Translating a Design from Board Station to Expedition

These are the instructions I came up with for the eshop. I was trying to follow the instructions in this document from Mentor Graphics. You will notice that I do not follow them exactly.

On page 29 of the above document, it refers to a program called SynchBSMigratedDesigns.exe. I never got this to work, but if you want to try it, you'll find it in S:\SynchBSMigratedDesigns_7.9.2.

  1. Release the Board Station Design. Make a directory in /net/archive with the same name as your design and release it there. This directory is then mounted as the O:/ directory in windows.
  2. Our translated projects are in U:\PCB_designs\<username>\<project name>. So make a directory in this location for your project. And then inside this directory, make a directory called layout.
    make directories
  3. Start the Board Station to Expedition translator
    starting translator
  4. Select Translate -> BS2EXP Wizard
    Start the Wizard
  5. Make sure all boxes are checked and check the "Open Design" box in the experimental section. This just makes it easy to know when the design is finished.
    Settings
  6. After you hit run, it looks like nothing is happening. The log is actually showing in the translator console window.
    running
  7. When it's finished, you should see your project in Expedition. Then quit the program.
    expedition
  8. Look in the layout directory. The translator created a library for the project. Move this library up one directory so that it's easier to find.
    move library
  9. Now need to reopen the Expedition file (it's the .pcb file in the layout/PCB directory). You'll immediately be prompted that it can't find the library.
    cannot find library

    Select the new location of the library and then quit the program.
    new library location

  10. Now we need to translate the schematic. Start the DA2DX translator.
    da2dx translator
  11. Make a directory called schematic which is where we'll put the translated files
    make a schematic directory
  12. Fill in the tranlator. Be sure to pick pcb_design_vpt for DA component. The Target directory should be the schematic directory just created. And the Central Library is the one that was moved from the layout directory.
    translator options
  13. Once the translation is complete, double-click on the .prj file in the schematic directory to open it in DxDesigner.
    open project
  14. Double-click on the top board to open it.
    open board
  15. Run DxDesigner Diagnostics to check for any problems. You shouldn't have any, but if you do, you need to fix them before moving on.
    run dxdesigner diagnostics
  16. We need to sync data between DxDesigner and Expedition. To do this, start Package.
    start package
  17. Options to use.
    package options
  18. You will get a lot of errors like this, which we'll have to fix.
    errors
  19. In the above example, the part that is giving the error is PN-PILOT. So, open the library for the project and edit this part.
    edit part
  20. In the Part Editor window that opens, click the Pin Mapping button.
    pin mapping
  21. Import a symbol for the part. Pick the symbol that's given in the error listing. In this particular error, it says the symbol is mcp_tl_anode:325_01.
    22. import symbol
  22. Finding the symbol
    find symbol
  23. Assigning the pins. You need to assign all pins listed under Logical Pins to a pin on the symbol. As you hit tab or move out of the assignment box, the pin name will disappear from the list on the left.
    assign pins
  24. Save the part after editing.
    saving the part
  25. Once you've assigned the symbol, you'll see an Associated Symbols menu beneath the part. This process must be repeated for all parts in the design.
    associated symbol
  26. This screenshot shows a part that has a lot of pins that need to be assigned.
    many pins to assign
  27. This is how the parts should look after all the symbols have been assigned.
    all symbols assigned
  28. Rerun Package and it should complete successfully. (Though many times it doesn't and you'll need to figure out what went wrong.)
    Package successfully completed
    29. Only move to this part after Package completes successfully
  29. Open the pcb layout file
    open pcb layout file
  30. Run Setup->Project Integration
    setup project integration
  31. Change the "Project file and Design" to the .prj file in your schematic directory. Once you enter that, you'll get this prompt to pick which PCB to use. Take the default.
    change project file
  32. After you click ok, you'll get this prompt. Click Yes.
    forward annotate
  33. This is the default window that comes up. You need to change the settings struck out in red.
    bad settings
  34. Here are the settings to use.
    good settings
  35. Click the red or amber buttons to run the processes and hope that they get to green.
    running processes
  36. You can now quit. When you do, you'll get this prompt, just save all.
    quit and save
  37. Now, for reasons I don't fully understand, we are to copy the PCB directory from layout to schematic.
    copy PCB directory
  38. Paste the PCB directory in the schematic directory
    paste PCB directory
  39. Open the pcb file (located in schematic/PCB).
    open copied PCB file
  40. You'll have to tell it to use the .prj file in the schematic directory.
    reassign the prj file
    pick schematic prj file
  41. To make sure everything is working, run Setup ->Project Integration again. The buttons should be green.
    setup - project integration
  42. The last step is to quit Expedition and open the prj file in DxDesigner. When you press the Expedition button, the project should open correctly in Expedition.
    expedition button
Updated: October 2011