Behaviour of assemblies in multiple sessions Creo Parametric 7

[SS_9086391]

Hello Everybody;

one of our users showed me a "it worked perfectly ok yesterday but now it doesnt" issue.

He opens two Creo-sessions because he wants to have different backgrounds for the main assembly and the sub-assembly he is working on.

- Main assembly opened in session 1

- Sub-assembly opened in session 2 versioned number is 1

- Changes made in sub-assembly > Save > versioned number is now 2

- Regenerates Main-assembly but changes in sub-assembly are missing

When you open the sub-assembly from the main assembly you can see that its still versioned number 1 !

As my colleague said, he always worked that way and now it doesnt.

Cant see anything suspicious in the config.pro

I can replicate this behaviour on my machine. 

However, when he opens both files in ONE session everything is normal and changes are taken over as expected.

There were some updates to the system yesterday, but nothing Creo related as far as i know.

Has anybody experienced simular behaviour ?

[Chris3 · Accepted solution]

It has never worked like he is expecting. When you open models in creo they are loaded into memory or "session". Unless you re-open those models or do an "update" in a linked environment (Windchill) there isn't a mechanism for updating what is in memory from a saved version on disk.

When you have one Creo session, all of the models are in memory so when you change something in the subassembly it shows up in the top assembly because again, everything is in the same memory allocation.

[MartinHanak]

Hi,

if you want to run two Creo sessions and you want to propagate subassembly changes into main assembly then you have to do something like that:

• suppress subassembly in main assembly
• erase old version of subassembly from main assembly session
• open new version of subassembly in main assembly session
• resume subassembly in main assembly

[tbraxton]

The reason given by the user for attempting this was to have different backgrounds when viewing models. The obvious simple solution would be to create a mapkey that will toggle the System Appearance (system colors) between backgrounds all within the same Creo session as required for visibility. This would avoid the file management issues altogether.