How can you safely rename Catia filename in an assembly?

[mcadjgfrank]

Greetings:

Let assume that you have top level assembly detail drawing containing 4 parts A, B, C, D and would like to rename the filename of these parts to E, F, G, H. How do you manage to do this so the assembly and the detail drawing can be opened after the rename operation?

Thanks in advance for your time and help.

 

[ferdo]

Hi,


You have to take into consideration this

http://www.eng-tips.com/faqs.cfm?fid=1318

Anyway you have also to edit the links. See

http://www.catiav5forum.de/jgs_db.php?action=show&eintrags_id=4&katid=4&sid=

Regards
Fernando

 

[Runz]

Save Management

Go into Save Management. choose a component, select save as, then give the new file name. Do this for all components that need renamed. Then select OK. New files are created with the new file names and these are now used with the CATProduct. The old files still exist (Old file names), so you may need to delete those files if they are no longer required.

May not be the best practice, but it is simple and effective.

 

[catiajim]

If all linked documents are open when you do this, then it should work without having to re-link anything (the CATParts can all be open in the Product, but they should be in Design Mode - CATDrawings should all be open in separate windows). Save your documents in the following order:
1. Save all CATParts under their new names
2. Save all CATProducs under their new names
3. Save all CATDrawings under their new names

If you cannot open all documents at the same time, you will end up having to re-link the unopened ones after the re-naming.

 

[mcadjgfrank]

Thank you all for your help.