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
- Draw the sketch (or sketches) first. See Starting a sketch.
- 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.
- Change the options. The preview follows every change.
- 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.
| Option | What it does | Default |
|---|---|---|
| Profile sketch | The sketch to extrude. Pick changes it. | The sketch chosen as above |
| End condition | How far the extrusion goes (see below). | Blind |
| Depth | Length in mm. Shown for Blind and Mid plane. For Mid plane it is labelled Total depth. | 10 mm |
| Operation | New body, Add or Cut (see below). | Chosen from the situation |
| Body name | Name of the new body. Shown for New body. | Body 1, Body 2, … |
| Flip direction | Extrude the other way. Not shown for Mid plane or Through all, both ways. | Off |
| Draft angle | Tapers the walls, in degrees. 0 means straight. Not available for Mid plane or Through all, both ways. | 0 |
| Draft outward | Tapers the walls outward instead of inward. Shown when the draft angle is above 0. | Off |
| End scale | Scales 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 wall | Builds a wall around the curve instead of filling it (see Thin walls). | Off |
| Shapes | One 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 condition | The extrusion goes |
|---|---|
| Blind | The Depth you type, from the sketch plane. |
| Mid plane | Half the Total depth each side of the sketch plane. |
| Through all | From the sketch plane through the whole body. |
| Through all, both ways | Through the whole body on both sides of the sketch plane. |
| Up to next | To 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.
| Option | What it does | Default |
|---|---|---|
| Thin wall | Switches the wall on. | Off |
| Wall thickness | Thickness in mm. | About 10% of the profile size, at least 1 mm |
| Side | Inside, 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 thickness | Thickness of the second side. Shown for Both. | Same as Wall thickness |
| End caps | Flat or Round. Shown when the sketch has an open chain. | Flat |
| Corners | Mitre 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.
- 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.
- 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.
| Option | What it does | Default |
|---|---|---|
| Profile sketch, Axis | The sketch and its axis line. | First construction line |
| End condition | Blind turns from the sketch plane by the Angle. Mid plane centres the turn on the sketch plane. | Blind |
| Angle | Degrees of turn. For Mid plane it is labelled Total angle. | 360 |
| Operation, Body name | Same controls as Extrude. A new Revolve always starts as Add | Add |
| Flip direction | Turn the other way. Not shown for Mid plane. | Off |
| Thin wall, Shapes | As 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.
- 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.
- Draw the profile as a closed shape in a second sketch on a plane that is perpendicular to the path at its start.
- 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.
| Option | What it does | Default |
|---|---|---|
| Profile (closed) | The profile sketch. | Newest unused closed sketch |
| Path (open) | The path sketch. | Newest unused open sketch |
| Guide curves | Open sketches the profile scales to follow. Add guide adds one; the guide must be as long as the path. | None |
| Twist over the path | Degrees of turn along the path. Hidden when there are guide curves. | 0 |
| Operation, Body name | As 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.
- Draw one sketch per profile, each closed, on its own plane (for example offset planes).
- Select the profile sketches in the tree in the order you want, using Ctrl-click, or leave nothing selected.
- 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.
| Option | What it does | Default |
|---|---|---|
| Profiles | The 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-order | Appears when the profiles do not follow each other along the loft. One click sorts them. | |
| Guide curves | Open 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 name | As for Extrude. Hidden for a surface. | Add |
| Start tension, End tension | How 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:
| Option | What it does | Default |
|---|---|---|
| Radius | Ball radius in mm. | Half the size set when it was dropped |
| Centre X, Centre Y, Centre Z | Position of the centre in mm. | Where it was dropped |
| Operation | New body, Add or Cut. | As dropped (Add or Cut) |
| Body name | Name 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
| Symptom | Cause 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 nothing | The 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 add | The sketch plane did not touch the existing body. Switch Operation to Add. |
| Extrude with a draft is shorter than Depth | The taper closes to a tip. Lower the angle or the depth. |
| Revolve fails | No construction line, or the profile crosses it. |
| Loft twists or folds | Profiles 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.