Inheritance Dimensions on Assembly Drawing in Table

[BrettL.]

Hello

I was wondering if anyone had any additional insight to display the dimensions of  a .prt level inheritance feature in a table at an assembly level drawing (Currently using Creo 4.0).

Background:

I have a .prt file that contains an inheritance feature, from which vardim is used to change the length of a feature

example: d3:iid_843 is modified using vardim.

The .prt is placed in an assembly. I would like to be able to display the dimension d3:iid_843 in a drawing table of the assembly. There seems to be 2 options for this but would really like a third option if possible.

Option 1

If the .prt is placed as model in the assembly level drawing and activated, I can reflect the d3 dimension in the table using &d3:iid_843

• Adds an "active model" to the drawing (not ideal for WC revision control)

Option 2

Create a relation in the .prt file, ex L1=d3:iid_89 and then place in the assembly drawing table using the correct session ID of the component in the assembly:  &L1:2

• Does not allow parametric editing of the value directly

• Would need to add more relations to reflect additional vardims

Option 3 - Desired

Add the dimension directly in the assembly level drawing table taking into account the the iid#  from the .prt file and the session ID number for the component. I have tried multiple syntaxes for this without success.

Thanks

BL

[tbraxton]

I have not tested this but it should work. If it does not work you can always undeclare the layout.

If you were to create a notebook (.lay file) and drive the variable dims from the notebook and then declare the notebook to both the part and the assembly then you have access to the value in both locations driven by a single parent (Notebook file).

The notebook can then be used to define all variable dims to configure variants. The notebook controls values for global parameters that are then used throughout the design as required. If you set them up in table form it works nicely as a configuration manager and can be undeclared when appropriate.

[BrettL.]

Thanks for the suggestion but a layout file is way more than I need for this project. Plus layout files in WC can be picky regarding references during save a copy operation. At the component level, the dimension of the iid# can be placed in a table as long as the model is active on the drawing and the iid# is known. It also is parametric.

I was hoping to extend that functionality to the assembly level drawing as well without adding a component as an active model on the drawing (creating a revision dependency in Windchill) 

-BL

[tbraxton]

With regard to Windchill references I don't see any way to create a shorter dependency chain than to include the part in the assembly referenced by the drawing as you mentioned. Any other parametric "pipe" for that part dimension is going to add another data object in the dependency chain (i.e. Layout) which has to be managed in WC.

Since the variable dim design intent is propagated by the inheritance feature I assume if you follow a top down design paradigm that your desire for the variable dim to be parametric in drawing context is so that if it is modified in the part then the value in the drawing table will update.

Your intent is not to modify the table value in a drawing to drive the part geometry, is it?

[pausob]

It's amazing how much time is wasted on Creo annotation work-arounds...

It seems that inherited dimensions can be shown on a drawing that involves the target part, but they can't be "absorbed" by the drawing's note or table.  Moreover, such dimensions cannot be shown or assigned to a combination state of the target part.

Anyway, what about option #4 - add an annotation dimension to your assembly (e.g. ad1) and then show that annotation in your drawing's table (&ad1).

I suppose you can do the same process directly in the drawing (the codes will be add1 / &add1)

[tbraxton]

I came across something that may be of interest while researching another issue. This may resolve the issue with access to the dimension in your drawing.

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

[pausob]

Yes, but I don't think this will solve the OP's issue which was being unable to place the dimension of a merge-inheritance feature inside an assembly component in the assembly drawing's table or note.

I think showing the dimensions of such a component on the assembly drawing view is possible, even without the step of preparing a combined state in the component.