Sketching and constraints
Draw the profile, fix it with constraints and dimensions, and keep it editable.
Starting a sketch
Choose a datum plane in the Browser, or a planar face on an existing body, and start a sketch from the ribbon or command search. The Sketch tab appears, and the rest of the ribbon stays available.
A sketch is a 2D profile on that plane. When you finish it, closed regions become profiles that features such as Extrude, Revolve and Sweep can use.
Drawing tools
| Tool | Key | Notes |
|---|---|---|
| Line | L | Chain continues after each click; Esc ends it. The key starts the line variant you used last. |
| Rectangle | R | Two-point or centre rectangle from the tool's drop-down. |
| Circle | C | Centre-diameter, perimeter or three-point. |
| Arc | — | Three-point, centre and tangent variants. |
| Spline | — | Through points or control points; dimensions can drive it. |
| Trim | T | Cuts the segment under the pointer back to the nearest intersection. |
| Offset | O | Parallel copy of a chain at a distance. |
| Project | P | Projects model edges into the sketch as reference geometry. |
| Construction | X | Reference geometry that is not part of the profile. |
Fillet, chamfer, polygon, slot, mirror and pattern are also in the Sketch tab. The Sketch Palette on the right exposes the same tools while a sketch is open.
Constraints
Constraints remove freedom without fixing a number. The common set: coincident, horizontal, vertical, parallel, perpendicular, tangent, concentric, equal, midpoint, symmetric and fix. Select the geometry, then the constraint; the solver applies it immediately.
A sketch that is under constrained reports its remaining degrees of freedom. Its icon and colour show the state: the sketch colour while under constrained, the fully constrained colour when nothing can move, and red when constraints conflict. The tooltip names the state.
Dimensions and expressions
Press D, click a line, circle or arc, and type the value. The dimension drives the geometry, so editing it later rebuilds the model. A dimension can be a plain number or an expression, and it can refer to user parameters (see Features and parameters).
With Sketch Dimension, the value box opens as soon as you click, so the sequence is D, click, type, Enter.
Snapping and constraints while drawing
- Auto-snap picks up endpoints, midpoints, centres and intersections as you draw.
- Hold Ctrl/⌘ or Alt/Option to suppress snapping for one gesture; the chord can be changed in Preferences › Sketch.
- Hold Shift to prefer a midpoint over a curve crossing.
- The pointer snaps where two curves cross, even without an endpoint there.
Closing the sketch
Finish the sketch when the profile is closed and dimensioned. Open contours can still be used by sweeps, thin features and sheet metal, but solid features need closed regions. Nested closed regions are treated as holes: two concentric circles make a ring, and a third circle inside the ring makes a separate disc.
To change a sketch later, double-click it in the Browser or the timeline. The model rebuilds from that sketch forward.
Common problems
- Over-constrained: the sketch turns red and the solver reports a conflict. Delete the newest constraint or dimension until it turns normal again.
- Profile not detected: a gap or a stray construction line is stopping the region from closing. Zoom in on the corners; Trim and Coincident fix most cases.
- Everything moves together: the sketch is under constrained. Add dimensions or constraints until the degrees of freedom reach zero.