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Check Geometry

In one sentence: Analyse a Part shape for OCCT validity errors — finding open shells, invalid edges, self-intersections, and other topology problems that would cause downstream failures.

Overview

Workbench: Part · Menu: Part → Check Geometry
Toolbar: Part Analysis · Shortcut: none

Check Geometry runs OCCT's built-in shape analysis tools on the selected shape and reports any validity issues. It distinguishes between errors (will cause failures) and warnings (may cause problems in some operations).

Intuition

OCCT requires shapes to satisfy strict topological rules: edges must be shared by exactly two faces, vertices must be at the ends of edges, shells must be closed if they represent a solid, and so on. Violations of these rules are called invalid geometry and cause failures in Boolean operations, meshing, export, and analysis.

Check Geometry is the diagnostic tool: run it after every import and after complex Boolean operations to ensure the shape is healthy before continuing. Fixing errors early is far cheaper than debugging failures three operations later.

When to use it

  • After importing STEP/IGES/STL — imported files frequently contain small gaps, degenerate edges, or other issues.
  • After Boolean Fragments or Slice — complex multi-shape Boolean operations can occasionally produce invalid topology.
  • After Shape from Mesh — mesh-to-shell conversion often introduces degenerate edges.
  • Before FEA meshing — invalid shapes cause meshing failures.
  • Before export — STEP export of invalid shapes produces files that other CAD tools reject.

Understanding the results

The Check Geometry panel shows a tree of shape elements. Each element is marked as:

Indicator Meaning
Green / no issue Valid
BOPAlgo_InvalidCurveOnSurface An edge curve does not lie on its adjacent face surface
Bad edge An edge has invalid curve parameterisation
Invalid tolerance An entity's tolerance is outside acceptable bounds
Self-intersection A face or edge intersects itself
Open shell A shell has boundary edges (is not watertight)

Step-by-step walkthrough

  1. Select the shape in the model tree.
  2. Part → Check Geometry.
  3. The Check Geometry panel opens at the bottom.
  4. Click Run Check (or it runs automatically).
  5. Expand the tree to see which sub-elements (faces, edges, vertices) have issues.
  6. Look up the error type and decide on a repair strategy:
  7. Open shell → find and fill the gap, or use Convert to Solid after closing the boundary.
  8. Invalid curve → the shape needs repair; use Defeaturing or re-import with different settings.
  9. Self-intersection → simplify the geometry causing the intersection.

Interpreting "shape is valid" vs "BOP check"

Check Geometry runs two tiers of checks:

  1. OCCT shape validity — basic topology rules. If this fails, the shape will not work in any operation.
  2. BOP (Boolean Operation) check — stricter requirements needed for Boolean operations. A shape can pass tier 1 but fail tier 2.

The "Run BOP check" option enables the stricter tier-2 check. Always enable it before running Boolean operations.

Python API

import FreeCAD as App
import Part

doc = App.newDocument()

box = doc.addObject("Part::Box", "Box")
doc.recompute()

# Check validity
shape = box.Shape
is_valid = shape.isValid()
print(f"Shape is valid: {is_valid}")

# Detailed check via Part.BRepCheck
# TODO: verify API — BOPTools may be needed for full BOP check
analyzer = Part.BRepCheck.Analyzer(shape)
analyzer.Init(shape)
is_ok = not analyzer.IsValid()
print(f"BRepCheck passed: {not is_ok}")

# Simpler validity check
import BOPTools.BOPFeatures as BF
# Use Check Geometry tool interactively for comprehensive results
print("Run Part → Check Geometry from the menu for a full report.")

Common mistakes and pitfalls

Valid shape ≠ manifold solid

A shape can pass the basic validity check but still not be a closed (manifold) solid. Always look at the specific topology type — ShapeType == 'Solid' and shape.isClosed() for solids.

Suppressed warnings can still cause failures

Some issues flagged as warnings (not errors) in Check Geometry can still cause Boolean operation failures. Treat all issues as potential problems.

See also