7 Replies Latest reply on Jul 30, 2009 11:41 AM by Kevin Bouwman

    Plate Weldment -> DXF?

    Terry Raymond

      I have a weldment part file with most of the bodies as waterjetted plates (1/4~1" thick).  I have drawing files that show views of the plates, as well as additional dimensions, views, notes, title block, etc.

       

      What is the easiest way to get clean 1:1 DXF files of each of these plates?

       

      Currently to get a usable DXF, I have to save the whole drawing as a DXF, open it in AutoCAD, rescale it, and remove all the excess notes & lines.  This is incredibly tedious.  What else can I do?

       

      In another program, I used to just right-click the view and chose "export to DXF".  Done!

       

      Thanks for any help!!

        • Re: Plate Weldment -> DXF?

          You could just create an additional sheet, insert your views (you can just copy and paste) then export the sheet to dxf.  Also check your options to ensure that you export the sheet you want and your scale output.  If you ensure that your views on that SW's sheet are the same scale then you can just pick the scale when you export and your dxf will be 1:1.

           

          Lorne

          • Re: Plate Weldment -> DXF?
            Tom Smith

            I used the ExportFlatPatternView API and made this little macro..  It creates the FLAT PATTERN config and saves a dxf in the same directory where the file is.  I made it so detailers can make a drawing of a part they dont have write access to in the vault.  Usually the first step in placing views on a drawing creates the FLATPATTERN.

             

            Run it on the sheet metal part, you don't even need a drawing!

            • Re: Plate Weldment -> DXF?
              Kevin Bouwman
              I create the plates as sheetmetal parts and then use the Export Flatpattern as DXF feature by right clicking on flatpattern in the feature tree.  I can then inport that DXF file directly into the CAM software for the machine that will cut the plate.  I also create drawings of the sheetmetal part for material planning and cost estimating.  Then I use Insert Part in the weldment part to mate the plates to the weldment.  There is a lot of room for improvement in the weldments feature to make this more elegent.  I believe a weldment should be a special type of assembly instead of a special type of multibody part.  This would be more intuitive to me.
                • Re: Plate Weldment -> DXF?

                  Kevin

                   

                  I believe that this is what they were trying to fix in SW 2009 by allowing a cutlist in an assembly drawing.  If you can call up a  cutlist of a weldment that is within an assembly, then you can insert your sheetmetal parts at the assembly level and detail the assembly including the weldment.

                   

                  Lorne