as internal standard procedure, I am using Symplified Representations to switch from these two configurations in assemblies:
- Complete assembly with all of its components
- Assembly for FEM calculations (--> for example with only the frame, without extra cosmetics, frills or structurally-irrelevant accessories)
the problem is that, in order to use the symmetry constraint in Simulate, I have to cut out a part of the assembly with an (for example extrusion) assembly-level feature, which is evidently useful only in the FEM Simp. Rep and therefore I would like to turn it off when I want the complete assembly: however I don't see the features in the list of the Simp. Rep. together with the components. (I also checked that it is not a problem of list settings like tree filters in the model tree).
Is it possible to do this someway?
I will let others chime in but I don't think this is possible. I think the only way to do what you are asking is to make a family table.
FYI - for the future, another approach to accomplish what you are doing is to make inheritance models for your assembly. With inheritance models you can turn features on/off and add features as needed for analysis.
thanks for your reply, the "problem" of the inheritance feature is that I would have to double the 3D model and save then two assemblies of the same product, thing that would not be advisable as we manage product data in Windchill.
Just a tip from me:
l had similar problem on part level. Inside Windchill can be each model only once.
But what to do, if l need to create more different settings of one part across many products? See link below for better understanding.
Use flexibility inside part and use it in assembly.
PTC community topic:
l know, that´s not answer to your question, but thise problems looks similar and it can give you some clue.
thanks for your reply.I got what your problem in that topic was, but the problem in using flexibility in my case is that the component, (throught the assembly-level feature) , when assembled, should bear a cut of material which depends on where on the assembly it is positioned: and then it should be switched to on and off with flexibility...so I don't think this could be done with flexibility.
One way would be to set the options of the extrusion of the assy feature to 'Part', then create a SimpRep with that feature excluded in the affected parts and finally in the Assy SimpRep reuse these part SimpReps (User Defined).
This will work but I would not recommend it. Propagating assy features to the part can be very nasty later...
Because this solution creates external references and behind the scenes family tables which are not as robust as another solution like inheritance models. External references and hidden family tables have a history of increasing processing time, increasing the likely hood of Creo crashing and or the assembly failing.
You mentioned that you didn't like inheritance models because it creates 2 of the same thing. This solution also creates two models; its just hidden to the user. Behind the scenes Creo is managing a family table (2 models) that turns the assembly level cut on and off.
thanks for your description. The problem to me is not much the memory occupied by 2 models but the bother to have to manage two items in Windchill, with two different names referring to the same product.
l use Constantin´s solution with User defined solution commonly. Have not see any problem yet.
Yes it creates external references, but it is necessary tax. If you will use it reasonably, l see no reason why don´t use User defined simply reps.
I do not see problems with the user defined simp reps.
But with the 'part' scope enabled in the assembly extrusion you create a reference from the part to the assembly. And this is something worth considering. I am not saying it is a no-go but at least the consequences should be considered.