Setting Constraints Defined in Dialog Box

This task shows you how to use this constraint command which detects possible constraints between selected elements and lets you choose the constraint you wish to create. You are going to constrain a hole.
Open the Hole1.CATPart document and create a hole anywhere on the pad top face.
  1. Right-click the circular face and select Other Selection... to select the hole axis.

  2. Use the Ctrl button to select the face as shown:

  3. Click Constraint Defined in Dialog Box .
    The Constraint Definition dialog box is displayed. 

    The constraints  you can set in Part Design workbench are:

    • Distance


    • Length


    • Angle


    • Fix/Unfix


    • Tangency


    • Coincidence


    • Parallelism


    • Perpendicularity


    The application detects three possible constraints between the axis and the face:

    • Distance

    • Angle

    • Fix

    The other constraints are grayed out indicating that they cannot be set for the elements you have selected.

  4. Check the Distance option.

  5. Click OK to confirm.
    The distance constraint is created.