Shell

Shell hollows a solid into walls of a given thickness. You pick the faces to remove; they become the openings. A box becomes a tray, a cylinder becomes a cup.

In the viewport

1. Click Shell on the toolbar. A small panel opens beside the model.
2. Click the face (or faces) to open in the viewport. Right-click a pick for the multi-select menu — same-type faces, the producing feature's other buckets (Extrude End Faces …), Select other.
3. Type the thickness. The statement is written as soon as the pick is complete.

1234

1. 1
   Selection

   The faces to remove — they become the openings. Each pick is a numbered chip; the ✕ drops one, and clicking a picked face again drops it too. Leave it empty and nothing happens: Shell always needs at least one face.
2. 2
   Thickness

   How thick the walls end up. Negative shells inward and keeps the outer shape; positive shells outward and keeps the inner cavity.
3. 3
   Join type

   How the offset walls meet at a corner: Arc rounds the join, Intersection runs both walls on until they cross, Tangent extends them tangentially. Arc is the safe default.
4. 4
   Apply

   Writes the statement and adds the timeline row; Exit writes nothing.

From solid to walls

A cylinder with both flat faces removed becomes a tube:

Beforecylinder(50, 100)

A Ø50 cylinder, 100 tall, solid all the way through.

Aftershell(-5)

The top and bottom faces are gone and what is left is a 5-thick wall. The outside is still Ø50 — a negative thickness grows the wall inward.

The solid

cup.part.js

import { cylinder } from 'fluidcad/core';

// A Ø50 cylinder, 100 tall — solid all the way through.
cylinder(50, 100)

The complete file

import { cylinder, select, shell } from 'fluidcad/core';
import { face } from 'fluidcad/filters';

// A Ø50 cylinder, 100 tall — no sketch needed for a primitive.
cylinder(50, 100)

// Select the flat circular faces (top and bottom) — the Shell tool writes
// this select() when the picked faces match a filter.
select(face().circle())

// Hollow the cylinder with 5-thick walls, removing the selected faces.
// Negative: the walls grow inward and the outside stays Ø50.
shell(-5)

Thickness direction

Sign	Result
Negative, e.g. -5	Walls grow inward — the outer shape stays the same
Positive, e.g. 5	Walls grow outward — the inner cavity stays the same

Passing faces directly

In code, the faces to remove can come from an operation's accessors instead of a select():

const e = extrude(30)
shell(-3, e.endFaces())        // remove the top face, hollow the rest

Several faces at once:

shell(-3, e.endFaces(), e.startFaces())   // open on top and bottom

With no faces at all, shell() takes the last selection — the Selection and filters page covers how those are written.

Accessing geometry

const s = shell(-3, e.endFaces())

s.internalFaces()      // the inner wall faces
s.internalEdges()      // edges on the inner walls