7 Replies Latest reply on Jan 22, 2011 6:51 AM by robert_davies

    cell creation problem

    richard.gale

      I am trying to create a new cell for a new part.  In Part Editor->Pin Mapping->Symbol/Cell Preview, both the symbol and cell layout are there. But when I place that device in the schematic, I assign the cell but the view of the cell layout does not show up in the window. I could not create the related PCB file of that schematic file. The forward annotation failed.

       

      Is there anyone who can tell me why that happens?

       

      Thanks,

        • 1. Re: cell creation problem
          Andreas.Schaefer

          Hello Gale,

          you didn't explain wich tools you are using, so I suppose, you use DxDesigner and DxDatabook?

           

          When you select the part in DxDatabook, do you have a column wich contains the Cell Name too?

          If not, I could be a bad DxDatabook configuration.

          Otherwise I would suggest a WebEx with you customer support.

          This often helps me to find such handling issues.

           

          regards,

          Andreas

          • 2. Re: cell creation problem
            richard.gale

            The tool that I use is Design Capture.

            • 3. Re: cell creation problem
              robert_davies

              DC doesn't use DxDataBook! First thing to check is whether you've updated the library information in DC since adding the part to the library. Try closing the DC project and re-opening it. Also check the part is indexed into the Central Library (that you have completed doing the part mapping). If it doesn't show up in the tree you've saved it without fully mapping pins to parts.

              I assume you're using the Alternate Cell dialog (or assign cell whatever it is called in DC) to view the cell? If not let me know exactly the steps you are using.

              Rob

              • 4. Re: cell creation problem
                richard.gale

                Hi Rob,

                 

                That works. The cell shows up in the Place Device->assign cell window. Thanks a lot.

                 

                But I still could not do the forward annotation correctly. I look into the PartPkg.log file. There are two errors:

                 

                "ERROR: Block Schematic1, Page 1, Symbol XCMP19:

                   Pin gnd: The Schematic symbol pin is not in the PDB."

                 

                "ERROR: Block Schematic1, Page 1, Symbol XCMP19:

                   Pin VCC: The Schematic symbol pin is not in the PDB."

                 

                The other pins of the symbols are input/output pins. Only the GND and VCC pins have problems. In the symbol editor, I defined the pin type of the GND pin is 'Ground' and the pin type of the VCC pin is 'Power'. Is it that correct? I updated the central library and I checked the part is indexed into the library.

                 

                Do you have any idea about it?

                 

                Thanks,

                • 5. Re: cell creation problem
                  robert_davies

                  There is a problem with using Power and Ground pin types when you import them to the PDB. They come is as a separate gate, I would suggest you change them to In/Out or Bidrectional and delete the gate and re-import the symbol.

                  • 6. Re: cell creation problem
                    richard.gale

                    Hi Rob,

                     

                    That works. But I need to create a new project and new schematic file and work on it. This time I did not define the pin type of all the pins.

                     

                    I still have the same errors if I work on the old schematic file even though I already updated the central library. It seems like the Part Database is not updated when the central library is updates.

                     

                    Do you know why?

                     

                    Thanks!

                    • 7. Re: cell creation problem
                      robert_davies

                      You need to run the packager with the Update Local Library data with newer Central Library Data. The refresh library option only refreshes the symbols seen by DxDesigner, it is the packaging process that updates part information.