Referenced part

[ctopher]

Help. I have a dwg that has referenced a part. The assy on the dwg does not use or reference the part. Every time I open the dwg it says it can not find the part and asks me if I want to find it. I click on no and save it, but does it again when opening. The assy does not do this. I tried support, but they don't know. Has anyone had this problem before? How can I fix this?
thank you

 

[MrPickles]

No hidden views on the drawing that may reference the part. That should be the one way that the DWG would need it and the ASS'Y wouldn't.

I think even if you say NO, it will ask again because it doesn't just delete it, it just doesn't load it.


-----------
Mr. Pickles

 

[RawheadRex]

If the drawing is referencing a part, then simply selecting "no" and saving is not going to have any effect.

I suggest browsing for the part (instead of clicking "no&quot the next time you open the drawing. Once the drawing is up then you're going to want to aggressively browse through the feature manager tree in the drawing file to figure out where the part is referenced.

Other things I would ask myself:

Are there multiple configurations in the assembly model? (If so perhaps that is an avenue to investigate.)

Do any of the components in the assembly have a Base Part associated with them?

Are there any sub-assemblies among whose children the offending file resides? If not then ask the first two questions about any and all sub-assemblies?

Realistically, the drawing isn't going to prompt you for a missing file if there isn't a legitimate reference or a bug that's been heretofore unheard of (which begs the question what version of SW are you using currently - if it's 2004 then maybe it is a bug). There's little doubt though that a legitimate reason exists for you to be prompted as you've described.

Good Luck,
Chris Gervais
Sr. Mechanical Designer
Lytron Corp.

 

[ctopher]

No hidden views, but there is section views and broken out views....and other views scaled up from the broken views.
Any suggestions how to fix the problem? The dwg is too complicated to re-draw.

 

[ctopher]

I am using SW 2003. The part it is looking for does not exist anymore. I deleted it hoping it would try to fix the problem. It thinks one of the parts used in the assy is referenced to it somehow, but when I open the part...it's not referenced to it. The only time I see a msg relating to the 'deleted' referenced part is when I open the dwg, or check-it in to PDMWorks. I have tried all avenues, but can not find any link somehow to the referenced part to stop it.

 

[meintsi]

Check your assembly...

See if you have a suppressed part in one of the drawing views with a bad (deleted or changed) configuration name.



Remember...
"If you don't use your head,
your going to have to use your feet."

 

[RawheadRex]

"I am using SW 2003. The part it is looking for does not exist anymore. I deleted it hoping it would try to fix the problem. It thinks one of the parts used in the assy is referenced to it somehow, but when I open the part...it's not referenced to it"

Did the file you deleted have any kind of in-context relations within it (i.e. sketch geometry created within the assembly environment)? If it is a derived part or a base part related to something in your assembly that would cause what you're seeing to happen. Based on your latest post I suspect that is the case.

I suggest restoring the model you deleted if possible and interogating it extensively along with the model in your assembly. Look at every sketch relation individually and check entity ID's and stuff like that. Start with External references as that is where you're most likely to find the problem.

FYI when you run into these kinds of issues I can't stress enough that is NEVER A GOOD IDEA to delete files. That actually can make the problem worse and potentially unrecoverable (I have seen it happen).

Good Luck,
Chris Gervais
Sr. Mechanical Designer
Lytron Corp.

P.S. I'd be happy to look at the specific models and give you a hand if that's reasonable for you to do.

 

[TheTick]

Is this the same file from the post you started last week?

All this machinery making modern music can still be open-hearted.

 

[ctopher]

Yes Tick. The file has been opening/saving slower...trying to solve what is going on.
Chris, The part was created in an assy, then saved as a copy, assy references were broken (and a new part was created). The part in the assy was replaced with the new one.
One more thing, the assy is 97,314kb, the dwg is 32,635kb. I don't know how many parts...maybe approx 100. Should these files be so big? Is this common? I once saw a maco somewhere that will compress SW files, but don't remember where I saw it.
thanks

 

[RawheadRex]

Sounds like the references weren't entirely "broken" (I know you're thinking "what an epiphany....why didn't I think of that?&quot but I might have an idea of how to solve your issue. Is there any reason you can't recreate the geometry in a new file without any in-context features, then replace the offensive part with the new "clean" version in the assembly? Afterward you can add any necessary in-context relation to the new part.

Sometimes the best thing to do is simply perform surgery and transplant. Without seeing the file firsthand it's hard for one to say "here's how to fix this" but I'm guessing that your file is corrupted.

Regarding the compression of files, there's a really cool utility called ECOSqueeze (I forget the website) that does a great job crunching files down to a manageable size. It's free and I have used it extensively (along with a few others here on this board) without encountering any trouble.

One additional question regarding the "lost file" if I may, how exactly did you break the assembly references?

Chris Gervais
Sr. Mechanical Designer
Lytron Corp.

 

[testy]

ECOsqueeze is available at

http://www.ecocom.com

 

[ctopher]

Thanks everyone. It's seems so far I was able to fix the problem. I saved as a copy of the dwg and assy as a new name, save a copy of a new part that was being referenced, then downloaded Ecosqueeze. The dwg now works faster, it doesn't ask to look for the ref part, and rebuild lights go away (they stayed on before). wow!
thanks again to Chris for suggestions too

ctopher
Sr Mech Designer