Strange Behaviour? 1

[dedevo]

I did a "Pack & Go" on my model a few weeks ago in order to generate drawings from an unchanging model. However, now that I am already a few weeks in, I have discovered that it didn't pack everything.
When I go to my top level assembly and do a "Find References" it is returning parts and assemblies from the original folder. Without getting into it, this is a HUGE problem.

Is there a way to nuke these references?
Is there a process to "replace" each of the references? Even if it is manual?
And is there a way to get "Pack & Go" to actually "Pack everything and go"?

Devon Murray, EIT [Mechanical]
Solidworks 2011 SP 2.0

 

[CorBlimeyLimey]

How many parts are incorrectly referenced?

 

[dedevo]

So far, the ones I've looked in to, it looks like the assemblies that had features suppressed (configurations) when "Pack & Go" started. All of these assemblies are calling the parts back in the old folder.
The new Top Level Assembly (CW001.sldasm) references the OLD TL ([WIP].sldasm). Now anything that references the new TL has to open the old TL to grab anything (ie. parametrically driven dimensions).

The problem is compounded with assemblies that have subs with multiple configs.
ie. My clamgate mechanism has unique LH/RH hinges. Somehow it saved only the LH config properly:
LH components came over fine
RH components remained behind

I only noticed this problem when I openned a random part to start a drawing for it, and it openned the old model and 5 others.

So far I've found 8 assemblies that have refs to the old folder.


I have about 70% of my drawings completed, but since I didn't notice this before, some of the drawing views are actually referencing the old parts now too! This is a nightmare...



Devon Murray, EIT [Mechanical]
Solidworks 2011 SP 2.0

 

[dedevo]

Here is a SS of my "Find References" for my TL assembly: CW001AM.sldasm
The old TL assembly is: [WIP] .....sldasm (3rd entry in the SS)
There are only 2 folders of interest: Jan 20, and Mar 2.

So CW001AM.sldasm is looking for all kinds of things back in Jan 20.


At this point I have so many drawings done, I might just convert to PDF and continue with the rest, being careful not to change Jan 20 at all. Then converting them all to PDF. This however means that I get 1 generation out of these drawings, and the next generation of the model will have to have it's references fixed. This might mean that part numbers change from version 1-2; which is where the nightmare part of this comes in
Maybe I should contact my VAR?

Devon Murray, EIT [Mechanical]
Solidworks 2011 SP 2.0

 

[dedevo]

Sorry, forgot to attach the SS

Devon Murray, EIT [Mechanical]
Solidworks 2011 SP 2.0

 

[Updraft]

Devon,

Calm down a little; your drawings are not all messed up. The first thing you need to do is determine the current versions of your parts. If you have drawings that are made from what amounts to an old copy of the part files then actually you can refresh them to the current version of the part.

There are several ways you can do this, but the simplest might be to open the current version of the part, then open the drawing file that you have been working on for that part. If the drawing file was pointing to an older "copy" then the filename is the same for the part files. SolidWorks only lets you have one file of a given name open at a time. With the part file open and then opening the drawing for that part you are forcing the drawing to look at the already opened version, thus you have updated its reference to the current version of the part. Now you can "Save As" the drawing to put it in a different (current files) location.

This also works for assemblies, i.e., open the individual part files then open the assemblies that reference them and those assemblies will be pointing to these open part files. Saving the assembly saves the pointers to these file locations.

You still have an issue of files getting moved. It sounds like you need to carefully study Pack and Go and all its options. You should also consider using the PDMWorks.

I hope this helps.

- - -Updraft

 

[dedevo]

Thanks Updraft.

The process works, very manual, but that's the price I pay for not knowing that PnG doesn't drill to every config.

I'm going to have to keep an eye on all of these references now.

Devon Murray, EIT [Mechanical]
Solidworks 2011 SP 2.0

 

[EEnd]

If you rename the original directory, you should get a dialog anytime you open something that is still referencing the old locations. You can then point it at the new locations.

Eric

 

[pdelnet]

This sounds familiar...
see

thread559-222434


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