12 Replies Latest reply on Feb 14, 2019 8:04 AM by greghall

    Xpedition FabLink Drawing Editor manufacturing outline

    stempialdo

      Hi there,

       

      If I try to import a board into the FabLink Drawing editor I get an error saying "The board outline of the design, is not completely inside the manufacturing outline".

      This is not actually the case as in Layout (VX.2.4) the manufacturing outline matches the board outline (or I get the same error even if I have extended the manufacturing outline as far as possible, way bigger than anything else in the design).

       

      As a result, the board import into the Drawing Editor is not really successful; it only imports the board outline without any parts, tracks or plane (all layers visibility enabled).

      In fact the component explorer only contains the drawing cell and the board outline. That means I can't create the assembly drawing etc..

       

      Does anybody know what I am doing wrong?

       

       

      cheers

      Flavio

        • 1. Re: Xpedition FabLink Drawing Editor manufacturing outline
          Jackie_D

          Hi Flavio

           

          Several thoughts about this:
          Are there Variants defined for the PCB? If yes, the FL Variant Data must be generated before trying to import the board into Drawing Editor.

           

           

          Even text or something on a User layer that crosses the manufacturing outline will cause the message, so try turning on User Layers as well in Display Control. It may also be worth doing ECO > Reset Cell to ensure that there is no cell placed near the edge where the graphics have been deleted but the cell origin is still placed.

           

          If this doesn't help, open a Service Request and we'll take a look at it.

           

          Regards

          Jackie

          • 2. Re: Xpedition FabLink Drawing Editor manufacturing outline
            stempialdo

            Hi Jackie,

             

            thanks for your reply.

            No, there are no variants defined for this PCB.

            Everything is enabled "loc: All on", plus all the User Draft layers. No luck with resetting the cells.

            The manufacturing outline is a big rectangle bigger than anything else but I am still getting the error message. Ok I will raise a Service Request.

             

            Do you know how to completely remove a cell from the design (with the origin included)?
            If for example I wanted to remove the Fab_Notes that I find the PCB template, even after removing the cell instance from the design in the Cell Editor I cannot delete the cell from the local library (I get the error message "This cell cannot be deleted because it is referenced in the design").
            Is there a special way to delete the instance of the cell so that I can be deleted in the cell editor?

             

             

            Thanks

            Flavio

            • 3. Re: Xpedition FabLink Drawing Editor manufacturing outline
              Jackie_D

              Hi Flavio,

               

              Even a Drawing Cell must be deleted in Place mode to remove it completely from the design.
              Deleting only the graphics of a drawing cell in Draw mode will leave the Cell Origin and reference to the cell. In this situation it is possible to run ECO - Reset Cell and get the whole cell back in the design.

               

              Regards

              Jackie

              1 of 1 people found this helpful
              • 4. Re: Xpedition FabLink Drawing Editor manufacturing outline
                .-.--.--

                Flavio,

                 

                In Xpedition, try running the script found at this link: Expedition/Cell Editor: What's Inside/Outside? It may help identify objects outside of the manufacturing outline.

                1 of 1 people found this helpful
                • 5. Re: Xpedition FabLink Drawing Editor manufacturing outline
                  stempialdo

                  Hi Jackie,

                   

                  thanks for your reply. Yes, deleting graphics in place mode works! Thank you for the tip.

                  I guess I need to be very careful not to delete items while in Graphics mode (otherwise if I do, then the graphic instance disappears and then I am doomed with no way to completely delete the cell).

                   

                  Also .--.. thanks for pointing out to the script; it works very well. Seems a bit of an overly complicated way to delete stuff but, given the above, I now understand why somebody went through the exercise of writing that script. Very useful! 

                   

                  Now there is nothing outside the manufacturing outline, as you suspected I had an "hidden" item outside (text with 0 height far away from the center). But the board import still gives that error.

                   

                  Anyway thank you for your help!

                   

                  Flavio

                  • 6. Re: Xpedition FabLink Drawing Editor manufacturing outline
                    Jackie_D

                    Hi Flavio

                     

                    Even if you delete items in Draw mode from a drawing cell so it is not possible to see where it is placed, you can still use ECO > Reset Cell and select the appropriate drawing cell name to have it refreshed from the local library onto the design and thus available for deleting in Place mode.

                     

                    The InsideOutside script is great for finding items that have wandered off for whatever reason :-)

                     

                    Regards

                    Jackie

                    • 8. Re: Xpedition FabLink Drawing Editor manufacturing outline
                      caleigh_gold

                      stempialdo I hope you found this discussion useful! Has your question been answered?

                      • 9. Re: Xpedition FabLink Drawing Editor manufacturing outline
                        stempialdo

                        Well it is useful to know how to spot a "rogue" graphic item in the design, but the original problem is still there as I keep getting the import error.

                        But I guess that problem is more for a service request rather than the form.

                         

                        But thanks for the assistance, I received good support!

                         

                        cheers

                        Flavio

                        • 10. Re: Xpedition FabLink Drawing Editor manufacturing outline
                          stempialdo

                          Hi there,

                           

                          I think I have found the root cause of my issue:

                          basically even if I change the manufacturing outline to something huge (and I remove anything outside it with that handy user script), I still get the error above.

                          However, I have now realized that the issue is that the import is not using an updated version of the PCB. In fact, even if I move IC's around or even change the PCB board outline, when I import the PCB into the Drawing editor I still see the "original" version of the PCB.

                           

                          That is strange because in the Drawing Editor manual it says:

                          Any modifications to one drawing file do not reflect in other drawing files; however, any

                          changes to a board/panel design dynamically update all drawing files that include that design.

                           

                          This is clearly not working for me (that's why changing the Manufacturing Outline in the PCB had no effect).

                           

                          Any clues? What am I doing wrong?

                           

                          thanks

                          Flavio

                          • 11. Re: Xpedition FabLink Drawing Editor manufacturing outline
                            stempialdo

                            For future reference, if anyone has the same "sync" problem between the PCB  and Fablink Editor:

                            the problem happens if you click "Cancel" in this warning after the import (and also if you tick the box..).

                             

                            So it was my bad!

                             

                            Hope this helps

                            Flavio

                            • 12. Re: Xpedition FabLink Drawing Editor manufacturing outline
                              greghall

                              Think actually the answer to your original question about the parts not being displayed.

                              Is that after opening Fablink, need to select Place -> Upload All Design Data

                              Then all components and tracks will be displayed on the panel.