Cannot save an assembly after changing a parameter

[Hidetaka]

I ran into a large assembly that I cannot save after changing some parameters.
The parameter does not seem to have anything to do with regenerating the assembly (it is date and designer name).
From the warning messages that appear after I tried to save the model, I have found 2 support articles, but I could not read them. Could someone please tell me what is in these two articles? Thank you so much!

https://www.ptc.com/en/support/article/CS258240
https://www.ptc.com/en/support/article/CS112336

[KenFarley]

The first (CS258240) indicates it is a result of regeneration failing. The "Resolution" in this case is:

• Reported to R&D as SPR 6497841
• Works to product specification for Creo Parametric
• Creo Parametric returns to old/unexpected values, when regeneration is not completed and not sure if new value is suitable or not.

The second (CS112336) seems to relate to "Model is not regenerated" and "Mass properties are not calculated" errors. Its "Resolution" is

• Reported to R&D as SPR 5152497
• To disable model regeneration and mass calculation when saving model
    Set config.pro options mass_property_calculate to by_request and regen_solid_before_save to no
• ​To enable model regeneration and mass calculation when saving model
    Set config.pro options mass_property_calculate to automatic and regen_solid_before_save to yes​

Disclaimer:
PTC recommends to backup the config.pro file before modifying it

[vnamboodheri]

Hello @hidetaka. 

It looks like you have a response from a community member. If it helped to answer your question please mark the reply as the Accepted Solution. 

Of course, if you have more to share on your issue, please let the Community know so other community members can continue to help you.

Thanks,
Vivek N.
Community Moderation Team.

[kdirth]

It is preferred that models are stored in default orientation and occasionally I find that I cannot save because I the only change I have done since the last save is change the view on the screen.  I will then either do a quick reorder (and back) or create a datum and delete it.

[BenLoosli]

I have found that changing a parameter value does not flag Creo to think the file has been modified and the file will not save with the message that file has not been changed. I then force another change, either a carriage return in the relations or delete an unnecessary parameter that we don't use. This will then 'force' the system to accept the change and do the save. 

[joe_morton]

Are you sure the model is not saving due to the changed parameters?

Did you try just regenerating and saving with the parameters still present? What happens if you delete one parameter at a time and save it?

[Dale_Rosema]

Just a long shot, but is the place where you are saving the assembly in your search path.

Could you be saving it to a directory that is not in your search path and then when you open it again you are opening the old iteration?