Sketching
Solids in Shack CAD start as sketches. A sketch is a set of curves on a flat surface; any closed area the curves enclose can be extruded into a solid. Sketches are saved in the project and stay editable.
Starting a sketch
| To sketch on | Do this |
|---|---|
| The XY plane | Sketch in the tool rail, or Model ▸ Sketch on XY Plane… (⌘K) |
| The XZ or YZ plane | Model ▸ Sketch on XZ Plane… or Model ▸ Sketch on YZ Plane… |
| A flat face of a body | Select the face, then Sketch on face in the bar over the viewport, On face in the tool rail, or Model ▸ Sketch on Selected Face… (⇧⌘K) |
XY is the ground plane the build plate sits on. A sketch on a face lies in the plane of that face, and that body becomes the target for any join or cut made from the sketch.
Only flat faces can host a sketch. A curved face can be selected, but the bar over the viewport explains that it cannot be sketched on.
The sketch bar
While a sketch is open, a bar across the top of the viewport holds everything you need. From left to right:
- the name of the surface and the number of curves drawn so far;
- what clicking does: Draw, Curves, Relate or Areas;
- the drawing tools;
- Construction, End chain, and the sketch's own undo and redo;
- Navigate, Cancel and Exit, which are always visible.
Drawing tools
Choosing a tool also switches clicking back to Draw.
| Tool | How to draw |
|---|---|
| Line | Click each point. Click the first point again to close the loop. Press Return, Esc or End chain to stop without closing. |
| Circle | Click the centre, then a point on the circle, or drag out from the centre. |
| Centre rectangle | Click the centre, then a corner. |
| Rectangle | Click two opposite corners, or drag between them. |
| 3-point arc | Click the start and the end, then a point the arc passes through. |
| Ellipse | Click the centre, then the end of the long axis, then a point giving the width. |
| Polygon | Set the number of sides first, then click the centre and a corner. |
While Show dimensions while drawing is on (the default), dimension chips show the size of the shape as you draw. Click a chip to type an exact value, such as a rectangle's width or a circle's diameter. Esc while typing puts the chip back to the value it had.
Construction geometry
Turn on Construction before drawing to make reference curves. Construction curves can be snapped to and are saved with the sketch, but they never bound an area, so they are not extruded.
Snapping
Points snap as you draw, and a small label names what was snapped to: Grid, Endpoint, Centre, Origin, Horizontal or Vertical.
Snapping is set in App Settings ▸ Sketching:
| Setting | Effect |
|---|---|
| Snap to grid | Points land on the grid. |
| Snap to endpoints and origin | Points land on existing endpoints and centres, and on the sketch origin. |
| Snap horizontal and vertical | Points align horizontally or vertically with the previous point. |
| Grid step | The grid spacing, 1 mm by default. |
Curves
Switch to Curves to pick a curve you have drawn. Its size is shown, and you can make it construction geometry or delete it.
Closed areas
Switch to Areas to pick what will be extruded. Shack CAD finds every closed area the curves enclose, and the bar says how many there are.
- Click inside an area to pick it. ⇧-click adds or removes another.
- An area with another closed shape inside it, such as a rectangle around a circle, is picked with the inner shape left open as a hole. Click inside the inner shape instead to pick it on its own.
- If nothing is enclosed yet, the bar says No closed area yet. Check that the outline really closes.
Picking an area opens the extrusion controls. See Extrude.
Undo inside a sketch
While a sketch is open, ⌘Z and ⇧⌘Z step through the sketch's own history. When you press Exit, the whole sketch becomes one step in the project's Undo.
Leaving a sketch
- Exit saves every curve drawn as one undoable step and closes the sketch.
- Cancel leaves without saving. Esc first clears a half-placed shape; pressed again, it leaves the sketch.
Editing a sketch later
Sketches are listed in the bodies list. Right-click one and choose Edit to reopen it. When you exit, bodies built from that sketch are rebuilt from the new curves.
If an edit changes the sketch so that the area a body was built from can no longer be identified with certainty, such as a hole grown past the outer boundary, Shack CAD refuses the rebuild rather than picking a different area.