4 Replies Latest reply on Jun 1, 2015 10:19 AM by Brian McEwen

    Adding and removing a NOT RELEASED stamp to a drawing?

    Frederic Hodshon

      WF - 5-27-2015.JPG

       

      not released.jpg

       

      I need to add a NOT RELEASED stamp to drawings at the PRELIMINARY APPROVAL state and remove it at the APPROVED STATE.

       

      AND create the final PDF at the approved state with drawing/assy/part version and revision levels on the drawing.

       

      I've been digging hard the last week or so, self training. I appreciate the help i have gotten here.

       

      almost there!

       

      fred hodshon

        • Re: Adding and removing a NOT RELEASED stamp to a drawing?
          Frederic Hodshon

          i think i found it - i will try and let you know!

           

           

          Stamping the Workflow State on SolidWorks Drawings in Enterprise PDM

           

           

          • Re: Adding and removing a NOT RELEASED stamp to a drawing?
            Jim Sculley

            Create a note on your drawing template sheet format.  Link the note to a custom property (call it Release Status or something).  Link the custom property to an EPDM variable and manipulate the value of the variable via transition actions.  For example, when the preliminary review transition happens, set the variable to 'NOT RELEASED'.  When it passes approval, set the variable to a single space character.

             

            I question the need for this giant note though.  You already have NR in the title block.  You shouldn't need to plaster 'NOT RELEASED' across the entire drawing.  People should be trained to not work with drawings that do not have an actual revision number/letter.

             

            Putting the revision/version (not sure what the point of having the version would be) in the BOM will require yet another variable linked to a custom property.  In my setup, the variable is TB_REVISION (title block revision).  It is linked to the revision annotation in my title block and it is kept synchronized with the EPDM file revision via transition actions.  You can add a column to your BOM template that also points to this custom property.

             

            There is one very big caveat when you put the revision of the parts on the BOM.  If you don't have a formal ECO/ECN process, people will revise the part and not rebuild all the drawings of assemblies where the part is used.  If you have generated PDFs, they will show the wrong revision for the revised parts compared to what you see when you open the SolidWorks drawing (the drawing will update when opened, even though you may not be able to save the changes).  Until you open the drawing, rebuild it, save it and regenerate the PDF, things are out of whack.

             

            We don't have a formal ECO/ECN process here, so to alleviate this problem, we don't put BOMs inside the drawing border. Thus the generated PDFs will not show bad data.  So how do we see the BOMs?  I wrote an add-in that lets users right click on an assembly model, assembly drawing or PDF of an assembly drawing and click 'Print BOM'.  The add-in will compare the revisions of the parts in the EPDM BOM with the revision column of the SW BOM saved in the drawing and flag any items that don't match.  The add-in then exports the BOM data into a nicely formatted Excel spreadsheet ready for printing.  The items that don't match are bold and red so they stand out.  Consumers of the BOMs know to contact Engineering when they see this so that we can update the assembly drawings.

             

            Jim S.

            • Re: Adding and removing a NOT RELEASED stamp to a drawing?
              Steve Zema

              Frederic,

              I've been requested to add watermarks to drawings per states also.  The process mentioned is the correct method.  But, I did find a bug in it.  When the drawing is opened in eDrawings, the watermark will be over the geometry and in black.  I've notified my VAR, and he has placed in a fix request.  It seems that eDrawings 2015 does not support this function, but eDrawings 2014 did.

               

              What you will have to do in the meantime, is to notify your users when they print from eDrawings and/or the EDPM preview window, that they need to set the print color from black & white to color greyscale.  This will lighten up the watermark, but will not place it behind the geometry.