About Sketcher Constraints

Sketcher > Constraining Geometry > About Sketcher Constraints

A constraint is a condition defining the geometry of the entity or a relationship among entities. Constraints can refer to geometry entities or construction entities. Create constraints or accept the constraints offered as you sketch. You can select an existing constraint, delete it, or get more information about it. The constraint tools work in Continue mode.

Some constraints can be applied to a single entity, and other constraints can be applied to pairs or groups of entities.

Number of Entities	Applicable Constraints
A single entity	Vertical Horizontal
Pairs of entities	Perpendicular Tangent Midpoint Coincident Mirror Equal Parallel
Three or more entities	Equal Parallel

• When you apply the Equal constraint to a group of weak dimensions, the dimensions are removed and replaced with E. To directly control these constrained dimensions, you must create a strong dimension for one of the entities.

• An entity or a chain of entities created with the Use Edge or Offset Edge command has the Same Points constraint symbol if the endpoints of the new entity are fixed.

Strong and Weak Constraints

Weak constraints are those that were automatically generated in sketches created before Pro/ENGINEER Wildfire 4.0. They appear in gray and may disappear when you add or remove geometry, dimensions, or constraints. Strong constraints are those that you define.

Constraint Conflicts

If you strengthen or add a constraint that conflicts with an existing strong dimension or constraint, any conflicting dimensions or constraints are highlighted and the Resolve Sketch dialog box opens.

To resolve the sketch, you must select one of the conflicting constraints or dimensions and click one of the following commands:

• Undo—Removes the selected constraint if you added it; weakens the selected constraint if you strengthened it.

• Delete—Deletes the selected constraint.

• Dim > Ref—Converts a conflicting dimension to a reference dimension.