Managing View/Annotation Plane Associativity

This task shows you how to manage view/annotation plane associativity, by changing the definition plane of a view.
  • When views are associative to the geometry, any modification applied to the geometry or to the axis system is reflected in the view definition.
  • When annotations cannot be visualized in the view, after modification of the definition plane, it means that these annotations have lost their associativity with this view and their definition is not compliant with the new definition plane.
  • When extracted to 2D (using the View from 3D command in the Generative Drafting workbench), views from 3D are currently not associative to the geometry of the 3D view. So, if you modify the geometry of a 3D view, the definition of the corresponding 2D view will not be modified at the next update, even if the 3D view is associative to the geometry. This limitation should be fixed in an upcoming release.
Open the Common_Tolerancing_Annotations_02 CATPart document.

  1. Right-click the Section View.1 annotation plane, and select the Change View Support... contextual command.
    The Change View Support dialog box is displayed, indicating that the view is currently associative to User Surface.1.
    For more information on Change View Support dialog box, see More about Change View Support Dialog Box.

  2. Select Associative in the Type combo list and select the face as shown below to associate the view to another geometry.

    The Change View Support dialog box is updated, indicating that the view will now be associative to User Surface.2.

  3. Click OK in the Change View Support dialog box.

    The Section View.1 annotation plane is now associative to the specified surface. If you move the view definition plane or modify the axis system, the view will be re-defined accordingly.
 

About View Associativity
 

A view becomes invalid in the following conditions:

  • If a view is created by selecting a planer geometry and this reference geometry is deleted or deactivated or unresolved. When the geometry is available again, the view becomes valid and remains associative to it.
  • If the geometry referenced by a view is deactivated or unresolved, the view becomes invalid. However, the position and orientation of the view remains unchanged.
 
Created view The plane associated with the view is deactivated. As a result, the view becomes invalid.
 

Diagnostic Report
  You can get the diagnostic report of a view by right-clicking the view in the specification tree and selecting Diagnostic report.
The 3D annotation diagnostic report dialog box appears showing the following information: 

If the geometry referenced by a view is deactivated or unresolved, the character “?” is displayed in the Reference field of the Change View Support dialog box.