Skip to content

Toggle Driving Constraint / Toggle Active Constraint

In one sentence: Flip a dimensional constraint between driving (controls geometry) and reference (reads geometry) mode (Toggle Driving), or completely enable or disable a constraint without deleting it (Toggle Active).

Overview

Workbench: Sketcher · Menu: Sketch → Sketcher constraints → Toggle Driving / Toggle Active
Toolbar: Sketcher Constraints · Shortcut: K, X (Toggle Driving) · K, Z (Toggle Active)

Tool Shortcut Description
Toggle Driving Constraint K, X Swap a dimensional constraint between driving (blue/coloured) and reference (grey/blue) mode
Toggle Active Constraint K, Z Enable or disable a constraint; disabled constraints appear greyed out and the solver ignores them

Intuition

Toggle Driving

Think of a ruler with a locking slider: in driving mode the slider controls the dimension and forces geometry to move; in reference mode the slider reads freely as geometry moves but does not constrain it. Toggle Driving flips the lock on and off.

Toggle Active

Think of a toggle switch on a circuit: flipping it off cuts power without removing the wire. Toggle Active cuts the constraint out of the solver temporarily — useful for debugging or experimenting with different constraint sets.

When to use them

Toggle Driving

  • A constraint is over-constrained (shown in red) because it conflicts with another; toggle it to reference to break the conflict while keeping the measurement visible.
  • You finished a sketch and want to add inspection dimensions (reference) without disturbing the fully constrained geometry.
  • You want to visually mark a derived measurement (e.g. the diagonal of a rectangle) without adding a constraint.

Toggle Active

  • You want to temporarily remove a constraint to see how the sketch behaves without it (for debugging).
  • You have alternative constraint configurations and want to switch between them non-destructively.
  • You want to study how geometry would behave if a constraint were removed, without deleting it permanently.

Step-by-step walkthrough

Toggle Driving

  1. Select a dimensional constraint (a distance, radius, angle, or lock constraint; geometric constraints like Parallel cannot be toggled to reference).
  2. Press K, X or right-click the constraint label → Toggle Driving.
  3. The constraint switches mode:
    • Driving → Reference: label turns blue (or grey depending on theme), (ref) suffix appears. The solver no longer uses this value to control geometry.
    • Reference → Driving: label returns to its normal colour. The solver re-imposes the value.

Toggle Active

  1. Select any constraint (dimensional or geometric).
  2. Press K, Z or right-click → Toggle Active Constraint.
  3. The constraint is greyed out and the solver ignores it. Press K, Z again to re-enable it.

Parameters

No numeric parameters. Both tools are pure toggles.

Common mistakes and pitfalls

Toggling a constraint to reference does not remove it from the tree

Cause: The constraint still exists in the model; it just has no effect on geometry. If you want to delete it entirely, select it and press Del.
Fix: For cleanup, delete reference constraints you no longer need.

Toggle Active leaves the sketch under-constrained

Cause: Disabling a constraint that was removing a DoF leaves that DoF free. The sketch reverts to under-constrained (white elements).
Fix: This is expected behaviour — Toggle Active is for exploration. Re-enable the constraint to restore full constraint.

Python API

Toggle Driving

import FreeCAD as App

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

# Toggle constraint index 2 to reference mode
sketch.setDriving(2, False)

# Toggle back to driving
sketch.setDriving(2, True)

doc.recompute()

Toggle Active

# Toggle constraint index 1 active/inactive
sketch.setActive(1, False)  # disable
sketch.setActive(1, True)   # re-enable
doc.recompute()

See also