extrudo

API docs

Revolve

d.revolve(inputs?, options?): FeatureHandle<'revolve'>

One feature of the timeline, in the create category. Its name follows the app's (Revolve1, then Revolve2, …); options.name gives it another, options.id its ID and options.index its place in the timeline. Inputs the table calls optional keep the default it names, so a call with none of them still makes a valid feature.

Inputs

Input Type Required or default What it does
profiles GeomRef | GeomRef[] (profile, face, sketchEntity) optional Profiles and flat faces to revolve, all in one plane.
axis GeomRef | GeomRef[] (axis, sketchEntity, edge) optional The axis to revolve about, which lies in the profiles' plane.
direction 'one-side' | 'symmetric' | 'two-sides' default one-side How the revolve goes round: one-side, symmetric or two-sides.
angle string | number | ParameterHandle default 360°, a full turn with no end faces Side 1's angle (the whole angle when symmetric); an angle.
angle2 string | number | ParameterHandle default 0° Side 2's angle, the other way round; an angle.
flip boolean default false Turn side 1 the other way round the axis.
operation 'new-body' | 'join' | 'cut' | 'intersect' default new-body New body, join, cut or intersect.
bodies GeomRef | GeomRef[] (body) optional The bodies to join, cut or intersect; by default every body the revolve touches (join) or overlaps (cut, intersect).

Faces

Role What it is
cap:start The face the sweep starts at: the profile in its own place.
cap:end The face the sweep ends at.
side:<curve> A wall, one per edge of the profile: the sketch curve it came from, or the body edge it was swept from.

handle.face(role) builds a reference to one of them and handle.faceName(role) its persistent name. A <…> is what varies: a side:<sketch curve> is the wall of the curve you pass, and a role of a face that no face carries takes that part out. A role this feature never names is a lost reference — a visible error, never a silent guess.

Example

import { Design, type LineHandle } from '@extrudo/api';

const d = Design.create({ name: 'My part' });

// Two solids to point faces, edges and bodies at.
const plate = d.box({ length: '40 mm', width: '20 mm', height: '10 mm' });
const shaft = d.cylinder({ diameter: '20 mm', height: '20 mm' });

// A sketch with two closed profiles, a hole and a guide line beside them.
let guide!: LineHandle;
const s = d.sketch(d.origin.xy, (k) => {
  k.rectangle([0, 0], [40, 20]);
  k.circle([10, 10], '3 mm');
  k.rectangle([50, 0], [60, 10]);
  guide = k.line([-5, 30], [45, 30]);
});

const profile = s.profileAt([1, 1]);
const sections = s.profiles();
const line = guide.ref();
const face = plate.face('side:front');
const edge = plate.edge([plate.faceName('side:front'), plate.faceName('side:right')]);
const vertex = plate.vertex([plate.faceName('side:front'), plate.faceName('side:right')]);
const corner = plate.vertex([plate.faceName('side:front'), plate.faceName('side:left')]);
const body = plate.body();
const step = 'att-part.step'; // an attachment of the design
const plan = 'att-plan.png';

// Revolve.
d.revolve({ profiles: profile, axis: d.origin.y, angle: '90 deg' });

See also