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
Does this happen when you open the file locally?
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?
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.
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.
I open the file from server. I also copied the file on my personal account on desktop but still the same problem.
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.
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.
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..
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.
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.
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..
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.
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.
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.
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...
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.
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.
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!
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?