We've been having a couple seemingly related frequent, but intermittent problems for a long time. The first one is when we bring a read only part (stored on our network) into an assembly hit save and it crashes. The second one is happens when you have an assembly open with read only parts or sub assemblies in it and you go to measure or mate one of these read only parts (sometimes all you need to do is put your cursor on top of it, or when you're inserting a new read-only part) and we get these repeated warnings saying "Document <network drive>\Partnumber.sldprt is opened for read-only access and is not available for write access. You must obtain write access to this document to complete the operation" <OK button> I understand the document is read-only, but the operation is not something you should be prevented from doing. Most of the time, this message comes up repeatedly (for the same part). You end up having to play whack-a-mole with the ok button...if you can click it fast enough you can get out of the loop and exit the command or whatever is making the message come up. This has happened in several different assemblies and with lots of different read-only files. It's independent of SP and version of SolidWorks. I've repeated the problem in several sp's of 2005, 2004 and 2006. At least 4 people have reported these problems, 2 of which have it happening on a regular basis. We're running XP. It seems to be log-in specific. We've had one user try another person's machine (that wasn't having the problem) and it happened there. We've re-loaded SW, Reloaded their window's profile, switched machine completely, they moved their cube (different network connection) and still the problem occurs. It does stop happening if the individual logs in as and administrator and has full write access to all files. But, we can't have that. We don't have a PDM system so we control permissions by storing files in different folders (a working directory and a controlled directory). Our VAR believes this to be a network/rights and privileges problem. Our IT department isn't sure what to do. If this is truly a Network or XP problem, than I'm having problems finding someone with enough knowledge of both XP and SolidWorks to figure this out. I appreciate any help or ideas. TIA -Christine
I've had a similar problem, although I did not crash, but did play the whack-a-mole game. I had a read only directory which I was using parts out of. That was the problem, SW wants to write a ~.tmp file for every opened assy or part, and wants to place it in the same directory as the part is opened from. The error message was misleading, the fix was pretty simple. Change the directory to read/write for everyone, then "select all" the files within the directory and make only the files present "read only". SW can then write its temp files and is happy. Hope the fix is as simple for you.
Two other things to consider: Under System Options - External References, make sure you check the box next to: "Don't prompt to save read-only referenced documents (discard changes)." Lastly, it is never good to work over a network. FWIW Eddie
Thanks Brian I'll give that a try to see if that fixes it. However, if that's really the problem than we're going to need PDM ASAP. Eddie, Yes we do have that box checked and I know network = bad Not much I can do w/ 20 users and no PDM. Thanks for your advice though. -Christine
Well we finally solved the wack-a-mole problem. It was a system option....external ref/ automatically generate names for referenced geometry was checked on (it's off by default). SolidWorks was trying to rename the faces of the read-only parts when it created a mate and error out. Apparently this setting makes your system very sensitive to read-only parts because it happened when measuring them as well. Strange, but I'm glad that ones over....Thanks VAR! -Christine
