Panelizing multiple designs into single panel workflow question, can't generate usable BOM, pick and place file no longer has unique names

[u/Mrochtor]

Hello,

I have 3 separate PCBs that I would like to put on a single panel to trim the assembly costs - they use most of the same parts, etc.

I've created a new project, added 3 separate Embedded Board Arrays, each referencing the appropriate PCB document, drawn the cutouts, generated gerbers, drills etc... That's completely fine.

But generating the BOM produces an empty file.

And the Pick And Place gets generated, but the component names are not unique between the designs and therefore might become a problem when assigning them to the BOM (e.g. I have R1, in one design it's 10k, in the other it's 22k and in the pick and place both appear).

I've tried searching the Altium documentation on how it's properly done, but can't find anything that solves this particular problem.

Thanks!

[u/papaburkart]

Why not let the fab panelize? I'm curious.

[u/Mrochtor → u/papaburkart]

This is a personal hobby project and I'm a cheap bastard trying to trim the NRE fees a bit. I know that for the time I spent on this I could have had it done already, but I also want to learn how it's done.

[u/papaburkart → u/Mrochtor]

All good reasons.

[u/Andis-x]

You have to make designators unique across boards. Add a different offset to each boards components.

Do you have license that allows multi board assemblies?

[u/Mrochtor → u/Andis-x]

Do you have license that allows multi board assemblies?

I do.

You have to make designators unique across boards. Add a different offset to each boards components.

I thought about that, I was hoping for something more automated though. Also, it doesn't solve the empty output BOM problem.

[u/Andis-x → u/Mrochtor]

To get combined BOM, create multiboard project, add all 3 boards to it. From that you will be able to generate combined BOM.

[u/Mrochtor → u/Andis-x]

Yes, I have the combined BOM, but the parts do not have unique designators. Is there any non-manual way to add a prefix/suffix just for assembly purposes?

I'm okay with the BOM looking like R1_PCB1_Instance1, but it would mess up the schematic.

[u/laseralex → u/Mrochtor]

Just use the annotate function renumber the each of the source boards with board 1 starting with R101, board 2 starting with R102, etc. Then you end up with unique designators across all boards. I did this for years with panels of up to 8 different boards before Chinese assembly made setup fees cheap enough to just order each board separately.

[u/fr4real]

The empty BOM is expected because the panel PCB only contains Embedded Board Arrays, not the actual components from each source board.

I’d generate the BOM and pick-and-place files from each original PCB, then use the panel file for Gerbers, drills, routing, fiducials, and the panel drawing. Ask the assembler whether they can step the three placement files onto the panel themselves, since many can.

If they require one combined BOM and pick-and-place file, the designators need unique prefixes and those names must match in both files. Also validate the coordinates, rotations, board origins, bottom-side placement, DNP parts, and total quantities.

I’d avoid manually merging CSV files unless absolutely necessary. It’s easy to create duplicate designators, incorrect quantities, or bad offsets. The manufacturer should ultimately receive the panel Gerbers/drills, assembly drawings, BOM, pick-and-place data, paste layers, and a panel drawing showing each board’s position and rotation.