When you change geometry of a part using Flexible Modeling features, standalone annotations (such as dimensions, notes, symbols, GTOLs, surface finishes, and others) may get affected by that change. Depending upon the type of annotation, the annotation is automatically updated to reflect changes made to the geometry. Such automatic updates are done to annotations (considering limitations mentioned below) only when you create a new drawing or you update a drawing in the Creo Parametric 2.0 M030 or later releases.

When you retrieve a drawing that contains Flexible Modeling features, a warning dialog box opens signifying presence of potentially out of date annotations, and you can review these out of date annotations.

Click Review on the warning dialog box. The Highlight by Attributes dialog box opens. Select the Show out-of-date check-box under the Out-of-date references area, to highlight the potential out of date annotations (with missing references) in purple color. The warning dialog box opens only for the first time when you retrieve a drawing.

The Update references option on the Highlight by Attributes dialog box is available only when you open a legacy drawing that contain Flexible Modeling features. Click Update references to update annotations.

Annotations corresponding to the Flexible Modeling features appear highlighted when you open the Highlight by Attributes dialog box.

You can click Continue on the warning dialog box, to open the drawing without reviewing the out of date annotations.

Driven dimension annotation in 2D and 3D is automatically updated with changes made to the geometry, as long as those changes do not make the dimension invalid based on its type, orientation, or the drawing view or annotation plane to which it belongs.

If the change makes the driven dimension annotation invalid, the dimension will become out of date, and appear highlighted in purple color when you select the Show out-of-date check-box on the Highlight by Attributes dialog box.

Driving dimension annotations are not updated to reflect changes made to the geometry, because these dimensions are still valid for the original feature at the point in the model history when that feature was created. Driving dimension annotations will appear highlighted in a purple color when you select the Show out-of-date check-box on the Highlight by Attributes dialog box, to indicate that they are potentially out of date, if the geometry of the feature, to which they belong, is changed by a Flexible Modelling feature.

GTOL’s, notes, surface finishes, and symbols in both 2D and 3D that are attached to geometry that is affected by flexible modelling features will update their attachment locations to reflect the changes to the model geometry due to Flexible Modeling features.