Driving 3D Constraints via Generated Dimensions

In this task, you will learn how to drive 3D constraints via generated dimensions. 
Open the Pinmounting.CATPart document and the GenDrafting_drive_3dconstraints.CATDrawing document.

Go to Tools > Options > Mechanical Design > Drafting:

  • On the Dimension tab, make sure that Activate analysis display mode is selected. You may then click the Types and colors button to view (and possibly define) the characteristics that will be assigned to dimensions generated from 3D constraints and to dimensions driving not-up-to-date 3D constraints.
  • On the Administration tab, make sure that the Prevent dimensions from driving 3D constraints check box is not selected.

  1. On the front view, double-click the dimension which defines the top radius (Dimension.5 object). The Constraint Definition dialog box appears.

  2. Type 30 in the radius field to change the radius definition, and click OK.

    The dimension is modified.

  3. On the top view, double-click the dimension which defines the rounded corner radius (Dimension.1 object).

    The Parameter Definition dialog box appears.

  4. Type 30 in the value field, and click OK.

    The dimension is modified.

  5. In the 3D window, click Update to update the part.

    The part is updated and reflects your modifications.

  6. In the drawing window, click Update to update the drawing. The drawing is updated with the latest modifications in the part.