Rotate

rotate() turns solids around an axis, in place or as copies.

In the viewport

1. Click Rotate on the toolbar. The Rotate dialog docks on the right.
2. Pick the tab: Move turns the solids in place; Copy keeps the originals and adds turned copies.
3. Click the solids to rotate — any face or edge click in the viewport selects the whole solid, or click their timeline rows. They fill the Solids slot as numbered chips.
4. Fill the Axis slot: click one of the world axes shown in the viewport (X red, Y green, Z blue), an axis() feature, or an edge. A circular edge gives its centre line.
5. Enter the Angle in degrees and click Apply.

The code behind it

Here the axis is an axis() feature offset from the origin — written in code, since the dialog's Axis slot takes world axes and picked edges. Two rotate-copies at 90° and 180° leave three plates.

turn.part.js

import { axis, extrude, rotate, sketch, line } from 'fluidcad/core';
import { coincident, distance, fix, horizontal, vertical } from "fluidcad/constraints";

sketch("xy", () => {
    const sg1 = line([100, 100], [300, 100]);
    const sg2 = line([300, 100], [300, 200]);
    const sg3 = line([300, 200], [100, 200]);
    const sg4 = line([100, 200], [100, 100]);
    coincident(sg1.end(), sg2.start());
    coincident(sg2.end(), sg3.start());
    coincident(sg3.end(), sg4.start());
    coincident(sg4.end(), sg1.start());
    horizontal(sg1);
    vertical(sg2);
    horizontal(sg3);
    vertical(sg4);
    fix(sg1.start(), [100, 100]);
    distance(sg1.start(), sg1.end(), 200);
    distance(sg2.start(), sg2.end(), 100);
  })

extrude(20)

// A vertical axis through (90, 90), just off the plate's corner.
const a = axis("z", { offsetX: 90, offsetY: 90 })

// Two rotate-copies of the last solid (the plate): `true` keeps the original.
rotate(a, 90, true)
rotate(a, 180, true)

Copies

On the Copy tab the original stays and a turned duplicate is added — the copy flag is the true before the targets:

The code behind it

The spoke is kept separate with .new() so each copy is a clone of the spoke alone, not of a spoke already fused into the hub. A final fuse() with no arguments merges every solid in the file into one wheel.

wheel.part.js

import { sketch, circle, extrude, rotate, fuse, line } from 'fluidcad/core';
import { coincident, distance, fix, horizontal, vertical } from 'fluidcad/constraints';

// A wheel hub with four spokes: one spoke is modelled, the others are
// rotate-copies of it.
sketch("xy", () => { circle([0, 0], 30); });
const hub = extrude(10);

// One spoke, from the hub outwards along X, kept separate so it can be copied.
sketch("xy", () => {
    const b = line([12, -3], [70, -3]);
    const r = line([70, -3], [70, 3]);
    const t = line([70, 3], [12, 3]);
    const l = line([12, 3], [12, -3]);
    coincident(b.end(), r.start());
    coincident(r.end(), t.start());
    coincident(t.end(), l.start());
    coincident(l.end(), b.start());
    horizontal(b);
    vertical(r);
    horizontal(t);
    vertical(l);
    fix(b.start(), [12, -3]);
    distance(b.start(), b.end(), 58);
    distance(r.start(), r.end(), 6);
});
const spoke = extrude(10).new();

// The Rotate dialog's Copy tab: the spoke stays and a turned copy is added
// each time. `true` is the copy flag; without it the spoke itself would move.
rotate("z", 90, true, spoke);
rotate("z", 180, true, spoke);
rotate("z", 270, true, spoke);

// Merge hub and spokes into one wheel.
fuse();

For more than a couple of copies use a circular copy or repeat pattern.

Code forms

import { rotate } from 'fluidcad/core';

rotate("z", 45)                    // turn the last object 45° around world Z
rotate("z", 45, body)              // turn a specific solid
rotate("z", 45, true, body)        // copy instead of move
rotate(a, 90, p1, p2)              // around an axis() feature, several targets

The axis is anything axis-like: "x" / "y" / "z", an axis() feature (offset or tilted from a world axis, read from an edge, or midway between two — see Axes), or an edge selection. Angles are in degrees.

Inside a sketch

rotate() works on solids only. Sketch geometry is oriented with constraints instead — angle(), horizontal() and vertical() pin a line's direction, and the solver turns the rest of the profile with it. Calling rotate() inside sketch(...) is an error.