Sketch Constraints

Apply geometric relationships such as tangency and perpendicularity to sketch curves.

As you create geometry, many sketch constraints are automatically applied. For instance, if you draw a line that is nearly horizontal, a horizontal constraint will be created on that line automatically, making it precisely horizontal for you. When you modify a sketch, the constraints ensure that the intended relationships between the sketch entities remain intact.

Apply or Remove Sketch Constraints

Apply sketch constraints to geometry to ensure that the intended relationships between sketch entities remain intact, or remove sketch constraints to allow more freedom to create free-form objects.

In sketch mode, right-click on a sketch curve, then toggle the icons at the top of the context menu on or off to apply or remove sketch constraints.


Constraint	Description
Fixed	Lock the position of any sketch curve. When a line is fixed, you can still move the end points to change the length. The end points of a line are separate entities and can be fixed independently. Note: To delete all fixed constraints, right-click on the constraint and select Remove Fix.
Horizontal	Lines are constrained to be horizontal. You can also use this contraint to align points.
Vertical	Lines are constrained to be vertical. You can also use this contraint to align points.
Midpoint	A point is constrained to be the midpoint of a curve.
Coincident	A point is constrained to be coincident with another sketch entity.
Collinear	Lines are constrained to lie along the same straight line.
Parallel	Lines are constrained to be parallel.
Perpendicular	Lines are constrained to be perpendicular.
Tangent	A line is constrained to be tangent to an arc, or an arc is constrained to be tangent to another arc.
Concentric	Arcs or circles are constrained to have the same center.
Equal	Lines are constrained to have the same length. Arcs and circles are constrained to have the same radius.
Offset	A sketch curve is offset from another sketch curve. Note: This constraint cannot be applied from the sketch constraint context menu.
Symmetric	Two curves are constrained to be symmetric about a construction line (e.g., mirrored curves).
Select Other	This is not a constraint. Select this option when selecting overlapping sketch entities to specify which sketch entity you wish to select.

Tip:

To hide all constraints, deselect Show constraints under Sketching in File > Preferences.
If your horizontal constaints appear vertical and vice versa, use the Align Axes option in the context menu to align the sketch axes so that the x-axis is horizontal and the y-axis is vertical.
Select Delete All Constraints from the context menu to remove all constraints from all sketches in the model.
Select Remove Fix from the context menu to remove all fixed constraints in the model.