Extrude

Status: Implemented

Extrude sweeps a closed planar profile along its plane normal: straight, two-sided, or drafted into a taper.

Walkthrough

Inputs

• id – a string, default null.
• profile – a single (multiple: false) reference_selection filtered to SKETCH and FACE, default null.
• consumeProfileSketch – a boolean. When true (default), removes the source sketch after a successful extrude. A face profile consumes nothing.
• distance – a number: forward distance along the profile-plane normal. Default 10.
• distanceBack – a number: backward distance for a two-sided extrude. Default 10.
• draftAngle – a number: draft / taper angle in degrees. 0 (default) is a straight extrude; a positive angle tapers inward, giving a smaller far cap.
• boolean – a boolean_operation, default { targets: [], operation: "NONE", mergeCoplanarFaces: true }.

Behaviour

• Two-sided: the profile plane is translated back by distanceBack and the solid is swept the total distance + distanceBack.
• Multi-region and holed profiles extrude: each region becomes a solid and hole loops become over-long through prisms that are subtracted, then the region solids union into one result.
• Draft: the outer loop gets exact drafted walls — tilted planes for straight segments, cone patches for circular arcs, and exact conic junction edges — with the far section as the exact in-plane miter offset (distance · tan θ; straight segments re-intersect at the corners, arcs shrink concentrically).
• Two-sided draft is the mould / parting-line form: the sketch plane is the parting plane and a positive draft tapers inward moving away from it in each direction. The two legs are unioned, and the wall-normal break leaves a real ridge edge at the sketch plane.
• Face naming, drafted or not: sidewalls are {id}:{edgeName}_SW in input-curve order, and the caps are {id}:{sketchId}:PROFILE:L{loopId}_START (the base cap, at −distanceBack) and ..._END (at +distance), one pair per region keyed by that region's outer loop identity. The un-keyed {id}:{sketchId}:PROFILE_START / _END is registered as the container for all of them, so a reference stored before per-loop naming still resolves. A face profile uses {id}:{faceName} as the cap base and keeps the un-keyed spelling.
• A two-sided draft has one wall per leg per edge.

Limitations

Every case below is a loud error:

• a straight extrude with a total length (distance + distanceBack) of zero.
• draft + hole loops — unsupported.
• draft + a negative distanceBack — unsupported; a two-sided draft also requires a non-negative forward distance.
• one-sided draft + zero distance — unsupported.
• A draft offset that exceeds the local feature size, so the miter or arc intersections vanish, is a kernel error.

Where to find it

Offered in the Modeling and All workbenches. Type code E.