Building a 45 Degree Custom Elbow

In this tutorial, you'll build a 45° pipe elbow with a square base flange and a round slotted flange, based on the original design by Too Tall Toby. It covers reusable spine sketches, sweeping individual sketch regions, boring with a removal sweep, sketching on swept end faces, circular sketch copies, stepped slot cuts, and circular feature repeats around an axis built from a sketch segment.

Create a new file called custom-elbow.fluid.js in your project.

Setup

Start with the imports.

import { axis, circle, copy, cut, extrude, hMove, move, rect, remove, repeat,
    sketch, slot, sweep, tArc, tLine, vLine } from "fluidcad/core";

Everything comes from fluidcad/core — the sketching primitives, the 3D operations, and the pattern utilities.

Step 1: The elbow spine

The whole part hangs off a single path: a vertical run, a 45° bend, and a straight exit. We draw it once on the front plane and reuse it for everything else — the pipe sweep, the bore sweep, and the pattern axis at the end.

const spine = sketch("front", () => {
    vLine(1.5)
    tArc(-4, 45);
    const topSegment = tLine(1.5);

    return {
        topSegment
    }
}).reusable();

vLine(1.5) draws a vertical line 1.5 units straight up from the origin. tArc(-4, 45) continues from its end with a tangent arc of radius 4 that stops once the path direction has turned to 45° — the negative radius flips the sweep direction so the arc bends away from the vertical run instead of curling back over it. tLine(1.5) then extends the path 1.5 units in a straight line, tangent to the arc, so the exit leg leaves at exactly 45°.

We return topSegment from the sketch callback — whatever the callback returns is attached as .regions on the sketch, so spine.regions.topSegment gives us a named handle on that last straight segment. We'll turn it into the pattern axis in the final step.

Normally the next 3D operation consumes a sketch. This spine is used three times, so .reusable() keeps it alive across all of them.

Step 2: The pipe

Sketch the profile

The pipe cross-section is two concentric circles on the top plane, centered where the spine starts.

const profile = sketch("top", () => {
    const innerPipe = circle(1.5)
    const outerPipe = circle(2);

    return {
        innerPipe,
        outerPipe
    }
});

circle(1.5) is the bore — 1.5 units in diameter — and circle(2) is the pipe's outside diameter, giving a 0.25 wall. Returning both attaches them as named regions, so we can hand each circle to a different sweep.

Sweep the outer pipe

const pipe = sweep(spine, profile.regions.outerPipe);

sweep(spine, profile.regions.outerPipe) drives the outer circle along the spine, producing a solid bent rod. Because we pass one specific region instead of the whole sketch, the innerPipe region stays available — we'll sweep it later to bore the pipe out. We capture the result as pipe so we can sketch on its end face in step 4.

Step 3: The base flange

Sketch the plate

The base flange is a rounded square plate with four bolt holes, drawn on the top plane around the foot of the pipe.

sketch("top", () => {
    rect(3.5).centered().radius(0.5)
    move([-2.5 / 2, -2.5 / 2])
    const c = circle(0.5)
    copy("circular", [0, 0], {
        count: 4,
        angle: 360
    }, c)
});

rect(3.5).centered().radius(0.5) draws a 3.5-unit square centered on the origin with 0.5-radius rounded corners. move([-2.5 / 2, -2.5 / 2]) jumps the cursor to one corner of the 2.5 × 2.5 bolt pattern, and circle(0.5) places a 0.5-diameter bolt hole there. copy("circular", [0, 0], { count: 4, angle: 360 }, c) copies that hole 4 times evenly around the sketch origin, landing one hole near each corner of the plate. Because the holes are closed shapes inside the plate outline, they extrude as cutouts automatically.

Extrude the plate

extrude(.375)

extrude(.375) raises the plate 0.375 units. It fuses with the bottom of the pipe into a single body.

Step 4: The upper flange

Sketch on the pipe's end face

The round flange sits on the angled end of the pipe, so we sketch directly on the face the sweep finished on.

sketch(pipe.endFaces(), () => {
    circle(4)
});

pipe.endFaces() returns the face at the end of the sweep path — the 45° face. Sketching on it orients the sketch to that plane, with the origin at the face center, so circle(4) drops a 4-diameter flange disc concentric with the pipe.

Extrude back into the pipe

const upperFlange = extrude(-.625)

extrude(-.625) extrudes 0.625 units in the negative direction — back down the pipe — so the flange ends up flush with the pipe's end instead of floating past it. We keep it as upperFlange to sketch the bolt slots on it next.

Step 5: Boring the pipe

So far the pipe is a solid rod, and both flanges block its ends. One sweep opens the whole passage.

sweep(spine, profile.regions.innerPipe).remove()

This sweeps the 1.5-diameter innerPipe region along the same reusable spine, and .remove() turns the sweep into a subtraction — instead of adding the swept solid, it carves it out of everything it passes through. The pipe wall, the base plate, and the upper flange all get bored in a single operation.

Step 6: The bolt slots

Sketch two stacked slots

The upper flange carries four radial bolt slots, each with a wider shallow relief around a narrower through-slot. We sketch one pair and pattern it later.

const slots = sketch(upperFlange.endFaces(), () => {
    hMove(3.25 / 2)
    const outerSlot = slot(1, .75 / 2)
    const innerSlot = slot(1, .45 / 2)

    return {
        outerSlot,
        innerSlot
    }
});

upperFlange.endFaces() is the face the flange extrusion finished on, so the sketch origin sits on the pipe centerline. hMove(3.25 / 2) slides the cursor out to the 3.25-diameter bolt circle. slot(1, .75 / 2) draws a slot 1 unit long with 0.375-radius end caps — 0.75 wide — extending radially outward from the cursor, and slot(1, .45 / 2) draws a narrower 0.45-wide slot on the same footprint. Returning both gives us a named region for each, because the two slots get cut to different depths.

Cut each slot to its own depth

const s1 = cut(slots.regions.innerSlot)
const s2 = cut(.25, slots.regions.outerSlot)

cut(slots.regions.innerSlot) with no depth cuts the narrow slot all the way through the flange. cut(.25, slots.regions.outerSlot) cuts the wide slot only 0.25 deep, leaving a stepped recess around the through-slot. We capture both cuts as s1 and s2 — they're the features we're about to pattern.

Step 7: Pattern the slots and clean up

const a = axis(spine.regions.topSegment)

repeat("circular", a, {
    count: 4,
    angle: 360
}, s1, s2)

remove(spine);

axis(spine.regions.topSegment) builds an axis from the spine's straight exit segment — the segment we named back in step 1. That line is the pipe's centerline through the upper flange, exactly the axis the bolt pattern revolves around. repeat("circular", a, { count: 4, angle: 360 }, s1, s2) repeats both cuts 4 times evenly around it, giving four stepped slots at 90° spacing.

Finally, remove(spine) deletes the reusable spine sketch from the scene — every consumer is done with it, so it shouldn't linger in the rendered model.

Full code

// @screenshot waitForInput
import { axis, circle, copy, cut, extrude, hMove, move, rect, remove, repeat,
    sketch, slot, sweep, tArc, tLine, vLine } from "fluidcad/core";

const spine = sketch("front", () => {
    vLine(1.5)
    tArc(-4, 45);
    const topSegment = tLine(1.5);

    return {
        topSegment
    }
}).reusable();

const profile = sketch("top", () => {
    const innerPipe = circle(1.5)
    const outerPipe = circle(2);

    return {
        innerPipe,
        outerPipe
    }
});

const pipe = sweep(spine, profile.regions.outerPipe);

sketch("top", () => {
    rect(3.5).centered().radius(0.5)
    move([-2.5 / 2, -2.5 / 2])
    const c = circle(0.5)
    copy("circular", [0, 0], {
        count: 4,
        angle: 360
    }, c)
});

extrude(.375)

sketch(pipe.endFaces(), () => {
    circle(4)
});

const upperFlange = extrude(-.625)

sweep(spine, profile.regions.innerPipe).remove()

const slots = sketch(upperFlange.endFaces(), () => {
    hMove(3.25 / 2)
    const outerSlot = slot(1, .75 / 2)
    const innerSlot = slot(1, .45 / 2)

    return {
        outerSlot,
        innerSlot
    }
});

const s1 = cut(slots.regions.innerSlot)
const s2 = cut(.25, slots.regions.outerSlot)

const a = axis(spine.regions.topSegment)

repeat("circular", a, {
    count: 4,
    angle: 360
}, s1, s2)

remove(spine);

What you practiced

• sketch().reusable() — keeping one path sketch alive for multiple consumers (two sweeps and an axis)
• returning shapes from a sketch — attaching named .regions handles to geometry for later reference
• tArc(radius, endAngle) — tangent arcs that stop at a target direction, with a negative radius to flip the bend
• tLine(length) — straight segments that continue tangent to the previous arc
• sweep(path, region) — sweeping one named region of a multi-region profile, leaving the rest available
• sweep().remove() — using a sweep as a subtraction to bore through several features at once
• sketch(op.endFaces(), ...) — sketching directly on the face an operation finished on
• extrude(-depth) — extruding backwards so a face-based feature stays flush with its face
• rect().centered().radius() — centered rounded-corner plates
• copy("circular", center, options, shape) — circular copies of sketch geometry
• slot(length, radius) — slots drawn from the cursor with round end caps
• cut(depth, region) — cutting different regions of one sketch to different depths
• axis(segment) — turning a named sketch segment into a pattern axis
• repeat("circular", axis, options, ...features) — patterning multiple cut features around an axis
• remove() — clearing a reusable sketch once every consumer is done with it