Skip to content

External Geometry (Projection / Intersection / Carbon Copy)

In one sentence: Bring geometry from outside the current sketch into the sketch plane as construction references — either projected onto the plane (Projection), intersected with the plane (Intersection), or copied wholesale from another sketch (Carbon Copy).

Overview

Workbench: Sketcher · Menu: Sketch → Sketcher geometries → External Geometry
Toolbar: Sketcher Geometries (External dropdown) · Shortcut: G, X (Projection) · G, W (Carbon Copy)

Tool Shortcut Description
Projection G, X Project a 3-D edge onto the sketch plane as a construction edge
Intersection — Find where a 3-D face or solid intersects the sketch plane
Carbon Copy G, W Copy all geometry and constraints from another sketch into this one

External geometry appears as purple (or yellow, depending on theme) dashed construction edges. It cannot be modified inside the sketch but acts as a constraint reference: you can snap to it, make geometry coincident with it, or use it to drive dimensional constraints.

Intuition

Projection

Think of shining a light perpendicular to the sketch plane: the shadow of a 3-D edge on the plane is the projected edge. Projection is how you say "this sketch element must align with that 3-D feature" — for example, a hole profile that must be centred on an existing boss, or a pocket outline that must align with an edge of the solid below.

Intersection

Instead of projecting onto the plane, Intersection finds where the sketch plane actually cuts through the solid — like a cross-section slice. This produces the exact boundary geometry of the solid at the sketch plane's position.

Carbon Copy

Carbon Copy is a full sketch import: all geometry and constraints from the source sketch appear inside the current sketch as editable elements. Unlike Projection, the result is regular geometry (not purple construction edges) that can be extended and constrained independently.

When to use them

  • Projection: You need a hole on a pad's top face that aligns with a circular edge on a lower face — project the lower circle, then make your new circle coincident with the projected centre.
  • Projection: You want to sketch a pocket that stops at a rib — project the rib's top edge as a reference line.
  • Intersection: You are sketching on a cross-section plane and need the exact solid boundary at that level.
  • Carbon Copy: You want to reuse the profile of one sketch (e.g. a complex gasket outline) in a second sketch for a matching feature.

When NOT to use them

  • Don't rely on external geometry as the actual profile edges — they are construction references. The profile you hand to Part Design must be drawn using Sketcher tools (lines, arcs, etc.), not the purple external edges.
  • Don't use Carbon Copy when you want a parametric link — Carbon Copy produces an independent copy; changes to the source sketch do not propagate. Use a ShapeBinder if you need a live parametric link.
  • You need to offset an entire 3-D surface outward or inward — use the Part Offset 3D Surface operation instead; External Geometry only brings references into a sketch, it does not reshape 3-D surfaces.

Step-by-step walkthrough

Projection

  1. Open a sketch attached to a face of an existing solid.
  2. Press G, X or activate Projection from the External dropdown.
  3. Click a 3-D edge in the viewport (an edge of the solid, an existing circle, a datum line, etc.). The edge projects onto the sketch plane as a dashed purple construction edge.
  4. Use the projected edge as a constraint reference: apply Coincident between a sketch vertex and a point on the projection, or Point on Object to force a sketch edge to touch it.
  5. Press Esc to exit Projection mode.

Intersection

  1. Open a sketch.
  2. Activate Intersection from the External dropdown.
  3. Click a face or solid body. FreeCAD computes where the sketch plane slices through the selected geometry and draws the intersection as a purple construction edge.
  4. Use the intersection as a reference for constraints.

Carbon Copy

  1. Open a sketch.
  2. Press G, W or activate Carbon Copy from the External dropdown.
  3. Click another sketch in the Model tree or viewport. All its geometry and constraints are copied into the current sketch as regular (non-purple) elements.
  4. The copied geometry has its own independent DoF and can be constrained freely.

Tip

Carbon Copy is particularly useful for producing two matching sketches (e.g. top and bottom profiles for a Loft) that share the same shape. Draw one, then Carbon Copy it into the second sketch on a different plane.

Parameters

Projection / Intersection

Parameter Type Description
Selected edge / face 3-D geometry reference What to project or intersect. A parametric link is maintained — if the 3-D geometry moves, the projection updates.

Carbon Copy

Parameter Type Description
Source sketch Sketch object The sketch whose geometry is copied. No live link is maintained after the copy.

External geometry in depth

Projection vs Intersection — choosing the right one

The key difference is the relationship between the sketch plane and the selected geometry:

Projection

The 3-D edge is not necessarily in the sketch plane. FreeCAD drops a perpendicular from each point of the 3-D edge onto the sketch plane and connects the resulting 2-D points.

Use Projection when: - You want to align a sketch feature with an edge that is below, above, or angled relative to the sketch. - You need the 2-D "shadow" of a 3-D curve.

Watch out for: Projected edges of curved 3-D paths (helices, swept edges) may produce distorted 2-D shapes that are hard to work with as constraint references.

Intersection

The sketch plane cuts through the selected face or solid. The result is the exact cross-sectional boundary at that level.

Use Intersection when: - The sketch plane passes through the solid and you need its exact cross-section boundary. - You are creating a sketch that will cut a pocket into an existing body and the pocket must follow the exact boundary of the solid at that level.

Watch out for: If the sketch plane does not intersect the selected geometry at all, Intersection produces nothing. Check that the sketch plane actually passes through the face or body.

Advanced usage

Toggling projection mode

Starting in FreeCAD 1.0, Projection and Intersection are separate menu/toolbar entries. In earlier versions a single "External Geometry" tool was used for both.

Detaching external geometry

External geometry creates a parametric reference: if the referenced 3-D edge moves (because a Pad height changed), the purple projection updates automatically. This is usually desirable. To break the link (convert to a static snapshot), select the external edge in the sketch and change it to a regular geometry element.

Common mistakes and pitfalls

Sketch becomes invalid when the referenced edge disappears

Cause: An external geometry reference points to a face or edge that was removed by a topology change (renamed face after a fillet was added).
Fix: Select the broken external edge (shown in red), delete it, and re-add the projection pointing to the correct new edge. This is the well-known "topological naming problem" — Part Design's ShapeBinder is more robust for long-term references.

Carbon Copy produces conflicting constraints

Cause: The copied sketch had constraints fixing elements to its own local origin; in the new sketch those constraints now conflict with other geometry.
Fix: After Carbon Copy, open the sketch and remove or reapply the origin constraints to suit the new context.

Projected edge appears but cannot be selected for Coincident

Cause: The external edge is a closed curve (circle, ellipse) and Coincident requires a specific vertex, but the tool is picking the edge body rather than a point on it.
Fix: Use Point on Object to constrain a sketch vertex to lie on the projected circle/arc, rather than Coincident.

Python API

Projection

import FreeCAD as App

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

# Project Face1 / Edge1 of a Pad onto the sketch
sketch.addExternal("Pad", "Edge1")
doc.recompute()

# The projected edge appears at a negative GeoId (e.g. -3)
# Use it in constraints: sketch.addConstraint(Sketcher.Constraint("Coincident", 0, 1, -3, 1))

Carbon Copy

# Carbon Copy is a GUI command; equivalent Python would be:
import FreeCAD as App
import Part

source = doc.getObject("SketchSource")
target = doc.getObject("SketchTarget")

for geo in source.Geometry:
    target.addGeometry(geo.copy(), False)

doc.recompute()
# Note: constraints are NOT copied by this approach; use the GUI command.

See also