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Cube

In one sentence: Create a parametric rectangular box (cuboid) whose length, width, and height can be changed at any time.

Overview

Workbench: Part · Menu: Part → Primitives → Cube
Toolbar: Part Primitives · Shortcut: none

The Cube primitive creates a rectangular box aligned with the world XYZ axes. All three dimensions remain live parameters in the Data panel — change them and the shape updates immediately without rebuilding.

Intuition

Every new FreeCAD model needs a starting shape. Cube is the fastest way to get a rectangular solid into the scene. From that first box, you subtract cylinders (holes), fuse flanges, or import STEP geometry and Boolean-combine everything into a finished part.

Unlike Part Design's Additive Box, a Part Cube does not need to live inside a Body container. It is a standalone shape that can be combined with any other Part object via Cut / Fuse / Common.

When to use it

  • You need a quick rectangular block to cut holes into or union with other shapes.
  • You are scripting geometry and want the simplest parametric solid.
  • You are working outside a Part Design Body (imported STEP workflow).

When NOT to use it

  • You are inside a Part Design Body — use Additive Box instead; it chains correctly in the feature tree.
  • You need a hollow tube — use Tube or subtract a smaller cylinder from a larger one.

Step-by-step walkthrough

  1. Switch to the Part workbench.
  2. Part → Primitives → Cube (or click the Cube toolbar button).
  3. A 10 × 10 × 10 mm box appears at the world origin.
  4. Select it in the model tree and open the Data panel.
  5. Edit Length, Width, Height to your required dimensions.
  6. Optionally set Placement to position the box.

Parameters

Parameter Type Default Description
Length Distance 10 mm Extent along the X axis
Width Distance 10 mm Extent along the Y axis
Height Distance 10 mm Extent along the Z axis
Placement Placement Identity Position and orientation of the box

Note: The box always starts at its corner (0, 0, 0) relative to its own placement. Its opposite corner is at (Length, Width, Height). Use Placement to centre or rotate it.

Common mistakes and pitfalls

Box at origin corner, not centred

By default the box occupies (0,0,0)→(L,W,H). If you expect it centred, set the Placement position to (−L/2, −W/2, −H/2) or use Part Mirror / Part Move to reposition.

Confusing Part Cube with Part Design Additive Box

Part Cube is a standalone shape. Part Design Additive Box lives inside a Body and participates in the feature chain. They look identical but behave differently in the tree.

Python API

import FreeCAD as App

doc = App.newDocument()

# Create a parametric cube
box = doc.addObject("Part::Box", "MyCube")
box.Length = 20.0   # mm
box.Width  = 15.0   # mm
box.Height = 10.0   # mm

# Reposition the box so it is centred on the origin
box.Placement = App.Placement(
    App.Vector(-10, -7.5, -5),   # position
    App.Rotation()               # no rotation
)

doc.recompute()
print(box.Shape.Volume)   # 3000.0

Shape access

# Access the underlying OCCT shape
shape = box.Shape

# Faces (6 faces on a box)
for i, face in enumerate(shape.Faces):
    print(f"Face {i}: area = {face.Area:.2f} mm²")

# Bounding box
bb = shape.BoundBox
print(f"Dimensions: {bb.XLength} × {bb.YLength} × {bb.ZLength} mm")

See also