Creating a Geometrical Tolerance 

This task shows you how to create a geometrical tolerance directly on the 3D geometry.
Geometrical tolerances are specifications included in a tolerance frame.

  1. Select the front planar surface as shown:

  1. Click Geometrical Tolerance  in the Annotations toolbar.

A message window appears informing you that you cannot use the active view. Therefore, the application is going to display the annotation in an annotation plane normal to the selected face.

  1. Click Yes to close the message window.
    The Geometrical Tolerance dialog box is displayed.

       

    The Tools Palette is displayed according to the type of face selected depending on the canonicity. In this scenario the Tools Palette is not used. For more information, refer to Propagating Geometry Selection for Feature Creation.
To create a geometrical tolerance you need to specify one geometric tolerancing symbol and fill in the tolerance value field. 

When fulfilling the second line "Spec 2...", a second geometrical tolerance will be created.
Both tolerancing specifications will be displayed as grouped.
 

  1. Set the perpendicularity symbol to define the tolerance.

  1. Enter the value of the tolerance: 0.5 and insert the At Maximum Material Condition symbol modifier

  1. Enter A as reference.
Modifiers are not displayed in tolerance and reference fields and appear with a "|" character.
 

  1. Click OK. The geometrical tolerancing annotation is attached to the 3D part.
    The geometrical tolerance entity is added to the specification tree.
    You have specified a perpendicularity of the front planar surface regarding to A datum surface.
    This toleranced surface shall be in 0.5-wide tolerance zone, on which a Maximum Material Condition (MMC) is applied.