Extrude¶

In one sentence: Push a face, wire, or edge along a direction (or along a custom axis) to create a solid, shell, or surface.

Overview¶

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

Extrude takes a 2-D profile (a closed wire, face, or edge) and sweeps it linearly along a direction, producing a 3-D solid or shell. It supports symmetric extrusion, taper angles, multiple sub-shapes at once, and custom extrusion directions.

Intuition¶

Extrusion is the simplest way to turn a flat 2-D sketch into a 3-D object: draw a rectangle, extrude it 10 mm, and you have a box. Draw an I-section, extrude it 500 mm, and you have a steel beam.

The Part Extrude tool is more flexible than Part Design's Pad: it works on any face or wire without requiring a Body, and it accepts custom axes, taper angles, and solid/shell mode.

When to use it¶

You have a Sketcher sketch outside a Body and want a solid from it.
You need to extrude with a taper angle (draft angle).
You need to extrude to a symmetric depth (equal both sides).
You want a surface (shell) rather than a solid.

When NOT to use it¶

Inside a Part Design Body — use Pad.
Non-linear sweep — use Sweep for curved paths.

Step-by-step walkthrough¶

Select the profile — a face, closed wire, or sketch.
Part → Extrude.
In the dialog:
Set Direction (default: sketch normal or Z axis).
Set Length Along (positive direction depth).
Optionally set Length Against for symmetric or asymmetric extrusion.
Set Taper Angle if you need draft.
Check Create Solid for a solid (default) or uncheck for a shell.
Click OK.

Parameters¶

Parameter	Type	Default	Description
Direction	Vector	Normal of profile	Extrusion direction
Length Along	Distance	10 mm	Depth in the positive direction
Length Against	Distance	0 mm	Depth in the negative direction (symmetric or asymmetric)
Taper Angle	Angle	0°	Draft angle applied to the lateral faces
Inner Taper Angle	Angle	0°	Draft angle for inner profiles (holes)
Create Solid	Bool	Yes	Solid (closed ends) vs shell (open ends)
Symmetric	Bool	No	Extrude equally in both directions (ignores "Against" length)

Deep dive: taper angles¶

A taper angle (also called draft angle in moulding) causes the extrusion to widen or narrow as it extends. Positive taper widens the profile; negative taper narrows it. For injection moulded parts, a typical draft is 1°–3°.

Note: If the taper is large enough that the profile would reduce to a point before reaching the full length, OCCT will truncate the solid at that point.

Python API¶

import FreeCAD as App
import Part

doc = App.newDocument()

# Create a hexagonal wire to extrude
import math
n = 6  # hexagon
r = 10.0  # circumradius
points = []
for i in range(n):
    angle = 2 * math.pi * i / n
    points.append(App.Vector(r * math.cos(angle), r * math.sin(angle), 0))
points.append(points[0])  # close

edges = [Part.makeLine(points[i], points[i+1]) for i in range(n)]
wire = Part.Wire(edges)
face = Part.Face(wire)

# Extrude 20 mm along Z
solid = face.extrude(App.Vector(0, 0, 20))
feat = doc.addObject("Part::Feature", "HexPrism")
feat.Shape = solid
doc.recompute()

# Using the parametric Extrude object:
import PartGui  # noqa — ensures Part commands are registered
sketch = doc.addObject("Sketcher::SketchObject", "Sketch")
# (add sketch geometry here)

ext = doc.addObject("Part::Extrusion", "Extruded")
ext.Base = sketch
ext.Dir = App.Vector(0, 0, 1)
ext.LengthFwd = 15.0
ext.LengthRev = 0.0
ext.Solid = True
ext.TaperAngle = 2.0  # degrees
doc.recompute()

Common mistakes and pitfalls¶

Extruding an open wire produces a shell, not a solid

If the profile wire is not closed, even with Create Solid checked, the result is a surface/shell. Close the wire first or use Face from Wires to create a closed face.

Extrusion direction default may be unexpected

For a non-horizontal sketch, the default direction (profile normal) may not be the world Z axis. Check the Direction vector in the dialog.