File Reuse and Rejuvenation

[EDCSRPM]

Is there a limit to the reuse of files?

We have been reusing files as the starting point for new designs since around 2005. At each reuse, changes are incorporated to take advantage of the latest NX functionality. As you may imagine, these files now have expression P values in the 10-30K+ range. All along we have used part clean up and manually ensured that the files are kept as streamlined as possible.

Lately we have begun seeing very odd issues arise of which there is no good rational to explain. Internally we are discussing defining and implementing a ‘file rejuvenation’ process. I would like to hear what others have to say on this topic.

Does Siemens have a suggestion as to known limitations and best approach to rejuvenate files?

Currently running NX7.5 going to NX9 4th quarter

 

[cowski]

What type of problems have you been having? If you can duplicate the problem consistently, send it to GTAC to have them take a look.

www.nxjournaling.com

 

[looslib]

New designs should start with a clean template at the latest release. This is the ONLY way to insure you get a clean file.

You are not alone in this. I had a user come complain that he had to always change the decimal places on angular dimensions to zero places. I opened a new file, created a sketch, extruded it, then opened a new drawing. My angular dimensions came in with zero decimal places since the company defaults had been set that way 3 years ago. He was using an old file to start a new file from.

In the long run, you save no time by modifying an existing file over starting a new one.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

If you're talking about reusing files which already contain models but which are simply modified and then saved with a new part name, that's not a problem in and of itself, but if this is a serial activity, in that a part may represent several generations of modifications and doing a Save-As, then there might be something to your concerns. The part cleanup is a good idea (make sure you set the various 'remove unused' options) before doing the 'Save-As'. If this get particularly bad and you want to at least save the solid/surface models and their feature structure, you could do a 'Cut & Paste' or..

File -> Export -> Part...

...and select the bodies of interest and Export (Paste) them into a NEW clean file. Now the only issue here would be that all of the expressions moved with your bodies/features, their names would be 'hashed' to make sure that they're unique, but there are ways of cleaning that up as well (I've got a GRIP program which will convert the unique expressions back to their original names).

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[EDCSRPM]

We are reusing files that contain model geoemetry that is driven by WAVE links from a top down control structure. As you suggested John, we were already looking at the file>>export option and have found the expression and WAVE links as challenges too.

Based on my work in CheckMate checker development it seems that NX holds on to a lot of "background" data such as geometry and other things off on layers outside of user access. Part clean-up doesn't seem to clean all of this.

Between the file>>export option and the Copy>>Cut>>Paste option does anyone have experience as to which results in a cleaner result.

Thanks for all the replies! It is always good to gain the experiences of others.

 

[JohnRBaker]

The 'Copy & Paste' is probably cleaner if it's ONLY the geometric objects that you wish to retain. If you would like to also retain things like Layer Categories, User-Defined Views, Part Attributes (if you've set them so that they are allowed to be copied), etc. then the File Export/Import might be better for you, but as you've already noted, some extra 'baggage' may come along for the ride as well.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.