Building a Fork
In this tutorial, you'll build a forked yoke from scratch, based on the original design by TooTallToby. It covers offset arc profiles, sketch-local mirror axes, side-mounted bosses with through-holes, and using .thin() annular cuts to leave central features standing.
Create a new file called fork.fluid.js in your project.
Setup
Start with imports — everything comes from fluidcad/core.
import { arc, circle, cut, extrude, local, mirror, move, offset,
plane, polygon, rect, sketch, vMove } from "fluidcad/core";
Step 1: The fork silhouette
The whole side profile is built up in a single sketch on the front plane: a U-shaped arch wall at the bottom, two rectangular legs flanking it, and a tall column on top.
Sketch the profile
sketch("front", () => {
arc(18)
offset(-36 + 18).close()
move([18, 0])
const r = rect(18, -40)
mirror(local("y"), r)
move([0, 18])
rect(36, 129 - 18).centered('horizontal')
});
arc(18) draws a semicircular arc of radius 18 from the origin — this is the inner edge of the arch. offset(-36 + 18).close() adds a parallel arc 18 units away and closes both ends, giving the arch a wall thickness of 18.
move([18, 0]) jumps the cursor to the right side of the arch, and rect(18, -40) drops an 18 x 40 leg straight down. mirror(local("y"), r) reflects that leg across the sketch's local Y-axis to produce the matching left leg.
Finally move([0, 18]) recenters the cursor on top of the arch and rect(36, 129 - 18).centered('horizontal') draws the 36-wide column going up to a total height of 129.
Extrude the body
extrude(36).symmetric();
extrude(36).symmetric() pushes the profile 18 units forward and 18 units back — a 36-deep body centered on the front plane.
Step 2: The side bosses
Each leg has a cylindrical boss sticking out the side. We'll model one and mirror it.
Sketch the boss
sketch(plane("right", 18), () => {
vMove(-(167 - 129))
circle(60);
});
plane("right", 18) creates a sketch plane on the right side of the column (x = 18). vMove(-(167 - 129)) moves the cursor down 38 units on that plane, placing the boss center inside the leg region. circle(60) draws a 60-diameter circle at that point.
Extrude and mirror
const distance = (80 - 36) / 2
const e = extrude(distance);
mirror("right")
extrude(distance) pushes the circle outward by 22 units — the gap between the body's 36-wide footprint and the model's 80-wide overall span, divided by two. We capture the result in e so we can sketch on its end face later. mirror("right") reflects the new boss across the right plane to produce the matching one on the left side.
Step 3: Bore through the bosses
sketch(e.endFaces(), () => {
circle(30)
});
cut();
e.endFaces() returns the outer circular face of the right boss, and circle(30) draws a 30-diameter circle on it. cut() with no argument removes material straight through everything in line with the sketch — including both bosses thanks to the earlier mirror — leaving a clean through-hole on each side.
Step 4: The cylindrical post
The top of the column tapers down through two stages. The first cut leaves a small cylindrical post standing on top.
Sketch the post
sketch(plane("top", 129), () => {
circle(30)
});
plane("top", 129) is the top plane raised to z = 129, sitting flush with the top face of the column. circle(30) draws a 30-diameter circle there — this defines the inside edge of the cut, the part we want to keep.
Cut the surrounding material
extrude(20).thin(20).remove()
.thin(20) widens the circle into a 20-thick annular ring around it, extrude(20) gives that ring a 20-unit depth, and .remove() subtracts the result from the body. Because the ring is wider than the column's half-width, it sweeps every corner away and leaves only the central cylinder standing.
Step 5: The square boss
The same trick works with a polygon. We use a 4-sided polygon to leave a rotated square section between the post and the main body.
Sketch the polygon
sketch(plane("top", 129 - 20), () => {
polygon(4, 36, 'circumscribed')
});
plane("top", 129 - 20) is the top plane offset to z = 109, exactly where the previous cut ended. polygon(4, 36, 'circumscribed') draws a 4-sided polygon circumscribed around a 36-diameter inscribed circle — a 36 x 36 square, oriented with its corners on the X and Y axes (rotated 45° relative to the main body).
Cut the surrounding material
extrude(45).thin(20).remove()
Same pattern as the post: a 20-thick annular ring around the square, extruded down 45 units and removed. The body's outer corners — which extend further out than the square's edges — get sliced away, leaving a clean rotated-square cross-section through that portion of the column.
Full code
// @screenshot waitForInput hideGrid
import { arc, circle, cut, extrude, local, mirror, move, offset, plane, polygon, rect, sketch, vMove } from "fluidcad/core";
sketch("front", () => {
arc(18)
offset(-36 + 18).close()
move([18, 0])
const r = rect(18, -40)
mirror(local("y"), r)
move([0, 18])
rect(36, 129 - 18).centered('horizontal')
});
extrude(36).symmetric();
sketch(plane("right", 18), () => {
vMove(-(167 - 129))
circle(60);
});
const distance = (80 - 36) / 2
const e = extrude(distance);
mirror("right")
sketch(e.endFaces(), () => {
circle(30)
});
cut();
sketch(plane("top", 129), () => {
circle(30)
});
extrude(20).thin(20).remove()
sketch(plane("top", 129 - 20), () => {
polygon(4, 36, 'circumscribed')
});
extrude(45).thin(20).remove()
What you practiced
arc()+offset().close()— building a U-shaped wall from a single semicirclelocal("y")— mirroring sketch geometry across the sketch's local axesplane("right", n)/plane("top", n)— creating offset reference planes for side and top featuresvMove()— moving the cursor vertically inside a sketchextrude(d)thenmirror("right")— modeling a single side feature and reflecting it.endFaces()— selecting the outer face of an extrusion to sketch onextrude().thin().remove()— cutting an annular ring around a profile to leave the central shape standingpolygon(sides, diameter, 'circumscribed')— drawing a regular polygon around a target inscribed circle