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Validate Sketch

In one sentence: Scan an existing sketch for missing coincident constraints, degenerate geometry, and solver errors, then let you fix them interactively.

Overview

Workbench: Sketcher · Menu: Sketch → Validate Sketch
Toolbar: Sketcher · Shortcut: none

Validate Sketch opens a diagnostic task panel that analyses a sketch for common problems: vertices that are geometrically coincident but lack a coincident constraint, extremely short edges that cause solver instability, and constraints that are flagged as degenerate. For each category of problem it offers a one-click fix.

Intuition

Think of Validate Sketch as a spell-checker for your sketch. It cannot re-draw bad geometry, but it can spot the silent errors that cause a sketch to refuse to close or produce corrupted solids downstream — specifically the case where two line endpoints look joined but are actually two separate points sitting on top of each other (a "false vertex gap").

This tool is most useful when you import geometry via DXF or IGES, or after Carbon Copy / External Geometry operations, because those paths often produce coincident-looking vertices that are not formally connected.

When to use it

  • A sketch imported from a DXF file reports that it is not closed or cannot be used as a profile, even though it looks perfectly closed in the viewport.
  • After using Carbon Copy, some vertices appear to share a point but the sketch has more DoF than expected.
  • You receive a sketch from someone else and want to audit it for constraint health.
  • The solver shows conflicts or redundancies that you cannot find manually.

When NOT to use it

  • Your sketch has genuine unconstrained degrees of freedom — Validate Sketch will not add missing dimensional constraints; you must add those yourself.
  • You want to fix topologically broken geometry (e.g. self-intersecting edges) — Validate Sketch cannot repair those; you must edit the geometry manually.

Step-by-step walkthrough

  1. Close sketch edit mode if you are currently inside the sketch (click Close in the Tasks panel or choose Sketch → Leave Sketch).

  2. Select the sketch in the Model tree (single click).

  3. Activate Validate Sketch via Sketch → Validate Sketch. The Validate Sketch task panel opens.

  4. Click "Analyse" to scan the sketch. The panel reports:

    • Missing coincident constraints — pairs of vertices within a tolerance that are not formally constrained to be coincident.
    • Degenerate constraints — constraints that reference non-existent geometry (usually a leftover after deleting a geometry element).

  5. Review each category and click the corresponding "Fix" button to automatically add the required constraints or delete the degenerate entries.

  6. Adjust the tolerance (default 0.1 mm) if needed — larger tolerance catches more misaligned vertices; smaller tolerance ignores near-coincident vertices that are intentionally close but not connected.

  7. Click OK to close the panel.

Tip

After running Validate Sketch, check the solver status again. If the DoF count dropped toward zero, the missing constraints were the root cause of the under-constrained sketch.

Parameters

Parameter Type Default Description
Tolerance Float (mm) 0.1 Maximum distance between two vertices for them to be considered "missing coincident". Increase if DXF geometry has small gaps.

Common mistakes and pitfalls

Validate Sketch does not enter edit mode

Cause: You must close sketch edit mode before running Validate Sketch — the tool analyses the sketch from outside.
Fix: Leave sketch edit mode (click Close / Leave Sketch), then run Validate Sketch.

False positives with intentional near-coincident vertices

Cause: A sketch that has two intentionally separate vertices very close together (e.g. a very short line) can be flagged as missing a coincident constraint.
Fix: Lower the tolerance before clicking Analyse so that only genuine gaps are detected. Alternatively, review each flagged pair before applying the fix.

Python API

There is no direct Python API for running Validate Sketch programmatically. The underlying constraint-adding logic uses addConstraint:

import FreeCAD as App
import Sketcher

doc = App.activeDocument()
sketch = doc.getObject("Sketch")

# Manually add a coincident constraint between point 0 of geo 0
# and point 0 of geo 1 (equivalent to what Validate Sketch would add)
sketch.addConstraint(Sketcher.Constraint("Coincident", 0, 1, 1, 1))
doc.recompute()

See also