Creo 6.0 unknown failures that usually fix themselves

[BP_10313542]

I have a complicated surface modelled part (over 1000 features) with a family table. When I open one of the instances, it immediately shows regeneration failures, but when I manually regenerate it again, it usually fixes itself. Why would these failures be occurring if there is nothing wrong with the part since it completes the regeneration manually?

[tbraxton]

It is most likely related to the family table instances. Without understanding the nature of the features in the family table this is speculation. Try opening the generic only and then verify the instances before opening an instance. If you do this, do you still see this behavior of feature failures?

Creo Parametric regenerates a model automatically in many cases, including when you open, save, or close a part or assembly or one of its instances and when you open an instance from within the Family Table.

PS

In my experience it does not seem like a good idea to use a model with 1000 features with a family table. I could be convinced otherwise but in general I would seek an alternate method of managing your design intent in this case.

[BP_10313542]

The family table fails in the verification process as well. When I open the failed instance, I manually regenerate it and, it fully regenerates with no failures (and the verification status changes to success). Even in the generic, when I have to regenerate a lot of features at once by inserting farther down the part, I manually regenerate again and the failures fix themselves. I understand it is a very complicated 1 piece model with over 1000 features, but i dont see an alternate method. I am curious if upgrading to a newer creo parametric software would eliminate these seemingly unknown failures

[BenLoosli]

What is being modified in each instance of the family table? Are you changing dimensions or changing features that make up the instance?

[BP_10313542]

Mainly changing dimensions; however, features are also turned on and off in the family table as well

[Patriot_1776]

There are some times when 2 regens are needed to completely regen a part.  TOTAL PITA.  This can be due to relations (usually) or really complicated geometry that references other geometry (what DOESN'T?).  As I understand it the "Verify" in Family Tables only regens once.  So, on a complicated part like yours, that could be it.  Try looking at the relations and seeing if you can't clean them up or re-order them.  You might be able to force a second regen via the relations, but I wouldn't count on that.  This has been an issue since at least when I started using it ('96/v15).  PTC really NEEDS to fix the software so that it will continue to regen until it's done all in one shot.  Perfect recent example for me is I was looking at an assembly, for some reason a setscrew was constrained backwards on only ONE of a pattern's instances.  I opened the subassembly, it looked fine, went back into the top assembly, went to redefine the pattern, canceled out of it, regen'd, and it solved the problem.  See if it's the same features failing every time and try redefining those.

I did the back panel of a vacuum once for Royal appliance in the late '90's, and it had over 1,400 features, so I feel your pain.

Best of luck!

[BP_10313542]

Thank you! This is really helpful to understand. I have few relations in the model. Often merge and solidify features fail, so I imagine its failing due to it being complicated geometry that has many references? I have also found that cancelling out and regenerating features sometimes fixes issues when it shouldn't! However, sometimes the part is working, I change nothing, regenerate, failures, and another regeneration does not fix the issue. Thats when its a big issue and I have to go back to the last saved working model.

[tbraxton · Accepted solution]

Creo is more than capable of managing very large number of references between models consisting of complex geometry. The high feature count or numerous references is not likely the source of your issue. Merge and solidify features failing is likely doe to the nature of how the model was originally constructed. I see this type of instability in models built using surfacing quite often, it is usually a result of how the features were defined when created. Does the generic model have geometry checks? Without models to query the determination of a cause of the issue is difficult.

When you query geometry checks, so you see this attached to any merge features in the model?

• Merge surfaces warning:Design intent is unclear.  Use "Info"/"Geom Check" menu for details.
• Warning In Troubleshooter dialog box
  • The boundary of the highlighted surfaces was extended. Unexpected results are possible.
  • Recommended actions: Try to modify the feature so that extending is not necessary.