods, and docs {"names":["loft"]} answers “unknown”. An agent that knows the method can still use it; for example this builds a valid solid:

part('L').loft([{ on: at('front', 0), draw: (s) => s.rect(20, 20) }, { on: at('front', 30), draw: (s) => s.circle(6) }])

Point your assistant at Scripting or give it the method names directly when you want these.

Linking the open app

The agent link lets an assistant see, and if you allow it change, the part you have open in the browser app. It runs only on your computer and is off until you turn it on.

  1. Make sure the server is running and the assistant is connected. If the app is not served from your own computer (for example the hosted app), start the server with --allow-origin https://<the app's address>; Safari does not allow a secure page to reach your computer, so use a local copy there.
  2. Ask the assistant to call bridge_pair. It gives you a code like 52311-ABCD-EFGH-JKMN-PQRS, valid for 10 minutes and usable once.
  3. In the app open Settings, Agent link, paste the code and press Turn on. The status bar now shows Agent: linked, view only.
  4. Optional: tick Allow the agent to change this document. Without it the agent can only read and take pictures. Untick it or press Turn off at any time; closing the page also ends the link, and nothing is remembered for next time.
ToolWhat it doesNeeds the edit box
bridge_pairGives the one-time pairing code. Calling it again ends any current link.no
app_statusWhether an app is linked and whether changes are allowed.no
app_stateThe open part, compact and paged: name, features with their errors, variables, selection and counts, with filters on id, name and type, chosen fields, a cursor, and sinceRevision for only what changed. detail: "full" adds the whole document. A result over the output budget (4000 characters by default, maxChars up to 48000) is summarised with a handle that fetch_result pages through.no
app_open_assetOpens a .ckpart, .solidcraft, STEP or mesh file in the app by path, from an allow-listed folder, so the file’s bytes never travel through the chat.yes
app_editApplies a set of edits (add, replace, remove, transform, set a parameter) as one transaction guarded by expectedRevision: it is checked step by step and committed as one undo step, or not at all.yes
app_interfacesThe part’s interfaces: hole axes and patterns without duplicates, unique planes, contact faces and coordinate frames.no
app_job_start, app_job_status, app_job_cancel, app_recipe_listRun a long job (a big open, a saved recipe, a batch) in the background, ask how it is going, stop it, and list the saved recipes.yes
app_screenshotA PNG of the model (view, size). It is a rendering of the part, not a copy of your screen.no
app_bodies, app_measure, app_clearance, app_interference, app_thickness, app_draft, app_dfmThe same measuring tools as above, asked of the part you have open: bodies, distance, gap, overlap, wall thickness, draft angles and the manufacturing checks. They only read, so they work without the edit box.no
app_run_scriptRuns a script on the open part in attach mode: its features are added after yours as one undo step, and the app shows a notice.yes
app_undo, app_redoStep the app’s undo history.yes

Failures come back as ordinary error results: app_not_connected (nothing linked: call bridge_pair), edit_not_allowed, app_timeout (the tab did not answer in 60 seconds), no_document, no_body. What is not there yet: the other tools (facts, probe, section, export…) on the open part, besides the measuring ones above, and a chat panel that uses them (see Chat: ask for a change in words). The chat panel is built; it runs your Claude Code through this server.

Resources

Besides tools, the server offers read-only resources:

URIContent
ck://docs/guideHow the script API works and the build-check loop.
ck://docs/methodsThe registered methods with signatures and summaries.
ck://recipes/<id>A complete example script. The ids are bracket, flange, box, bc-pulley, bc-washer, bc-hex-nut, bc-enclosure, bc-motor-end-cap, pickleball and speedboat-dash.
ck://documentThe open part as JSON.
ck://notesThe scratch notes.

Errors

A failed tool call returns isError: true and a JSON body {"ok": false, "error": {"code", "message", "hint"}}. A script that fails reports its errors inside the run_script result. The line is given for runtime errors. A syntax error, or an error found only when the finished document is rebuilt, has "line": 0, which means no line is known. For example this is not js returns {"line":0,"message":"Unexpected identifier 'is'"}.

CodeMeaning
bad_inputAn argument is missing, has the wrong type, or is unknown. The message names the field.
unknown_toolNo tool has that name. The hint lists the tools.
no_such_featureinspect or a similar call named a feature that does not exist.
no_such_checkpointrestore named a checkpoint that was not saved.
nothing_to_undo, nothing_to_redoThe history has nothing in that direction.
no_bodyOnly export raises it: the document has no solid to export.
snapshot_unavailableThe snapshot renderer is not available. The checkout includes it, so you only see this in a build without it.
snapshot_failedThe renderer returned no image. Try another view or a smaller size.
script_crashThe script runner failed unexpectedly.
internal_errorThe kernel or the tool failed unexpectedly. Retry, or restore a checkpoint.

Protocol-level errors use JSON-RPC codes: -32700 (parse error), -32600 (invalid request; a message that has an id but no method is treated as a client reply and ignored), -32601 (method not found), -32602 (invalid parameters), -32603 (internal error) and -32002 (resource not found).

Tool output is capped at about 48,000 characters. Long lists are cut with a “more items” marker.

Flags and environment

Pass flags after ck-mcp.mjs. In a client configuration they go in the args array, for example "args": ["<checkout>/packages/mcp/bin/ck-mcp.mjs", "--idle-seconds", "600"].

FlagWhat it does
(none)Normal mode. Connects to the shared background process, starting it if needed.
--stdio-directNo background process: the kernel lives inside this one, and its state ends with the client. Useful for tests and simple setups.
--daemonRun the background process in the foreground.
--status, --stopReport on, or stop, the background process.
--idle-seconds NThe background process exits after N idle seconds (default 1800).
--wasm PATHThe kernel binary to use.
--allow-origin URL[,URL]Let a specific web page use the agent link routes (a page served from your own computer is always allowed there). Everything else still refuses web pages.
VariableWhat it does
CK_WASMPath of the kernel binary, if --wasm is not given.
CK_MCP_HOMEThe state folder (default ~/.ck-cad).
CK_MCP_IDLE_SECONDSThe idle time, if --idle-seconds is not given.

The state folder is created with mode 0700. Inside it, daemon.json (mode 0600) holds the port, process id and token of the running process. Only protocol messages go to the client’s standard output.

Security

  • The background process listens on 127.0.0.1 only, on a random port.
  • Every request must carry a 256-bit random token, made at start and held in daemon.json, as an Authorization: Bearer header.
  • The Host header must be 127.0.0.1 or localhost with the right port, which blocks DNS rebinding.
  • Any request with an Origin header is refused, except the agent link routes (/bridge/...), which accept a page from your own computer or an origin you listed with --allow-origin, and only with a one-time pairing code you pasted yourself and the session it buys. That session cannot call anything else in the process.
  • Any other program running as your user can read daemon.json. Treat the process as trusted by that user.
  • Scripts run in a restricted environment that stops accidents. It is not a security boundary. Do not run scripts you do not trust.

Limits

  • One document per process, and one linked app at a time (the agent link does not change the process’s own document). run_script with mode: "new" replaces it; undo brings it back.
  • Checkpoints (20) and history (50 states) are in memory and end when the process stops.
  • The process exits after its idle time (30 minutes by default). The next call starts a new one, with an empty document.
  • The first start takes a few seconds. Later starts are fast.
  • Script sketches have no constraints.
  • GLB export writes flat-shaded triangles. GLB is available only through this server, not the app’s Export menu.
  • The server is a developer tool, started from a checkout. It is not installed from the app.

Next

Chat: ask for a change in words

The Chat panel lets you type a change (“40x40 plate with four countersunk M5 holes, R8 corners”) and an assistant edits the part you have open. It uses the Claude Code you already have on your computer, under your own login and plan. There is no key to paste, no account with us, and no server of ours in between.

Before you start

  • Claude Code, installed and signed in (run claude once in a terminal and sign in).
  • The local service from the CivilKit CAD source (see Agents and the MCP server for Node 22 and the kernel file). The service starts Claude Code for the chat and connects it to the part you have open. In the Mac app and on the web the service is the same one; the Mac app does not start it for you yet.

Open it

  1. Press the chat button in the top bar (or open the Chat tab of the left panel).

  2. Without the service the panel shows the setup card. In a terminal run the command it shows, for example

    node <checkout>/packages/mcp/bin/ck-mcp.mjs --pair
    

    (on the hosted app it adds --allow-origin with the app’s address). It prints a code like 52311-ABCD-EFGH-JKMN-PQRS.

  3. Paste the code in the panel and press Link. The link is the same agent link as in Settings; it is off again whenever the page closes.

Use it

  • The assistant can also read numbers off the part without changing it: how far apart two bodies or faces are, whether a lid clears its box by the gap you need, whether two bodies overlap and by how much, the thinnest wall and where it is, the draft angle of each face against a pull direction, and the manufacturing checks for injection moulding, CNC or printing. Ask, for example, “is there at least 0.2 mm between the lid and the box?” or “does every wall have 1 degree of draft?”. These readings need no permission: they work with Allow it to change this document off.
  • Type a message and press Send (or Ctrl/Cmd+Enter). The reply streams in, and each thing the assistant does (looking at the part, taking a picture, running a script) appears as a line.
  • Stop ends the turn at once. A script that is already running finishes, because a change is applied whole or not at all.
  • Model: Sonnet (balanced, the default), Opus (most capable) or Haiku (fastest).
  • Tell it about: Selection sends the names of what you have selected, View asks it to look at a picture of the part first, Comments sends the script saved with the part with its // comments. All three are off until you tick them.
  • Allow it to change this document is the same box as in Settings, Agent link, and it is off every time the link starts. Without it the assistant can look, measure and take pictures but not change anything. With it, each script, undo and redo it runs is one undo step and shows a notice, and Undo takes it back like any other step.
  • New chat forgets the conversation; otherwise a follow-up message continues the same one.

The assistant adds features after the existing ones; it does not edit or delete features you made by hand (use Undo, or say what you want and do the edit yourself).

What is sent

To Claude, through your Claude Code: your message, the boxes you ticked, and what the assistant’s tools return: the part’s features and variables, the numbers of a measurement (distances, volumes, face names), a picture of it when it takes one, and the scripts it writes. Claude Code keeps its own session files on your computer as it always does. Nothing is stored in your document and nothing goes to us.

When something goes wrong

The panel says it in words and never loses your message: the service is not running or the link was lost (start it and paste a new code), Claude Code is not found or not signed in, you hit a usage limit, Claude is busy, another chat is already running, or the assistant reached its limit of 24 steps for one message (what it did so far is in the part; undo it or ask it to carry on).

The local kernel service

The app’s geometry kernel normally runs inside your browser. You can instead point the app at a local kernel service: the same kernel built as a native program that runs on your own computer. This chapter covers why you might want that, how to switch to it, how the access token works, and what happens when the service goes away.

The local kernel service is experimental and optional. Nothing changes unless you switch it on, and the built-in kernel is always the fallback.

Why use it

  • It is faster on large parts, because it runs as a native program and keeps its caches warm between edits.
  • It is not limited by the browser’s memory ceiling, so very large documents open that the built-in kernel cannot hold.
  • It is the same kernel. The results are the same up to rounding in the last digits of some floating-point values.

If your parts rebuild quickly on the built-in kernel, you gain little. See Troubleshooting for slow rebuilds.

What you need

Start the service

  1. Start ck-native. It listens on 127.0.0.1 (your own computer only), by default on port 7461.
  2. On its first start, the service creates an access token and stores it in its own configuration folder. It prints where the token file is. It never prints the token itself.
  3. To show the token so that you can paste it into the app, run ck-native --print-token. It prints the token and exits.

Treat the token like a password. Anyone who has it can run the kernel on your machine.

If you load the published app from a web address rather than running it yourself, start the service with --allow-origin and the app’s address. By default the service accepts only the local development address. See the kernel guide for the service’s options.

Switch the app to the service

  1. Open Settings: click the gear icon at the right of the top bar, or run Workspace settings from command search (F).
  2. Open the Kernel tab.
  3. For Kernel to use, choose Local service (faster, runs on this computer).
  4. Check Service address. The default is http://127.0.0.1:7461. Use 127.0.0.1 or localhost. Other addresses are not supported.
  5. Paste the token into Access token.
  6. Choose Test connection. It shows the kernel version, protocol version and number of cores, or says why the service cannot be used. A test switches nothing.

As soon as you change the mode, address or token, the open part is reopened on the new kernel. Your undo history is kept. To go back, choose Built-in (runs in this browser) and the part moves back.

Once you choose the service, a Kernel chip appears in the status bar. It does not show while you use the built-in kernel by choice. The chip reads:

ChipMeaning
ConnectingReaching the service.
Local followed by a versionConnected to the service.
Built-in (service off)You chose the service, but it could not be used. The built-in kernel took over.

Click the chip to open the Kernel tab.

The access token

  • The token is stored in this browser’s local storage and nowhere else. It is sent in a request header, never in an address, and it does not appear in notices, status text or logs.
  • Clear the Access token field to remove it from the browser.
  • Every request to the service must carry the token. A missing or wrong token gives “the token is missing or was refused”.
  • The service also supports pairing: a one-time code from ck-native --pair that a client exchanges for its own token, which can later be revoked with ck-native revoke. The app does not offer a pairing step yet. Paste the shared token as described above.

Same kernel or not at all

When the app connects, it checks two things:

  • The service speaks the same protocol version.
  • The service was built from the same kernel build as the one built into this app.

If either differs, the app refuses the service, stays on the built-in kernel, and shows a notice with the reason, for example “it is a different kernel build than this app”. The two kernels are never mixed inside one document. If you see this, build the service from the kernel version that matches the app.

If the service stops

If the service cannot be used when the app starts (not running, token missing or refused, or version mismatch), the app uses the built-in kernel and a notice says why.

If the service fails while you work, because it was stopped, restarted, timed out your session, rejected the token, or took more than five minutes to answer, the app:

  1. Shows one notice: “The local kernel service stopped: … The part was reopened on the built-in kernel.”
  2. Reopens the part on the built-in kernel from its last good state, keeping your undo history. The edit that was running when the service failed is not applied. Repeat it.
  3. Stays on the built-in kernel until you choose Try the service again in the Kernel tab, or change the setting. It never flips back and forth on its own.

A request that the service refuses for its own reason, such as a crash on one operation or a request that is too large, is reported on that request like an error from the built-in kernel. It does not trigger the fallback.

If you cancel a long rebuild, the request in flight is aborted and the service starts a clean session.

Browser caveats

Any web page can try to call a local server, so the service demands the token and checks where the request comes from. What a browser allows depends on where the app is loaded from. Treat the points below as things to test on your setup, not as guarantees.

  • The app served from your own computer’s development address, talking to 127.0.0.1, works in every browser.
  • The app served over https (a published site) calling http://127.0.0.1 is allowed in Chrome and Firefox for local addresses, if the service lists the app’s address as allowed. Recent versions of Chrome may ask once for permission to access devices on your local network. Allow it.
  • Safari may block an https page from calling an http address. Use the built-in kernel there.
  • The service is for the same computer only. A network or remote address is not supported.
  • Browser extensions or security software that block local connections make the test say “no answer from the service (is it running, and is the address right?)”.

Next

Commands and shortcuts

This chapter lists every command in the app with its exact label, where to find it, and its keyboard shortcut. Use it to look up a name you have seen, or to find the key for something you do often.

How to find a command

  • Ribbon. The tabs at the top: Home, Features, Frame, Sheet metal, Surfaces, View, Select, Evaluate and Assembly. While a sketch is open, the ribbon shows a Sketch tab instead.
  • Command search. Press F, or choose Search commands in the top bar, and type any part of a command’s name. Every command in this chapter is there with its shortcut. Press Enter to run the highlighted one.
  • Top bar. File commands (New, Open, Save, Export and more) live in the bar above the ribbon, not on a tab.
  • Right-click menu. The menu on the canvas lists the commands that suit what you have selected.
  • Tool palette. The palette at the left edge (when it is on) holds most modelling commands in sections.

Buttons that hold several related commands (for example Extrude with Extruded cut) are drawn once on the ribbon. The button runs the command you used last, and its flyout lists the rest. The tables below list every member of such a button separately, in the group where the button sits.

Where the ribbon shows a shorter caption than the command’s name, the table gives both. Command search and tooltips use the full label. A command is greyed out until it can run. The “Available when” column says what it needs.

Shortcut conventions

  • Ctrl means Ctrl on Windows and Linux and Cmd on macOS.
  • Single letters are used for view, pick and sketch tools, so most modelling commands use Shift plus a letter. For example Extrude is Shift+E.
  • While a sketch is open, the sketch tools take their own letters (for example L for Line), and the Shift+letter modelling shortcuts do not run. Combinations with Ctrl (such as Ctrl+S and Ctrl+Z) still work. See “Sketch tab” below.
  • Shortcuts do not fire while you are typing in a text, number or list field.

Ribbon tabs

Home tab

Sketch

Start a sketch. See Starting a sketch.

CommandRibbon captionShortcutAvailable when
Sketch on selected face or planeSketchSAn open document
Sketch on selected faceOn faceOne face selected
New sketch: front planeFront
New sketch: top planeTop
New sketch: right planeRight
New sketch from DXFDXF sketchAn open document
Import DXF into sketchImport DXFA sketch open
New sketch from SVGSVG sketchAn open document
Import SVG into sketchImport SVGA sketch open

Create

Solids, holes and the panels for Catalog, Variables and Script. See Extrude, revolve, sweep and loft and Holes and threads.

CommandRibbon captionShortcutAvailable when
ExtrudeShift+EAn open document
Extruded cutCutShift+CAn open document
Thin extrudeAn open document
Thin cutAn open document
Thin revolveA sketch with a construction axis line
RevolveShift+RA sketch with a construction axis line
LoftShift+OTwo or more sketches
SweepShift+WA closed sketch and an open path sketch
HoleShift+HOne face selected, or a sketch of points
ThreadShift+TCylindrical faces selected (face mode)
CatalogShift+KAn open document
VariablesAn open document
Script

Modify

See Fillets, chamfers, shells and drafts.

CommandRibbon captionShortcutAvailable when
FilletShift+FEdges selected, or two or more faces
ChamferShift+BEdges selected, or two or more faces
ShellShift+SFaces selected (face mode)
Press PullFaces selected (face mode). See Press Pull

Pattern

See Patterns, mirror and scale.

CommandRibbon captionShortcutAvailable when
Linear patternLinearShift+LA feature to repeat
Circular patternCircularShift+PA feature to repeat

Edit

See The feature tree and history.

CommandRibbon captionShortcutAvailable when
UndoCtrl+ZAn open document
RedoCtrl+Shift+ZAn open document
Repeat last commandAfter a command has run that can run again
RebuildCtrl+BNot while sketching
RenameF2Not while sketching
Suppress / unsuppressSuppressCtrl+Shift+UFeatures selected
Delete featureDeleteDeleteFeatures selected
Roll forwardRoll fwdThe history is rolled back
Group into folderCtrl+GTwo or more features selected

Features tab

Reference

Reference geometry. See Reference geometry and Curves on faces.

CommandRibbon captionShortcutAvailable when
PlaneShift+NAn open document
AxisShift+AAn open document
HelixA sketch with a circle
Project curveProjectA solid or a surface, and a sketch or curve to project
Edit curveA document with a curve to rebuild: picked edges, or a sketch or curve feature

Create

One button holds Gear, Gear pair, Propeller, Impeller, Knurl, Screw, Washer, Add fastener to hole, Spring, Nut, Standoff, Heat-set insert, Case, Tray and Bearing. See Parametric wizards.

CommandRibbon captionShortcutAvailable when
GearShift+YAn open document
Gear pairAn open document
PropellerAn open document
ImpellerAn open document
KnurlAn open document
ScrewAn open document
WasherAn open document
Add fastener to holeThe wall of a hole selected (also in the right-click menu of a Hole feature or a pattern of holes in the tree)
Teardrop holeThe wall of a round hole selected (face mode). See Teardrop holes for 3D printing
Heat-set seatThe wall of a round hole selected (face mode). See Heat-set seat on a hole
SpringAn open document
NutAn open document
StandoffAn open document
Heat-set insertAn open document
CaseAn open document
TrayAn open document
BearingAn open document

Modify

See Fillets, chamfers, shells and drafts, Cases and moulds (Split body, Lip joint) and Patterns, mirror and scale.

CommandRibbon captionShortcutAvailable when
DraftShift+GA solid and faces selected
RibA solid and an open sketch
Lip / grooveLipA solid and faces selected
MirrorShift+MA solid and a feature to mirror
Split bodyA solid
Lip jointA solid
ScaleA solid
Pipe cutA solid and faces or edges selected

Bodies

See Bodies and combining.

CommandRibbon captionShortcutAvailable when
Delete bodyDel. bodyA solid and a face selected
Delete faceDel. faceA solid and a face selected

Sheet metal tab

The tab between Frame and Surfaces. See Sheet metal.

Rules

CommandRibbon captionShortcutAvailable when
RulesRulesAn open document

Create

CommandRibbon captionShortcutAvailable when
Base flangeBaseNo first plate yet, and a closed sketch (selected or the last)
Edge flangeEdgeA sheet that is not unfolded
Contour flangeContourNo first plate yet, and an open chain of sketch lines
Convert to sheetConvertNo sheet yet, and a solid body
HemHemA sheet that is not unfolded
FoldFoldA sheet that is not unfolded, and a sketch with a line
CutCutA sheet that is not unfolded, and a closed sketch on a plane parallel to the base
CornerCornerA sheet that is not unfolded

Flatten

CommandRibbon captionShortcutAvailable when
UnfoldUnfoldA sheet that is not unfolded
RefoldRefoldAn unfolded sheet
Flat patternFlatA sheet

Export

CommandRibbon captionShortcutAvailable when
Flat pattern DXFDXFA sheet
Bend table (CSV)Bends CSVA sheet
Bend table (JSON)Bends JSONA sheet

Surfaces tab

Create

See Surfaces.

CommandRibbon captionShortcutAvailable when
Planar surfacePlanarA closed sketch
Extruded surfaceExtrudedA sketch with curves
Revolved surfaceRevolvedA sketch with an axis line
Lofted surfaceLofted
Fill surfaceFillShift+I
Extend surfaceExtendShift+X

Edit

See Surfaces and Curves on faces.

CommandRibbon captionShortcutAvailable when
Trim surfaceTrim
KnitAt least one surface
ThickenA surface
FreeformA solid or a surface, and faces selected

View tab

Views

Camera. See Moving around the model.

CommandRibbon captionShortcutAvailable when
Iso7
Top1
Front2
Right3
Back4
Left5
Bottom6
FitZ
Switch between perspective and parallel viewProjectionP
Switch the up axis between Y and Z (camera only)Up axis

Display style

Display style, hide and show. See Selecting things.

CommandRibbon captionShortcutAvailable when
ShadedAlt+1
Shaded with edgesWith edgesAlt+2
WireframeAlt+3
Hidden lines removedHiddenAlt+4
GhostAlt+5
Hide body or objectHideHSomething selected to hide
Show allAlt+HSomething hidden

Appearance

Lighting and background are radio choices. The Show menu turns display layers on and off, and stays open while you tick several. The command names for layers are the layer names.

CommandButtonRibbon captionShortcut
StudioLighting
FlatLighting
High contrastLightingContrast
TechnicalLighting
ThemeBackground
LightBackground
DarkBackground
GradientBackground
EdgesShow menu
SketchesShow menu
CurvesShow menu
PlanesShow menu
AxesShow menu
GridShow menu
RelationsShow menu
Overall sizeShow menuShift+D
ThreadsShow menu

Workspace

Panels and settings. See Units and settings.

CommandRibbon captionShortcutAvailable when
Command searchSearchF
Show or hide the side panelSide panel[
Toggle drawerDrawer\
Reset layout
Workspace settingsSettings

Select tab

Pick

See Selecting things.

CommandRibbon captionShortcutAvailable when
FaceQ
EdgeE
CornerV
BodyB
Select allCtrl+ANot while sketching
Invert selectionInvertCtrl+IAn open document with a body
Deselect allDeselectCtrl+Shift+ASomething selected
Box selectBoxX
Select bodyBodyAn open document
Show in treeA selection

Expand

Grow the current selection. See Selecting things.

CommandRibbon captionShortcutAvailable when
Select tangentTangentA selection
Select parallelParallelA selection
Select similarSimilarA selection
Select loopLoopA selection
Select connectedConnectedA selection
Select same sizeSame sizeCylindrical faces selected

Position

See Moving things: the move / rotate ball and handles.

CommandRibbon captionShortcutAvailable when
Move / rotate ballMove ballF10A selection that can be moved

Evaluate tab

Measure

See Measure and inspect.

CommandRibbon captionShortcutAvailable when
MeasureMA solid
Mass propertiesMassA solid
Interference checkOverlapA solid
Section viewSectionA solid

Surface analysis

See Surfaces.

CommandRibbon captionShortcutAvailable when
Zebra stripesZebraAlt+ZA body on screen
Gaussian curvatureGaussianA body on screen
Mean curvatureMeanA body on screen
Draft analysisDraft checkAlt+DA body on screen
Curvature combCombAlt+CA body on screen

Assembly tab

Components

See Assemblies and mates.

CommandRibbon captionShortcutAvailable when
Insert partAn open document
MateComponents in the document

Review

See Assemblies and mates.

CommandRibbon captionShortcutAvailable when
Bill of materialsBOMComponents in the document
Exploded viewExplodeComponents in the document
Interference checkOverlapComponents in the document

Top bar

These commands are not on a ribbon tab.

CommandWhereShortcut
New partNew part buttonCtrl+N (1, below)
OpenOpen buttonCtrl+O
SaveSave buttonCtrl+S
ExportExport menuCtrl+E
LibraryLibrary button
Search commandsSearch commands buttonF
Workspace settingsGear icon at the right

The More file actions menu (three dots, right of Export) holds the rest of the file commands:

CommandShortcut
Save asCtrl+Shift+S
Save geometry in file
Recover earlier versions…
Import STEP / STL / OBJ / GLB / 3MF / SolidWorks / SketchUp
Import SketchUp with hidden geometry
Rotate imported model

Save geometry in file is a switch. Rotate imported model is available only while an imported SketchUp model is on screen. See Saving and opening and Importing.

The Export menu lists:

CommandMenu caption
Export STL (binary)STL
Export STL (ASCII)STL text
Export OBJOBJ
Export STEPSTEP
Export sketch as DXFSketch DXF
Export 3 views as DXFViews DXF

An export command is available only when there is something to export: a solid, or for the sketch DXF a sketch. See Exporting.

The Part / Drawing switch at the right of the top bar switches between the model and its drawing sheet. See Drawings. Double-click the active document tab to rename the document; right-click a tab for Rename, Close and Close the other tabs.

Sketch tab

While a sketch is open, the ribbon shows one tab, titled “Editing” followed by the sketch name. Its groups, left to right, are Select, Finish (OK and Cancel), Make (Extrude, Revolve), Draw, Dimension, Constrain, Modify, Reference and Status. The tools below also appear in command search.

Sketch tools have their own single-letter shortcuts, active while a sketch is open and a text field is not focused.

GroupTools (shortcut)
DrawLine (L), Rectangle (R), Centre rectangle, Rounded rectangle, Circle (C), Centre arc, 3-point arc (A), Tangent arc, Ellipse, Polygon, Slot, Arc slot, Point, Text (Q), Centreline, Spline, Control-point spline, Add spline point, Bridge curve
DimensionDimension (D)
ConstrainHorizontal (H), Vertical (V), Coincident, Midpoint, Fix, Equal, Parallel, Perpendicular, Collinear, Tangent, Concentric, Symmetric
ModifyTrim (T), Extend (E), Fillet, Chamfer, Offset (O), Mirror, Linear pattern, Circular pattern, Move entities, Copy entities, Rotate entities, Scale entities
ReferenceProject edges (P), Construction (X)

See Sketch tools and Constraints and dimensions.

Right-click menu

The menu on the canvas depends on what is selected. Each row runs the command of the same name and shows the same shortcut and the same reason when it is disabled.

SelectionRows
NothingNew sketch: front plane, New sketch: top plane, New sketch: right plane; Extrude, Extruded cut; Select body, Select all, Invert selection; Fit
A faceSketch on selected face, Hole, Add fastener to hole, Teardrop hole, Shell, Fillet, Chamfer; Linear pattern, Circular pattern; Show in tree; Select tangent, Select parallel, Select similar, Select loop, Select connected; Invert selection, Deselect all
An edgeFillet, Chamfer; Show in tree; Select tangent, Select parallel, Select similar, Select loop, Select connected; Invert selection, Deselect all
A cornerFillet, Chamfer; Invert selection, Deselect all
A bodySelect body; Move body; Linear pattern, Circular pattern, Shell; Invert selection, Deselect all

Move body is listed but disabled with the reason “The kernel cannot move bodies yet” when the kernel in use does not support it.

Other commands outside the ribbon

CommandWhereNotes
AutoSelection mode bar over the viewport (switch it on in Workspace settings)A toggle. On, hover and click pick the corner, edge or face nearest the pointer. Off, you pick one kind with Q, E, V or B. It is not in command search.
Move bodyRight-click menu on a selected bodyListed but disabled when the kernel in use cannot move bodies. Not in command search.

Keys that are not commands

KeyDoes
Ctrl+YRedo (alongside Ctrl+Shift+Z). Not while sketching.
BackspaceDelete the selected features (alongside Delete).
EscClear the selection. Also cancels placing and closes dialogs.
Arrow keysOrbit the view in 15 degree steps when the canvas has focus.
Alt+arrow keysPan the view when the canvas has focus.
Alt+clickSelect the whole body.
Ctrl+Enter in the Script tabRun the script.
Shift+Alt+F in the Script tabFormat the script.
Ctrl+Tab, Ctrl+Shift+TabSwitch to the next or previous document tab. Use the Ctrl key, not Cmd. (1)
Ctrl+Alt+1 to 9Jump to a document tab (9 is the last).
Ctrl+Alt+T, Ctrl+Alt+WNew document tab, close the active tab.
Enter in a sketchConfirm the sketch (the same as OK).
R, F, Alt, Esc while placing a catalog itemRotate, flip, no snapping, cancel. See Catalog parts.

Arrow keys and Alt+arrow do not act while a sketch is open or when no document is open.

(1) In a normal browser tab, the browser may keep Ctrl+N (new window) and Ctrl+Tab / Ctrl+Shift+Tab (switch browser tab) for itself, so the app never sees them. If they do not respond, use the buttons or menus instead.

Next

Install as an app and work offline

This chapter covers installing CivilKit CAD as an app in its own window, using it without a network, how updates arrive, and what the app keeps on your device.

CivilKit CAD runs in the browser. After the first visit it can also start without a network, because the app files are saved on your device. Installing it is optional and only changes how it looks and starts.

Install it

Browsers that support installing a site offer it once the site qualifies (it is served over https and has its app files saved). When the app is installable, an Install button appears in the top bar. Its tooltip reads “Install CivilKit CAD as an app: its own window, and it opens without the browser.”

  1. Choose Install in the top bar.
  2. Confirm in the browser’s own install dialog.
  3. CivilKit CAD opens in its own window, and it gets an icon you can start from like any other app.

Per platform:

  • Chrome and Edge (desktop): use the Install button, or the install icon at the right end of the address bar. Once installed, double-clicking a .ckpart file can open it in the app (choose CivilKit CAD under Open with).
  • Android (Chrome): open the browser menu and choose Install app (or Add to Home screen).
  • Safari on Mac: choose File, Add to Dock.
  • Safari on iPhone and iPad: tap Share, then Add to Home Screen. There is no Install button in the top bar on these.
  • Firefox (desktop): does not install sites as apps; the app still works offline in a tab.

Notes:

  • The button shows only in browsers that offer installation, and only while the app is not already installed. If you do not see it, look for an install option in your browser’s menu or address bar.
  • Some browsers do not send the install offer the Install button depends on. There, use the browser’s own menu if it has an install or add-to-home-screen option.
  • The installed app has the name “CivilKit CAD” and runs in a standalone window without the browser’s address bar.
  • Uninstall it from your browser’s app list or your system’s app list. Your saved parts are files on your computer and are not removed.

Work offline

The first time you open the app with a network, it saves the app files on your device: the page, the program, the geometry kernel and the icons. After that:

  • The app starts without a network. If you open the page address with no connection, the saved copy loads.
  • Everything that runs in the browser works: sketching, modelling, saving to your computer, importing and exporting files.
  • Samples you opened before are available. A sample you have never opened is fetched when you first pick it, so it needs a network the first time.
  • Library parts are available offline only after you installed them or dropped them once. See The library and samples.
  • The local kernel service and the MCP server work on your own computer and do not need the internet either. See The local kernel service.

On a phone or tablet the geometry kernel (about 7 MB) is not saved when the app is installed, so the first load stays light; it is saved the first time the app starts the kernel, which happens as soon as you open or build a part. Open a part once while online before you rely on offline use there.

To be sure it works offline, open the app once while online and wait for it to finish loading.

Updates

When a new version is published:

  • The app checks about every five minutes, and whenever you return to its tab. If it finds a newer version, a notice appears in the top bar: “A new version (0.6.5) is available.” with Reload and Later (without the number if it cannot be read). Settings > About > Check for updates looks right away and shows the time of the last check.
  • Automatic. An installed app on an iPad is usually suspended, not closed, so it can sit on an old version for weeks. When you open it again (or it starts) and a newer version is out, the app reloads by itself and shows “Updated to 0.7.2” for a moment. It does this only when nothing is unsaved, no sketch, feature editor, wizard or dialog is open, and you have not touched the screen yet; in any other case you get the notice below and nothing reloads under your hands. After more than a minute in the background the check does not wait for the five-minute interval. Turn it off in Settings > General > Update automatically to always get the notice.
  • Reload reloads the app. If your part has unsaved changes, the app asks first what to do with them. Later dismisses the notice for now.
  • Without a network, the check quietly waits until the next try.
  • On the next load the app fetches the page from the network first and falls back to the saved copy. A deployed update is therefore picked up on your next online visit. The program files themselves have fixed names tied to their content, so an old copy never mixes with a new one. Older saved copies are removed automatically.

Files saved by earlier versions still open in newer ones.

What is stored on your device

All of this stays in your browser’s storage for this site. The app has no account and no cloud storage. Your parts go to a file only when you save.

WhatWhereWhy
App files and the geometry kernelBrowser cacheStarting offline and starting quickly.
Autosave of the open partLocal storageRestoring your work after a crash or a closed tab. Documents over about 3 MB of text are not autosaved.
Rolling snapshots of the open partBrowser databaseUp to ten earlier states, taken at most every 30 seconds while you work, for Recover earlier versions….
A saved picture of the model’s viewBrowser databaseShows a part before the kernel has rebuilt it. It is a cache and is rebuilt when stale.
Recent files and samples (names and thumbnails)Local storageThe recent list in the Library picker.
Workspace settings, theme, language, navigation and sketch preferencesLocal storageRemembered between visits.
Libraries you added, installed library parts and licence confirmationsLocal storage and browser databaseSee The library and samples.
Local kernel service address and access tokenLocal storageOnly if you use the service.

Saving a part with Save or Save as writes a file to your computer. In browsers that support direct file access, Save can overwrite the same file. Otherwise the browser downloads a new copy each time. See Saving and opening.

Clearing it

Clear this site’s data in your browser’s settings to remove everything above, including settings, libraries and the saved app files. That does not touch files you saved on your computer. Browsers may also clear a site’s storage on their own when disk space runs low, or after a long time without a visit. Save your work to files, and do not rely on autosave or snapshots as the only copy.

Private or incognito windows may block storage. The app still runs, but your settings and autosave last only for that session.

Next

Languages

This chapter covers which languages the app supports, how to change the language, and what stays in English whatever you choose.

What is supported today

The app ships in English only. English is also the fallback: if text is missing in another language, the English text shows.

The app is built so that another language is one more translation file with no change to the program itself. A partial translation is allowed, and anything not yet translated appears in English.

Change the language

  1. Open Settings: click the gear icon at the right of the top bar, or run Workspace settings from command search (F).
  2. On the General tab, find Language.
  3. Choose a language from the list.

The choice is remembered on this device.

The Language list appears only when the app has more than one language to offer. With English alone, there is nothing to choose, so the list is not shown. Development builds also offer a pseudo-language used for testing, which wraps English text in markers. It is not a real language.

What is translated

The interface text: ribbon tabs and buttons, command names, menus, dialogs, settings, tooltips and messages. Plural wording follows the rules of the chosen language. Numbers and units are formatted by the browser’s own number handling and the app’s unit settings, not by the translation file.

What is never translated

  • Your own names. Part names, feature names, sketch labels and body names stay as you typed them.
  • Messages from the geometry kernel. Error and hint text for failed features, for example a message saying a feature is still referenced by another, is English text built by the kernel layer. The app does not yet map the kernel’s error codes to translated messages.
  • Agent and script tooling. The text of the MCP server and its guides stays in English. See Agents and the MCP server.

Right-to-left layout is not supported yet.

Next

Troubleshooting

This chapter is a task list of common problems with their causes and fixes. The messages quoted here are the ones the app shows.

A feature failed

A failed feature shows in red in the feature tree, and the status bar counts the errors. The app sorts the failures into a cause and its consequences. One broken feature usually breaks everything built on it, so fix the cause first.

  1. Read the summary: “The edit broke the model at feature: reason.” It adds how many later features could not be built because of it.
  2. Under What to try the app gives advice for the cause.
  3. Choose Undo this change to go back, or Cancel edit if you are still in the feature’s editor. Select with a feature id selects that feature.
  4. Show consequences lists the later failures marked “blocked by id”. They should clear once the cause is fixed.

If an edit would break the model, it is not applied: “This edit was not applied; your model is unchanged.”

Reason shownWhat it means and what to do
it removes nothing / it cuts nothingThe cut no longer touches the body. Move the profile so it overlaps the body, or flip the cut direction.
a face or edge it uses no longer existsThe feature was built on a face or edge that is gone. Pick it again, or undo the change that removed it.
the combine failedTwo bodies could not be joined. Make sure they overlap in a volume, not just along a face, or nudge one by a small amount.
the rounding failed / does not fitUse a smaller radius, fewer edges at once, or round them in a different order.
the rounding runs off the faces beside itThe radius is wider than the faces next to it. Use a smaller radius, keep Tangent chain on, or round fewer edges.
the radius is too large for these edgesUse a smaller radius.
this edge or corner shape cannot be rounded yetRound fewer edges at once, use a chamfer instead, or leave the rounding to the end.
the corner needs exactly three edgesA corner chamfer needs a corner with exactly three edges. Pick another corner, or chamfer the edges.
the wall is thicker than the part allows / the shell could not be madeUse a thinner wall, or open a different face.
the sketch is not a closed outlineClose the gaps in the sketch, then try again.
the sweep failedCheck that the profile sits at the start of the path and that the path has no sharp kinks.
the loft failed / makes an invalid solidCheck the profiles have the same number of segments, run in the same order, follow each other along one direction, and do not cross. A point profile must be first or last.
the profile crosses the axisMove the profile to one side of the revolve axis.
the fill boundary is not validThe edges around the hole no longer form one closed loop. Pick the edges again.
the surfaces do not cut each otherThe trim tool no longer crosses the surface. Move the tool.

When none of these fits, the generic advice is: undo the last change, or adjust the values of the feature until it builds again.

See also Checks and diagnostics.

A command is greyed out

Hover the button to see the reason. Common ones:

  • “Open or create a part first”: there is no document.
  • “Select edges, or two or more faces, to round”: Fillet and Chamfer need edges, or two or more faces.
  • “Select a second face (or select edges) to round”: you have one face selected.
  • “Switch to edge selection to round edges”: you have edge-shaped picks while the pick mode is Face. Press E.
  • “Select one or more faces to leave open”: Shell needs faces.
  • “Draw a construction line for the axis”: Revolve needs a construction line in the sketch.
  • “Add a feature to repeat first”: a pattern needs something to repeat.
  • “Nothing to build this feature from: pick what it needs first”: the command needs a selection or a sketch of the right kind.

The Commands and shortcuts chapter lists what each command needs.

“These faces do not share an edge”

You selected two or more faces to round but none of them meet along an edge. Select faces that touch, or select the edges directly.

Rebuilds are slow

  • A Rebuilding model… panel with a timer appears for slow work, with a Cancel button. Cancel stops the rebuild.
  • The status bar shows Last rebuild with the time of the latest one.
  • When you open a saved part, a Cached view chip shows the stored picture while the model rebuilds. Edits wait for the rebuild to finish; picking is available a moment later.
  • Heavy features cost the most: modelled threads (the thread editor shows “About n s to rebuild, many more triangles”), long patterns, gears with many teeth, propellers and impellers, and free-form lofts. Use cosmetic threads while you design, and switch to modelled threads at the end.
  • Suppress features you do not need while you work. See The feature tree and history.
  • Very large parts (over 150 features) get a smaller memory cache, which trades some speed for memory.
  • The local kernel service runs the kernel natively on your own computer and is faster on large parts.
  • Close other busy tabs. The browser kernel shares your computer’s memory with them.

A variable change was refused

“The part would not rebuild with that change, so nothing was changed.” The new value breaks a feature (for example a hole bigger than its plate). Try a value nearer the old one, or fix the feature the value feeds.

Imports fail

Drop or open a file, or use Import STEP / STL / OBJ / GLB / 3MF / SolidWorks / SketchUp in the More file actions menu. The messages:

MessageFix
“Cannot open name: only .ckpart, .json, .step, .stp, .stl, .obj, .glb, .3mf, .sldprt, .skp, .dxf, .svg, .FCStd and .solidcraft files are supported.”Convert the file to a supported format.
“Drop one file at a time.”Drop the files one after another.
“Open or create a part first, then import the STEP file.”Use New part, then import.
“Could not import name: message”The message names the cause. See Importing.
“Imported bodies are view only and are not saved with the part.”This is a notice, not an error. STEP and SketchUp imports appear as view-only bodies, and so does a SolidWorks part that could not be built as an editable body.
“SketchUp surface model: n open edges; solids operations may not apply.”The file is a surface model, not a closed solid.
“n hidden faces were left out.”Choose Show hidden geometry or Import SketchUp with hidden geometry to include them.

DXF import into a sketch:

MessageFix
“Open a sketch first (or use New sketch from DXF)”Open a sketch, or use New sketch from DXF.
“Binary DXF is not supported. Save the drawing as ASCII DXF” and “That file is not an ASCII DXF”Re-save the drawing as ASCII DXF.
“The DXF has n entities; the limit is max.”Simplify the drawing. The limit is 20,000 entities.
“The DXF has coordinates beyond max mm from the origin; move the drawing near the origin and try again”Move the drawing close to the origin in your drawing program.
“Nothing to import: the DXF has no lines, arcs, circles, polylines or splines”The file has only entities the importer does not read, such as text or dimensions.
“The DXF uses a unit code (n) that is not converted; read as millimetres”Check the size, and scale if needed.

SVG import into a sketch:

MessageFix
“Open a sketch first (or use New sketch from SVG)”Open a sketch, or use New sketch from SVG.
“That file is not an SVG drawing”The file is not text SVG (a compressed .svgz, or another format). Save it again as plain SVG.
“The SVG declares entities, which are not read. Save it again as plain SVG”Export the drawing again without a custom DOCTYPE.
“The SVG has n entities; the limit is max.” and “The SVG file is larger than n MB”Simplify the drawing. The limits are 20,000 entities and 10 MB.
“The SVG has coordinates beyond max mm from the origin; make the drawing smaller or move it near the origin and try again”Scale the drawing down or move it close to the origin in your drawing program.
“Nothing to import: the SVG has no paths, rectangles, circles, ellipses, lines or polygons”The file has only text, images or other content the importer does not read. Convert text to outlines first.
“The SVG has no size in mm, cm, in or pt, so 1 px = n mm (96 dpi) was assumed”Check the size of the sketch and scale it if needed, or give the SVG a width and height in mm and a viewBox.
“n element(s) use a clip path, mask or filter, which is ignored”The whole shape was imported. Trim the sketch yourself where the clip would have cut it.
“The imported geometry could not be solved”Check the drawing for overlapping or contradictory geometry.

For FreeCAD files, the message says how many features were mapped and lists the first warning. Features that the app cannot convert are listed. See File formats at a glance.

Exports fail or look wrong

MessageFix
“There is no solid to export yet”Build a solid first.
“Open a sketch or select one in the feature tree to export it”A sketch DXF export needs a sketch.
“The sketch has no geometry to export”Draw something first.
“name is not watertight (n open edges, n non-manifold edges): a slicer may need to repair it”The mesh has gaps. Use Check to find the cause, or export STEP for a clean solid.
“n sketch entities could not be written to the DXF”Those entities have no DXF form. The rest is written.
“Could not export: message”The message names the cause.

See Exporting.

Saving problems

  • “Could not save: message”. The browser refused to write the file. Check the folder’s permissions and free disk space, then try Save as.
  • Save downloads a new copy every time. Your browser does not support saving over the same file. Each save is a new download. Move the newest one over the old one yourself.
  • “This part is too large for automatic backup in the browser. Save it to a file to be safe.” Autosave skips documents over about 3 MB of text. Save to a file regularly.
  • “The browser has no room left for the automatic backup. Save to a file to be safe.” Browser storage is full. Clear other site data or save to a file.
  • “Automatic backup is not available in this browser.” Storage is blocked, for example in a private window. Save to files.
  • A recent file does not reopen. “name can only be reopened with Open” or “The browser did not give access to name again”: use Open and pick the file again.
  • You closed the tab before saving. On the next start, “Restore your last session?” offers Restore or Start new. Choose Earlier versions… to open the rolling snapshots, or use Recover earlier versions… from the More file actions menu. Snapshots are kept for the open part: up to ten.

Your parts are not stored anywhere but on your device. See Install as an app and work offline.

Unsaved changes

The “Unsaved changes” dialog (“Save changes to name before you continue?”) appears before you open another part, run a script, or reload for an update. Choose Save, Don’t save, or Cancel.

The 3D view is blank or very slow

The viewport is drawn with WebGL. If it stays blank:

  • Make sure hardware acceleration is on in your browser’s settings.
  • Update your graphics driver and the browser.
  • Try another browser.

The library

Messages from the Libraries tab and what to do:

MessageFix
“Only https addresses are accepted.”Use an https address or github:owner/repo.
“That is not a library address.”Check the address.
“The library could not be reached.”You may be offline. The saved copy keeps working.
“The downloaded part does not match its checksum and was refused.” / “does not have the size the library lists”The file changed or was damaged. Do not use it. Refresh the library.
“This part is not saved on this device and there is no network.”Install the part while online.
“That library is already in the list.”Nothing to do.
“Parts library shapes need a flat face”Drop on a flat face. Primitives work on curved faces.
“Nothing to cut yet: drop a block first”Cuts and edge rounders need a body.

See The library and samples.

Scripts

A script error shows as “Line n: message”. Click it to select the line. If the script builds no part, it says “the script builds no part: start with part(“Name”)“. See Scripting for limits (40,000 characters, 2,000 steps, 100,000 loop turns).

Wizards

  • Propeller, marine: “The hub fuse failed at n degrees; built with a section spacing of m degrees.” is not an error. The wizard retried and succeeded. If nothing builds, try a section spacing of 6 or 7 degrees, or a pitch/diameter ratio above 0.8.
  • Impeller: “Built with n sections per blade instead of m” likewise.
  • Gear: a warning about undercut offers Use shift. See Parametric wizards.

The local kernel service

“The local kernel service is not used” and “stopped” notices give the reason: no answer from the service, token missing or refused, a different build than the app, or a timeout. The app falls back to the built-in kernel. See The local kernel service.

The app will not update or start offline

  • A New version is available notice means you have an older tab open. Choose Refresh.
  • To start offline, you must have opened the app once online. See Install as an app and work offline.
  • If the app misbehaves after an update, reload the page. If that does not help, clear the site’s data in the browser. Save your work to files first, as this removes settings, snapshots and autosave.

Still stuck

Save your part to a file, note the message you see and the steps that led to it, and compare with Limits and known gaps, which lists what the app does not do.

Next

Limits and known gaps

This chapter lists what the app does not do, or does not do reliably, so you can plan around it. Each item says what happens and, where there is one, the workaround. Items are ordered roughly by how soon you are likely to meet them.

The geometry kernel has its own, more technical list of limits in the kernel guide.

Check the result

  • A part can build and still be wrong. In some cases the kernel returns a valid-looking solid whose volume differs from the true one. This has been seen with overlapping curved primitives, outward shells and three-section lofts. Run Check and compare Mass properties with what you expect. See Checks and diagnostics.
  • The picture is a mesh. The 3D view draws a tessellation of the exact solid. Exact volumes, areas and sizes come from Mass properties and Measure, not from the mesh. Rarely, a small crack appears in the mesh of an imported or text part (TESSELLATION_OPEN in the check). The solid is still valid.
  • Misspelled settings in files you edit by hand can be ignored. A field with an unknown name is skipped without a warning, and the feature uses its default. If you edit a part file as text, compare the result with Mass properties.

Rounding, shells and booleans

  • Large fillet radii are refused. A radius that approaches half the thinnest side of the part answers “the radius is too large for these edges” or “the rounding runs off the faces beside it”, even when the shape is geometrically possible. Use a smaller radius, or round in steps.
  • Corner blends are limited. Unequal radii at a corner where three edges meet end in a mitre, not a smooth patch. Variable-radius fillets are the weakest case. Rounding a loop of tangent edges can occasionally take very long or fail.
  • Outward shells and shells of drafted cylinders often give a wrong volume. Prefer inward shells, or build the wall with offsets and cuts.
  • Booleans on curved shapes are the weak spot, especially anything involving a torus, cones against cylinders, or chains of three curved bodies. If combine fails (“the combine failed”), make the bodies overlap in a volume, nudge one by a small amount, or reorder the operations.
  • Long patterns (about 100 instances) make a combine take seconds to tens of seconds.
  • Lofts: there is no closed (ring) loft. A three-section circle loft is a different surface from a smooth loft-through-sections, so volumes can differ noticeably. There is no sweep control over the profile’s orientation along the path.
  • Threads: pipe-thread tapers, threads on conical faces and rounded thread roots are not modelled.
  • Sheet metal is partial. Base, edge and contour flanges, hems, folds, cuts, corners and the flat pattern exist (see Sheet metal); flanges on curved edges, a jog, a mitre flange, louvres and forming tools do not, and its Known limits list the rest.
  • Sketch text is planar and single-line. It does not wrap onto curved faces and does not support complex scripts.

Surfaces and analysis

  • There is no surface sweep, no offset surface, no surface-by-network, and no mesh-to-solid conversion.
  • Surface analysis (zebra, curvature maps, draft analysis, curvature comb) is computed on the displayed mesh, not on the exact surfaces. It does not compare continuity between faces.
  • Extend surface takes one border edge at a time.

Assemblies and appearance

  • A part can hold inserted components and mates. A mate refers to faces, not edges.
  • Some mate kinds are not available: profile centre, path, linear coupler, cam and universal joint. A hinge has no built-in angle limit; add a Limits mate (distance or angle) to restrict its range.
  • A part has one material for mass properties. A custom material lives in the browser that made it. A file that names a custom material, opened elsewhere, keeps the name, and Inspect then asks for a density.
  • Colours and appearance are view settings. They are not an undo step, and they are not exported to STEP.
  • Insert from the library does not carry over the appearance of the inserted part.

Importing

  • View only is a choice, not the rule. STEP and SketchUp ask which of the two you want when they open, and remember it per kind. The default for STEP is an imported solid feature saved with the part; the default for SketchUp is a reference mesh saved with the part. View only gives a body that is drawn but not saved with the part, and the next edit replaces it. A SolidWorks part opens as an editable imported body that is saved with the part. When both the feature history and the exact-solid import fail, the part opens view only.
  • STEP import does not read assemblies, placements, colours or names. Shell-based surface models and open shells are not imported. A small share of files in real use import with defects.
  • SolidWorks import reads the geometry of the active configuration only, and rebuilds the feature history only where the kernel can; otherwise the part opens as the file’s exact solid with no feature tree. Sheet and wire bodies are refused. A file whose geometry the kernel cannot read to a closed solid is refused.
  • SketchUp import is a surface body of planar faces: no curves, dimensions, scenes or text. Files over 50,000 faces are refused by default.
  • OBJ, GLB and 3MF open as reference meshes only. They do not become a solid, textures are not read, and a file with several objects comes in as one mesh. Ask for a STEP file when you need a solid.
  • DXF import reads ASCII DXF only, up to 20,000 entities and coordinates within 1,000,000 mm of the origin. Splines with a general knot vector become short line segments. Unsupported entity types, such as text and dimensions, are skipped and listed.
  • SVG import reads paths, rectangles, circles, ellipses, lines, polylines and polygons (with groups, use of shapes in the same file, and transforms), up to 20,000 entities, a 10 MB file and coordinates within 1,000,000 mm of the origin. Text, images, scripts, fills, strokes, gradients and clip paths are not read; an element with a clip path or mask is imported whole. A file that declares entities is refused. Without a size in mm, cm, in or pt, a pixel is taken as 0.2646 mm (96 dpi).
  • FreeCAD files convert feature by feature. Features the app cannot convert are listed, and the resulting geometry may be partial. Fillets and chamfers are left out; add them again in the app. See Importing.

Exporting

  • Model export formats are STEP, binary and ASCII STL, OBJ, 3MF, glTF (GLB), and DXF (a sketch, or three views). Drawings have their own exports: PDF, SVG, DXF and print. The bill of materials saves as CSV. See Exporting and Drawings.
  • STEP export writes geometry only: no colours, names, layers or assemblies.
  • DXF export of a sketch uses layer 0 and a CONSTRUCTION layer. The three-view model DXF has no hidden lines, dimensions or text and uses a single layer. The drawing DXF is richer, with one layer per line style (see Drawings).
  • STL and OBJ are meshes, with the mesh tolerance noted above. Use STEP when you need exact surfaces.

Library and catalog

  • Mirror in the Placement row is not applied to library parts. Rotate and Direction apply only to drops on a plane or the ground.
  • A library part drawn on several planes, tied to fixed directions, or an assembly, lands at its own origin.
  • Parametric catalog parts need a flat face, edge rounders act on every edge of the face, and only two anchors (bottom and centre) are offered.
  • Private GitHub repositories are not supported, and a folder library is remembered only through its saved copy.
  • There is no download progress bar.

Wizards

  • Gears: spur, ring, helical, herringbone and rack. No bevel or worm gears. Large gears rebuild slowly.
  • Marine propeller: joining a blade to the hub can fail for some section spacings, especially for a low pitch at the hub. The wizard retries other spacings. The root of the blade has no fillet. A rake of about 25 degrees or more can leave small gaps in the display mesh.
  • Impeller: one blade shape, no shroud surface, no root fillet, fixed hub contour.
  • Airfoil propeller: no root fillet; the blade shape is fixed when built, so change it in the wizard.
  • Corner holes: exact only for a flat rectangular face with equal corner radii. Other outlines use the bounding box.
  • Nuts, standoffs and heat-set inserts: the dimensions are entered from the standards’ and catalogues’ public tables and are marked unverified until checked. No nyloc rings, flanges or wings, no washer face on a nut.
  • Springs: only the geometry is made, not the spring rate or the stress. Closed and ground springs, cones, progressive, extension and torsion springs are wound along a curve and take a few seconds to preview.
  • None of the wizards calculates strength or performance.

Automation

  • A script run from the Script tab builds a new part. It does not change the part you have open. An agent linked in Settings can run a script on the open part (app_run_script), and its features are added after yours as one undo step; see Agents and the MCP server.
  • Scripts are limited to 40,000 characters and 2,000 steps. They are not sandboxed against hostile code.
  • Sketches drawn by a script are plain geometry without constraints; sketchFeature takes a raw sketch with constraints.
  • The MCP server is a separate local program with its own document, started from a source checkout. See Agents and the MCP server.
  • The local kernel service is experimental, works only on the same computer, and needs a build that matches the app.

Platform

  • English only. No right-to-left layout. Kernel error text is English. See Languages.
  • Browser storage may be cleared by the browser or blocked in private windows. Autosave skips parts over about 3 MB of text. Save to files.
  • Saving over the same file works only in browsers with direct file access. Others download a new copy each time.
  • Memory. The in-browser kernel keeps caches in memory that does not shrink while the tab lives. A part of several hundred features can take about half a gigabyte of the tab’s memory. Close other tabs, or use the local kernel service.
  • The kernel is single-threaded. Free-form parts, propellers and long patterns take seconds to tens of seconds in the browser. The local kernel service is about two to three times faster.

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Glossary

Terms you will meet in the app and in this guide, in alphabetical order. Where a chapter covers the idea in depth, the entry links to it. For the technical meaning of a term inside the geometry kernel, see the kernel glossary.

Assembly A part document that holds other parts as components and relates them with mates. The ribbon opens the Assembly tab for such a document. See Assemblies and mates.

Autosave A backup of the open part that the app keeps in the browser while you work. It is not a substitute for saving a file. See Install as an app and work offline.

Body One connected solid piece of the model. A part can hold several bodies, for example two blocks that do not touch. You can select a body as a whole in Body pick mode. See Bodies and combining.

Bore A round hole through the middle of a part, such as a shaft hole in a gear or a propeller hub.

Catalog The side-panel tab with ready-made shapes and parts that you drop onto a face. See Catalog parts.

Chamfer A flat bevel that replaces a sharp edge. See Fillets, chamfers, shells and drafts.

Command search The pop-up opened with F that finds any command by name and shows its shortcut. See Commands and shortcuts.

Component A part placed inside an assembly. A component can be fixed in place or free to move until mates hold it. See Assemblies and mates.

Configuration A named set of variable values. Choosing one switches the variables to its values and rebuilds the part. See Equations and variables.

Constraint A relation inside a sketch, such as horizontal, tangent or equal, that the sketch solver keeps true when you change something. See Constraints and dimensions.

Construction geometry Sketch lines and curves that guide the drawing, such as a revolve axis, but do not form part of the outline. See Sketch tools.

Cosmetic thread A thread shown and described on a hole or a cylinder without modelling the helix. It is quick to rebuild. A modelled thread has the real helix and is slower. See Holes and threads.

Cut A feature that removes material, such as Extruded cut. See Extrude, revolve, sweep and loft.

Datum A reference plane, axis or point you add to build on, such as a Plane or Axis feature.

Dimension A sketch constraint that fixes a size or distance to a value, such as a length or a radius. See Constraints and dimensions.

Draft A small taper on a face, so that a moulded or cast part can be released from its mould. See Fillets, chamfers, shells and drafts.

Edge A line or curve where two faces meet, or the boundary of a face. Edges are what Fillet and Chamfer work on. See Selecting things.

Exploded view An assembly display that moves components apart so you can see each one. It is a view setting and does not change the model.

Extrude A feature that pushes a sketch profile along a direction to make a solid. See Extrude, revolve, sweep and loft.

Face A bounded piece of the surface of a body, such as the top of a block or the wall of a hole. Faces are what you sketch on and what Shell opens. Each face has a persistent name so later features can keep referring to it.

Feature One step in building a part: a sketch, an extrude, a fillet, a hole, a pattern, a plane and so on. Features run in order from the top of the feature tree to the bottom. See The feature tree and history.

Feature tree The list of features in the left panel. It shows the order of building, which features failed, and what depends on what. Also called the history.

Fillet A rounded blend that replaces a sharp edge. See Fillets, chamfers, shells and drafts.

Fully defined A sketch is fully defined when its constraints and dimensions leave nothing free to move. The sketch status shows whether it is fully defined. See Constraints and dimensions.

Ground plane The horizontal reference plane for the current up axis. It is Top when Y is up and Front when Z is up. The first body of a catalog drop sits on it.

Handle A small arrow or dot in the viewport that you drag to change a size, a depth or a radius. See Moving things: the move / rotate ball and handles.

Interference An overlap between bodies or components. The Interference check command finds overlaps. See Measure and inspect.

Kernel The geometry engine that builds, measures and checks solids. It runs inside your browser, or as a local service on your computer. See The local kernel service.

Library A source of parts you can drop into a model: the bundled samples, the parametric catalog parts, and libraries you add. See The library and samples.

Loft A feature that joins two or more sketch profiles with a smooth solid. See Extrude, revolve, sweep and loft.

Mass properties The volume, surface area, centre of mass and mass of a body, computed exactly from its faces. The mass uses the part’s material. See Measure and inspect.

Mate A relation between two components of an assembly, such as coincident, angle or hinge, that fixes some of their relative motion. See Assemblies and mates.

Mesh The triangles the app draws. The exact solid is turned into a mesh for display. Sizes and volumes come from the exact solid, not from the mesh.

Move / rotate ball The ball you place on a selection (F10) to move, turn and copy it. See Moving things: the move / rotate ball and handles.

Part One document, saved as a .ckpart file, that holds a list of features and builds a model. Files saved by earlier versions still open. See Saving and opening.

Pattern A feature that repeats other features in a line (Linear pattern) or around an axis (Circular pattern). See Patterns, mirror and scale.

Persistent name The stable name of a face or edge, such as F2.C1. Because it comes from the feature that made it, later features that use it keep working after you edit earlier ones.

Profile A closed outline in a sketch that a feature uses, for example the outer rectangle and the circles inside it. An outline with gaps is not a profile, and the app says “the sketch is not a closed outline”. See Starting a sketch.

Rebuild Running all the features again, from the top, to produce the model. The app rebuilds after most edits, and the Rebuild command forces it. Also called regeneration.

Reference plane One of the three standard planes (Front, Top, Right) or a plane feature you add. Sketches sit on planes and on flat faces. See Starting a sketch.

Revolve A feature that spins a sketch profile around an axis to make a solid. It needs a construction line for the axis. See Extrude, revolve, sweep and loft.

Rollback Moving the build point back up the feature tree, so the model shows only the features above it. Roll forward returns. Features below the marker are kept but not built. See The feature tree and history.

Section view A cut-away display that shows the inside of a body at a plane. It is a view setting. See Measure and inspect.

Shell A feature that hollows a body, leaving walls of a chosen thickness and opening the faces you select. See Fillets, chamfers, shells and drafts.

Size box The box of handles shown around a selected shape, for resizing and moving it. See Moving things: the move / rotate ball and handles.

Sketch A flat drawing of lines, arcs, circles and curves on a plane or a face, with constraints and dimensions. Features turn sketches into solids. See Starting a sketch.

Solver The part of the app that moves sketch points so the constraints and dimensions are satisfied. See When a sketch will not solve.

Suppress Switch a feature off without deleting it. A suppressed feature is skipped on rebuild, and features that depend on it fail until you Unsuppress it. See The feature tree and history.

Surface A face or group of faces with no thickness, not a closed solid. You can build surfaces, trim and knit them, and Thicken them into solids. See Surfaces.

Sweep A feature that moves a profile along a path to make a solid. See Extrude, revolve, sweep and loft.

Thin feature An extrude or revolve that makes a wall of a set thickness instead of a filled solid.

Tolerance A distance below which two things are treated as the same. It matters when files from other programs have tiny gaps, and when two bodies almost touch. The check tools report problems that exceed it. See Checks and diagnostics.

Valid A body is valid when the check finds no open edges, bad orientation or other defects. A feature can build and still produce an invalid body. See Checks and diagnostics.

Variable A named value, such as a width, that features use through an expression and that you edit in the Variables tab. Changing it rebuilds the part. See Equations and variables.

View-only body A body from an imported STEP, SolidWorks or SketchUp file. You can look at and measure it, but it is not a feature of the part and is not saved with it. See Importing.

Wizard A guided panel that builds a whole part from a few parameters, such as the gear, propeller and impeller wizards. See Parametric wizards.

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