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.
| From | How |
|---|---|
| A blank part | The Start here card offers Sketch on Front Plane, Sketch on Top Plane and Sketch on Right Plane. |
| The ribbon | On 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 keyboard | Select 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 view | Press 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 viewport | Select 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 menu | With 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 this | Do this |
|---|---|
| Keep the sketch | Click 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 it | Click Extrude in the Make group. The sketch is finished and the Extrude editor opens on it. |
| Keep the sketch and revolve it | Click 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 editing | Click 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+Hor Show all brings everything back. - Select a sketch and press
Hto 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.