Renaming reference designators without affecting the silkscreen

[snake-4]

I'm using the Python API to panelize different designs. The reference designators have to be renamed because the same designator refers to different components on different boards. Setting the refRenamer argument works fine but it'd be better if there was a way to keep the silkscreen texts as-is.

[yaqwsx]

The silkscreen of reference and the reference value are coupled in KiCAD. You cannot have one reference and show the other. What you could do is hide the reference and place a new text with the original reference. We don't support this in KiKit, however, you can implement it.

However, I don't think it is a good idea. What is your use case? If it is building assembly data for a multi-design panel, I have plans for approaching this much cleanly: when building a panel, all information about a component are baked into the panel board (i.e., all information that are stored in schematic). Hence, the panel becomes a self-contained entity and we completely avoid a problem with pairing board and schematic components.

[snake-4]

My use case is indeed building the assembly data.

References must be renamed but adding a prefix to all of them makes the silkscreen overlap in a lot of places. New references are only relevant to the P&P machine so I figured I'd keep the texts the same.

[snake-4]

Also, about your second paragraph; I'm using appendBoard and It appears to me that component information is already baked into the panel board. The footprint and the fields are there and that's enough to generate a component placement file and a BOM. If only kikit fab was implemented in a way that doesn't require the schematic, I'd directly generate the fab files of the panel using KiKit.

[snake-4]

This is what I ended up doing in case anyone else faces the same problem:

import pcbnew

def rename_references(board: pcbnew.BOARD, prefix: str):
    for footprint in board.GetFootprints():
        ref = footprint.Reference()  # type: pcbnew.PCB_TEXT

        if ref.IsVisible():
            pcb_txt = pcbnew.PCB_TEXT(board)
            pcb_txt.SetPosition(ref.GetPosition())
            pcb_txt.SetLayer(ref.GetLayer())
            pcb_txt.SetText(ref.GetText())
            pcb_txt.SetAttributes(ref.GetAttributes())

            # GetDrawRotation accounts for KeepUpright property of footprint texts
            pcb_txt.SetTextAngle(ref.GetDrawRotation())
            board.Add(pcb_txt)

        ref.SetText(prefix + ref.GetText())
        ref.SetVisible(False)