3D Operations
A sketch is flat. The operations in this section turn it into a solid and then reshape that solid. Each one is a button on the toolbar with a docked dialog (or, for the pick tools, a small value panel), and each one writes a statement to the part file that you can read, edit and chain methods on.
The operations
| Operation | Toolbar | What it does |
|---|---|---|
| Extrude | Extrude | Pulls a sketch along its plane's normal — a plate, a boss, or (on the Remove tab) a pocket |
| Revolve | Revolve | Turns a sketch around an axis |
| Sweep | Sweep | Moves a profile along a path |
| Loft | Loft | Blends between two or more profiles |
| Shell | Shell | Hollows a solid, opening the picked faces |
| Fillet | Fillet | Rounds edges |
| Chamfer | Chamfer | Bevels edges |
| Wrap | Wrap | Bends a sketch onto a cylinder or cone and embosses or engraves it |
| Rib | Rib | Grows a wall from a spine line until it meets the surrounding solid |
| Helix | Helix | Makes the helical wire that springs and threads are swept along |
Extrude, Revolve, Sweep, Loft, Wrap and Rib make material and have the Add / New / Remove tabs described below. Fillet, Chamfer and Shell modify a solid you point at: they are pick tools — click the button, click edges or faces in the viewport, type the value — and they need the selection to say which edges or faces.
Add, New and Remove
Every material-making dialog starts with the same three tabs. They decide how the new geometry meets the solids already in the scene:
| Tab | Code | Result |
|---|---|---|
| Add | extrude(30) (default, or .add()) | Fuses with every solid it touches. A boss on a plate becomes one body. |
| New | extrude(30).new() | Stays a separate body, even where it overlaps another. The Shapes panel lists it on its own row. |
| Remove | cut(30) / revolve(...).remove() | Subtracts its volume from every solid it intersects — pockets, grooves, tunnels. The depth runs into the material, opposite the sketch normal, the way a drill entering the face you sketched on does. |
A fourth control, Scope, narrows Add or Remove to particular solids: cut().remove().scope(box) cuts only from box. For extrude the Remove tab writes cut(), which is the same feature as extrude().remove().
Each operation's page walks through its dialog control by control, shows the sketch and the solid it becomes side by side, and puts the same base part through the three tabs — plain and again with thin walls on: extrude, revolve, sweep, loft.
Auto-fusion is the Add tab: touching solids merge unless you say otherwise. The Boolean operations section covers fusing, subtracting and intersecting solids that already exist, and Part covers the isolation boundary that keeps separate components from fusing.
Accessing geometry
Most operations return an object with accessors for the faces and edges they created:
const e = extrude(30)
e.endFaces() // top face(s)
e.startFaces() // bottom face(s)
e.sideFaces() // side face(s)
e.endEdges() // edges on the top
e.startEdges() // edges on the bottom
e.sideEdges() // edges on the sides
These are what the pick tools write when your clicks match a whole bucket, and what you pass by hand to sketch on a face, fillet edges, colour faces, or place a connector. The accessors available depend on the operation — each page lists its own.
When a later operation modifies or removes a face or edge, references to it may no longer be valid. For example, if you fillet an edge, the original edge is replaced by the fillet surface — so a reference to that edge won't work for subsequent operations.
Exception for faces as planes: even if a face is modified or destroyed by a later feature, you can still use it as a sketch plane. FluidCAD remembers the plane's position and orientation regardless of what happens to the face geometry.
const e = extrude(30)
fillet(5, e.endEdges()) // ✅ works — edges exist at this point
// After fillet, the original end edges are gone (replaced by fillet surfaces).
// But sketching on the end face still works:
sketch(e.endFaces(), () => { // ✅ works — face reference is valid as a plane
circle([0, 0], 20)
})
As a rule of thumb: reference geometry as close to its creation as possible, before later features reshape it.
Primitives
Two solids need no sketch at all:
import { sphere, cylinder } from 'fluidcad/core';
sphere(50) // sphere with diameter 50
cylinder(50, 100) // cylinder: diameter 50, height 100
Both accept chained .translate(), .rotate() and .mirror() — see Transforms.