8 Replies Latest reply on Nov 11, 2013 12:39 AM by sravankumar.padarthy

    Orcad to DxDesign conversion




      I have an Orcad schematic (.dsn).  The schematic is of a microcontroller with extensive use of buses and net aliases.  I am finding that DxDesigner is not able to translate the net alias.


      For example, if the net in Orcad has been defined as  FPGA_IO_1  and aliased using ADIO_2, it shows up in DxDesigner as just FPGA_IO_1.  The net aliasing is moved under the property name called ALIAS and its value is FPGA_IO_1ADIO_2.  ALIAS appears as a property of the net.  I don't think ALIAS is a standard DxDesigner property and it is originating from the conversion process.


      To fix this, I am currently manually selecting the net and changing its name to FPGA_IO_1|ADIO_2 which seems like DxDesigner's way of doing net aliases. Is there a better way?  Is there some way I can translate the Orcad schematic such that the net alias is done correctly?





        • 1. Re: Orcad to DxDesign conversion

          At the moment there is no workaround to this but we have been working on a similar issue for the next release of the software. Is it possible for you to send a test case to us to see if it is the same problem?

          • 2. Re: Orcad to DxDesign conversion

            Hi Robert,


            Created the service request with the Orcad file.  Please keep the files as confidential as these are intellectual property of Greenlight Innovation.


            SR: 2543353179





            • 3. Re: Orcad to DxDesign conversion

              FYI for others, and so that this thread pops up in search results -


              Orcad translation issues are as follows:


              1) In Orcad, the pin numbers on some components like diodes and transistors are A,C, B,E,C instead of numbers.  This causes issues in DxDesigner as it expects the pin numbers to be actual numbers. Symbols with these have to be edited manually in symbol editor 
              2) After the import, all symbols in the schematic have the reference designator which match the original .dsn file.  However, if PCB interface is run, the reference designators get re-assigned.  To work around this, I discovered that each symbol needed to be edited in symbol editor to add a property called REFDES with value equal to R? or C? or J?, etc depending on the component type.
              3) Net aliases do not get translated properly
              4) DEVICE property in DxDesigner doesn't permit spaces, but the default translation configuration setting file that comes with PADS allows for spaces.  I changed this manually to make space as an illegal character in DEVICE property as well
              • 4. Re: Orcad to DxDesign conversion

                Have you tried EDIF format of converting the schematic?

                • 5. Re: Orcad to DxDesign conversion



                  I have an orcad schematic.I translated the dsn file into dxdesigner.While exporting the netlist for PADS layout i am getting the  following error


                  pcb: Note 5996: Using Config File C:\MentorGraphics\9.5PADS\SDD_HOME\standard\pads95.cfg

                  pcb: Warning 5720: Check Schematic1.err for VIEWBASE messages

                  pcb: Error 5709: Could not open schematic Schematic1

                  pcb: Note 5626: Summary of Log Files/pcb.err

                  Status 0, Notes 1, Warnings 1

                  Errors 1, Failures 0, Fatals 0, Internals 0


                  Kindly help me to fix this error..





                  • 6. Re: Orcad to DxDesign conversion

                    Hi Geetha,



                          Kindly let me know the version you are trying to convert.




                    • 7. Re: Orcad to DxDesign conversion

                      I converted already in 9.5.I am trying to export the netlist in PADS Layout Version 9.5

                      • 8. Re: Orcad to DxDesign conversion

                        Check your library list in setup-settings-libraries


                        You should have a local library with “.” as the path, if not add it and try exporting netlist


                        This is one of the reason why you get 5709 error, for more causes see MG245554 in supportnet