Not quite a PCB review, some wisdom requested

[analogoutput]

See

KiCad footprints and models

Gahh. I just noticed this. Alps RK09K 9mm vertical board mount pot footprint: [image] Alpha RD901F 9mm vertical board mount pot footprint: [image] Spot the difference? It’s not as if Alps uses that pin numbering. From https://tech.alpsalpine.com/prod/e/pdf/potentiometer/rotarypotentiometers/rk09k/rk09k.pdf: [image] Weird.

and the subsequent two posts. I always use my variant of the Alpha footprint. This I why I said

@analogoutput

And those are if using footprint where pin 1 is counterclockwise, which is not true of some footprints, so check that too.

@Dave

I have noticed some vertically mounted resistors that could be very tight.

So could the electrolytic capacitors — of which I see zero. Really? No 10uF bypass caps near the power header? No 10R resistors or Schottky diodes on the rails either — well, that’s a choice and if you’re confident there will be no shorts and no power reversal that’s fine. But the 10uF caps are really recommended — mounted horizontally if they’re between the boards or board and panel.

@Dave

It would also appear you may have some missing connections as indicated by the remaining rats nest lines, These may well be connected via the pin headers but is something I would recheck.

They look like +12V and ground. I do see what looks like a header connection for +12V, it’s not obvious to me there’s a header connection for ground, though.

These kinds of leftover ratsnest lines, and the consequent nonzero unrouted count, bug me, so I use GND1 on one board, and I created power symbols +12V_1 and -12V_1, to make totally separate ratsnests for separate boards.

@Dave

The footprint you have selected for the transistors is very fiddley to solder, a wide version is in the standard kicad library.

Hear hear. I still let the tight footprint through sometimes by accident and kick myself. Though I haven’t actually had trouble soldering one since one of my first PCBs when I went through about three pairs of transistors soldering and unsoldering until I got it without issues.

Here

you could avoid some very convoluted routing by putting some traces on the other side. Not really a problem, more an aesthetic thing. I also would connect C11 directly to pin 16 via a single straight trace but that’s probably fine. And I’d use wider traces for the power rail, as you did on the other board.