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Trim / Split / Extend

In one sentence: Modify existing sketch edges by removing the portion beyond an intersection (Trim), cutting an edge into two at a point (Split), or lengthening an edge until it meets another edge (Extend).

Overview

Workbench: Sketcher · Menu: Sketch → Sketcher geometries → Trim / Split / Extend
Toolbar: Sketcher Geometries (Curve Edition dropdown) · Shortcut: G, T (Trim) · G, Z (Split) · G, Q (Extend)

Tool Shortcut Description
Trim G, T Remove the segment of an edge on one side of an intersection
Split G, Z Cut an edge into two separate edges at a clicked point
Extend G, Q Lengthen a line or arc until it meets a target edge

Intuition

Trim is the sketcher equivalent of an eraser that only removes the piece you don't want: click on the part of a line or arc that extends past an intersection, and that excess is deleted while the rest stays.

Split is like scoring a piece of card with a knife: the edge stays in place but is now two independent edges that can be constrained separately.

Extend is the opposite of Trim: click on the end of a line or arc and FreeCAD projects it forward until it hits the next available edge, then stops.

When to use them

  • Trim: You have drawn a grid of lines to create a lattice, and you want to remove the interior crossing segments to leave only the outer frame.
  • Split: You want different constraint values on two halves of a single line (e.g. a line that runs through a Boss centre — split it so you can constrain each half's length independently).
  • Extend: You drew a line that falls short of the enclosing rectangle and want it to meet the boundary without knowing the exact endpoint coordinate.

When NOT to use them

  • Don't use Trim when you just want to shorten a line — adjust the endpoint position with a constraint or drag the endpoint; Trim removes geometry structurally.
  • Don't use Split when the result should be one continuous edge — the split creates two separate objects that need a Coincident constraint to stay joined.
  • Don't use Extend if the target edge is not visible — Extend only reaches edges that are present in the sketch; it cannot extend to external geometry.

Step-by-step walkthrough

Trim

  1. Press G, T or select Trim from the Curve Edition dropdown.
  2. Click the segment you want to remove. The portion of the edge on the clicked side of the nearest intersection is deleted. Both the trimmed edge and the intersecting edge remain; only the unwanted segment disappears.
  3. Repeat for other segments to trim. Press Esc to exit.

Tip

Trim uses the clicked location to determine which segment to remove — click close to the end you want gone, not near the intersection.

Split

  1. Press G, Z or select Split.
  2. Click the point on an edge where you want to cut it. A new vertex appears at that location, and the original edge becomes two edges sharing that vertex (connected by an automatic Coincident constraint).
  3. You can now apply different constraints to each half independently.

Extend

  1. Press G, Q or select Extend.
  2. Click the endpoint of the edge you want to extend (the end that should grow). The cursor shows a preview extending toward the nearest intersecting edge.
  3. Click again (or just hover — the tool may auto-extend) to confirm. The edge grows until it meets the target.

Extend changes the endpoint position

Extending a line changes its endpoint coordinates. If the endpoint was previously constrained (e.g. by a coincident constraint to another vertex), the extension will conflict. Remove the conflicting constraint first.

Parameters

All three tools are interactive-only with no numeric parameters beyond the click position. After running them, apply constraints as normal.

Common mistakes and pitfalls

Trim removes the wrong segment

Cause: You clicked close to an intersection, and the tool picked the adjacent segment instead of the intended one.
Fix: Press Ctrl+Z to undo, then click more clearly on the target segment, farther from the intersection point.

Split leaves the sketch with more DoF than expected

Cause: Split creates two edges with a shared vertex, but any constraints on the original edge's midpoint are not automatically redistributed to the new structure.
Fix: After splitting, check the DoF counter and add any needed constraints to the new intermediate vertex.

Extend does not reach the target

Cause: The target edge is a construction element (dashed) or an external geometry projection, and Extend may not recognize it as a valid endpoint.
Fix: Convert the target to a regular edge, or manually extend by dragging the endpoint and adding a Coincident constraint.

Python API

Trim

import FreeCAD as App
import Sketcher

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

# Trim geo index 2 at the point closest to (15, 0)
sketch.trim(2, App.Vector(15, 0, 0))
doc.recompute()

Split

# Split geo index 1 at parameter value 0.5 (midpoint)
sketch.split(1, App.Vector(5, 5, 0))  # point on the edge
doc.recompute()

Extend

# Extend the endpoint (vertex 2) of geo 0 toward geo 1
sketch.extend(0, 0.5, 2)  # geoId, parameter, endPoint (1=start, 2=end)
doc.recompute()

See also