Constraining a Sketch

Constraints are used to impose geometric limitations on sketch entities as well as to control their position on the sketch plane.

You can apply a constraint to a single sketch entity to define how it relates to the sketch plane, or to multiple sketch entities to define the relationship between them. It is possible to constrain the active sketch using sketch entities from another existing sketch or geometry. The constraints that are shown in the right-click menu differ depending on the selection of sketch entities.

To apply a constraint:

1. In the 3D-CAD view scene, select the sketch entities that you want to constrain.
2. Right-click one of the selections and select the type of constraint you want to apply.

   Only constraints that are relevant to your selection appear in the right-click menu. See Constraint Types.

Each constraint that you apply is depicted by a symbol, such as for a concentric constraint, and is added to the sketch. Move the mouse pointer over these symbols in the 3D-CAD View scene to highlight the pair of sketch entities that are associated with the constraint.

To delete a constraint, select the constraint symbol it in the 3D-CAD View scene and press the <Delete> key.

When you apply a constraint to a pair of sketch entities, 3D-CAD can move one of the sketch entities in order to satisfy the constraint. You cannot influence which sketch entity moves—3D-CAD determines which entity to move. If, however, you want to ensure that a particular sketch entity does not move when the constraint is applied, apply a fixation constraint to one of the sketch entities.

When you apply constraints to multiple sketch entities at the same time, 3D-CAD applies the constraints to each pair of sketch entities. Consequently, you end up with multiple constraint symbols added to your sketch. Move the mouse pointer over each constraint symbol to highlight the pair of sketch entities that are associated with each constraint.

To use the sketch plane origin for constraining a sketch, create a point at [0, 0] and fix it in position. You can then use this point to constrain sketch entities in relation to the origin.

If the new constraint cannot be satisfied, due to any existing constraints or dimensions on the sketch, an error message is shown and the constraint is not applied. To resolve this issue, delete any existing constraints or dimensions that are counteracting the new constraint.

3D-CAD considers lines to be infinitely long and circular arcs to be complete circles when constraints are applied. Therefore, a point that is constrained to coincide with a line does not always appear to lie on the line. Similarly, a point that coincides with a circular arc does not appear to lie on the arc. In each case, the point is coincident with some point on the line segment that defines the infinite line, or the arc that defines the full circle.