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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

ToolKeyNotes
LineLChain continues after each click; Esc ends it. The key starts the line variant you used last.
RectangleRTwo-point or centre rectangle from the tool's drop-down.
CircleCCentre-diameter, perimeter or three-point.
Arc—Three-point, centre and tangent variants.
Spline—Through points or control points; dimensions can drive it.
TrimTCuts the segment under the pointer back to the nearest intersection.
OffsetOParallel copy of a chain at a distance.
ProjectPProjects model edges into the sketch as reference geometry.
ConstructionXReference 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

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.

Tip: dimension to the origin and between features, not with chains of dimensions from edge to edge. When a parameter changes, a well-dimensioned sketch moves the way you expect.

Common problems