Filtering Annotations

This task shows you how to filter the display of annotations.
You can filter annotations display though the following features:
  • Views/annotation planes
  • Annotation sets
  • Geometrical elements
  • 3D annotations
  • Any Part Design feature
  • Any Generative Shape Design feature
  • Restricted areas
  You can filter annotations in the Visualization mode context. See Annotations and Cache System.
In the case of Part Design or Generative Shape Design features, only the annotations that are directly or indirectly applied to the geometrical elements which compose the feature will be displayed when applying the filter. In the case of restricted areas, only the annotations that are directly or indirectly applied to the geometrical elements which compose the restricting part of the restricted area will be displayed when applying the filter.
Open the Annotations_Product_04.CATProduct document.
  1. Click the Filter icon:
    The Filter dialog box is displayed.
    • The Definition area allows you to filter the display of annotations in the 3D viewer using the following criteria:
      • All: displays all the geometrical tolerance annotations.
      • None: displays no geometrical tolerance annotation.
      • By type: non semantic.
      • By sub-type: text, datum, datum targets, geometrical tolerances, Note Object attributes.
      • By feature (Part Design or Generative Shape Design feature) or geometrical element.
      • By value  <, > , =, > =, <= functions against a specified value.
      • By capture.
    • The Refine filter option filters out tolerances still filtered: it allows you to filter from the current annotation filtering with another criteria in relation with. For example you can filter geometrical tolerances first, then select this option and filter these geometrical tolerances by values. This is equivalent to the AND Boolean operator.
    • The Show geometry attachments option displays the annotation leader if exists, and all the linked annotations between the leader and the filtered annotation if needed.
    • The Results area provides the following information:
      • Number of specified tolerances attached to the 3D model
      • Number of tolerances selected according to the choice indicated in the two previous fields

    However, when default tolerances are specified, the number of tolerances displayed attached to the model does not correspond to the number of tolerances effectively specified. The default tolerance annotation is displayed once and the default tolerance specification is applied to several entities. These several specific toleranced entities are considered in the count of the Tolerances in the document field.


  2. Set the Filter choice field to By sub-type.

  3. Set the Simple Datum sub-type.

  4. Click Apply. The Number of selected tolerances field displays 3.
    Only simple datums are displayed.

  5. Click Cancel to cancel the operation. All annotations are visible again.