freecad-sketcher

name: freecad-sketcher description: Use this skill for parametric 2D/3D technical drawings using FreeCAD Sketcher and TechDraw. Triggers when the user wants constrained parametric floor plans, mechanical sketches, layout diagrams, or any drawing where dimensions drive geometry. Also use when the user mentions FreeCAD, .FCStd files, Sketcher, TechDraw, parametric CAD, or technical drawings. Use this skill even for seemingly simple 2D layouts — the parametric constraint approach prevents coordinate drift and makes edits safe. Always read this skill before writing any FreeCAD scripting code.

FreeCAD Sketcher + TechDraw Skill

Philosophy

The FCStd is the artifact; images are derived previews. Work iteratively: open, edit, save, export, visually check, repeat. Every dimension is a constraint.

Parametric-first: Spreadsheet parameters are the single source of truth (SSOT). All sketch constraints must be bound to spreadsheet cells via setExpression(). All TechDraw dimensions must reference projected entities (References2D) so they auto-update when parameters change. Never use hardcoded coordinates, one-shot Python variables, or point-based makeDistanceDim.

Critical Pitfalls

These are the most common silent failures. Read before writing any code:

• setExpression, not direct assignment. fillet.Radius = float(...) stores a scalar — the FCStd has no link back to the spreadsheet. Use fillet.setExpression("Radius", "Params.X").
• Never use makeDistanceDim. It creates non-parametric point-based dimensions. Always use DrawViewDimension with References2D = [(view, "EdgeN")].
• TechDraw HLR requires Xvfb. QT_QPA_PLATFORM=offscreen does NOT provide the OpenGL context the HLR thread needs. Use xvfb-run -a or a manual Xvfb :99 display.
• TechDraw HLR is async. After doc.recompute(), call wait_for_view() — it polls getVisibleEdges() with processEvents(). A bare time.sleep() will never deliver the Qt signal and getVisibleEdges() will stay empty forever.
• Never hardcode face/edge indices. "Face6" or "Edge3" shift when the model changes. Always find faces/edges by geometric properties (CenterOfMass.z, Radius, Area, vertex positions).
• Tangent with point refs implies coincidence. Tangent(line, 2, arc, 1) means the endpoints are already joined — adding a separate Coincident at the same points over-constrains the sketch.
• Single compound → single TechDraw view. Multiple Part::Feature objects lose their relative positions (each view centers its own bounding box independently).
• Closed faces only in TechDraw. Open wires or loose edges crash the HLR projector with NCollection_Array1::Create.
• Angle expressions need deg unit. sk.setExpression(f"Constraints[{i}]", "Params.Angle * 1 deg") — raw values without * 1 deg are treated as dimensionless, producing wrong angles.
• dim.X/dim.Y must be set. DrawViewDimension defaults to (0, 0) — all dimension text overlaps without explicit placement.

Setup

Target version: FreeCAD 1.1.0. The API surface changed between 0.21 and 1.0 (Topological Naming Protection, PySide6 migration). Pin to 1.1.0 to avoid compatibility surprises.

wget -q "https://github.com/FreeCAD/FreeCAD/releases/download/1.1.0/FreeCAD_1.1.0-Linux-x86_64-py311.AppImage" -O /opt/FreeCAD.AppImage
chmod +x /opt/FreeCAD.AppImage
apt-get install -y xvfb          # required for TechDraw HLR
pip install ezdxf[draw] --break-system-packages  # for DXF→PNG rendering

Alternatively: apt-get install -y freecad-python3 xvfb with sys.path.insert(0, '/usr/lib/freecad-python3/lib').

Script Execution Model

For iterative work (exploring geometry, debugging dimensions), use Interactive Mode instead of standalone scripts — see the Interactive Mode section below.

FreeCAD has two binaries with very different lifecycle models:

What needs Xvfb vs offscreen

TechDraw invocation (freecadcmd + xvfb-run):

OUTDIR=/tmp/out xvfb-run -a /opt/FreeCAD.AppImage freecadcmd parametric_sketch.py
INPUT=/tmp/bracket.FCStd OUTDIR=/tmp/out xvfb-run -a /opt/FreeCAD.AppImage freecadcmd export_page.py

Scripts use module-level code, call FreeCADGui.showMainWindow(), and end with os._exit(0) to bypass the Qt6 TLS crash — see <debug/qt_shutdown_segfault.md>.

3D rendering (freecad GUI binary + direct Xvfb): Do NOT use xvfb-run with the freecad binary — it can hang. Start Xvfb manually:

Xvfb :99 -screen 0 1024x768x24 -nolisten tcp &
sleep 1
DISPLAY=:99 INPUT=/tmp/model.FCStd OUTDIR=/tmp/out /opt/FreeCAD.AppImage freecad render_fcstd.py

Headless geometry only (no rendering):

QT_QPA_PLATFORM=offscreen OUTDIR=/tmp/out /opt/FreeCAD.AppImage freecadcmd build_cube.py

Fonts

FreeCAD bundles osifont in <ResourceDir>/Mod/TechDraw/Resources/fonts/. Register it with fontconfig for deterministic TechDraw exports across machines:

ln -sf /opt/squashfs-root/usr/Mod/TechDraw/Resources/fonts /usr/local/share/fonts/techdraw
fc-cache -f

Sketcher

One Sketcher::SketchObject holds all geometry and constraints. For parametric designs, use a Spreadsheet::Sheet to drive constraint values via setExpression(). For simple examples, Python variables as constraints are fine — but they won't survive GUI editing.

@sketcher.md

Part Features

TechDraw projects Part::Feature shapes via HLR. Shape topology rules:

• Part.Face from closed wire: works
• Part.Compound of Faces: works
• Open Part.Wire or loose-edge Compound: crashes with NCollection_Array1::Create

All geometry must be closed faces — model walls as closed polygons tracing inner and outer outlines (shell approach). See <examples/compound/build.py> for an L-shaped wall shell.

Single compound, single view. Put ALL faces in one Part.Compound → one Part::Feature → one TechDraw::DrawViewPart. Multiple features with multiple views lose relative positions because TechDraw centers each view's bounding box independently.

TechDraw

DrawPage + DrawSVGTemplate. Dimensions must reference projected edges via References2D, not hardcoded coordinates. The wait_for_view() pattern (polling getVisibleEdges() with processEvents()) is required after every doc.recompute().

@techdraw.md

Part Design

The Part Design workbench (PartDesign::Body) is the standard approach for solid 3D modeling. Feature tree: Sketch → Pad → Pocket → Fillet/Chamfer. Always use setExpression for all feature properties to keep the FCStd parametric.

@partdesign.md

3D Modeling with Part Primitives

Use Part primitives and boolean operations for simple solid geometry (alternative to Part Design for basic shapes):

import FreeCAD
import Part

cube = Part.makeBox(20, 20, 20, FreeCAD.Vector(-10, -10, -10))
cylinder = Part.makeCylinder(5, 22, FreeCAD.Vector(0, 0, -11), FreeCAD.Vector(0, 0, 1))
result = cube.cut(cylinder)

feat = doc.addObject("Part::Feature", "CubeWithHole")
feat.Shape = result

See <examples/cube_with_hole/build.py> for a complete example.

Visual Debugging

When edge-finding predicates fail or you need to understand TechDraw projection geometry, use the debug renderers.

render_debug_edges.py draws each visible edge with a unique color and labels it with its index, curve type, and dimensions. Run under Xvfb with the freecad binary:

Xvfb :99 -screen 0 1024x768x24 -nolisten tcp & sleep 1
DISPLAY=:99 INPUT=/work/model.FCStd OUTDIR=/output /opt/FreeCAD.AppImage freecad render_debug_edges.py
# Produces: FrontView_debug_edges.png, TopView_debug_edges.png, etc.

render_debug_faces.py colors each face of a Part Design body with a unique color and logs face index, surface type, area, and center-of-mass. Same invocation, produces debug_faces.png.

Workflow: produce FCStd → run debug renderer → inspect output PNGs → identify which Edge/Face to target → write geometric predicate → use find_unique_edge (asserts exactly 1 match) or find_ranked_edge (deterministic ranking among multiple matches).

Export

Example scripts produce FCStd files. Use export_page.py to export to DXF, SVG, and PDF. Arguments are passed via env vars (INPUT, OUTDIR) because the freecad binary treats CLI args as files to open:

Xvfb :99 -screen 0 1024x768x24 -nolisten tcp & sleep 1
DISPLAY=:99 OUTDIR=. /opt/FreeCAD.AppImage freecad parametric_sketch.py   # → bracket.FCStd
DISPLAY=:99 INPUT=bracket.FCStd OUTDIR=. /opt/FreeCAD.AppImage freecad export_page.py  # → bracket.{dxf,svg,pdf}

DXF → PNG: python3 render_dxf.py output.dxf output.png. See <examples/render_dxf.py>.

Gotchas

@gotchas.md

@interactive.md