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Rename multiple files

Valued Contributor
Valued Contributor

I have a project that was done in one large assembly per customers request. Now that they have the files of the assembly, they find that they are unable to work with the large file and want to break it up into separate sub assemblies with the drawings. The problem that I have is the file structure is such that the first part of file name is the tool number. When this gets broken up they are going to have separate tool numbers for each of the subassemblies. Is there an easier way to rename files and maintain the associativity between the files than doing a save as & saving to a new file name. Solid Edge has the Revision manager that works great for this & Solidworks uses their SW Explorer to allow you to do this easily.Is there something like that for NX

8 REPLIES

Re: Rename multiple files

Siemens Phenom Siemens Phenom
Siemens Phenom

An alternative to using Save As would be to use the Create New command to create the new Sub Assemblies and then copy/paste and drag/drop the sub-assemblies/components within the Assembly Navigator to build the desired structure(s). Either way you're going to have to deal with associativity issues.

Ben

Note: for any new users reading this thread - please do not rename files using your OS. Instead use "File > Save As".

Re: Rename multiple files

Siemens Phenom Siemens Phenom
Siemens Phenom

Another option for this is to use Assembly Cloning. If the entire assembly starts with the same characters now it maybe easiier to clone each sub assembly on it's own and go back to the original top level and do a substitue..

 

Scott

Re: Rename multiple files

Phenom
Phenom

When it comes to assembly restructuring, I find NX is very limited and primitive compared to other software you mentioned. I’ve submitted many ERs in this issue.

 

To rename the assemblies and components I use” Make Unique”, since it’s straight forward. But it breaks all the links. Then you have to go through the components and re-link them back. If you have only couple of links, it’s not too bad.

 

I think your best bet is “Save As”. I don’t know if you know the following:

 

  1. Expand the Assembly Navigator
  2. RMB “Descriptive Part Name” column and Select “Export to Browser”
  3. Make a bottom level part (a renaming part) “Make Work Part” (NOT “Make Display Part”)
  4. File->Save As
  5. Give a new file name to the current working part (#3).
  6. Very important: Follow the “Cue Line” and give step by step upward the new names as requested. If you don’t want to rename, press “Cancel”
  7. No support for new file names given from NX.” Just Blank”! Hence use the list exported #2 to copy and paste.

 

If you follow these steps you could rename and preserve the associativity.

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: Rename multiple files

Experimenter
Experimenter

I think BatchRenameFiles Tool is the best tool which can easily rename multiple file.
You cn find it by useing google search- BatchRenameFiles Tool  

Re: Rename multiple files

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi @jonathanf345,

 

The BatchRenameFiles tool should be avoided at all costs.  NX part files should not be renamed using the OS, or tools that batch rename using OS commands.  NX relies on internal identifiers that do not get renamed unless NX is used to rename the file.  Using a tool like the one you have proposed will leave the internal ID's out of sync with the filename and cause problems with assemblies and interpart associations.  You have been warned.

 

Regards, Ben

Re: Rename multiple files

Phenom
Phenom
Hi,
I suggest you for rename Nx file, the clone command with the rename option.
Thank you...

Using NX 11 / RuleDesigner PDM

Re: Rename multiple files

Experimenter
Experimenter

Cloning was designed exactly for the purpose you have described.  You can choose which files to copy, which ones not to copy, and it prompts you to rename them - all while keeping the relationships.

Re: Rename multiple files

Experimenter
Experimenter

All the new bells and whistles NX likes to add with each release they have yet to fix the simpliest tools that would help designers.  Copying a job because it's similar is a valuable cost saving option.  But whether you use "save as" or "make Unique" there are issues.  Unique option is only god for unlinked parts.  Save as- randomly breaks links (especially bodies) and than you are from that point on plagued with internal errors, constant model updates and out right NX crashes.  Siemens needs to polish its tool before expands its abilities.

 

-Wishing I could go back to NX7.5