When I have to change the part name of a drawing and model, the views in the drawing turn into dotted line boxes. What can I do to get my drawing back?
Open the drawing, and in the file open dialog box, I believe there is a 'references' button. Click this and point your drawing file to the renamed part file.
Or, change the names of the files using SW Explorer.
Or, change the drawing file name, open the drawing, open the part file, do a save as on the part file to the new name.
Or, search around here, plenty of answers here on this one.
The reference configuration drop down box is empty.
The file name in SolidWorks Explorer is already changed to the current one. Is there something I am supposed to do here?
What I did was open the part, save as, changed the name. Then opened the drawing, save as, changed the name. Then I deleted the old part and drawing. I believe I closed the part and drawing after I did each save as...
Is it to late to fix my problem? And just start making a new drawing...?
No need to redo anything, you need to fix your reference from the drawing to the part file. The file name is the link of how the drawing finds the part.
So, close everything in SW, do a file>open, you will get the dialog box below. Click on your drawing, then click on the references button. Choose your part file. All should be good.
Keith Rutter: What I did was open the part, save as, changed the name. Then opened the drawing, save as, changed the name. Then I deleted the old part and drawing. I believe I closed the part and drawing after I did each save as...
Next time I'd suggest opening your drawing and going to File > Pack and Go. That's a process that will copy the open file and all it's children, either to a new folder or the same one, depending on which you choose from the dialog box. You can double-click on the file names in the "Save to Name" column in the dialog box to assign a new name to the new files. I believe this will work much better than the method you tried to use.
You need to fix the references of the drawing OR keep your drawing open and then do a saves as on both part and drawing. You can also use SOLIDWORKS explorer to rename/fix references OR pack and go option to rename and create a copy.
If you rename to part or assembly file using Windows Explorer its a pain to fix, even using references. Fastest method is to change the filename back using Windows Explorer then rename using SW explorer:
I didn't read your method til now. Using "Save As" is just creating a copy, doesn't update the drawing (which contains the path to part file). Both drawings were looking for the old name.
I think it does work to some degree if you open part and drawing at same time, then SaveAs the part, the drawing will update the path. I think I blew up an few assemblies doing this years ago but I dont know if it works for drawings.
Drawings, as far as I know, are not referenced by anything so they don't require the same care in changing their filename.
Whenever doing a save as, and their are assy's & drawings involved to be updated, open the dwgs and assy's first.
Otherwise, always rename within SW Explorer.
You can right-click in a view and do a replace of the part.
Thank you for all the responses!
For future reference, what is the fastest was to change the name of a part and drawing without causing any problems? I often have to change the name of drawings, parts, and assemblies. I'm looking for the best/fastest way to get this done right the first time.
Why can't you them correct in the first place itself? If that is not the design intent then use SW explorer.
Depending on the circumstances involved either
the "SaveAs" method where everything is open and then delete the old
the RMB>Solidworks>Rename method if you dont need to open the files. Start at the parts, then assemblies, then drawings.
Caution: I have never found a way to successfully rename parts where virtual parts are used. You have to do something during the SaveAs to update the references but I have never figured it out fully. Procede with caution and backups.
Keith Rutter: For future reference, what is the fastest was to change the name of a part and drawing without causing any problems?
For future reference, what is the fastest was to change the name of a part and drawing without causing any problems?
You can re-name a drawing any time. That shouldn't cause any problems. For renaming parts or assemblies, the method I use is to right-click on the model in Windows Explorer and choose SolidWorks > Rename, as shown below. (I believe you need to have SW Explorer installed to get this option.) That will bring up a dialog box which will show all files referencing this model and a space for you to enter the new name. Keep in mind that I almost always have all my files for each project in the same folder, so finding the relations isn't a problem. If you have files scattered in multiple locations then SW might not find all the referencing files.
Part of the problem is a lot of the parts/drawings I have are older files which were created by other people. A lot of these parts and assemblies are also configurations. Now there i'm using a new data logging software (non-SW) where the names of the parts, drawings, and assemblies may have too many characters to be entered into the data logging software. This is why I have to change the names.
So I can just have the part, drawing, and assembly open while doing a save as and everything will be just fine?
That's what I do. Just have everything open when you change the part name. If you do change a part and later find it's used in another drawing the drawing will show a dashed box where the part should be. Click the dashed box, and the popup will have an icon that will allow you to browse to the file.
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