Setting the Datum Mode  

This task will show you how to create a geometry with the History mode deactivated, which means that for each created element there are no links to the other entities that were used to create that element.

If it is not displayed, open the Getting_Started1.CATPart document.

  1. Click Pad .
    The Pad Definition dialog box is displayed.

  2. Click Sketch in the Pad Definition dialog box.

  1. Select Plane.2 either from the geometry area or the specification tree. You are now in the Sketcher Workbench.

  1. Click Create Datum in the Tools toolbar to deactivate the History mode.

  2. Select the internal cylindrical surface of the part as shown here.

  1. Select Project 3D Elements in the Operation toolbar.
    The projection is created.

  2. Select Exit Workbench from the Workbench toolbar.
    You are now back in the Part Design workbench. Both the part and the dialog box are still displayed.

  1. Set the length value.

  2. Select Mirrored extend.
    The part will be displayed as shown here based on the newly created Sketch.3.
 
 

  1. Click OK in the Pad Definition dialog box.
    The pad has been created and now edit Sketch.1.

  1. Double-click Sketch.1 from the specification tree.
    You are now back in the sketcher workbench.

  1. Double-click the smallest circle radius value from the geometry.
    The Constraint Definition dialog box is displayed.

  1. Change the radius value to 70mm for instance.
 
 
 
 

  1. Click OK in the dialog box.
    The created pad has not been updated as elements created with the Datum mode activated are no longer associative the other geometry.
 
Note that:
  • the associativity between elements is no more kept when using the Datum mode.
  • this option has the same effect when using the Offsetting a use-edge element.
  • a click on the icon activates the Datum mode for the current or the next command.