Setting Constraints

3D constraints are defined by means of one of the two constraint

commands available in this workbench. Depending on the creation mode chosen for creating wireframe geometry and surfaces (see CATIA Wireframe and Surface User's Guide), constraints set on these elements may react in two ways. You create references if support elements were created with the Datum mode deactivated. Conversely, you create constraints if you constrain datums. For more about datums, please refer to Creating Datums.

The constraints you can set in Part Design workbench are:

Distance

Length

Angle

Fix/Unfix

Tangency

Coincidence

Parallelism

Perpendicularity

This task shows you how to set a distance constraint between a face and a plane, then a reference between the face and another plane.

Open the Constraint1.CATPart document.

Select the face you wish to constrain and Plane.1. This plane is a datum (there are no links to the other entities that were used to create that plane).

Click the Constraint icon

The application detects the distance value between the face and the plane. Moving the cursor moves the graphic symbol representing the distance.

Click where you wish to position the constraint value.

The constraint is created.

The name of a constraint displays when passing the mouse over that constraint.

Now, set another constraint between the same face and Plane.2. Plane.2 is not a datum. Repeat the instructions described above using the face and Plane.2.

The application creates a reference. Creating a reference means that each time the application integrates modifications to the geometry, this reference reflects the changes too.

The reference is displayed in parentheses as shown below:

You cannot set a distance constraint between two faces belonging to Part Design features linked by their specifications. In the example below, the application creates a reference between the faces, not a driving constraint.

To know how to modify a constraint, refer to Modifying Constraints.