Thickness¶

In one sentence: Hollow out a solid to a uniform wall thickness by removing selected faces and offsetting the remaining shell inward.

Overview¶

Workbench: Part · Menu: Part → Thickness
Toolbar: Part Modeling · Shortcut: none

Thickness takes a solid, removes one or more selected faces (the "openings"), and offsets the remaining faces inward by the specified thickness, producing a hollow shell. It is the standard operation for creating injection-moulded plastic parts or sheet-metal shells.

Intuition¶

Imagine pressing a thick block of clay into a mould with a flat bottom. The result is a hollow box: the clay forms the walls and bottom, with the top open. Part Thickness does the same digitally: you pick which faces become openings, and FreeCAD creates the hollow shell at your specified wall thickness.

When to use it¶

Creating injection-moulded plastic housing from a solid model.
Producing a hollow container (box, tube, vessel) from a solid primitive.
Sheet-metal shell modelling (followed by flattening in a sheet-metal workbench).

When NOT to use it¶

Hollow cylinder — use Tube which is parametric.
Uniform 3-D offset — use Offset 3D if no faces are removed.

Step-by-step walkthrough¶

Select the solid in the model tree.
In the viewport, Ctrl+click the face(s) that will become the opening.
Part → Thickness.
In the dialog, set the Thickness value.
Set Mode (Skin) and Join type (Arc, Intersection, or Tangent).
Click OK.

Parameters¶

Parameter	Type	Default	Description
Faces	Face list	—	Faces to remove (openings)
Value	Distance	1 mm	Wall thickness
Mode	Skin / Pipe / RectoVerso	Skin	How the offset is constructed
Join	Arc / Intersection / Tangent	Arc	How corners are treated
Make Solid	Bool	Yes	Create a closed solid (not a shell)
Reversed	Bool	No	Offset outward instead of inward
Intersection	Bool	No	Handle self-intersections

Python API¶

import FreeCAD as App
import Part

doc = App.newDocument()

box = doc.addObject("Part::Box", "Box")
box.Length = 30; box.Width = 20; box.Height = 20
doc.recompute()

# Hollow the box with 2 mm walls, top face open
# Top face of the box is Faces[5] (index 5 for the default box)
opening_face = box.Shape.Faces[5]

thick = doc.addObject("Part::Thickness", "Shell")
thick.Faces  = [(box, ["Face6"])]  # FreeCAD uses 1-based face names: Face6 = Faces[5]
thick.Value  = 2.0                  # mm wall thickness
thick.Mode   = "Skin"
thick.Join   = 0                    # 0=Arc, 1=Intersection, 2=Tangent
doc.recompute()

print(f"Shell volume: {thick.Shape.Volume:.2f} mm³")

Note: Face selection in Thickness uses the FreeCAD face name string (e.g., "Face6") rather than the Python list index. Use the viewport selection to pick faces interactively.

Common mistakes and pitfalls¶

Thickness larger than smallest feature

If the specified thickness is larger than the smallest feature of the solid, OCCT produces an error or self-intersecting geometry. Ensure wall thickness is less than half the smallest dimension.

Must select at least one opening face

Without selecting an opening face, Thickness tries to offset all faces inward equally, producing an OCCT error for a closed solid (the result would be a solid inside a solid with zero-thickness walls). Always select the faces to open.