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How can i stop showing " a document named " xxxx" is already opened" when opening an Assembly

Question asked by Jakob Arent on May 6, 2013
Latest reply on Aug 20, 2018 by P. Farnham

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Hello,

Need some help with an issue when opening an assembly in solidworks. After changing the numbering system i have some trouble to open an assembly. The message " document named "xxxx" is already opened, do you want to show this already opened document?" appears too often.... I don't have a problem to click on yes..... but because my assembly has many of the same part the message pops up many many many time. To open the assembly i need to go through many (100) click. And that is frustrating.... The thing is not evey multiple part is doing that just two or three "special parts" seem to have that. Tried to clean the session and rename part. Even deleted one of the parts and created a new part... But it is still doing that. Is somebody able to help me?

Thanks

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Glenn Schroeder May 6, 2013 12:50 PM
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Hello Jakob,

It sounds like your assembly may be referencing more than one part with the same name. You might try making a new folder, then when you get your assembly open, do a Pack and Go operation (File > Pack and Go) into this new folder. That will copy your assembly to the new folder, along with all the parts and assemblies that it contains. If that works OK, then use this new assembly instead of the old one.
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Dean Baragar Jun 24, 2013 9:01 AM
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This has recently started to happen alot for us as well. I searched our entire network and there is only one copy of the parts that it asks about. It also happened when I first opened my model, and I clicked "no" to every part, then closed and reopened, and everything worked fine. So it doesn't seem to be a problem with the actual parts, and its a different part each time.
It also seems to be a recent problem (maybe May or even June), but my coworkers are still on SP2, and it started happening to them around the same time, even though their computers haven't been updated. Could it be possible that my opening a part with SP3 is not compatible with their SP2 and vice versa. We will try to update their computers and see if that helps.
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Justin Green @ Dean Baragar on Jul 3, 2013 9:44 AM
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I am in the same boat as you are. I only have one part file that is used in several different assembly models. These assemblies are then used to create a final assembly of the piece of equipment being made. It becomes extremely annoying when there is nothing different about the part files, their locations or anything else. It is happening on all of our computers here. Originally we thought that someone had the same part file open elsewhere, but that is not the case. It would be great if someone from Solidworks could at least come up with an explanation for why this is happening.
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John Burrill @ Justin Green on Jul 3, 2013 11:00 AM
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I haven't seen this happen. I'm on SP4.0EV. It sounds like a combination external reference types is confusing SolidWorks.
For example, if you have widget with in-context references to a phalangie in a blammer assembly and also the same phalangie in a plopper assembly, Solidworks might go into a periodic cycle of loading the widget and the phallangie as blammer assembly references and then load the external referneces of the widget which includes the plopper assembly which includes another reference to the phallangie and instead of using the phallangie in memory, it tries to reopen it. It might do this for every reference of the widget to the phallangie or even every feature in the widget with an incontext reference until the rebuilds converge.
So that's a working hypothesis that matches the symptoms. It could be wrong, but the process of establishing that it's wrong will probably reveal other clues about what's going on.
The next step is to figure out the topology of the assembly. The best tool I know of for doing that is the save and check-in document dialog of Workgroup PDM. This gives you a tree structure of all of your assembly references and called external references and their nested tree structures, so you'll be able to identify recursion. You can export that to a delimited text file for future reference
Look for instances of parts appearaning in the assembly tree and the external references tree of an assembly component. See if breaking those external references helps.
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John Burrill @ Justin Green on Jul 3, 2013 11:14 AM
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Another possibility occured to me.
If you recover a virtual component from the SolidWorks back-up directory and load the assembly containing the virtual component, often it will not store the component in the assembly despite it having the nomenclature <#assembly name>^<#component_name>.sldprt, it will be stored outside the assembly and check into the vault with that name and do all kinds of crap that virtual parts shouldn't do. If that happens and you make a new virtual part with the same name: like <#assembly>^<part1>, then I could see SolidWorks alternating between the recovered part and the virtual part which is unpacked to a temporary folder when the assembly is opened. With SolidWorks going back and forth on that, it might throw dialogs like the one you talked about.
If that's the case, you need to rename the recovered virtual part.
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Justin Green @ John Burrill on Jul 3, 2013 12:00 PM
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Your first scenario makes some sense, however all the parts are individual parts with no in - context references. I can open one assembly that contains four parts that are also in a second assembly. If I were to then open the second assembly, this message appears for each of the four parts that are also in the first assembly. We haven't changed anything with how the parts or assemblies are created. All the parts that Solidworks says are already opened, technically are opened, but shouldn't affect the opening of the assembly.
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Scott Harvey Jul 4, 2013 5:31 PM
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To be blunt, you have two files named the same thing in two different locations.

If they are supposed to be differnent, then name them different names.

If they are supposed to be the same you need to investigate. SW is telling you they are different files. Look at the references. You will find that one is located on your desktop and the other is somewhere else. They could be the exact same part from the geometry to the file properties to the document properties but since you copied the file ( probably pack n go ) then there are now two seperate references for the same part.

If this is not it, then upload your files here. Start with a new session of SW and recreate the problem. Once you found the right two assemblies to create this problem pack n go those two assemblies. If they are too big then zip them and provide the drop box or google drive location.
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Dean Baragar @ Scott Harvey on Jul 11, 2013 3:19 PM
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Hi, I searched my entire network, and there is only 1 file with the name that comes up. I know that multiple files with the same name is bad, and since I've been here, have been cleaning up some of the older stuff that was done that way, but these particular parts have only 1 copy.
Sorry for replying so late, I've been out of the office for 3 weeks.
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Thao Dang Aug 14, 2013 10:19 AM
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Try this to see if it works for you. Go to System Options--External References--Load referenced documents and select "None". I had the same problem and this worked for me. Good luck.
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Anthony Green Oct 17, 2013 5:40 PM
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I agree with the original post. Yes: there may be a refence issue. No: I don't care when I'm in a hurry. A 'yes to all' (this session only) check box would be most helpful
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Nigel Bennett Nov 8, 2013 4:20 AM
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We are having problems with this, too. If I change configurations of an assembly it seems to think the blasted parts files used in the original configuration are stored somewhere different from those in the new configuration, and I'm spending ages, clicking the silly button like I'm shooting space invaders. WE HAVE NOT MOVED OUR FILES AND THERE'S ONLY ONE COPY OF THEM ON THE SERVER.

Anthony's request for a "yes to all" button would be a brilliant idea if the original problem of why SW thinks there are different parts cannot be solved.
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John Lhuillier @ Nigel Bennett on Nov 8, 2013 8:02 AM
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This seems to be an issue that was started in one of the service packs in 2012. We've run into this as well & all of the files that it is trying to open are within the same folder. We get this a lot with standard hardware that we've placed into the assembly file from the standards folder we have & then save them into the job folder. Almost seems like Solidworks is placing a map in the folder to pull files from the original place they were pulled from first rather than the folder that it is currently saved in. I do see in 2014 they added a tick box in that dialog to not ask again.
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Nicholas Martin Nov 20, 2013 9:36 AM
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We have ran into this issue a few times over the past couple weeks. at first i honestly thought it was a user issue, because i never had the problem when i opened up the assemblies on my computer.

but it turned out that it wasnt a user issue. it was a issue with our file locations and names. We had a few parts that would create this pop up. my suggestion would be to investigate the file locations manually via right clicking and viewing the part properties. for some reason when i checked the references with the file/find references command, the parts showed up in the same location. but when checked manually via right clicking on the part and viewing the properties, the locations were different. once i updated the file locations manually, my problem was fixed. hope this help all of you.

2013 sp5
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Rick Sink Nov 20, 2013 12:59 PM
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We have had this same issue. We run SW 2013, SP 4.0. We "fixed" it by changing the threshold for Large Assemblies...Tools/Options/Assemblies/check Large Assemblies and then enter a number smaller than the assembly that's giving you a problem. This will force the assembly to load lightweight.

This is not a real fix in that I think the only reason it works is that parts are not being totally loaded and their paths, if they are different, are not being detected by SW.

Digging a little deeper into this, in the assembly, you can RT-CLK on a part that is giving you trouble, then select the Component Properties icon for the part. The dialog box that pops up will show the path to the part. When we did this, we found the same part had different paths. But it was even more subtle than this. Below are two paths for the same part that appear to actually point to the same locations...

\\mainserver\share\R&D\CAD\WIP READERS FLAT FOLDER\HDW0018.SLDPRT

S:\R&D\CAD\WIP READERS FLAT FOLDER\HDW0018.SLDPRT

Both these paths are on our network, and the part only lives in one place, but SW thinks there is a slightly different path designation, depending on which occurrence of the part one is looking at in the assembly. I don't know whether this is a SW problem or a problem with our network configuration or setup. I'll have to leave this to others to figure out.

Hope this helps.

Rick
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Jim Pazen Nov 21, 2013 10:47 AM
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>>>Hi, I searched my entire network, and there is only 1 file with the name that comes up. I know that multiple files with the same name is bad, and since I've been here, have been cleaning up some of the older stuff that was done that way, but these particular parts have only 1 copy.

When we started getting these messages, I went through and made d@#*ed sure I only had one source file for the parts showing up. These all come from one location. There are no duplicate file names.

Next time I went to open this same assembly, a DIFFERENT component gave me the same message. I've been using SW since the year 2000, have never worked in a company that had EPDM, and have never had this problem before. The products we make are snowflakes, very similar, but never exactly the same. They all use use these common parts/assy's.

This is a new "undocumented feature". My favorite help desk tech at my VAR (who is pretty d@#*ed sharp) cannot find a solution, other than "Buy EPDM". Not an answer my bosses will accept. I can't do a pack and go on all these files, I'd end up with 50 folders with 50 common part files, plus all the duplicated hardware. Not acceptable.

SW needs to find the cause of this bug and fix it. NOW. It never happened before the later SP's for 2012, and continued into 2013. If this never hapened for over 12 years, why is it happening now?

Jim
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Justin Green @ Rick Sink on Nov 21, 2013 11:01 AM
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This is the conclusion that I have come to as well. I have began noticing that the filepath that Solidworks will use to open a part will vary between the network location, and the local location, even though the file is local. It's hard to understand why Solidworks would go through the network location to open a local part. I am hoping there is a simple solution to this.
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Nicholas Martin Nov 25, 2013 11:19 AM
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update on our assembly. the problem is back, but it only shows up for our one user. anyone else who opens up this assembly, opens it just fine, no errors at all. the file locations show the same on all the parts. checking his settings and will see how this goes.
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Rick Sink @ Nicholas Martin on Nov 25, 2013 11:31 AM
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Check his load lightweight settings...see my previous post. In my case, for a largish assembly, changing the threshold from 500 parts to 1500 parts "solved" the problem. Of course, you have to be loading lightweight to begin with for this to work.

I have still not come across a root cause fix for this problem to eliminate the UNC drive versus mapped drive references to the same part in the same folder.

Rick
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Jim Pazen @ Rick Sink on Nov 25, 2013 12:21 PM
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That might help if we were using lightweight mode, but we're not. Next contestant, please...
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Mark Glover @ Jim Pazen on Feb 17, 2014 11:37 PM
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As Rick says it is definitely a mapped drive problem. The simple fix is to simply delete the mapped drive folder and put the shortcut to the network folder somewhere else so it is not assigned it's own drive letter.

In our case we had to redo the file locations for templates as they are in the network folder and that was it. Now instead of going to X:/drawings we go to C:/drawings(server) - Shortcut. The extra click of going into C: then the folder is well worth it for the hundred clicks saved when we had to open an assembly.
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Jim Pazen @ Mark Glover on Feb 18, 2014 10:44 AM
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>>>As Rick says it is definitely a mapped drive problem. The simple fix is to simply delete the mapped drive folder and put the shortcut to the network folder somewhere else so it is not assigned it's own drive letter.

Thanks for the input, but if this is a mapped drive problem, why did it never show up between 2000 and 2012? This is a bug in the software, that every time I apply a new workaround, finds a different way of exhibiting itself. It's long past time for Dassault to man up and A} admit there is a problem in the code and B} fix the D@#$ code. As I said before, I've been using SW for 14 years now, and never had the problem until the later SP's of 2012. We spend too much money on this product to be expected to jump through hoops to cover their butts so that they don't have to fix their bad code. That is not only unacceptable, but deeply unprofessional. I realize that it might cost the shareholders .00001 cent each to fix. Tough. It's time to take care of the customer. Do it. NOW.
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Bruce Goodell @ Jim Pazen on May 13, 2014 1:31 PM
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I've only noticed this when we upgraded to 2014 for some reason. I am not sure if this is the issue or how to fix it yet, but I have an assembly with multiple configurations. The difference in the configurations is mainly a particular subassembly. each one of these subassemblies has identical parts, except for maybe a few, like longer posts....etc. It happens more often when I open a drawing referencing each one of these configurations. I looked up the properties on one of the parts that were popping up with an already open dialog box. The first configuration was fine( F:\engineering\.....). However, when I check one of the other configurations with that same part it was showing (\\Goliath\engineering\.....).

I am curious if SW is thinking those are 2 seperate locations when in fact they are the same location. My drive has always been mapped the same and we have never allowed solidworks to locate files directly through the network like that. At least to the best of my knowledge anyway.
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Jerry Steiger @ Bruce Goodell on May 16, 2014 9:10 PM
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Bruce,

It would probably be a good idea to show this to your VAR. You may have discovered a particularly insidious bug.

Jerry S.
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John Lhuillier @ Bruce Goodell on May 18, 2014 10:10 AM
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I don't think it's a mapped drive problem. This started back in one of the 1st couple of service packs in 2012. We don't work over a network with SW files & this happens to us a lot. The only thing they've done to fix it is to add the Dont ask again tick box when the prompt comes up.
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Jim Pazen @ Jerry Steiger on May 19, 2014 10:37 AM
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Jerry, please read the rest of the thread. Several of us have been working with our VAR's, to no avail. This is a nasty little "undocumented feature" that is obviously hard to troubleshoot, since it appears in one place, but not another, or, once fixed for one part shows up for another. If nothing else, read my posts, they'll bring you up to speed on this.

I see you've posted a lot, so you probably have some pretty good knowledge and are helpful, but c'mon friend, get the full picture before jumping on the simplest solution -- Pass the buck -- At least two VAR's and support people at SW are very aware of this. I've worked with a very sharp support tech and spoken to SW about this.

I'm always a rotten SOB on Moday mornings, and a wise@&& in general, so please take my rant with a grain of salt...but do read the whole thread. You may discover the answer, and a means to perpetual motion, just by spending the few minutes required...

Jim
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How can i stop showing " a document named " xxxx" is already opened" when opening an Assembly

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