part()

part(name, callback) declares a named part. Everything the callback does — sketches, features, connectors, exposures, parameters — belongs to that part.

import { part, sketch, circle, extrude } from 'fluidcad/core';

export const disc = part('Disc', () => {
    sketch('xy', () => {
        circle([0, 0], 40);
    });
    extrude(5);
});

In the viewport

Click Part on the toolbar. FluidCAD appends part('Part N', () => {}) to the file, activates it, and routes the next features into its body. Rename it from the timeline row's right-click menu. There is no Apply: the statement is written the moment you click.

The definition is lazy

part() returns a definition, not built geometry. The callback runs:

• when the file renders on its own — the open part file stays what-you-see-is-what-you-get, so a part nothing exports or inserts still shows in the viewport;
• once per variant when an assembly inserts it: insert(def) and insert(def, { Width: 120 }) are two builds, while two insert(def, { Width: 120 }) share one.

Because the body runs later, it must be self-contained: read parameters with param() inside the callback, not from variables computed outside it.

Arguments

Argument	Meaning
name	The part's display name — in the timeline, the Parts panel, and the STEP product tree on export.
callback	The body. Its return value is ignored; publish geometry with expose().

What the definition gives you

Member	Meaning
def.features.<name>	The source object an expose() published, for another part to build on: extrude(15, donor.features.profile).
insert(def)	In an assembly: an instance of the part with instance.connectors.<name> and instance.features.<name> bound to it.

Export it

An assembly can only insert what the part file exports:

export const bracket = part('Bracket', () => { /* … */ });

The Insert dialog scans the workspace for exported definitions and lists each with a thumbnail and the file it came from. Two files may each export a part — the assembly's import gets a local alias automatically when the dialog writes it.

Fusion boundary

Solids inside a part fuse with each other and with nothing outside it: put a bolt and the bracket it sits in into two parts and they stay two solids. Inside one part, .new() keeps a feature as a separate body.

Units

The part's numbers are in its file's unit. Inserted into a project with a different unit it is rescaled on the way in — a 2 in boss is 50.8 mm in a millimetre assembly. insert(def, { Length: 10 }) means 10 in the part's unit. See Units.