How to dissociate "Hide/Show" behavior of multi-instanced parts within an assembly?

[JoshMcGowan]

I have a part file that has multiple bodies in it.
This part file is used multiple times in a product assembly.
I'd like to have instance 1 of the part show body A and hide body B, while simultaneously having instance 2 of the part hide body A and show body B.
Is this possible? I'm looking for something akin to the "flexible subassembly" feature, but rather than dissociating mechanical constraint behavior among sibling subassemblies, I want to dissociate hide/show behavior among sibling part files.

Example spec tree:

Product1
-Part1.1
+BodyA <-- I want this shown
+BodyB <-- I want this hidden
-Part1.2
+BodyA <-- I want this hidden
+BodyB <-- I want this shown

Edit: If it matters, I'm working in Catia V5. My company may or may not switch to V6 in the next few months though. So V5 solutions are preferred but if there are any V6 specific solutions then I'd still be interested in hearing about them.

Thanks very much for any help!

 

[MarkAF]

As far as I am aware, what you request is not directly possible in the program architecture. Here are a few possible alternative methods. Unfortunately they all involve creating additional files.

Copy the reference part model and make unique parts, and edit each as needed. This might be useful if the original model is a static reference, and is not changing through the design process right now.

Another method would be interesting if the original model is still being designed and updated. Create a new part. Within the new part, copy/paste (as result with link) the Bodies you are interested in from the reference part. Hide or show the individual bodies as required.
Repeat for as many instances as is needed.
It's clumsy, but should be possible to achieve the end result.

Edit - Here is a third method that uses Manage Representations at the assembly level. This is new territory for me that I'm trying to figure out a bit; I certainly don't know the ins and outs of this functionality.
Save your CATPart file as a CGR with a different hide/show state on its bodies for each state that you want to represent. Maybe PartNumber-1.cgr, PartNumber-2.cgr, PartNumber-3.cgr, etc.
At the Assembly level, right-click on the part model in the tree and pick on Representations > Manage Representations. In the Manage Representations panel, click on Associate... and select each of the CGR files you just created. This will add alternative shape representations.
For each instance in the assembly, go to the same Manage Representations panel and select Activate for one of the shapes.
This would also be useful if your reference part is a static model, and not currently changing through the design process.

For Catia V6 (3DExperience), the modeling behavior is not fundamentally changed in this regard. More capacity is introduced like you're talking about, but it's at the assembly product level.

-Mark

 

[Little Cthulhu]

The only viable enterprese-level option here is to create multiple representations as MarkAF mentioned above. Although I suggest using .CATShape format because it can store copied geometry from original part with link so you don't end up with multiple independent copies of the same geometry.

In general I believe your bodies should be modeled as separate parts since they need to be managed independently.

 

[itsmyjob]

Would you mind explaining what is the business case behind such modeling choice (having body A and B (and maybe more) in one part when you show only one of them in the product ??? CATIA is more oriented to 1 solid per part.

Eric N.
indocti discant et ament meminisse periti ​