Building a 3D Printable Desk Organizer

In this tutorial, you'll build a four-compartment octagonal desk organizer with a square inner pocket, based on the original design by TooTallToby. It covers polygon sketches with circumscribed sizing, sketch-level rotate and fillet, chamfering and shelling by extrude faces, multi-loop sketches via offset, ribs on a rotated reference plane, circular patterning, and a thin revolve cut for trimming.

Create a new file called desk-organizer.fluid.js in your project.

Setup

A single import line covers every operation used in this model.

import { plane, sketch, extrude, fillet, rect, chamfer, move, repeat, rotate, arc, shell, polygon, offset, aLine, rib, revolve } from 'fluidcad/core';

Everything comes from fluidcad/core — no filters needed. Selections in this model use the extrude handle (outer.startEdges(), outer.endFaces()) instead of plane-based filters.

Step 1: Octagonal base

Sketch the footprint

sketch("top", () => {
    polygon(8, 140, 'circumscribed')
    rotate(45 / 2)
    fillet(20)
});

polygon(8, 140, 'circumscribed') draws an 8-sided polygon circumscribed around a circle of radius 140 — meaning 140 is the apothem (the perpendicular distance from center to a face), not the circumradius. This makes the flats of the octagon land on the 140 mark.

rotate(45 / 2) spins the polygon by 22.5° within the sketch so a flat face — not a vertex — sits on the X axis. That orientation matters in step 4: it lines up the inner square's diagonals with four of the octagon's flats.

fillet(20) rounds each of the eight polygon corners with a 20-unit radius, softening what would otherwise be sharp vertical edges on the body.

Extrude upward

const outer = extrude(110);

extrude(110) pushes the octagon 110 units along the top plane's normal (upward), creating a tall octagonal prism. Storing the result as outer gives us a handle for selecting the start/end edges and faces of this extrude in the next steps.

Step 2: Chamfer the bottom and shell from the top

chamfer(8, outer.startEdges())

shell(-5, outer.endFaces())

outer.startEdges() returns the edges around the start of the extrude — the bottom of the prism, where the sketch lived. chamfer(8, ...) bevels them with an 8-unit chamfer, giving the body a clean foot.

outer.endFaces() returns the end face of the extrude — the top of the prism. shell(-5, ...) hollows the body inward with 5-unit walls and removes the top face, opening the prism into a cup with a 5-thick floor and walls.

Step 3: Inner square pocket

Sketch a square ring

sketch("top", () => {
    rect(50).centered();
    offset(-5);
});

rect(50).centered() draws a 50×50 square centered on the origin. offset(-5) adds an inset profile 5 units inside the square, leaving both loops in the sketch — outer 50×50 and inner 40×40. A sketch with a closed inner loop inside a closed outer loop extrudes as an annular profile (a frame), not a solid block.

Extrude the inner column

extrude(160);

extrude(160) pushes the square ring 160 units upward — taller than the outer prism's 110, so it pokes up above the open top. With no .new() call, the new solid auto-fuses with the existing body, fusing through the floor of the cup so the inner square wall stands as a continuous part of the organizer.

Step 4: Add a rib and pattern it around

Build a rotated reference plane

const p = plane("front", { rotateY: 45 })

plane("front", { rotateY: 45 }) takes the front plane (XZ) and rotates it 45° around the Y axis. Inside this rotated plane, drawing along the X axis traces a path running diagonally between the inner square corners and the surrounding octagon — exactly where we want the first rib to sit.

Sketch the rib spine

sketch(p, () => {
    move([(-140 / 2) + 5, 110]);
    aLine(45, 20)
});

move([(-140 / 2) + 5, 110]) parks the cursor at x=−65 (just inside the polygon's left flat) and y=110 (the height of the outer body's open top). aLine(45, 20) draws an angled line at 45° with length 20 — a short seed for the rib. The line itself doesn't need to span the full gap; .extend() will stretch it to the surrounding solids.

Build and pattern the rib

rib(5).parallel().extend();

repeat("circular", "z", {
    count: 4,
    angle: 360
})

rib(5) builds a 5-thick rib from the spine. The chained calls do the heavy lifting:

• .parallel() — extrudes the rib in-plane (perpendicular to the spine within the rotated plane) instead of normal to the sketch, so the rib stands up as a wall connecting the inner square to the outer shell.
• .extend() — stretches the spine endpoints outward until they meet surrounding solids: the inner square wall on one side, the outer octagon's inside wall on the other.

repeat("circular", "z", { count: 4, angle: 360 }) rotates the most recent operation — the rib — around the Z axis four times for a full revolution, producing four rib walls 90° apart that divide the cavity into four compartments.

Step 5: Trim the top with a thin revolve cut

Sketch the trim arc

sketch("front", () => {
    arc(140, 0, 90)
});

arc(140, 0, 90) draws a quarter arc on the front plane: radius 140, sweeping from 0° to 90° — from (140, 0) up to (0, 140). Because the arc is centered on the Z axis, revolving it around Z sweeps every point on the arc through a full circle, generating a hemispherical surface of radius 140 sitting on top of the model. That's the surface that will dome off the inner column and trim everything above it.

Revolve as a thin cut

revolve("z").thin(30).remove()

revolve("z") revolves around the Z axis to build that hemisphere. .thin(30) turns the open arc into a 30-thick shell rather than a closed solid — without it, the open arc couldn't define a watertight body to revolve. .remove() subtracts the revolved shell from the model.

The result is a hemispherical trim surface that domes the top of the inner square column — clipping the four corners of the column down to a smooth spherical cap — and slices any material that pokes above the hemisphere off the outer rim. The 30 thickness is intentionally exaggerated; it just needs to be thick enough to fully consume the excess material from the inner extrude.

Full code

// @screenshot waitForInput
import { plane, sketch, extrude, fillet, rect, chamfer, move, repeat, rotate, arc, shell, polygon, offset, aLine, rib, revolve } from 'fluidcad/core';

sketch("top", () => {
    polygon(8, 140, 'circumscribed')
    rotate(45 / 2)
    fillet(20)
});

const outer = extrude(110);

chamfer(8, outer.startEdges())

shell(-5, outer.endFaces())

sketch("top", () => {
    rect(50).centered();
    offset(-5);
});

extrude(160);

const p = plane("front", { rotateY: 45 })

sketch(p, () => {
    move([(-140 / 2) + 5, 110]);
    aLine(45, 20)
});

rib(5).parallel().extend();

repeat("circular", "z", {
    count: 4,
    angle: 360
})

sketch("front", () => {
    arc(140, 0, 90)
});

revolve("z").thin(30).remove()

What you practiced

• polygon(sides, size, 'circumscribed') — sizing a polygon by its apothem rather than its circumradius
• rotate() and fillet() inside a sketch — orienting and rounding a sketch profile before extruding
• Extrude handles (startEdges, endFaces) — selecting bottom edges and top face of an extrude without plane filters
• chamfer() — beveling edges by an absolute distance
• shell() with a face selection — hollowing a body and removing one face to open it
• rect() + offset() for an annular sketch — keeping both loops in the sketch to extrude a frame instead of a block
• plane("front", { rotateY: ... }) — rotating a reference plane to angle a rib path diagonally
• rib().parallel().extend() — building a stiffening wall from a short seed line that extends to surrounding solids
• repeat("circular", "z", ...) — circular-patterning the previous operation around an axis
• revolve().thin().remove() — using a thin-walled revolve as a trim cut to clean up a profile