In Context Parts and Family Tables

[ToddCarpenter]

I know I'm asking this wrong, so forgive the noob question...

I have an assembly with a single part I've modeled "In Conext" (SolidWorks term, not sure it applies here), but in short, it's nothing more than a rectangle, and I need to instance the assembly.  My problem is my assembly Family table is working fine, but my part is not.  I know how to do this in SolidWorks, but I'm guessing it has to be different in Creo, I'm just not sure how.

Do I need to create Family Table instances of the part as well?  I'm guessing I do, but all the of the geometry in the part is tied to the assembly - meaning there are no dimensions in the part, so how do I do this?  Or do I need to make the part "Flexible"?

I'm using Creo Parametric 2.0 DateCode M130.

Thanks for any help...

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[dschenken · Accepted solution]

I guess you could create a parallel family table in the piece part, and have those in the parent table as a replacement component. When you Verify the assembly it should regenerate the component family table instances as well.

Flexible won't do it because that is a way to over-ride lower component dimension values, and the component hasn't got any.

I'm not sure how Solidworks would accommodate the situation, but I think it's probably by ignoring it rather than creating a auditable result. That is, PTC would end up with component parts that have a certain size that could be checked independently of the assembly, while Solidworks may chuck it and opening the 'in context' part would fail unless the assembly was already open. PTC will complain that the related assembly is not in memory, but the part will still have geometry.

[dgschaefer]

As a general rule, modeling "in context" as Solidworks teaches is not a good practice in Creo. (I'm not convinced is's good in SW, but that's a question for another forum. ) Creo has very robust top down design tools to accomplish what you are looking to do, namely driving your components by the design intent of the entire assy.  Do some research here in the Community, in the help and the Knowledge Base on skeleton modeling.  More complex than building in context, but far more robust, in my view.

Now, generating a family of parts like you want isn't easy with a skeleton, but it is possible.  The reality, however, is that a single assy cannot drive all the dims of a family of parts, right?  Only one version fits that specific assy, the others fit other versions of that assy or other assys. 

[OlivierJOLY]

Hello, it is possible to manage external references with family table in Creo. There is an exemple available in Creo 2 help guide if you search with keywords "family table" and "reference model".

http://www.ptc.com/cs/help/creo_hc/creo20_hc/pma/fundamentals/fund_ten_sub/Example_Adding_a_Reference_Model_to_a_Family_Tab.html#Example_Adding_a_Reference_Model_to_a_Family_Tab_Example1359_41.  It works fine, especially when you have to deal with skeleton and dimensions are then not present in your models.

You can find a very simple example I created here https://www.dropbox.com/s/ihf7jza55k359xo/AB.zip?dl=0

Regards

Olivier