Hi,
I have a problem on Solidworks that when I open some of my drawings saved on the computer, after few seconds the drawing disappears!! If the software is unable to locate the file then how come in the first place it shows the diagram?! The diagrams are saved on the server. How can I solve this problem?
Any helpful opinion to solve this problem is appreciated!
Thanks guys
I am using Solidworks 2018. How can I check if my graphics driver are compatible with the solidowrks I have installed on my computer? After 8 seconds I can see only a square in the same place I could see the drawing. I try to add the images here I can see.
Sarah Karimi wrote:
I am using Solidworks 2018. How can I check if my graphics driver are compatible with the solidowrks I have installed on my computer? After 8 seconds I can see only a square in the same place I could see the drawing. I try to add the images here I can see.
To answer your question about the graphics card, you can run SWX Rx. Open SWX and in the upper right hand corner click on the house icon and find SOLIDWORKS Rx
When you open that click on the Diagnostics tab. It will tell you about your system and software:
You should do this to find out about your system, but the problem you show is not related to a graphics card. The problem is that the drawing cannot find the file it is looking for.
From the drawing go to File --> Find References. This will show you the name of the drawing file and the name and folder of the part file it is looking for. Then you can check that folder to verify that the part file is not in that folder. That is why you are getting this.
If you DO know where the part file is then open the part file BEFORE opening the drawing. The drawing will then refer to the open version of the part file if it is the same file name it is looking for. Then when you save the drawing it will update its reference location for the part file.
I highly recommend you and your compatriots put all the part and drawing files in the same directory. I'm willing to bet money the problem is the part and drawing files have been moved around separately.
Dennis it was actually helpful to know in general and I updated the graphics driver but the problem of disappearing drawings remains.
Sarah Karimi wrote:
I am using Solidworks 2018. How can I check if my graphics driver are compatible with the solidowrks I have installed on my computer? After 8 seconds I can see only a square in the same place I could see the drawing. I try to add the images here I can see.
You see the squares with the diagonal lines because the Drawing has lost the link to the model. Presumably the model was either moved or renamed using improper procedures. See My Drawing or Assembly can't find dependent files.
Hi Glenn, thanks for the explanation. But what if I don't know under what name the files have been saved or if I don't know where they are saved. You know there are thousands of files on the server and I don't know if their names or places have been changed!
Sarah Karimi wrote:
Hi Glenn, thanks for the explanation. But what if I don't know under what name the files have been saved or if I don't know where they are saved. You know there are thousands of files on the server and I don't know if their names or places have been changed!
Okay, we're getting somewhere here now. Open Start>SW>SW Explorer and navigate to the drawing. Right click on it and choose "Select in Tree". Then select the References tab:
If some of those files aren't linked right they should show up as red or something.
I don't use SW Explorer often, but it is a good tool for something like this.
Hold on...I don't know what shows up in SW Explorer if a reference is broken...It's just a guess that it'd show up in red or something. Anybody know if that's true?
BTW 2019 brings some nice improvements to the external references tool, see attached PDF... Which may also work for this, if SW Explorer doesn't.
And Sarah Karimi, whoever is "renaming" SW files needs to STOP. They can use SW Explorer or Pack and Go, if necessary. But, they need to understand how SW works. Better yet, y'all should investigate PDM.
Well, there is no one who renames or removes them anymore. A previous employee did it before he was resigning from his job to put everyone in a mess! That's why we have this problem!
That's a shame. I wish there was an easy fix.
Ouch! Guess he was not hoping for a glowing reference!
It's a long story, but we had an employee way back that decided to put a bunch of company data onto his personal drive and then delete said data from our network. It was discovered while he was on vacation and we could not find a file. I did a bunch of detective work and found his scheme. Seems he thought it would make him indispensable, turns out it got him fired.
Good riddance to your former coworker, he will get his eventually! Karma does not forget!
Shawn Stugard - lol - that reminds me of one of my jobs.. Prior to leaving I was working on a fair sized project and I always had the latest files on my PC, not the server, because of server issues. So after I left the IT guy upgraded my computer and did a complete reformat without copying or saving the C Drive, sure I got the blame for deleting the entire folder, the blame went away when they asked the IT guy if he made a copy of the drive before he did the reformat.... It was a 4,000 part assembly complete with drawings - plus a few other projects.... Start over time...
This is what happens when companies allow issues to fester and people do what they have to do to work around them. If there are server issues(or whatever) preventing the engineers from doing their job "the right way" and IT or management refuses to fix it since "we are getting by". Then they have no one to blame but themselves for being complacent. I've seen so many times that companies spend big bucks on a piece of software that is supposed to fix a problem or speed up some process, then in the end no one ends up using it because they couldn't figure it out or it caused problems elsewhere. Major changes need a champion, somebody who understands the value and is willing to push everyone else to get to the goal.
Does this happen when you open the file locally?
Sorry for not responding for a long time! I was out of office and I could just come back. The files are saved on the server, however even if I save the files on my desktop then the drawings disappear again after 8 seconds! They disappear only when the file format is in .SLDASM or .SLDDRW but I can easily open and check the files with extension .SLDPRT
I'm getting a feel that drawing still remains open but views are gone an you're seeing a big cross marks in every view. If yes then drawing is not able to locate the model used in that drawing.
Click on File > References and check if the referenced model for that drawing is in correct location or not?
I open the file from server. I also copied the file on my personal account on desktop but still the same problem.
Sarah,
The file has a temporary image of what it looked like when it was last saved, all of the SWX files do. That is what you are seeing initially. But that image is disappearing because the model it is referencing is not where the drawing is expecting it to be.
If you keep the part/assy and its drawing in the same directory then you should have bi-directional opening of the files, i.e., you can open the drawing directly from the part/assy file or you can open the part/assy file directly from the drawing.
The thing is that I have not done these drawing myself. So basically I dont even know the person who has made these files and where he/she saved them in the first place. But only some files have this problem, not all of them.
Did you try and right click the drawing view and opening up the part? If the part opens then add a view in the drawing, it can be off the page. Then select every view, right click and select Show..
If that doesn't work then.....
If you have the part name, open File Explorer and type in the part file name and see where the part is, if the part is deleted and/or moved to another computer, then there is no history or any way to get the drawing image..
Sarah Karimi wrote:
The thing is that I have not done these drawing myself. So basically I dont even know the person who has made these files and where he/she saved them in the first place. But only some files have this problem, not all of them.
To assess who last saved (but not necessarily edited) a file, right-click and select Properties:
On the Security tab, click Advanced:
The owner is the one who last saved the file (unless someone changed the owner using the "Change" link shown:
Kevin
Hey Kevin,
Little correction here, the owner is the one who created the file, not the one who last saved it.
If you would like to see who last saved the file, you can hover over the file and it should pop up
In the screenshot below, ''Propriétaire'' is Owner and ''Dernier enregistrement par'' is ''Last saved by''
I just discovered two new fields available. Right click in the top fields up there. Unfortunately, last saved by isn't available. But, there's now SW Open Time and SW Last saved with is:
The SW last saved with was introduced in 2015 version and Open time was introduced in 2018 version.
And you can set this options for all the folder in your system using the File and Folder options.
Matt Peneguy wrote:
I just discovered two new fields available. Right click in the top fields up there. Unfortunately, last saved by isn't available. But, there's now SW Open Time and SW Last saved with is:
About a month or so ago, these disappeared from my list of columns. Some Windows 10 improvement, I'm sure..
I've scrolled the list, looking to see if they've been renamed, but nothing looks SW-ish.
I do have this column though:
Kevin
I'm still on Windows 7 here at work. I'm guessing it was a windows update that wiped it out for you. If I remember, I can check it at home. A repair on the install may bring it back, if you need the functionality.
Yes, another interesting one you can use is the description one to have your part descriptions show up.
Dennis Dohogne wrote:
Sarah,
The file has a temporary image of what it looked like when it was last saved, all of the SWX files do. That is what you are seeing initially. But that image is disappearing because the model it is referencing is not where the drawing is expecting it to be.
If you keep the part/assy and its drawing in the same directory then you should have bi-directional opening of the files, i.e., you can open the drawing directly from the part/assy file or you can open the part/assy file directly from the drawing.
What Dennis Dohogne Is saying is correct. You have to have the part/assy in the same location as the drawing. If you move all the files to one location and open the drawing it should keep the drawing from going away.
Danny Edwards wrote:
Dennis Dohogne wrote:
Sarah,
The file has a temporary image of what it looked like when it was last saved, all of the SWX files do. That is what you are seeing initially. But that image is disappearing because the model it is referencing is not where the drawing is expecting it to be.
If you keep the part/assy and its drawing in the same directory then you should have bi-directional opening of the files, i.e., you can open the drawing directly from the part/assy file or you can open the part/assy file directly from the drawing.
What Dennis Dohogne Is saying is correct. You have to have the part/assy in the same location as the drawing. If you move all the files to one location and open the drawing it should keep the drawing from going away.
Respectfully disagree, they do not need to be in the same location, they just need to be linked and the only way, (I know), to get the part back into the view is to do like I posted, you need to find the part first..
Ok That is one way also here is a way to see the references with the a drawing and all locations it pulls. In Solidworks go to open. Then select the drawing file the hit the references button.
Then you will see what file it is showing to see where it is getting the info from.
If it is not in the same location. You can hit the replace and replace where it is pulling the part/assy is looking for.
Hope this helps.
John Stoltzfus wrote:
Danny Edwards wrote:
Dennis Dohogne wrote:
Sarah,
The file has a temporary image of what it looked like when it was last saved, all of the SWX files do. That is what you are seeing initially. But that image is disappearing because the model it is referencing is not where the drawing is expecting it to be.
If you keep the part/assy and its drawing in the same directory then you should have bi-directional opening of the files, i.e., you can open the drawing directly from the part/assy file or you can open the part/assy file directly from the drawing.
What Dennis Dohogne Is saying is correct. You have to have the part/assy in the same location as the drawing. If you move all the files to one location and open the drawing it should keep the drawing from going away.
Respectfully disagree, they do not need to be in the same location, they just need to be linked and the only way, (I know), to get the part back into the view is to do like I posted, you need to find the part first..
John, just an FYI there are other ways to change the part file the drawing is referencing, even changing to a part file of a totally different name. This can even be view-specific by selecting a view, RMB and selecting Replace Model. In that dialogue box you can select the views you want affected by the change and then at the bottom you can browse for a new part/assy file and it can be any name and located anywhere you can reach.
There are other ways as well such as when opening a drawing file you can find the Change Reference path and follow that. I have seen many use this approach for making a drawing and then copying it and making the copy refer to a different part file, but keep the drawing complete.
Dennis Dohogne - I think what the OP is referring to or has a question about is that Sarah Karimi apparently doesn't know where the part is... Sure you can replace the model, but that isn't the question, however what you say about finding the Change Reference Path, that would be another way to go...
It is probably going to take hours to transfer all files to one location! but i am going to try this tomorrow! it might actually work!
I tried to use the reference but it still doesn't work! I am not sure if it has anything to do with the name of the file, but the name of the files usually have comma to show different revisions of components. I deleted comma in one of the files and the drawing doesn't disappear anymore so I did it for other files, but it dint work for them. I also updated my graphics driver and it is up to date!
Hey Sarah,
You probably have a bunch of messages blocked to not show again, which includes one prompting you that it cannot find the part for this drawing and asking you to dismiss or to find it manually.
If you've either moved the part, moved the drawing or renamed the folder they were in, this will happen.
I assume some of the drawings and parts are deliberately been deleted. And some of the drawings are really detailed and time consuming so it would take days to re draw them! I am trying to find the best efficient way!
is the auto back up set to keep copies of the parts on systems. I have used this before to find parts that have been removed from a location on the server since we set the auto back up to save to the pc.
THIS drove me bonkers until I figured it out! You'll open the drawing and it skips right over the fact it can't find the parts where it used to be and you get the dreaded blank X views.
Make sure there's nothing in the area shown below that would indicate it's not asking for your input on where a missing part file is
If I were you, I'd remove any blocked errors that speak of rebuilding/updating and the one about external references. I like knowing when it rebuilds and you should always have external references loaded imho. If you don't want them to update then you need to lock them.
if at all possible open the parts and the assembly first and then your drawing should open fine.
file management, is important that files do not get moved or renamed once drawings have been started.
referencing drawings to parts is possible but not always fun and easy.
Sarah Karimi wrote:
Hi,
I have a problem on Solidworks that when I open some of my drawings saved on the computer, after few seconds the drawing disappears!! If the software is unable to locate the file then how come in the first place it shows the diagram?! The diagrams are saved on the server. How can I solve this problem?
Any helpful opinion to solve this problem is appreciated!
Thanks guys
I get this problem all the time. I work in a contract machine shop (job shop). Customers will send me the SWX drawing file but not the model file. If you only need to view the file and not really do anything else, there is a way.
Click open and find the drawing file. Hover over the file then select Quick View from the mode box.
You'll be able to view the drawing but that's it. To be able to make changes to the drawing you'll still need access to the model.
Tony Tieuli wrote:
Sarah Karimi wrote:
Hi,
I have a problem on Solidworks that when I open some of my drawings saved on the computer, after few seconds the drawing disappears!! If the software is unable to locate the file then how come in the first place it shows the diagram?! The diagrams are saved on the server. How can I solve this problem?
Any helpful opinion to solve this problem is appreciated!
Thanks guys
I get this problem all the time. I work in a contract machine shop (job shop). Customers will send me the SWX drawing file but not the model file. If you only need to view the file and not really do anything else, there is a way.
Click open and find the drawing file. Hover over the file then select Quick View from the mode box.
You'll be able to view the drawing but that's it. To be able to make changes to the drawing you'll still need access to the model.
That's great advice, Tony. That view Sarah is seeing temporarily is the same as what would stay there if using the Quick View option you suggest.
that might actually solve the problem for a while! i am going to try it on Monday! thanks! i let you know if it will work. But this is how I should do?
Launch Solidworks -> Part -> Open -> Choose the file and Quick view ?
You can use eDrawings to open/view/measure the models. You can also eDrawings for the drawings as well.
Sarah Karimi wrote:
that might actually solve the problem for a while! i am going to try it on Monday! thanks! i let you know if it will work. But this is how I should do?
Launch Solidworks -> Part -> Open -> Choose the file and Quick view ?
That'll work. You just need to hover over the file icon and then pick Quick view.
Tony,
I had just taken a screen shot of "quick view" but I saw you beat me to it.
It is a really great tool when things go south!
I'm just going to throw this out there because I encountered a problem where certain parts weren't showing up when I projected views. What was really strange was that if I deleted the projected view and projected it again, other random parts wouldn't show. So the behavior wasn't repeatable. The last step I took before I contacted the VAR was to close out of SW, reboot and reopen the drawing. When I did that the problem went away. All I can figure is something got kludged in the memory. So, have you tried restarting SW?
It's a shot in the dark.
Sarah,
Can you post the part and drawing so we can take a look at it?
Danny Edwards wrote:
Sarah,
Can you post the part and drawing so we can take a look at it?
Where's the fun in that! I don't like to solve puzzles with all of the available information!
Kidding aside, if you use File>Pack and Go and pack it up in a zip file, all of the files along with their references will be put in the zip file. Uploading that file should give us everything we need to diagnose the problem.
She hasn't respondedin a day so there's no need to continue trying to help her until she does guys.
Alex Lachance wrote:
She hasn't respondedin a day so there's no need to continue trying to help her until she does guys.
Oh come on Alex, that's not how we do things:
TELEPHONE SUPPORT FOR CAR ! NEED HELP
Though, I would like to know what the final solution was.
Thanks for your understanding Matt Peneguy! Actually I was out of office and I just came back and life can be hectic sometimes so you cant even have an hour for yourself! it was a really chaotic period of time! I like your attitude of no-pressure very nice of you!
Sarah Karimi wrote:
Thanks for your understanding Matt Peneguy! Actually I was out of office and I just came back and life can be hectic sometimes so you cant even have an hour for yourself! it was a really chaotic period of time! I like your attitude of no-pressure very nice of you!
Sarah Karimi. Did the quick view solution work for you?
use "Quick view" to open a drawing without having the Parts or Assy. obviously with limitations.
I also get drawings from Customers or Students, lot of times without the Parts or Assy. this allows me to take a look and print the drawings.
Hello,
Perhaps the assembly files (or their folders) have been moved.
If so, this would break the reference path the drawing uses.
Have you tried searching for one of the missing assembly files, starting at the root drive(s) of your server?
It doesn't take much inattention or indifference to inadvertently drag a folder and drop it somewhere without noticing (unless the folder contained a large amount of data, "large" also being network speed dependent).
Or were the missing files moved to the previous person's local drive? Have you searched their system?
Do you have backups? Old files are usually better than zero files.
Kevin
Sarah,
What are you left seeing exactly ? Does everything disappear?
Have you checked your graphics driver to see if it's up to date and certified for the Solidworks version your using?