Solid features

Use extrude, revolve, Booleans, fillet, chamfer, shell, offset, and draft with explicit topology intent.

Extrude and revolve

const profile = cad.sketch("profile", plane.xy(), (sketch) =>
  sketch.profile(
    sketch.rectangle("outline", { width: mm(40), height: mm(20) }),
  ),
);

const extrusion = cad.extrude("extrusion", profile, {
  distance: mm(10),
  symmetric: true,
});

const revolution = cad.revolve("revolution", profile, {
  angle: deg(270),
  segments: 96,
});

Manifold additionally supports twisted and top-scaled extrusion:

const twisted = cad.extrude("twisted", profile, {
  distance: mm(50),
  twist: deg(90),
  scaleTop: [scalar(0.75), scalar(0.75)],
  divisions: 32,
});

Check the support matrix before using these options with another kernel.

Booleans

Boolean features have one target and one or more tools:

const joined = cad.union("joined", target, [toolA, toolB]);
const cut = cad.subtract("cut", target, [holeA, holeB]);
const common = cad.intersect("common", target, [clip]);

An empty tool array is rejected during authoring. The result is one solid; input solids remain feature dependencies and are not mutated.

Fillet and chamfer

Edge treatments require an explicit edge selection:

const rim = topology.edges
  .createdBy(extrusion, { role: "extrude.edge.end-rim" })
  .exactly(4);

const rounded = cad.fillet("rounded", extrusion, {
  edges: rim,
  radius: mm(2),
});

const beveled = cad.chamfer("beveled", extrusion, {
  edges: rim,
  distance: mm(1),
});

The selection resolves against the direct input solid. A missing, ambiguous, or wrong-cardinality selection fails before the treatment is applied.

Shell and offset

const endCap = topology.faces
  .createdBy(extrusion, { role: "extrude.face.end-cap" })
  .select();

const hollow = cad.shell("hollow", extrusion, {
  openings: endCap,
  thickness: mm(2),
  direction: "inward",
  tolerance: mm(1e-6),
});

const expanded = cad.offset("expanded", extrusion, {
  distance: mm(1),
  direction: "outward",
  tolerance: mm(1e-6),
});

Shell removes selected opening faces and offsets the remaining skin to create a constant wall. Whole-solid offset has no opening selection. Both use positive magnitudes plus an explicit direction.

Draft

Draft is an atomic multi-face exact feature available through the matched owned OCCT facade:

const sides = topology.faces
  .createdBy(extrusion, { role: "extrude.face.side" })
  .atLeast(1);

const drafted = cad.draft("drafted", extrusion, {
  faces: sides,
  angle: deg(2),
  pullDirection: scalarVec3(0, 0, 1),
  neutralPlane: {
    origin: vec3(mm(0), mm(0), mm(0)),
    normal: scalarVec3(0, 0, 1),
  },
});

Stock OCCT does not advertise draft. Capability checks reject the feature before input geometry is allocated on an unsupported backend.

Exact-history boundary

Stock OCCT can construct most exact features, but its Boolean, edge-treatment, and solid-offset topology history is partial. The optional owned facade advertises complete bounded evolution only for the exact feature slices and ABI versions documented in the OpenCascade guide.

Construction success and complete topology evolution are distinct guarantees.