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Loft

Loft blends two or more sketch profiles on different planes into one smooth solid. Reach for it when the cross-section changes along the length — a vase, a duct that goes from rectangular to round, a hopper.

In the viewport​

  1. Sketch each section on its own plane (a standard plane, an offset plane, or a face). Click Loft on the toolbar.
  2. Click each profile in the timeline or the viewport. They stack up in the Sketches slot in the order you pick them, and that order is the order the surface passes through them — drag the chips to change it.
  3. Click Apply.
The Loft dialog with two sketches picked in loft order
  1. 1
    Add / Remove / New
    What the lofted solid does to the model — fuse, cut, or stand alone. See Add, New and Remove below.
  2. 2
    Sketches — in loft order
    Two or more sections, numbered in pick order. The surface runs through them in that order, so a wrong order gives a twisted or self-crossing solid; drag a chip by its handle to reorder.
  3. 3
    Guides
    Up to two open curves the surface must follow along its sides. Each guide has to pass through every profile. Optional — see Guide curves below.
  4. 4
    Start condition
    How the surface leaves the first profile: None, Normal (perpendicular to the profile plane) or Tangent (bulging out inside the plane), with a magnitude.
  5. 5
    End condition
    The same for the last profile. The two ends are set independently.
  6. 6
    Thin walls
    Lofts a wall of the thickness you type instead of a filled solid. Cannot be combined with guides.
  7. 7
    Scope
    Which solids the Add or Remove applies to.
  8. 8
    Apply
    Writes the statement and adds the timeline row; Exit writes nothing.

From sections to a solid​

A vase is four circles on planes 40 apart, each a different diameter. Loft passes one surface through all of them:

BeforeBefore modefour sections

The sections, bottom to top: a Ø60 foot on the ground plane, a Ø100 belly at 40, a Ø44 neck at 80 and a Ø70 lip at 120. Nothing is solid yet.

AfterAfter modeloft(foot, belly, neck, lip)

One solid whose section follows the circles — out to the belly, in at the neck, out again at the lip.

The four sketches
vase.part.js
import { sketch, plane, circle } from 'fluidcad/core';
import { diameter, fix } from "fluidcad/constraints";

// Nothing solid yet — four round sections on planes 40 apart, each fully constrained. Only the
// diameter changes from one to the next: a Ø60 foot, a Ø100 belly, a Ø44 neck
// and a Ø70 lip.
const foot = sketch("xy", () => {
    const c = circle([0, 0], 60);
    fix(c.center(), [0, 0]);
    diameter(c, 60);
  })

const belly = sketch(plane("xy", { offset: 40 }), () => {
    const c = circle([0, 0], 100);
    fix(c.center(), [0, 0]);
    diameter(c, 100);
  })

const neck = sketch(plane("xy", { offset: 80 }), () => {
    const c = circle([0, 0], 44);
    fix(c.center(), [0, 0]);
    diameter(c, 44);
  })

const lip = sketch(plane("xy", { offset: 120 }), () => {
    const c = circle([0, 0], 70);
    fix(c.center(), [0, 0]);
    diameter(c, 70);
  })
The complete file

The sketches go into loft() in the order the surface should pass through them — the same order the chips take in the Sketches slot.

import { sketch, plane, loft, circle } from 'fluidcad/core';
import { diameter, fix } from "fluidcad/constraints";

// Four round sections on planes 40 apart, each fully constrained. Only the
// diameter changes from one to the next: a Ø60 foot, a Ø100 belly, a Ø44 neck
// and a Ø70 lip.
const foot = sketch("xy", () => {
    const c = circle([0, 0], 60);
    fix(c.center(), [0, 0]);
    diameter(c, 60);
  })

const belly = sketch(plane("xy", { offset: 40 }), () => {
    const c = circle([0, 0], 100);
    fix(c.center(), [0, 0]);
    diameter(c, 100);
  })

const neck = sketch(plane("xy", { offset: 80 }), () => {
    const c = circle([0, 0], 44);
    fix(c.center(), [0, 0]);
    diameter(c, 44);
  })

const lip = sketch(plane("xy", { offset: 120 }), () => {
    const c = circle([0, 0], 70);
    fix(c.center(), [0, 0]);
    diameter(c, 70);
  })

// The surface passes through the four sections in the order they are listed,
// swelling out to the belly, pinching in at the neck and flaring at the lip.
loft(foot, belly, neck, lip);

Multiple profiles​

Every sketch in the list is a section the surface has to pass through, so adding a section is how you shape the result. The same vase built up one section at a time:

Two sectionsTwo sections modeloft(foot, lip)

Foot and lip only. The surface runs straight between them — a tube tapering gently from Ø60 to Ø70.

Three sectionsThree sections modeloft(foot, belly, lip)

The Ø100 belly added in the middle. The surface has to pass through it on the way up, so the tube swells out.

Four sectionsFour sections modeloft(foot, belly, neck, lip)

The Ø44 neck between belly and lip pinches it back in — the vase.

The three-section column's code

Each column's file contains only the sketches it lofts; the highlighted line is the only difference in what loft() is handed.

vase.part.js
import { sketch, plane, loft, circle } from 'fluidcad/core';
import { diameter, fix } from "fluidcad/constraints";

// The foot and lip again, with the Ø100 belly between them.
const foot = sketch("xy", () => {
    const c = circle([0, 0], 60);
    fix(c.center(), [0, 0]);
    diameter(c, 60);
  })

const belly = sketch(plane("xy", { offset: 40 }), () => {
    const c = circle([0, 0], 100);
    fix(c.center(), [0, 0]);
    diameter(c, 100);
  })

const lip = sketch(plane("xy", { offset: 120 }), () => {
    const c = circle([0, 0], 70);
    fix(c.center(), [0, 0]);
    diameter(c, 70);
  })

// Three sections: the surface now has to pass through the belly on its way
// up, so the tube swells out in the middle.
loft(foot, belly, lip);

The profiles must be on different planes — typically parallel planes at different offsets — and the order in the list matters: a belly listed after the neck would make the surface double back on itself.

Guide curves​

Guides are side rails the transition surface must follow. Pass one or two open curves; each guide has to pass through every profile. A single sketch may carry several guide curves (for example a curve and its mirror()) — each connected curve counts as one guide:

Loft riding two guide rails

The code behind it
import { sketch, plane, loft, line, circle, bezier, mirror, yAxis } from 'fluidcad/core';
import { coincident, equal, perpendicular, fix } from 'fluidcad/constraints';

const p1 = sketch("top", () => {
    // A square rotated 45°, 50 across the flats
    const s1 = line([35.355339, 0], [0, 35.355339]);
    const s2 = line([0, 35.355339], [-35.355339, 0]);
    const s3 = line([-35.355339, 0], [0, -35.355339]);
    const s4 = line([0, -35.355339], [35.355339, 0]);
    coincident(s1.end(), s2.start());
    coincident(s2.end(), s3.start());
    coincident(s3.end(), s4.start());
    coincident(s4.end(), s1.start());
    equal(s1, s2);
    equal(s2, s3);
    equal(s3, s4);
    perpendicular(s1, s2);
    fix(s1.start());
  })

const p2 = sketch(plane("top", 80), () => {
    circle([0, 0], 30);
  })

// One sketch, two rails: the bezier and its mirror each count as one guide
const g1 = sketch("right", () => {
    bezier([Math.sqrt(2) * 25, 0], [50, 40], [15, 80])
    mirror(yAxis())
}).reusable()

loft(p1, p2).guides(g1)

Here the bezier and its mirror form two rails; the square's corners ride them all the way up to the circle. Guides can also be passed as separate arguments:

loft(p1, p2).guides(rightRail, leftRail)

Guides compose with start/end conditions: the condition fades out around each guide's contact point, so the rails keep their sides of the surface while the condition shapes the rest. Guides cannot be combined with thin walls.

loft(p1, p2).guides(g1).startCondition('normal')

Start and end conditions​

The condition rows control how the surface leaves the first profile and arrives at the last one:

  • 'none' — no constraint (default)
  • 'normal' — the surface takes off perpendicular to the profile plane
  • 'tangent' — the surface takes off inside the profile plane, bulging outward

Loft with normal end conditions

The code behind it
import { sketch, plane, loft, line, circle } from 'fluidcad/core';
import { coincident, equal, perpendicular, fix } from 'fluidcad/constraints';

const p1 = sketch("top", () => {
    // A square rotated 45°, 50 across the flats
    const s1 = line([35.355339, 0], [0, 35.355339]);
    const s2 = line([0, 35.355339], [-35.355339, 0]);
    const s3 = line([-35.355339, 0], [0, -35.355339]);
    const s4 = line([0, -35.355339], [35.355339, 0]);
    coincident(s1.end(), s2.start());
    coincident(s2.end(), s3.start());
    coincident(s3.end(), s4.start());
    coincident(s4.end(), s1.start());
    equal(s1, s2);
    equal(s2, s3);
    equal(s3, s4);
    perpendicular(s1, s2);
    fix(s1.start());
  })

const p2 = sketch(plane("top", 80), () => {
    circle([0, 0], 30);
  })

// The surface leaves the square and arrives at the circle perpendicular
// to their planes, swelling the transition outward
loft(p1, p2)
    .startCondition('normal', 1)
    .endCondition('normal', 1)

The magnitude scales the takeoff strength (default 1). Negative values flip the direction — a 'tangent' condition with a negative magnitude pinches inward instead of bulging:

loft(p1, p2).startCondition('normal', 2)     // stronger perpendicular takeoff
loft(p1, p2).endCondition('tangent', -0.5)   // gentle inward pinch at the top
loft(p1, p2).startCondition('normal')        // conditions can differ per end
          .endCondition('tangent')

Conditions require closed profiles and work with thin walls (both walls follow the condition).

Add, New and Remove​

A tank lid, and one loft from a Ø44 circle on a plane halfway through the lid to a 16 × 16 square 50 up. Only the tab changes:

AddAdd modeloft(s1, s2)

The loft fuses with the lid — a round-to-square nozzle grows out of it.

NewNew modeloft(s1, s2).new()

The nozzle is a separate solid seated in the lid.

RemoveRemove modeloft(s1, s2).remove()

The nozzle's volume is cut out — a funnel-shaped recess down to the first profile.

The Add column's code

The New and Remove columns only change the highlighted line.

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

// The base part every column shares: a 100 x 100 x 12 tank lid.
sketch("xy", () => {
    const sg1 = line([-50, -50], [50, -50]);
    const sg2 = line([50, -50], [50, 50]);
    const sg3 = line([50, 50], [-50, 50]);
    const sg4 = line([-50, 50], [-50, -50]);
    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(), [-50, -50]);
    distance(sg1.start(), sg1.end(), 100);
    distance(sg2.start(), sg2.end(), 100);
  })
const lid = extrude(12)

// First profile: a Ø44 circle on a plane halfway through the lid (6 up).
const s1 = sketch(plane("xy", { offset: 6 }), () => {
    circle([0, 0], 44);
  })

// Second profile: a 16 x 16 square outlet, 50 up.
const s2 = sketch(plane("xy", { offset: 50 }), () => {
    const t1 = line([-8, -8], [8, -8]);
    const t2 = line([8, -8], [8, 8]);
    const t3 = line([8, 8], [-8, 8]);
    const t4 = line([-8, 8], [-8, -8]);
    coincident(t1.end(), t2.start());
    coincident(t2.end(), t3.start());
    coincident(t3.end(), t4.start());
    coincident(t4.end(), t1.start());
    horizontal(t1);
    vertical(t2);
    horizontal(t3);
    vertical(t4);
    fix(t1.start(), [-8, -8]);
    distance(t1.start(), t1.end(), 16);
    distance(t2.start(), t2.end(), 16);
  })

// Add tab: the loft fuses with the lid — a round-to-square nozzle grows out of it.
loft(s1, s2)

Thin walls​

Turn on Thin to offset every profile's edges by the thickness and loft the bands — a shell instead of a filled loft:

Thin loft

The code behind it
import { sketch, loft, plane } from 'fluidcad/core';
import { circle, line } from 'fluidcad/core';
import { coincident, distance, fix, horizontal, vertical } from "fluidcad/constraints";

const s1 = sketch("xy", () => {
    circle([0, 0], 100);
  })

const s2 = sketch(plane("xy", { offset: 100 }), () => {
    const sg1 = line([-40, -40], [40, -40]);
    const sg2 = line([40, -40], [40, 40]);
    const sg3 = line([40, 40], [-40, 40]);
    const sg4 = line([-40, 40], [-40, -40]);
    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(), [-40, -40]);
    distance(sg1.start(), sg1.end(), 80);
    distance(sg2.start(), sg2.end(), 80);
  })

loft(s1, s2).thin(5)
loft(s1, s2).thin(5)     // 5 units outward
loft(s1, s2).thin(-5)    // 5 units inward
loft(s1, s2).thin(5, -3) // dual offset

All profiles must be sketches with matching topology (same number of wires).

Thin in the three modes​

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

AddAdd modeloft(s1, s2).thin(2)

A 2-thick hopper wall fused with the lid.

NewNew modeloft(s1, s2).thin(2).new()

The hopper wall as a separate body.

RemoveRemove modeloft(s1, s2).thin(2).remove()

Only the wall is cut — a tapered ring slot in the lid.

The Add column's code
import { sketch, extrude, loft, plane, circle, line } from 'fluidcad/core';
import { coincident, distance, fix, horizontal, vertical } from "fluidcad/constraints";

// The base part every column shares: a 100 x 100 x 12 tank lid.
sketch("xy", () => {
    const sg1 = line([-50, -50], [50, -50]);
    const sg2 = line([50, -50], [50, 50]);
    const sg3 = line([50, 50], [-50, 50]);
    const sg4 = line([-50, 50], [-50, -50]);
    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(), [-50, -50]);
    distance(sg1.start(), sg1.end(), 100);
    distance(sg2.start(), sg2.end(), 100);
  })
const lid = extrude(12)

// First profile: a Ø44 circle on a plane halfway through the lid (6 up).
const s1 = sketch(plane("xy", { offset: 6 }), () => {
    circle([0, 0], 44);
  })

// Second profile: a 16 x 16 square outlet, 50 up.
const s2 = sketch(plane("xy", { offset: 50 }), () => {
    const t1 = line([-8, -8], [8, -8]);
    const t2 = line([8, -8], [8, 8]);
    const t3 = line([8, 8], [-8, 8]);
    const t4 = line([-8, 8], [-8, -8]);
    coincident(t1.end(), t2.start());
    coincident(t2.end(), t3.start());
    coincident(t3.end(), t4.start());
    coincident(t4.end(), t1.start());
    horizontal(t1);
    vertical(t2);
    horizontal(t3);
    vertical(t4);
    fix(t1.start(), [-8, -8]);
    distance(t1.start(), t1.end(), 16);
    distance(t2.start(), t2.end(), 16);
  })

// Add + Thin: a 2-thick hopper wall instead of a solid nozzle, fused with the lid.
loft(s1, s2).thin(2)

Accessing geometry​

const l = loft(s1, s2)

l.endFaces()       // face at the last profile
l.startFaces()     // face at the first profile
l.sideFaces()      // the transition surface(s)
l.endEdges()       // edges at the last profile
l.startEdges()     // edges at the first profile
l.sideEdges()      // edges along the sides
l.internalFaces()  // inner wall face(s) of a thin loft (closed profiles)
l.capFaces()       // cap face(s) of a thin loft (open profiles)

Fusion scope​

loft(s1, s2).new()                // create a separate solid
loft(s1, s2).add()                // fuse with touching solids (default)
loft(s1, s2).remove()             // subtract from all intersecting solids
loft(s1, s2).remove().scope(box)  // subtract only from the box