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FMRV1-Visitor
1-Visitor
August 17, 2020
Solved

Master Representation, Configurations, Overlapping Geometry, 2D Drawings

  • August 17, 2020
  • 3 replies
  • 5608 views

Hello!


I would like to preface by saying that I have lurked through the community forums in hopes of finding a resolution to my specific situation, but I haven't seen something that applies.  I have however run into methods of Family Tables and Configurations, and "Model Properties > Flexible" edits -- none of which have resolved my case. I can't help but feel as though I am missing something rather obvious. Your patience is greatly appreciated!


Attached you will have a very simplified example of the modeling I'm doing at this moment.

---------------

I am modeling an FPCBA using vanilla Creo 5.0.*.  In this situation, I would like to have a configuration that pertains to the in-assembly geometry (Figure_A), and I would like to have a configuration that pertains to a 2D Drawing geometry (Figure_B).


Currently, the default Master Rep defaults to Figure_C, which overlaps both configurations. Although the appearance of the model in Master Rep is undesirable, I can live with this. The problem is that the Master Rep creates overlap of geometry features which then have cascading errors for whichever design I did second. This leads to error messages when saving, and obfuscates which errors are "true" and which errors are due to the overlap. I can't seem to edit this Master Rep to only reflect the geometry of Figure_A.


Is there any method to avoid the series of errors associated with the overlapping geometry? Or better yet, is it possible to change the Default Representation to represent only one configuration so as to avoid the errors?

Any suggestions are appreciated!

 

Thank you

Best answer by kdirth

An option to try is to use Flexibility.

  • Create the flat version
  • Suppress the flat version (to prevent references to it)
  • Create the as assembled version
  • Suppress the assembled version
  • Resume the flat version
  • Assemble into the assembly
  • Apply flexibility to the part
    • In the varied items dialog, select the features tab and add features of both versions
    • Change the status of the features as needed

If several features are required for each version, group each set of features and suppress and resume the groups.

 

Can give more detail if needed.  Predefining flexibility in the part could also help if it is used in more than one assembly.

3 replies

P
Pettersson15-Moonstone
15-Moonstone
August 18, 2020

If it's a simple part like this, the easiest solution is probably to do it in Sheetmetal. Make the bent version using a simple extrude command, then create a flat state. In Creo 5, you can choose whether you want your flat state as a family table instance or as a simplified rep. That'll be the easiest solution to this particular problem, since it's a simple flat sheet that is bent in a single direction.

 

For more general cases, things like Spinal Bend, Warp or Flatten Quilt are things that can take you between two different configurations, which is necessary if you want to be able to switch between them as simp reps, for example. Let us know if you want to explore this more, but for your particular problem, I'd use Sheetmetal.

F
FMRV1-VisitorAuthor
1-Visitor
August 18, 2020

Hello Pettersson,

 

Thank you for your advice.  The sheet metal approach is not applicable to this scenario.  Family Tables are not applicable either. The geometry I have provided you is overly simplified, since what I am working on is confidential.  If geometry were as simple as that which I provided then Spinal Bend, Warp, or Flatten Quilt would work.

 

This scenario has also applied to other parts that are not FPCBA's.  The features aren't driven by individual parameters, they are driven by different geometry.

 

I seek a generalized approach towards overlapping geometry as a result of creating configurations using Creo's representations and how to overcome the errors resulting from this.

Thanks again

P
Pettersson15-Moonstone
15-Moonstone
August 19, 2020

Ok, I think I understand your issue better now. It is indeed an annoying problems. As you point out, you can't suppress features in the master rep and activate them in a simp rep. And applying geometry on top of geometry can cause issues.

 

How about a feature after the first configuration that cuts away all geometry? I'd do it with a datum plane and Solidify, or even more stable, make an all solid surfaces selection, copy and Solidify. That would never have a problem with lost references or dimensions that need updating.

 

This way, the master rep would look like the second configuration you model, and a simp rep could suppress the Solidify feature and everything after it, revealing the first configuration.

    kdirth
    kdirth21-Topaz IAnswer
    21-Topaz I
    August 18, 2020

    An option to try is to use Flexibility.

    • Create the flat version
    • Suppress the flat version (to prevent references to it)
    • Create the as assembled version
    • Suppress the assembled version
    • Resume the flat version
    • Assemble into the assembly
    • Apply flexibility to the part
      • In the varied items dialog, select the features tab and add features of both versions
      • Change the status of the features as needed

    If several features are required for each version, group each set of features and suppress and resume the groups.

     

    Can give more detail if needed.  Predefining flexibility in the part could also help if it is used in more than one assembly.

    There is always more to learn.
      kdirth
      kdirth21-Topaz I
      21-Topaz I
      August 18, 2020

      Here is a simple example in CREO 4.0.

      There is always more to learn.
        F
        FMRV1-VisitorAuthor
        1-Visitor
        August 19, 2020

        @Pettersson --  I see this route as promising, and parts of it seem to reflect what one of my colleagues was suggesting.  I'm going to give it a try with an upcoming part.  Thank you for taking the time to provide this advice!

         

        @kdirth -- A-ha! I think the complexity of having multiple features in each configuration for flexibility could be simplified by the use of groups!  For some reason I thought that I would still have to go through each individual feature within flexibility.  I will also be giving this a try.  Thank you as well!

         

        Since time is of the essence, I actually have assigned a co-op to remodel the second configuration by first offsetting the predominant datum planes far enough that the two configurations do not geometrically overlap. The downside here is that we have had to remodel the full part twice, rather than taking some common geometry from which to seed into each of the configurations. The repercussion is that when first making the assembly, there are now floating "2D Drawing" representations, but this is trivial, since the in-assembly representation can be changed to reflect the FPCB's 2D or 3D-in-Assembly reps.

         

        I'm going to give both of your methods a try in hopes of making it more streamlined for my colleagues as well.  I believe that with one or both of the methods, I will have a viable workaround!

         

        Thank you again to both of you! Take care and stay safe!

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