Regeneration Issues - Unexpected Feature Failures

[VMcD]

We recently updated from Creo 2.0 to Creo 7.0.4.0 (tested in 7.0.6.0 too) and we are seeing issues with regeneration and unexpected feature failures. It seems Creo 7 is not as robust as Creo 2?

1. Open the model, nothing to regenerate. Model looks complete.
2. Delete unused sketch
3. Extend feature fails

1. Force regen of model with Model Player
2. Trim features creates extra edge
3. Style surface fails

Has anyone dealt with this issue before?

Are there any best practices or config options to make older Creo model behave?

[tbraxton]

I have seen models created in older releases fail when opened in a newer release. I have always been able to "fix" the failures. I am not aware of any config options that would mitigate this in general.

Have you tried to open this Creo 2 model in Creo 4, 5, or 6 and does it have the same issues as you note above?

Does your Creo 2 model use absolute or relative accuracy? This may be relevant depending on what is failing. Does the model have geom checks present in Creo 2? If so, are these geom checks associated with the features failing in Creo 7?

Creo 7 introduces multi-body as well as defaults to absolute accuracy.  These may be relevant to the issue.

Without seeing the actual model, it is almost impossible to diagnose. It is worth a try to force a regen in a build prior to Creo 7 to see if the same issues are there.

[MartinHanak]

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@VMcD wrote:

We recently updated from Creo 2.0 to Creo 7.0.4.0 (tested in 7.0.6.0 too) and we are seeing issues with regeneration and unexpected feature failures. It seems Creo 7 is not as robust as Creo 2?

1. Open the model, nothing to regenerate. Model looks complete.
2. Delete unused sketch
3. Extend feature fails

1. Force regen of model with Model Player
2. Trim features creates extra edge
3. Style surface fails

Has anyone dealt with this issue before?

Are there any best practices or config options to make older Creo model behave?

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Hi,

your problem is "model dependent". Please upload it for testing purposes.

[Chris3]

Are you sure the same thing doesn't happen in Creo 2? There have been other threads about things not working in Creo 7 and then when the OP when back and retested in a prior release the same thing happened.

While it is true that PTC changed the default tolerance to absolute in Creo 7 that does not change pre-existing models nor does it have any effect if you have start parts.

While PTC has changed some of the behind the scenes modeling we still have models done in the 90s that open without issue.

[VMcD]

Thanks for responding. 

Good points, I will see if Creo 2 version is reproducible. I’ve also opened a Case. 

I’ve tried using Model player to force Regen, I get different failures. 

We’ve changed this part from Relative to absolute accuracy hoping to help with stability.
Could it have the opposite effect?

BTW
I’m unable to share the model because it is a product in development. 
This is a highly surfaced part with 600 features. 

[Chris3]

Just changing the accuracy from relative to absolute will cause the model features to fail. This happens in any version of Creo. It has to do with the way the feature dependencies are made.

PTC does not recommend switching all of your models to absolute just because. Hear Lino Torri's response to that question at 56:40

https://community.ptc.com/t5/Creo-Parametric-Tips/Creo-quot-Large-Assembly-Management-quot-Tips-amp-Techniques/m-p/761387 

[tbraxton]

If you use Creo to create models that are used to manufacture from you should use absolute accuracy. If you use any of the top down design tools within Creo you should use absolute accuracy. There is a reason that Creo 7 defaults to absolute accuracy and that is the implementation of muti-body in the core engine.

Relative accuracy is an archaic construct from the early days of Pro/E when it enabled for faster model regeneration on what were relatively slow computers. Relative accuracy is dimensionless and absolute accuracy has units of length. If you share data between models, then you want to make sure that the models have the same absolute accuracy (multi body for instance).

[tbraxton]

Changing the accuracy in a model is very likely to cause some features to fail. I would not change the accuracy yet other than for testing. It will affect any models that are children of this one potentially causing other models to fail.

Is the model in question a child of any other models?

If regenerates in Creo 2 then PTC guarantees that it will regenerate in any newer release. Let PTC support investigate if this is not the case.

FYI I have a model that was created in Creo 4 and does not regenerate identically in Creo 7. I was able to resolve the issue. I supplied this model to PTC and they came back with the canned answer Creo 7 functions to spec as the reason for the issue. It was due to an undocumented change in the default behavior of a copy quilt operation being changed sometime after Creo 4 that was never documented in the change notes.

[VMcD]

Hi all,

@anursingh asked for an update. Here it is.

Since I'm unable to share the data here I opened 2 PTC cases and 2 SPRs have been opened.

I'll post an update when I get one.