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Defeaturing

In one sentence: Remove selected faces from a solid (and attempt to heal the resulting holes) to simplify the shape for FEA, CFD, or export.

Overview

Workbench: Part · Menu: Part → Defeaturing
Toolbar: Part Analysis · Shortcut: none

Defeaturing removes selected faces from a solid shape and attempts to extend or patch the adjacent faces to close the resulting holes. The goal is to simplify geometry — removing fillets, chamfers, small holes, logos, or other fine features that are irrelevant for the intended downstream operation (such as FEA meshing or CFD simulation).

Intuition

A part from a CAD library often has hundreds of fillets, text engravings, and fine features. Loading this directly into an FEA solver produces millions of mesh elements for details that have negligible structural influence. Defeaturing strips those features away, leaving a simplified shape that meshes efficiently.

It is the digital equivalent of filing down a fillet on a physical test specimen: the core geometry remains, the fine feature is gone.

When to use it

  • Simplifying imported STEP parts for FEA or CFD analysis.
  • Removing fillets and chamfers from a model to check the "sharp-edged" base geometry.
  • Removing decorative features (text, logos, fine cosmetic features) that inflate file size and mesh complexity.

When NOT to use it

  • Structural features — never defeature loadbearing fillets or stress- concentration-reducing rounds before a structural analysis. They exist precisely because the stress field depends on them.
  • Features you plan to re-add parametrically — defeature only for one-way simplification workflows (analysis, export). The defeatured shape is static.

Step-by-step walkthrough

  1. Select the solid in the model tree.
  2. In the viewport, Ctrl+click the faces to remove (e.g., a fillet face, a small hole's cylindrical face).
  3. Part → Defeaturing.
  4. FreeCAD attempts to heal the surface after removing the selected faces.
  5. Check the result with Check Geometry.

Common pitfalls

Defeaturing may fail on complex feature removal

OCCT's face removal algorithm cannot always heal the gap left by a removed face. If the adjacent faces cannot be extended to close the hole, Defeaturing reports a failure. Try selecting fewer faces or a simpler feature.

Result is a static shape

The defeatured shape is not parametric. Changes to the original solid do not propagate. Defeature as the last step before export or meshing, not as part of the live model.

Python API

import FreeCAD as App
import Part

doc = App.newDocument()

# Create a filleted box (has fillet faces to defeature)
box = doc.addObject("Part::Box", "Box")
box.Length = 30; box.Width = 20; box.Height = 15
doc.recompute()

fillet = doc.addObject("Part::Fillet", "Filleted")
fillet.Base = box
fillet.Edges = [(i, 2.0, 2.0) for i in range(1, 13)]
doc.recompute()

# Defeaturing: remove a fillet face (use interactively to pick the face)
# Programmatic approach (OCCT RemoveFeature):
defeat = doc.addObject("Part::Defeaturing", "Simplified")
defeat.Source = fillet
# defeat.FacesToRemove = [fillet.Shape.Faces[12]]  # select fillet face by index
# doc.recompute()
print("Use Part → Defeaturing interactively to select faces to remove.")

See also