Introducing the Tolerancing Advisor 

This task introduces the Tolerancing Advisor.
The Tolerancing Advisor lets you create allowed annotations according to the selected geometrical element or existing annotation. See Symbols for Geometrical Tolerances to see the list of available geometrical tolerances.
  Allowed annotations are:
  • Semantic (Dimensions) and non semantic annotations (Text, Surface Texture, Flagnote). See Semantic Control settings.
  • Datum.
  • Datum target.
  • Datum reference frame.
  • Semantic and non semantic annotations can be created on constant sections of variable fillets.
  • According to the selection, here a planar surface without annotation, available commands are as follows:
    • Text with Leader
    • Flag Note with Leader
    • Surface Texture
    • Semantic Datum
    • Straightness Specification
    • Flatness Specification
    • Profile-of-Line Specification
    • Profile-of-Surface Specification
  • Related Geometric feature type:
    • Angular Dimension Related to an Origin and Linear Dimension Related to an Origin are now available.
    • Distance Creation and Linear Dimension Related to an Origin are now available when you select two geometrical elements with same canonicity having constant thickness.
    • A revolute circle can be seen as a plane with its revolute axis seen as its normal.
    • The Invert Oriented button in the Limit of Size Definition dialog box enables you to invert the orientation of a Related Dimension.
    • The options Symmetric Lower Limit and Single limit in the Limit of Size Definition dialog box may not be active nor modifiable according to the elements selected.
    • If the option Always try to create semantic tolerances and dimensions is active, it takes the above into account.
  • If a revolute surface is selected along with a suitable datum reference the following commands are proposed to create runout tolerances:
    • Circular Runout Specification - Single revolute surface selected,
    • Total Runout Specification - Single revolute surface selected,
    • Circular Runout Specification - Multiple revolute surfaces selected,
    • Total Runout Specification - Multiple revolute surfaces selected.

    A suitable datum reference is the rotation axis of the selected geometry. If the datum reference is not selected, then these commands will not be proposed even if a revolute surface is selected.

  Remember that:
  • When the dimension supports are related to a parameter (sketch's constraints, knowledge, etc) for which tolerances are still defined, they are taken into account for the dimension tolerances.
Open the Tolerancing_Annotations_01.CATPart document:

  1. Click Tolerancing Advisor in the Annotations toolbar.

  2. The Semantic Tolerancing Advisor dialog box appears.

    This is the minimal appearance for this dialog box because no geometrical element or annotation has been selected and no datum reference frame has been created yet.
     

  3. Select the surface as shown on the part.

  4. The Semantic Tolerancing Advisor dialog box is updated according to the selected surface.

     
    • The Geometric Tolerance & Annotation Creation Commands frame contains all the semantic annotations that will be created in relation with the selected element and the geometrical feature type.
    • The Geometric Tolerance & Annotation Creation Commands frame contains a combo list for all capabilities applying for the selection.
    • Multiple selection of geometries is possible in the following two ways:
      • Manual multiple selection using the Ctrl key (or the Shift key for selection in the specification tree).
      • Automatic multiple selection by using the selection propagation commands in the Tools Pallet or in the Tolerancing Advisor.
    • In case of multiple geometries selection, the dimension and annotation created using the Tolerancing Advisor, is attached to the first selected geometric feature.
       
      In case, a dimension or annotation is already created for a group of geometrical elements the behavior is different. If you reselect these geometrical elements in another order, then the new dimension or annotation is attached again to the first geometrical element as the pre-existing dimension or annotation without taking into account the new order of selection.
    • The Propagation Selection options are displayed according to the type of face selected depending on the canonicity. In this scenario the options are not used. For more information, refer to Propagating Geometry Selection for Feature Creation.

  5. Click Text with Leader (1 Plane): .

  6. Enter Milling in the Text Editor dialog box when it appears.

  7. Click OK in the dialog box.

    The annotation text  is created.
    The Semantic Tolerancing Advisor dialog box is updated.
     
    The Text with Leader icon is orange-colored:
    This color inform you that an annotation has been created; you can still create other annotations.

  8. Select the two surfaces as shown.
     

    The Semantic Tolerancing Advisor dialog box is updated.
     

  9. From the list in the Geometric Tolerance & Annotation Creation Commands frame, select All possible types (default).
    The Geometric Tolerance & Annotation Creation Commands frame now displays all the possible commands.
     

  10. Click Text with Leader (All possible types (default)): .

  11. Enter the text and click OK.

  12. Click Close in Semantic Tolerancing Advisor dialog box.