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Assmbly moved to released folder, now no references 1

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badgerdave

Mechanical
Mar 4, 2011
55
Hi all,

I have a bit of a conundrum. We've recently moved to SolidWorks but neglected to get the PDM.
This hasn't been too much of a problem, we've just handled different revisions the same as with AutoCAD, by adding Rnn to the end of the file name.

We're getting some assmblies completed in SolidWorks now and generally we work on models/drawings in one folder, and when they are ready to be released. We move them to a released directory that's separated into folders by the first three digits of the part number (000 through 060).

We're finding that the assemblies are losing their references and each part file has to be found and re-referenced in the assembly individually. I dread having to do this for some more complex assemblies.

Is there any way around this? Possible to have SolidWorks search a certain directory for the file name? maybe a macro could help?

Any help would be much appreciated. Thanks!!
 
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If you have SW2011-SP4, you can now (at long last) Move files within SolidWorks Explorer whilst retaining references.
 
In my opinion, solidworks is not good at finding files when they have been moved. I tend to keep all of my files in "my documents". One of the worst things you can do is have multiple copies of a file in different location and different revision with the same filename. For example, c:/mypart.sldprt and c:/new/mypart.sldprt.

Did your assemblies and parts go from one folder during development to two or more folders for release? ie, c:/part1.sldprt, c:/part2.sldprt, c:/assy1.sldasm in development and c:/released parts/part1.sldprt, c:/released parts/part2.sldprt, c:/released assys/assy1.sldasm.

if this is the case, and you used windows explorer to move the files, solidworks will not be able to find the parts when the released assy is opened.

google "soldiworks explorer"
and google "solidworks search routine"

now, to actually answer your question, there is a box in tools->options->file locations->external references where you can add all of your released folders. solidworks will search there when it doesn't find a part in the same folder as the assembly.

 
I wish I could give you about 88888 stars for that one.
 
Perhaps if you used "Pack and Go" to move the files to the new directory instead of using windows explorer, you would bypass the problem altogether, retaining references the entire time?
 
CBL and applejack are making a major point in that copies are a problem so you should be concerned about properly moving files. Pack and Go is really handy for bundling a project and sending it offsite to someone outside your system or for working on the files at home (heaven forbid an engineer do work at home). However, P&G is too often misused in a production environment. P&G makes it very easy to copy related files, but in a production environment it makes it too easy.

CBL's suggestion to look into the newly added/improved capabilities of SWX Explorer is your best bet short of using a PDM system. But wait, what level of SWX are you using? SWX Premium and Professional, the mid and top-level systems, include Workgroup PDM. It may not be the ultimate system, but it sure has lot of advantanges over trying to manage the files and revisions manually. You might very well have a better solution available and resident on your system already.

- - -Updraft
 
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