9 Replies Latest reply on May 7, 2014 10:07 AM by Patrick O'Hern

    Working on and off of a server

    Jay Rabe

      I'd try to search for help on this but i dont think it would be that easy. At work we have a few people working on cad at any given time.  We have a cad folder on a server.  The people I work with dont like pdm, so they have Cad/customer folders/project folders/pieces to assembly(s) and a top level folder in where all of the part and assembliy files are for complete models with different configurations.  I'm trying to understand how they do things but keep making dumb mistakes, mainly with the same part # files getting pulled from the wrong places.


      So say they want me to edit a completed assembly thats on the server.  What they want me to do is with solidworks closed, copy the folder from the server to my machine, edit the parts, then when everything is good make revision changes/tracking in the drawings and properties for whatever parts modded and use synctoy (server synchronizing program) to update the server with the revised items. They dont seem to have issues with solidworks freaking out when they do it. The machine I use was recently wiped with fresh Win 7 and SW14 installs but had a few people previous to me using it and possibly setting strange preferences.  It shows files created "by this computer" from years ago when its been wiped a few times.


      Things get ugly for me though. If i copy a folder there is sometimes a folder of purchased items, and occasionally a plumbing or some other folder that the model's parts refers to in the customer folder (im still learning how they do things.) If solidworks doesnt find the required files in the folder it just grabs them from the server wherever it can find them (which i'm not thrilled about because if one of the files i need to edit is actually being pulled off the server its links get all screwed up and i'm working on the "good" part.)  If I screw up its a nightmare. Also, fairly often solidworks also ignores the file i pulled down to my machine locally and uses/references/changes the same file name on the server instaed of localy, same "good" part danger/issue.  Its to the point where i copy a folder to my machine with windows explorer (sw closed,) unplug the network, then open it and solidworks and make changes.  I've had many occurances where when i plug the network back in and try to reopen the model from my local copy it starts grabbing files from the server and the seemingly good local assemblies are referenced all over the place with the wrong parts, broken mates, and its a big mess.


      The worst occurances for me so far have been models partially linked to the server. They seem to overrule the older versions of the same file name in the "correct place" on my machine when trying to open an assembly. Sometimes the old versions overrule the new versions on my local copy too though.  I'm sure i'm doing something wrong, or at least different...  Because of mates and dependancies of different assemblies using the same part they (work) dont change the part # if they make a rev change so its easy to screw up solidworks' links


      Now I'm sure PDM was created to help with issues like this. But, I've been at this job for a month, I'm not going to try to convince them to change how to do things.  So my questions are:


      - Is there a way to limit solidworks to only work in a certain file/files? Say limit it to the customer file and subfolders only?


      - Is there a way to have solidworks ask instead of just opening the same file name in some other location?


      - how does solidworks know where to pull parts from, how does it decide which folder/drive/server to open a part from? This doesn't seem as straightforward as i'd think it would be...


      - Is there something I'm missing that would make this easy?


      - I've tried to replace parts with the part in the correct location. Solidworks says that it wont because it would cause a neverending loop or says i cant replace the part with one of the same name. Is there a way to just point it to the right location of the same file name?  I've had to delete and re-mate anything thats linked to the wrong file location so far which is a nightmare.


      - If you couldnt use PDM how would you make changes on an assembly on/from a server while maintaining a current copy until you're happy with the new one?


      I've never used solidworks off of a server before.  It was always local models and a just go for it approach if something needed changing. I know my backup thinking is part of the issue, I dont know how to dummy proof myself.


      Thanks in advance for any leads, ideas, solutions, etc.



        • Re: Working on and off of a server
          Glenn Schroeder

          Welcome to the forum.  That sounds like a nightmare and you have my sympathies.  I sometimes forget how lucky I am that I'm pretty much a one-man show and I can arrange things and do things how I want.


          With that being said, you'll probably get better suggestions from other people, but my best advice would be to use Pack and Go to bring the parts to your local machine to work on a project, but then getting them back on the server might be a problem if the files are scattered all over the place.  I work directly from a server, and we don't use PDM either, and what I typically do is have all the files for one project in one folder.  For example, if it's project number 690900-2 then we have a folder for that project on the server, with everything related to that project in that folder.  Inside that folder I have another folder named "Drafting".  For simple projects, where I don't expect much editing, all the SW files are in this folder.  For more complex projects, or for ones that will have periodic edits where I don't want to lose previous versions, there are sub-folders, with the date they were started as the folder name.  Pack and Go works very well with this system.  Maybe you could explain your issues and try something like this if someone else doesn't come in with a better idea?

          • Re: Working on and off of a server
            Mark Kaiser

            We don't use any pdm either.


            Here's how we do it.


            Any folders on the server that contain parts/assemblies/drawings, that are signed engineering drawings, only one person can copy files into this folder(s).  CAD users can not copy anything into this folder, they have read only permissions.  The only folders CAD users have write permissions to are hardware files, nuts, bolts, pins, etc., purchased items that we don't manufacture or have drawings on.


            We have a temp folder on the server where CAD users put there finished work.  Once the project is signed off (drawings signed), the manager uploads the CAD files to the proper location on the server. 

            • Re: Working on and off of a server
              Jay Rabe

              Thanks everyone for their input.  I can't have them lock files as read only as we are all swamped with stuff to do. I realize its the safe thing to do though. 2 of us are paper drawings to sheet metal cad guys doing many many new parts per day. The rest of us are creating from scratch and updating models for our stuff.  We have our servers continuously backed up just in case things get really ugly.

              The solidworks video was helpful and eye opening.  I really dont understand why they have it automatically pull from those places in that order.  It seems this would make a mess out of things more often than i've seen people mention it.  How do you know if solidworks has cleared out of ram???  I cant figure out what the benefit of their opening a file preference system is over just prompting you that it cant find a file in the location you specified.  Am I missing something?

              I tried to do a pack and go again today. It was a copy of a "master" assembly that had different versions of nearly the same stuff. It was still linked to its previous versions somehow, any changes i made in the pack and went? file in a sub folder of the parent folder was making changes to the original too.  Starting a new topic for this here called "Different copies of almost the same assembly."


              Today i put the local cad folder on my machine to c:\ and made a folder "ASolidworks" right in C: so its alphabetically the top folder. I was previously working out of a folder on the desktop, so a few folders deep on c:. Moving the cad folder to c: seemed to help a lot.  I was able to work on updating models locally and used synctoy to update the server without issue.


              I still was having issues with solidworks referencing the server when opening a local copy (after having solidworks closed for a few minutes.) The sucky part is that i have to watch while it opens the files to see if it jumps to the server.  If it does I unplug the network cable, shut down solidworks for a few minutes, then reopen the part.  Not ideal.  Why isnt there a clear file references/ram button if you have nothing open in solidworks if they're opening files in this strange preference? This seems like a bad option you need to hunt down and unckeck.

              • Re: Working on and off of a server
                Rick Becker

                Whenever we use Pack & Go we Always use the Save to Zip File: option. We have discovered that this will break all references outside of the files contained within the zip file.


                We have been told that there is a magical 20 minutes after closing a file that SolidWorks retains reference/links to in RAM.


                See if these links help...


                Search Routine for Referenced Documents


                Tools & Techniques for Handling Files with References in SolidWorks


                SolidWorks - How to Repair Broken References


                Good luck.

                  • Re: Working on and off of a server
                    Jay Rabe

                    Thanks for those links! Definitely explained what's going on and gave me some really good ideas on how to make it work correctly.

                      • Re: Working on and off of a server
                        Jerry Steiger



                        I didn't look through all of the links, so this may be a repeat of something you have already learned. You might be able to change a setting and make you life easier. It could be that your colleagues have this setting and that is why you have so much trouble and they apparently don't. Under Tools/Options/System Options/External References, check "Search file locations for external references". Then under Tools/Options/System Options/File Locations, go to "Show folders for: Referenced Documents" and add the folder or folders that you want to keep and find files in on your machine. 


                        Jerry S.

                    • Re: Working on and off of a server
                      Patrick O'Hern

                      If you are still having trouble with files referencing the wrong location, try using File/Open inside of SolidWorks and click the "References" button.  You can look through the list of files and make sure everything is pulling from the correct folder.  If the wrong folder is listed on a particular file, just click on it and type in a new location.  Once everything is set up correctly, open the file and then immediately save it.  That should update all of the references.


                      As Glen mentioned, you should ALWAYS keep your file names unique between projects.  For standard items like nuts, bolts, ect., it's fine to use generic names, and keep them all in a single folder of referenced files.  But anything that is specific to a single job should include that job name/number in its filename and be copied directly into the job folder.   This will save you a ton of headaches as it gets rid of any chances of pulling the wrong files.


                      Another benefit to having the job name/number in the filename is that Pack and Go can easily change all of the files to the new name when copying to a new job.