7 Replies Latest reply on Oct 26, 2016 9:24 AM by Andy Sanders

    Drawing missing details

    Darren Wrighton

      I have some older Solidworks parts and drawings. The problem is that when loading the already created drawing, i get this below:




      As the drawing is loaded the correct images flash on screen momentarily and then disappear leaving these boxes. These drawings have been moved from their original location.


      Any help much appreciated.

        • Re: Drawing missing details
          Glenn Schroeder

          The drawing has lost it's reference to the model (or models).  If you can find the models, open them first, then open the drawing.  That should fix it.


          That's assuming moving files is what caused the lost reference.  If the file names changed then it's more complicated.

          • Re: Drawing missing details
            Josef Kasik

            Please follow these steps:

            1. SolidWorks menu File > Open

            2. In the Open dialog you shoul locate the drawing, then only one click on this drawing

            3. In the Open dialog you should see the Refrences... button, click on it

            4. Now, you should see the drawing references on lost models

            5. Double click on models and try to find new location with a new file names of lost models

            6. Click OK

            7. Open the drawing with new references

            • Re: Drawing missing details
              John Stoltzfus

              If you know the part file, then open it and split the window in your screen and drop in the part from the open file, select all the views and right click "Show"



              If that works just delete the view that you inserted and re-save the drawing file..


              If you don't know where the part is - then it becomes a lot more complicated

              • Re: Drawing missing details
                Andy Sanders

                Check Options-->System Options-->Messages/Errors/Warnings


                You may have run into the situation before where it throws up a warning opening a drawing and it couldn't find the parts.  You may have hit "Suppress" option and then hit the check box to never show the Error box again.


                Now, instead of asking you to locate the files it cant find, it just blows by and suppresses them anyway and presents you with those blank boxes with the X in them.


                Check to see if you have any of that kind of dismissed error lurking in that System Setting location.  Find it and pick the check box next to it.  This clears your "never show again" choice and you should see a box pop up next time you open the drawing.


                This has happened to me before and I learned this the hard way!