Skip to content

Parallel Constraint

In one sentence: Force two lines to be parallel — to run in the same direction at any angle, without specifying what that angle is.

Overview

Workbench: Sketcher · Menu: Sketch → Sketcher constraints → Parallel Constraint
Toolbar: Sketcher Constraints · Shortcut: P

Parallel removes 1 degree of freedom: the relative angle between the two lines. After applying it, the two lines will always have the same orientation; you can then set the shared angle with a single Angle constraint applied to either line.

Intuition

Think of railway tracks: both rails run in the same direction, always the same distance apart. Parallel is the constraint version of "these two things go the same way" — wherever you point one, the other follows the same bearing.

When to use it

  • You have two edges that should remain parallel while other dimensions change (e.g. the two sides of a channel).
  • You want to force a line to be parallel to a reference edge such as an external geometry projection.
  • You are building a parallelogram or trapezoid outline.

When NOT to use it

  • Both lines should be horizontal or vertical — use Horizontal/Vertical on each line separately; two horizontal lines are automatically parallel.
  • The lines must be parallel AND a specific distance apart — add a Distance constraint between them after Parallel.

Step-by-step walkthrough

  1. Select two lines — click the first, then Ctrl-click the second.
  2. Press P or activate Sketch → Parallel Constraint.
  3. The lines rotate to be parallel. One of them will stay fixed; the other adjusts to match its angle.
  4. Add an angle constraint to either line to fix the shared orientation if needed.

Parameters

No numeric parameters. Removes 1 DoF.

Common mistakes and pitfalls

Two fully constrained lines cannot be made parallel

Cause: Both lines already have all their DoF consumed by existing constraints, so adding Parallel is redundant.
Fix: If the parallelism is implied by the existing constraints, no action is needed. If the constraint is genuinely needed, remove one angle-related constraint first.

Python API

Minimal example

import FreeCAD as App
import Sketcher
import Part

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

line0 = sketch.addGeometry(
    Part.LineSegment(App.Vector(0, 0, 0), App.Vector(20, 5, 0)), False)
line1 = sketch.addGeometry(
    Part.LineSegment(App.Vector(0, 10, 0), App.Vector(20, 15, 0)), False)

sketch.addConstraint(Sketcher.Constraint("Parallel", line0, line1))
doc.recompute()

See also