Intersect

Intersect cuts the sketch plane through 3D faces and brings the section curves into the sketch. Like a projection, the result is fixed reference geometry: the solver never moves it, it renders as locked (green) geometry, and your sketch geometry can be constrained against it. Where Project flattens what you would see of a face from the sketch plane, Intersect gives you the true outline where the plane passes through it — the wall of a bore, the profile of a curved cavity, the section of a rib.

In the viewport

1. Click Intersect on the sketch toolbar. The Intersect dialog opens with one Selection slot.
2. Click the 3D faces to section. Each pick becomes a chip; a right-click offers the same multi-select groups the modify tools do. Only faces can be picked — a plane meets an edge in a point, which is no sketch geometry.
3. Apply writes the intersect(…) statement at the top of the sketch body, where the references it creates are available to every constraint after it.

The code behind it

divider.part.js

import { sketch, line, circle, extrude, intersect, yAxis } from 'fluidcad/core';
import { coincident, distance, horizontal, vertical, symmetric } from "fluidcad/constraints";

// A Ø60 tube, 100 long with a 6 mm wall — a thin extrude of one circle,
// drawn on the yz plane so the tube runs along X, centred on the plane.
sketch("yz", () => {
    circle([0, 0], 60)
})
const tube = extrude(100).symmetric().thin(6)

// A divider plate, 6 thick, across the middle of the bore. It is drawn on
// the same yz plane, halfway along the tube, where nothing in the sketch
// says how wide the bore is — Intersect does.
sketch("yz", () => {
    // The tube's inner wall cut by the sketch plane: one circle, fixed
    // reference geometry the plate's corners can land on.
    const wall = intersect(tube.internalFaces()).guide()
    const b = line([-3, -24], [3, -24]);
    const r = line([3, -24], [3, 24]);
    const t = line([3, 24], [-3, 24]);
    const l = line([-3, 24], [-3, -24]);
    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);
    distance(b.start(), b.end(), 6);
    symmetric(b.start(), b.end(), yAxis());
    // Two opposite corners on the wall: the plate spans the bore exactly,
    // and follows it if the tube changes.
    coincident(b.start(), wall);
    coincident(t.start(), wall);
})

// The plate, 10 long, centred on the plane like the tube.
extrude(10).symmetric()

Double-click the intersection's row in the timeline to re-source it: the viewport rolls back to just before the statement and the dialog reopens with its faces highlighted.

From another part

Inside a part you can section the faces of a part declared before it, exactly as with Project: the dialog names the owning part, and Apply waits for Expose and intersect, which writes an expose() into that part for each picked face and references it as <part>.features.<name> in your sketch.

By hand

intersect(tube.internalFaces())    // a bore's wall → its circle at the plane
intersect(body)                    // a whole solid → its full section outline
intersect(face1, face2)            // several sources at once

Sections usually carry .guide() so the reference stays out of the profile and only the geometry drawn against it is extruded or cut.

Constraining against a section

A section is a first-class constraint target, with the same forms as a projection: a single sectioned entity is used directly, and a multi-edge section is addressed with .ref(i):

sketch("yz", () => {
    const wall = intersect(tube.internalFaces()).guide()   // one circle
    coincident(b.start(), wall)                              // a corner on the wall
    concentric(c, wall)                                      // a hole concentric with it
})

const outline = intersect(body).guide()          // several edges
coincident(p, outline.ref(0).start())
tangent(outline.ref(2), l)

Because references are fixed, a sketch made only of sections reports Fully constrained by itself — the geometry you add is what brings degrees of freedom.