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How to: turn a sketch into a solid

A sketch does not produce a solid by itself. It produces a face, and you give that face a thickness afterwards. This is the step people miss — the sketch applies, something appears in the tree, and nothing looks three-dimensional.

Before you start: Sketching covers the tools and constraints in full. This page is the path from an empty plane to a solid you can cut.

1. Start the sketch

From the Create panel:

  • Start Sketch — sketch on a plane
  • on Face — select an existing face first, then sketch on it

Use on Face whenever the profile belongs to an existing shape. The sketch inherits that face's plane, so you do not have to place it by hand.

2. Draw roughly, then constrain

This is the intended order, and it is faster than it sounds. Draw the shape approximately with the pen tools, then pin it down:

  1. Draw with Line, Circle, Rectangle, and the rest
  2. Select geometry and apply constraints — Distance for dimensions, Align X / Align Y, Parallel, Tangent
  3. Fix at least one point with Fixed, or the whole profile can slide

Snapping is automatic while you draw, and the indicators tell you what caught — see Keyboard and mouse.

If the sketch will not move the way you expect, open Constraints / Parameters and look for a constraint you did not intend to add. Over-constraining is the usual cause.

3. Apply

Apply, at the bottom of the sidebar. Cancel discards the sketch.

What you get depends on what you drew:

What you drew What appears in the Feature Tree
A closed region Sketch Surface — a face
A closed region with a closed region inside it One Sketch Surface, with the inner loop as a hole
Three separate closed regions Three Sketch Surface entries
An open run of lines Sketch Curve

Construction geometry produces nothing. That is what it is for.

4. Give it thickness

Select the Sketch Surface entry and look at the Active Property Editor:

Property Effect
Extrude Height Thickness. Defaults to 0.0, which is why a fresh sketch surface is flat
Fill Closed Whether a closed outline gets a face at all. On by default
Use Pipe / Pipe Radius Instead of extruding, sweep a round tube along the outline

Set Extrude Height to a non-zero value and the face becomes a solid.

A negative value extrudes the other way. That is the whole trick to cutting a pocket into the face you sketched on: sketch on Face, set a negative height, set Operation to Subtract (Cut).

5. Combine it

Set Operation like any other entry — Add (Fuse) to join, Subtract (Cut) to cut. It combines with everything above it in the tree. See The Feature Tree and parts.

Editing the sketch later

Select the entry and press Edit Sketch in the Property Editor. The original sketch reopens with its constraints intact.

The rebuilt entry keeps its position in the tree, so fillets and other downstream operations stay attached — as long as the sketch still produces the same number of separate closed regions. Split one region into two and the rebuilt entries go to the end of the tree instead, and the add-on warns you that downstream features may need reassigning.

If Edit Sketch is greyed out and says "Hidden by rollback point", the entry is below an active pin. Unpin it first.

See also