Revolve¶

In one sentence: Spin a 2-D profile around an axis to create a solid of revolution — the Part workbench equivalent of a lathe operation.

Overview¶

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

Revolve takes a profile (face, wire, or edge) and sweeps it around a defined axis by a specified angle. A full 360° sweep produces a closed solid of revolution; a partial sweep produces a sector.

Intuition¶

A lathe creates solids of revolution by spinning a profile around the spindle axis. Part Revolve is the digital equivalent: define the profile on one side of the axis, revolve it, and FreeCAD produces the rotational solid.

Common shapes created with Revolve: - Turned shafts and bushings — revolve an L-shaped profile around the shaft centreline. - Bowls and vases — revolve an open curve. - Flanges — revolve a rectangular profile with an offset from the axis. - Partial sectors — revolve < 360° for a segment.

When to use it¶

Any axially symmetric part: shaft, bushing, flange, bottle, bowl.
Creating a partial solid of revolution (sector, half-revolution).

When NOT to use it¶

Profile crosses the axis — OCCT may produce self-intersecting geometry. Keep the profile entirely on one side of the axis.
Inside a Part Design Body — use Revolution (Part Design).

Step-by-step walkthrough¶

Create the profile — a Sketcher sketch or a wire on one side of the intended rotation axis.
Select the profile.
Part → Revolve.
In the dialog:
Set Axis (default: Y axis).
Set Angle (360° for full revolution).
Check Create Solid.
Click OK.

Parameters¶

Parameter	Type	Default	Description
Axis	Vector	Y axis (0,1,0)	Direction of the revolution axis (passes through Placement origin)
Angle	Angle	360°	Angular sweep
Create Solid	Bool	Yes	Solid vs surface
Symmetric	Bool	No	Revolve ±Angle/2 symmetrically

Python API¶

import FreeCAD as App
import Part

doc = App.newDocument()

# L-shaped profile for a shaft shoulder
# (points defining the cross-section on the XZ plane, rotated around Z)
import math

profile_points = [
    App.Vector(5, 0, 0),   # inner bottom
    App.Vector(10, 0, 0),  # outer bottom
    App.Vector(10, 0, 20), # outer top
    App.Vector(7, 0, 20),  # shoulder step
    App.Vector(7, 0, 30),  # top
    App.Vector(5, 0, 30),  # inner top
    App.Vector(5, 0, 0),   # back to start
]
edges = [Part.makeLine(profile_points[i], profile_points[i+1])
         for i in range(len(profile_points)-1)]
wire = Part.Wire(edges)
face = Part.Face(wire)

# Revolve around Z axis
axis = App.Vector(0, 0, 1)
solid = face.revolve(App.Vector(0, 0, 0), axis, 360)  # full revolution

feat = doc.addObject("Part::Feature", "Shaft")
feat.Shape = solid
doc.recompute()
print(f"Volume: {feat.Shape.Volume:.2f} mm³")

Common mistakes and pitfalls¶

Profile must not cross the rotation axis

If the profile crosses the axis, OCCT produces self-intersecting geometry that is invalid for further operations. Keep the entire profile on one side.

Axis direction vs. axis position

The revolution axis passes through the Placement origin of the profile object in the direction specified. Ensure the profile is positioned correctly relative to that axis.