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Refine Shape

In one sentence: Create a cleaned-up copy of a shape by merging co-planar faces and removing redundant internal edges left by Boolean operations.

Overview

Workbench: Part
Menu: Part → Create a Copy → Refine Shape
Shortcut: none

Creates a new Part::Feature with the same overall geometry as the selected shape, but with redundant internal edges removed and adjacent co-planar faces merged into single faces.

Intuition

When you perform a Boolean Fuse or Cut in FreeCAD, OCCT preserves all the original face boundaries in the result — including seam edges where two faces are now perfectly co-planar (they could be one face, but the history says they were two). Refine Shape merges them, producing cleaner geometry with fewer faces.

Think of it as erasing pencil guide lines after the drawing is done — the shape looks the same, but the unnecessary lines are gone.

This is particularly important before applying Fillet or Chamfer: excess edges on planar regions can cause fillet failures because OCCT tries to apply a fillet to a zero-curvature boundary.

When to use it

  • After Boolean Fuse, Boolean Cut, or Boolean Common operations, to clean up redundant edges on planar regions.
  • Before applying Fillet or Chamfer to a Boolean result.
  • Before export (STEP, STL) when you want a minimal face count.
  • After Shape from Mesh to merge co-planar triangles into single planar faces.

When NOT to use it

  • Don't use it on shapes with intentionally coincident edges — if a face must remain as two separate faces for downstream selection or reference, refining will merge them.
  • Don't use it if you need to reference specific faces by index — after refining, face indices change because faces are merged. Any existing references to the old face indices will become invalid.

Step-by-step

  1. Select the shape to refine (typically a Boolean result).
  2. Choose Part → Create a Copy → Refine Shape.
  3. A new Part::Feature appears with the cleaned topology.
  4. Inspect the result: the number of faces should be less than or equal to the original.

Parameters

This tool has no task panel. The refinement is applied automatically to the selected shape.

Common mistakes and pitfalls

Face count change invalidates downstream references

If any other features (sketches, fillets, other Booleans) reference faces of the original by index, those references may break after refining because face indices change. Create the refined shape before adding downstream references.

Refine Shape does not fix invalid topology

It cleans up co-planar seam edges, but it cannot repair self-intersections, open shells, or non-manifold geometry. Use Check Geometry for diagnosis.

May not merge curved faces

Refine Shape merges co-planar faces and tangentially continuous curved faces. Disjoint curved faces that happen to share a seam edge may not always merge as expected.

Python API

import FreeCAD as App
import Part

doc = App.newDocument()

# Create a Boolean operation that produces redundant edges
box1 = doc.addObject("Part::Box", "Box1")
box1.Length = 20; box1.Width = 10; box1.Height = 10

box2 = doc.addObject("Part::Box", "Box2")
box2.Length = 20; box2.Width = 10; box2.Height = 10
box2.Placement = App.Placement(App.Vector(20, 0, 0), App.Rotation())

fuse = doc.addObject("Part::Fuse", "Fused")
fuse.Base = box1
fuse.Tool = box2
doc.recompute()

print(f"Faces before refine: {len(fuse.Shape.Faces)}")   # more faces with seam edges

# Refine the shape using removeSplitter()
refined_shape = fuse.Shape.removeSplitter()
feat = doc.addObject("Part::Feature", "Refined")
feat.Shape = refined_shape
doc.recompute()

print(f"Faces after refine: {len(feat.Shape.Faces)}")    # fewer, cleaner faces

See also