Building a Lantern

In this tutorial, you'll build a hexagonal lantern from scratch, based on the original design by TooTallToby. It covers a wide range of FluidCAD features: polygons, draft extrusions, shelling, projecting geometry, pattern cuts, lofting, and revolving.

Create a new file called lantern.fluid.js in your project.

Setup

Start with imports and some variables that define the lantern's dimensions. Using variables makes the model parametric — change a number and the whole lantern updates.

import {
    axis, circle, color, cut, extrude, loft, move, offset,
    plane, polygon, project, repeat, revolve, select, shell,
    sketch, sphere, translate
} from 'fluidcad/core';
import { face } from 'fluidcad/filters';

const sides = 6;
const draft = 8;
const windowOffset = 6;
const wallThickness = 7;
const middleHeight = 150;

• sides — number of sides for the lantern's cross-section (hexagonal)
• draft — draft angle in degrees, so the body tapers as it goes up
• windowOffset — how far the window cutouts are inset from the face edges
• wallThickness — wall thickness after shelling
• middleHeight — height of the main body

Step 1: The middle body

The lantern's main body is a hexagonal prism with a slight taper and hollow walls.

Extrude with draft

Sketch a hexagon on a plane that's offset 24 units above the origin (to leave room for the base below), then extrude it upward with a draft angle. The .new() keeps it as a separate solid — we'll need to reference its faces later without interference from other parts.

sketch(plane("xy", { offset: 24 }), () => {
    polygon(sides, 100);
})

const middle = extrude(middleHeight).draft(draft).new()

The draft angle makes the hexagon slightly narrower at the top than the bottom, giving the lantern its characteristic tapered shape.

Shell it hollow

Select the top and bottom faces, then shell the body to create hollow walls:

select(
    face().onPlane("xy", middleHeight + 24),
    face().onPlane("xy", 24),
);

shell(-wallThickness)

face().onPlane("xy", middleHeight + 24) finds the top face (at height 174), and face().onPlane("xy", 24) finds the bottom face. These two faces are removed, and the rest of the solid is hollowed out with walls of wallThickness (7 units).

Step 2: Cut the windows

Each side of the lantern gets a window. We'll create one window and repeat it around the body.

Project and offset

To create a window that fits exactly within a side face, we project the face outline onto a sketch, then offset it inward:

sketch(middle.sideFaces(0), () => {
    project(middle.sideFaces(0))
    offset(-windowOffset, true)
})

• middle.sideFaces(0) gives us the first side face of the hexagonal body — we use it both as the sketch plane and as the geometry to project.
• project() traces the face's outline onto the sketch.
• offset(-windowOffset, true) shrinks the outline inward by 6 units. The true removes the original projected outline, leaving only the inset shape.

Cut and repeat

Cut through the wall, then repeat the cut for all sides:

const c = cut(7)

repeat("circular", "z", {
    count: sides + 1,
    offset: 360 / sides
})

cut(7) removes 7 units of material (matching the wall thickness). The repeat("circular") re-applies this cut around the Z axis, once for each side of the hexagon. We use sides + 1 because count includes the original.

Step 3: The base

The base is two stacked hexagonal layers — a wider bottom tier and a narrower upper tier.

polygon(sides, 150, "xy");

const pl1 = extrude(12)

polygon(sides, 115, pl1.endFaces());

extrude(12)

• The first polygon(sides, 150, "xy") draws a hexagon with diameter 150 directly on the XY plane (no sketch block needed — the plane is passed as the last argument).
• extrude(12) creates a 12-unit tall base slab. It auto-fuses since we didn't use .new().
• The second hexagon (diameter 115) is drawn on the top face of the first layer (pl1.endFaces()), then extruded another 12 units. This creates a stepped base.

Step 4: The top

The top mirrors the base with a wider cap, then lofts up to a narrow tip.

Cap and tip

const topPlane = plane("xy", { offset: middleHeight + 24 });
polygon(sides, 165, topPlane);

const top = extrude(12)

polygon(sides, 50, plane(topPlane, { offset: 52 + 12 }));

const tip = extrude(12)

• topPlane is positioned at the top of the middle body (height 174).
• A wide hexagon (diameter 165) is extruded 12 units to form the cap.
• A small hexagon (diameter 50) is placed 64 units above topPlane and extruded 12 units for the tip.

Loft between cap and tip

loft(top.endFaces(), tip.startFaces())

loft() creates a smooth transition between the top of the cap and the bottom of the tip. This forms the sloped roof of the lantern.

Step 5: The ring and handle

Finally, a small sphere sits on top, and a ring loops above it as a handle.

Sphere

let s = sphere(25 / 2)
translate([0, 0, 257], s)

A small sphere (diameter 12.5) is placed at the very top of the lantern at height 257.

Ring

const ringAxis = axis("y", { offsetZ: 290 })

sketch("left", () => {
    circle([0, 290 + (65 / 2) - (7 / 2)], 7)
});

revolve(ringAxis).new()

• axis("y", { offsetZ: 290 }) creates a Y-axis shifted up to height 290 — this is the center of the ring.
• A small circle (diameter 7) is sketched on the left plane, positioned to form the ring's cross-section.
• revolve(ringAxis) rotates this circle around the offset axis, creating a torus (ring). The .new() keeps it separate from the rest.

Full code

import {
    axis, circle, color, cut, extrude, loft, move, offset,
    plane, polygon, project, repeat, revolve, select, shell,
    sketch, sphere, translate
} from 'fluidcad/core';
import { face } from 'fluidcad/filters';

const sides = 6;
const draft = 8;
const windowOffset = 6;
const wallThickness = 7;
const middleHeight = 150;

// Middle Body
sketch(plane("xy", { offset: 24 }), () => {
    polygon(sides, 100);
})

const middle = extrude(middleHeight).draft(draft).new()

select(
    face().onPlane("xy", middleHeight + 24),
    face().onPlane("xy", 24),
);

shell(-wallThickness)

// Cut Windows
sketch(middle.sideFaces(0), () => {
    project(middle.sideFaces(0))
    offset(-windowOffset, true)
})

const c = cut(7)

repeat("circular", "z", {
    count: sides + 1,
    offset: 360 / sides
})

// Base
polygon(sides, 150, "xy");

const pl1 = extrude(12)

polygon(sides, 115, pl1.endFaces());

extrude(12)

// Top
const topPlane = plane("xy", { offset: middleHeight + 24 });
polygon(sides, 165, topPlane);

const top = extrude(12)

polygon(sides, 50, plane(topPlane, { offset: 52 + 12 }));

const tip = extrude(12)

loft(top.endFaces(), tip.startFaces())

// Ring & Handle
let s = sphere(25 / 2)
translate([0, 0, 257], s)

const ringAxis = axis("y", { offsetZ: 290 })

sketch("left", () => {
    circle([0, 290 + (65 / 2) - (7 / 2)], 7)
});

revolve(ringAxis).new()

What you practiced

• Parametric variables — defining dimensions at the top so the whole model adapts when you change a value
• plane() with offset — positioning sketches at specific heights
• polygon() — creating hexagonal profiles
• .draft() — tapering an extrusion
• .new() — preventing auto-fusion to keep parts separate
• select() + shell() — hollowing a solid by removing specific faces
• project() + offset() — tracing a face outline and shrinking it for window cutouts
• repeat("circular") — repeating a cut around an axis
• loft() — smoothly connecting two faces at different heights
• axis() with offset + revolve() — creating a ring (torus) by revolving a circle around an offset axis