Perpendicular Constraint¶

In one sentence: Force two lines (or a line and a curve) to meet at exactly 90°, removing one rotational degree of freedom from the pair.

Overview¶

Workbench: Sketcher · Menu: Sketch → Sketcher constraints → Perpendicular Constraint
Toolbar: Sketcher Constraints · Shortcut: N

Perpendicular removes 1 DoF — the relative angle between the two elements — and fixes it at 90°. It does not require the two elements to actually intersect; it only constrains their directions to be orthogonal.

Intuition¶

Think of a draughtsman's set square: one arm always points exactly 90° from the other, regardless of which way you rotate the square. Perpendicular is that 90° relationship, permanently encoded as a constraint.

When to use it¶

You need a right-angle corner that is not produced by the Rectangle tool (e.g. an L-shaped profile drawn as a polyline).
A line should meet a circle's radius (line through centre perpendicular to tangent).
Two datum axes in a construction layout must be orthogonal.
A construction line should be perpendicular to an edge for use as a normal or offset reference.

When NOT to use it¶

You need a right-angle and an intersection — Perpendicular alone does not make lines meet; also add Coincident at the desired meeting point.
You used Rectangle — Rectangle already applies right-angle constraints at all four corners; do not add extra Perpendicular constraints.

Step-by-step walkthrough¶

Select two lines (or a line and an arc/circle).
Press N or activate Sketch → Perpendicular Constraint.
The selected elements rotate to be perpendicular. The constraint icon appears at the intersection or between the elements.

Tip

When applied to a line and a circle, Perpendicular forces the line to be tangent (perpendicular to the radius at the tangent point). Combined with Tangent, this gives you precise tangent-line constructions.

Parameters¶

No numeric parameters. Removes 1 DoF.

Common mistakes and pitfalls¶

Lines do not intersect despite being perpendicular

Cause: Perpendicular only constrains the angle, not the position. Two lines at 90° can still be anywhere relative to each other.
Fix: Add a Coincident constraint or Point on Object to make them actually meet.

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, 0, 0)), False)
line1 = sketch.addGeometry(
    Part.LineSegment(App.Vector(0, 0, 0), App.Vector(0, 20, 0)), False)

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