Merging two board files into single board file?

I'm facing a challenge where I need to merge two Allegro PCB Editor board files into a single board file. I've found two methods to achieve this, and I'd like to share them with you.

Method A: Merging Schematics and Board Files

If you have access to the schematic files for both boards, follow these steps:

1. Assign unique refdes: Ensure that the reference designators (refdes) in both schematics and board files are unique to avoid conflicts.
2. Merge the schematics: Combine the two schematics into a single schematic file.
3. Generate Allegro PCB Editor netlist: Create a netlist from the merged schematic and read it into the larger board file.
4. Export sub-drawing: Open the smaller board file, select File > Export > Sub-drawing, and check the Preserve Refdes button. Select the entire board and choose an origin point. Save the sub-drawing as a `.clp` file.
5. Import sub-drawing: Open the larger board file in PCB Editor, select File > Import > Sub-drawing, and import the `.clp` file. Place it on the board.

Method B: Merging Board Files Only

If you only have access to the board files, follow these steps:

1. Create a module: Open one board file, select Tools > Create Module, and window around the entire board. Choose an origin and save the module as a `.mdd` file.
2. Place the module: Open the second board file, select Place > Manually, and choose Module Definition from the drop-down list. Select the module (if it's in a module path, check the Library option in Place > Manually > Advanced Settings). Enter a letter (e.g., "d") in the Module Instance name field.
3. Rename refdes and nets: The module will be placed on the board with refdes named as "d_D1", nets as "d_N005", etc. You can rename both refdes and nets after placement.

I hope these methods help you merge your Allegro PCB Editor board files successfully!

Questions and Discussions

Have you tried merging board files using these methods? Share your experiences!

Are there any specific challenges you've faced while merging board files?

Do you have any questions about these methods or Allegro PCB Editor in general?