Sweep

Sweep moves a profile along a path to make a solid: pipes, rails, handles, cable runs — anything that follows a curve. It takes two sketches, a profile and a path, and they should lie on different planes.

In the viewport

Draw the path as a sketch (an open chain of lines and arcs, or a helix) and the profile as a second sketch on a plane that crosses the path, usually at its start. Then click Sweep on the toolbar.
Fill in the dialog — both slots are usually filled for you from the two most recent sketches.
Click Apply.

1
Add / Remove / New
What the swept solid does to the model — fuse, cut, or stand alone. See Add, New and Remove below.
2
Sketch
The profile that travels along the path. One sketch; click a sketch row in the timeline or its wires in the viewport to change it.
3
Path
The curve to follow — a sketch, a helix, or edges picked in the viewport. Edge picking stays live while the dialog is open: clicking an edge re-sources the path to edges, clicking a sketch switches it back.
4
Thin walls
Sweeps a wall of the thickness you type instead of the filled profile — a pipe rather than a rod.
5
Scope
Which solids the Add or Remove applies to.
6
Apply
Writes the statement and adds the timeline row; Exit writes nothing.

From two sketches to a pipe

A ring profile and a bent path, and the solid they make between them:

Before Before mode

path + profile

Seen square to the front plane: the path — a line and two arcs, tangent where they join — with the ring profile edge-on at its start, the short line at the bottom.

After

sweep(spine, profile)

The ring carried along the path, staying square to it the whole way. The hole in the profile becomes the bore.

The two sketches

pipe.part.js
import { sketch, circle, line, arc } from 'fluidcad/core';
import { coincident, vertical, tangent, radius, fix } from 'fluidcad/constraints';

// The profile: a ring (two concentric circles — the inner one is a hole) on
// the top plane at the origin, where the path starts.
sketch("top", () => {
    circle([0, 0], 40);
    circle([0, 0], 20);
  })

// The path: a line and two arcs on the front plane, joined end to end and
// tangent at the joints so the pipe bends without kinks.
sketch("front", () => {
    const l = line([0, 0], [0, 100]);
    const a1 = arc([0, 100], [-100, 100], [-50, 100]);
    const a2 = arc([-100, 100], [-180, 180], [-180, 100]).cw();
    coincident(l.end(), a1.start());
    coincident(a1.end(), a2.start());
    vertical(l);
    tangent(l, a1);
    tangent(a1, a2);
    fix(l.start());
    radius(a1, 50);
    radius(a2, 80);
  })

The complete file

import { sketch, sweep } from 'fluidcad/core';
import { circle, line, arc } from 'fluidcad/core';
import { coincident, vertical, tangent, radius, fix } from 'fluidcad/constraints';

// The profile: a ring (two concentric circles — the inner one is a hole),
// drawn on the top plane at the origin, where the path starts.
const profile = sketch("top", () => {
    circle([0, 0], 40);
    circle([0, 0], 20);
  })

// The path: a line and two arcs on the front plane, joined end to end and
// tangent at the joints so the pipe bends without kinks.
const spine = sketch("front", () => {
    const l = line([0, 0], [0, 100]);
    const a1 = arc([0, 100], [-100, 100], [-50, 100]);
    const a2 = arc([-100, 100], [-180, 180], [-180, 100]).cw();
    // Join the segments...
    coincident(l.end(), a1.start());
    coincident(a1.end(), a2.start());
    vertical(l);
    // ...and make the bends smooth
    tangent(l, a1);
    tangent(a1, a2);
    // Pin the start at the origin (where the profile sits) and size the bends
    fix(l.start());
    radius(a1, 50);
    radius(a2, 80);
  })

// Sweep the profile along the path: path first, profile second.
sweep(spine, profile)

The first argument of sweep() is the path (spine), the second the profile.

Extend

.extend() continues the swept solid past the end of the path, straight along the path's tangent there. Use it for lead-ins and run-outs — a pipe that runs straight past its last bend:

Sweep extended past the path end

The code behind it

import { sketch, sweep } from 'fluidcad/core';
import { circle, line, arc } from 'fluidcad/core';
import { coincident, vertical, tangent, radius, fix } from 'fluidcad/constraints';

const profile = sketch("top", () => {
    circle([0, 0], 40);
  })

const spine = sketch("front", () => {
    const l = line([0, 0], [0, 100]);
    const a1 = arc([0, 100], [-60, 160], [-60, 100]);
    coincident(l.end(), a1.start());
    vertical(l);
    tangent(l, a1);
    fix(l.start());
    radius(a1, 60);
  })

sweep(spine, profile).extend("end", 80)

sweep(spine, profile).extend("end", 80)                      // 80 units past the end
sweep(spine, profile).extend("start", 20)                    // 20 units before the start
sweep(spine, profile).extend("start", 20).extend("end", 80)  // both ends

Add, New and Remove

The pictures use a drawer front and a Ø16 circle swept along an arch drawn on its front face. The circle is centred on the face, so the tube runs half in, half out of the panel. Only the tab changes:

Add

sweep(path, profile)

The tube fuses with the panel — a rounded pull rail.

New

sweep(path, profile).new()

The tube is a separate solid — a rail seated in the panel.

Remove Remove mode

sweep(path, profile).remove()

The tube's volume is cut out — a rounded finger-pull channel.

The Add column's code

The profile sits on plane(path, 'start'): a plane at the start of the path, normal to it, so the circle is swept square to the curve. The New and Remove columns only change the highlighted line.

import { sketch, extrude, sweep, plane, circle, line, arc } from 'fluidcad/core';
import { coincident, distance, fix, horizontal, vertical } from "fluidcad/constraints";

// The base part every column shares: a 120 x 60 drawer front, 15 thick,
// standing on the front plane.
sketch("xz", () => {
    const sg1 = line([-60, 0], [60, 0]);
    const sg2 = line([60, 0], [60, 60]);
    const sg3 = line([60, 60], [-60, 60]);
    const sg4 = line([-60, 60], [-60, 0]);
    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(), [-60, 0]);
    distance(sg1.start(), sg1.end(), 120);
    distance(sg2.start(), sg2.end(), 60);
  })
const front = extrude(15)

// The path: a shallow arch drawn on the panel's front face, 80 wide.
const path = sketch(front.endFaces(), () => {
    const a = arc([-40, 20], [40, 20], [0, -40]).cw();
    fix(a.start(), [-40, 20]);
    fix(a.end(), [40, 20]);
  })

// The profile: a Ø16 circle at the path's start, on a plane normal to the
// path there. Its centre sits on the panel face, so the tube runs half in,
// half out of the panel.
const profile = sketch(plane(path, 'start'), () => {
    circle([0, 0], 16);
  })

// Add tab: the tube fuses with the panel — a rounded pull rail.
sweep(path, profile)

Thin walls

Turn on Thin for a pipe instead of a rod: the profile's edges are offset by the thickness and the band between them is swept.

Thin sweep

The code behind it

import { sketch, sweep } from 'fluidcad/core';
import { circle, line, arc } from 'fluidcad/core';
import { coincident, vertical, tangent, radius, fix } from 'fluidcad/constraints';

const profile = sketch("top", () => {
    circle([0, 0], 40);
  })

const spine = sketch("front", () => {
    const l = line([0, 0], [0, 100]);
    const a1 = arc([0, 100], [-100, 100], [-50, 100]);
    const a2 = arc([-100, 100], [-180, 180], [-180, 100]).cw();
    coincident(l.end(), a1.start());
    coincident(a1.end(), a2.start());
    vertical(l);
    tangent(l, a1);
    tangent(a1, a2);
    fix(l.start());
    radius(a1, 50);
    radius(a2, 80);
  })

sweep(spine, profile).thin(5)

sweep(spine, profile).thin(5)     // 5 units outward
sweep(spine, profile).thin(-5)    // 5 units inward
sweep(spine, profile).thin(5, -3) // dual offset

Thin in the three modes

The same rail with Thin on and a wall of 2:

Add

sweep(path, profile).thin(2)

A 2-thick tube wall fused with the panel.

New

sweep(path, profile).thin(2).new()

The tube wall as a separate body.

Remove Remove mode

sweep(path, profile).thin(2).remove()

Only the wall is cut — two curved slots; the core between them stays.

The Add column's code

import { sketch, extrude, sweep, plane, circle, line, arc } from 'fluidcad/core';
import { coincident, distance, fix, horizontal, vertical } from "fluidcad/constraints";

// The base part every column shares: a 120 x 60 drawer front, 15 thick,
// standing on the front plane.
sketch("xz", () => {
    const sg1 = line([-60, 0], [60, 0]);
    const sg2 = line([60, 0], [60, 60]);
    const sg3 = line([60, 60], [-60, 60]);
    const sg4 = line([-60, 60], [-60, 0]);
    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(), [-60, 0]);
    distance(sg1.start(), sg1.end(), 120);
    distance(sg2.start(), sg2.end(), 60);
  })
const front = extrude(15)

// The path: a shallow arch drawn on the panel's front face, 80 wide.
const path = sketch(front.endFaces(), () => {
    const a = arc([-40, 20], [40, 20], [0, -40]).cw();
    fix(a.start(), [-40, 20]);
    fix(a.end(), [40, 20]);
  })

// The profile: a Ø16 circle at the path's start, on a plane normal to the
// path there. Its centre sits on the panel face, so the tube runs half in,
// half out of the panel.
const profile = sketch(plane(path, 'start'), () => {
    circle([0, 0], 16);
  })

// Add + Thin: a 2-thick tube wall instead of a solid rod, fused with the panel.
sweep(path, profile).thin(2)

Open profiles

Thin sweep also works with open profiles. The ends are capped — select them with capFaces() / capEdges():

Thin sweep — open profile

The code behind it

import { sketch, sweep } from 'fluidcad/core';
import { line, arc } from 'fluidcad/core';
import { coincident, vertical, tangent, radius, fix } from 'fluidcad/constraints';

const profile = sketch("top", () => {
    line([-30, 0], [30, 0])
  })

const spine = sketch("front", () => {
    const l = line([0, 0], [0, 100]);
    const a1 = arc([0, 100], [-100, 100], [-50, 100]);
    coincident(l.end(), a1.start());
    vertical(l);
    tangent(l, a1);
    fix(l.start());
    radius(a1, 50);
  })

sweep(spine, profile).thin(5).new()

Accessing geometry

const s = sweep(spine, profile)

s.endFaces()       // face at the end of the path
s.startFaces()     // face at the start of the path
s.sideFaces()      // the swept surface(s)
s.endEdges()       // edges at the end
s.startEdges()     // edges at the start
s.sideEdges()      // edges along the sides
s.internalFaces()  // internal faces (if profile has holes)
s.internalEdges()  // internal edges
s.capFaces()       // cap face(s) of a thin sweep (open profile)
s.capEdges()       // cap edges of a thin sweep (open profile)

Fusion scope

sweep(spine, profile).new()                // create a separate solid
sweep(spine, profile).add()                // fuse with touching solids (default)
sweep(spine, profile).remove()             // subtract from all intersecting solids
sweep(spine, profile).remove().scope(box)  // subtract only from the box

In the viewport​

From two sketches to a pipe​

Extend​

Add, New and Remove​

Thin walls​

Thin in the three modes​

Open profiles​

Accessing geometry​

Fusion scope​

In the viewport

From two sketches to a pipe

Extend

Add, New and Remove

Thin walls

Thin in the three modes

Open profiles

Accessing geometry

Fusion scope