About Driving Dimension Annotation Elements
You can make model driving dimensions created and owned by features into permanently displayed dimensions in the model by selecting the feature or one of the feature dimensions and creating a Driving Dimension Annotation Element (DDAE) for it. The resulting DDAE is displayed in the model according to the annotation orientation that was active at that time. The DDAE is also listed as an annotation element in the Model Tree inside the feature that owns it. DDAEs can be created for model dimensions that can normally be shown in drawings. DDAEs do not have user-defined or system references in the annotation element. Note the following points about DDAEs:
You cannot make DDAEs nongraphical. You can delete them from the feature that contains them. When you delete a DDAE, the driving dimension of the feature is not deleted, only its annotation element representation is deleted.
DDAEs can only exist within the feature in which you create them.
One DDAE can include only one dimension. After a DDAE includes a dimension, another DDAE cannot include the same dimension. DDAEs cannot be created for notes or other feature annotation types.
If you modify the properties or value of the dimensions in a feature, then the changes are propagated to the DDAE. Similarly, if you modify the properties or value of DDAEs, then the changes are propagated to the dimension.
If you modify the feature such that the DDAE still exists but the Annotation Element's annotation plane is no longer compatible with its current annotation plane, then the Annotation Element becomes inactive.
If a dimension no longer exists in the feature, then Creo Parametric deletes the corresponding DDAE from the feature.
You cannot create a DDAE for pattern instance notes. DDAEs can be created only for dimensions.
You cannot create DDAEs for instances in a pattern. However, you can create DDAEs for the instances in a pattern table, as a pattern table creates new dimensions for the instances when patterning a feature.
When creating a family table or a relation you can select DDAEs on the Model Tree.
You can select a DDAE as an existing annotation when defining an annotation orientation.
When creating a new Annotation Element you cannot select a DDAE as an existing annotation.
You can change the value of a DDAE by clicking Value on the shortcut menu that opens when you right-click the driving dimension annotation on the Model Tree or in the graphics window.
You can delete a DDAE by clicking Delete on the shortcut menu that opens when you right-click the driving dimension annotation on the Model Tree or in the graphics window. The actual driving dimension is not deleted from the feature, only the displayed annotation element is deleted.
Component placement dimensions are shown on the Model Tree with the placement constraints of the component. If you create a DDAE with a placement constraint in an assembly, and hide the placement folder using the Model Tree filters, then DDAE will not be displayed in the Model Tree.
Creo Parametric displays DDAEs in Data Sharing Features (DSFs) and merge features. When switching between merge and inheritance features, the placement constraints remain the same. Therefore, there is no change in the DDAEs. 
You cannot create DDAEs for ordinate dimensions, dimensions in Auto Round feature, and for some dimensions in anatomic features.
The Undo and Redo functionality for DDAEs is similar to other annotation elements. In addition, the Undo and Redo commands are also available for actions such as creating and deleting DDAEs and changing the orientation of DDAEs.