Is there a way to add dimensions from a merged part into the dwg of the higher level part?

[ptc-5264891]

I am using Creo Parametric 7.0. 

Background:

I am producing a mdl/dwg for manufacturing which uses the final machining mdl as a merged part.  I am doing this to create a mdl/dwg template for automation which will be driven by the final machining mdl. Majority of the dimensions from the final machining mdl are needed for the manufacturing dwg.

Question:

Outside of manually recreating these dimensions in the manufacturing mdl, does anyone know if there is a way to display the dimensions from the merged final machining mdl in the manufacturing dwg?

Thank you!

[tbraxton]

The inheritance option when using merge will enable access to the dimensions from the source model in the derivative part (mfg model). 

Dimensions of an External Inheritance feature cannot be shown in the target model Creo Parametric

Solution:

1. Optional: Source (base) model: Create or activate a Combined State using a specific Simplified Representation, which includes Annotation Planes and specific settings
2. Optional: Source (base) model: > View Manager > All: Save the Combined State which is active
3. Source (base) model: Annotate > Show Annotations to permanently display annotations and dimensions as of choice in current state
4. Target model: Annotate > Show Annotations on the inheritance feature

• Note: The combined state can then be used for the model's drawing

[kdirth]

Dimensions from a merge cannot be displayed.  If you toggle the merge to an inheritance, you can show dimensions.

[ptc-5264891]

This seems to be the solution! Thank you!

I will keep this open until I have tested our program and replacement / regeneration proves successful!