Subtract

Subtract carves one solid out of another. The base is the solid you keep; the tool is the solid whose volume is taken away. Whatever the tool occupied becomes a hollow in the base, and the tool itself is gone.

That makes it the operation for cavities shaped by a real body: a mould around a part, a clearance pocket the size of the component that has to fit in it, a channel cut by a swept or lofted shape.

In the viewport

1. Click Boolean on the toolbar and choose the Subtract tab.
2. Click the solid you want to keep — it fills the Base slot, and the Tool slot arms itself next.
3. Click the solid to remove. It fills Tool.
4. Click Apply.

1234

1. 1
   Subtract tab

   Swapping to this tab turns the single Solids slot into the two slots below. The first two solids you had picked become the base and the tool; any extras are dropped, since a subtract takes exactly two.
2. 2
   Base

   The solid that survives — one solid only. While this slot is armed, picking a different solid replaces what is in it.
3. 3
   Tool

   The solid that is taken away, also one only. Click a slot to arm it (blue border) before re-picking; a chip’s ✕ empties the slot, and so does clicking the solid that is already in it.
4. 4
   Apply

   Writes subtract(base, tool). Both slots must be filled first; Exit closes the dialog without writing anything.

Getting the two the wrong way round is the usual mistake, and it is easy to spot: you end up with the tool full of a base-shaped hole. Click Base to re-arm it and pick again.

The same two cubes, with the second one taken out of the first:

Beforetwo solids

Cube A is the base, cube B the tool. They share a 30 × 30 × 60 corner.

Aftersubtract(a, b)

Cube A with that corner taken out of it. Cube B is used up doing the cutting and is no longer in the Shapes panel.

The code behind it

The notch is exactly the corner the two cubes shared — nothing more is removed than the tool actually occupied.

cubes.part.js

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

// Cube A. The four lines and the constraints that hold them square are what
// the Rectangle tool writes; `fix` pins one corner, the two `distance`s size
// the square.
sketch("xy", () => {
    const bottom = line([-30, -30], [30, -30]);
    const right = line([30, -30], [30, 30]);
    const top = line([30, 30], [-30, 30]);
    const left = line([-30, 30], [-30, -30]);
    coincident(bottom.end(), right.start());
    coincident(right.end(), top.start());
    coincident(top.end(), left.start());
    coincident(left.end(), bottom.start());
    horizontal(bottom);
    vertical(right);
    horizontal(top);
    vertical(left);
    fix(bottom.start(), [-30, -30]);
    distance(bottom.start(), bottom.end(), 60);
    distance(right.start(), right.end(), 60);
});
const a = extrude(60);

// Cube B. The same square, shifted 30 mm along X and Y, so the two cubes
// share a 30 x 30 x 60 corner.
sketch("xy", () => {
    const bottom = line([0, 0], [60, 0]);
    const right = line([60, 0], [60, 60]);
    const top = line([60, 60], [0, 60]);
    const left = line([0, 60], [0, 0]);
    coincident(bottom.end(), right.start());
    coincident(right.end(), top.start());
    coincident(top.end(), left.start());
    coincident(left.end(), bottom.start());
    horizontal(bottom);
    vertical(right);
    horizontal(top);
    vertical(left);
    fix(bottom.start(), [0, 0]);
    distance(bottom.start(), bottom.end(), 60);
    distance(right.start(), right.end(), 60);
});
const b = extrude(60).new();

subtract(a, b);
// Cube A survives with a 30 x 30 x 60 notch where cube B passed through it.
// Swap the arguments and you keep cube B with the notch instead.

Code forms

import { subtract } from 'fluidcad/core';

subtract(base, tool)     // keep base, remove tool's volume

Both arguments are required, and swapping them gives a different solid. The faces the cut leaves behind are the tool's surfaces where they ran through the base:

const s = subtract(box, cyl)
s.internalFaces()        // the cavity walls
s.internalEdges()

Subtract or cut?

If you can draw the shape you want to remove, sketch it and use the extrude dialog's Remove tab instead — that writes cut(), which stays tied to its sketch, so changing the sketch changes the pocket. It is the right tool for holes, slots and pockets.

subtract() is for removing a body that already exists as a solid: a STEP import, a revolve, a loft, the result of another feature.

And inside a sketch you need neither. A closed profile drawn inside another closed profile becomes a hole as soon as the sketch is extruded.