Windchill smartlock and regeneration in Creo

[ilyachaban]

Why objects which is regenerated in creo changes it's state from 

to 

after regeneration. 

Object is read only why has it been chagned during regeneration?

[BenLoosli]

Set regenerate_read_only_objects to NO in your config.pro

[ilyachaban]

We can’t change this. The parameter is set to YES because it comes directly from the drawing.

We use parameter in relations whici part_number = REL_MODEL_NAME

This parameter is hown on drawing. And if this parameter id used by instance of family table. then after regeneration each instance get's number of generic. Total disaster happens then when manufacturers get's our drawings with generic numbers in it. 

[ilyachaban]

According to your recommendation on test data i've tried to change this parameter ot NO and still same issue.

[BenLoosli]

What version of Creo are you using?

Are you using Windchill with your data?

Are these family tables saved in the current version of Creo?

Try this hidden config.pro option.

Article - CS170675 - Definition and values of hidden config option regen_read_only_insts in Creo Parametric 2.0

[ilyachaban]

Creo verson 11.0.3.0
Windchill version 13.0.2.4

all objects has been created in new creo and checked into new windchill. Everything is stored and created in versions where it's used

[ilyachaban]

Hidden config option didn't help. All three values does change top level assembly. Each time red symbol appears after regeneration. On retrieval there is no errors/warnings

[ilyachaban]

AND THAN I REGENERATE 

[Van_AG · Accepted solution]

Open and regenerate the assembly

Execute the Tools > Compare Assembly command

Select the same assembly from the workspace.
Creo will show you what has changed after regeneration, and you will be able to locate the problem

In my example, the AUTH_NAME parameter gets its value from PTC_WM_MODIFIED_BY through an equation

According to PTC training materials

Locking a CAD document in the workspace sets a read-only status on the content stored in the local
workspace cache.

It may be desirable to make an object read-only for any of the following reasons:
• To reduce the number of times that the Conflicts dialog box is presented for objects that are
not intended to be modified.
• To provide better visibility into changes made implicitly by the CAD application. For example, you
are alerted to unplanned or unexpected changes that are required during regeneration.
• To prevent the object from being accidently modified.

This indicates that the model is not completely locked in the Creo session.

"Works to product specification"

[ilyachaban]

Thank you so much. Have never used this tools. Now it's diverged from one big problem to many small problems. Which we will solve along the way. 

For now after researching different model there is alot of geometry issues and alot of parameter issues. So now we can start working on it. Also there is parameter which helped to reduce amount of correct models which is: regen_simp_retrieve NO

So whole problem is pinpointed and work finally began

[ilyachaban]

According to the: https://www.ptc.com/en/support/article/CS32596?source=search

didn't help 🫠

[Catalina]

Hi @ilyachaban 

I wanted to see if you got the help you needed.

If so, please mark the appropriate reply as the Accepted Solution or please feel free to detail in a reply what has helped you and mark it as the Accepted Solution. It will help other members who may have the same question.

Of course, if you have more to share on your issue, please pursue the conversation.

Thanks,

[ilyachaban]

Hello, 
There is no solution for now. There is also parallel branch together with PTC Support so if there will be any aplicable solutions i will write it down here.