Hi all!

I ordered a new batch of PCBs for my SBC, and, now that I have received them, the power rails are, inexplicably, shorted together, even with no components soldered on. I can't see anything in my schematic that suggests that anything is amiss, and so I'm not sure if there was an issue with manufacturing, or if there is a problem with my board

I attached the gerbers and schematic here in case anyone wants to try and see if they spot the problem, but mostly I would be grateful for suggestions on how I could figure out whether this is on my end or whether I should get in touch with the manufacturer. The schematic is a bit terse, I apologize—I could redraw it, but I'm afraid that I would accidentally fix the problem and make things even worse.

TBH, I'm all out of ideas, though maybe I'll get some fresh inspiration tomorrow after a few hours of sleep.

Thanks!


—Marco

_________________
http://WilsonMinesCo.com/ lots of 6502 resources
The "second front page" is http://wilsonminesco.com/links.html .
What's an additional VIA among friends, anyhow?

The mounting hole (H2) at upper left corner next to U9 may be the problem. It is a plated-through hole but there are no clearance pads for power nor ground plane so power and ground are shorted.
Bill

Thanks, Garth. I'm not sure what's going on with those errors, but I think that the design rules are within specs. JLCPCB's capabilities page provides 35mil as the minimum spacing between traces for 4-layer boards, and in the past they have always managed to deliver on that promise. In fact, I have occasionally pushed them past the limit (never on purpose—it took me a while to learn how to set up DRCs correctly), and, while they always warned me that the end product might not work out the way I want, in the end they always delivered working boards.

From that perspective, I have to say that they have been really good to work with, and very patient with a newbie

Ah, I hadn't considered that. I will look into how to set those up better next time!

Bill, thank you so much, I think that's it! That mounting hole was clearly not rendered at all in the inner layers. That's got to be some kind of weird bug in KiCAD… I didn't notice because I was looking at the actual layout inside the program instead of looking at the gerbers, and the problem doesn't show up there:


Interestingly enough, I just plotted the gerbers again, and now they look fine. Gotta love software

Well, mystery solved! At least it's not some design mistake, and in the end it only cost me a few dollars… and a couple weeks' of wait time. I suppose I could try cutting that corner off the board to see if it solves the problem, though I suspect that the risk of shorting the power planes along the cut would still be pretty high.

Thanks again for all the help!

Perhaps if you have a drill press or jig you can carefully redrill the hole and, if all is well, maybe the boards can still be used enough to find the next fault!

I'll give that a try… if nothing else, taking a drill to the thing will feel therapeutic. I mean, I may accidentally drill more than one hole… accidents happen all the time

_________________
http://WilsonMinesCo.com/ lots of 6502 resources
The "second front page" is http://wilsonminesco.com/links.html .
What's an additional VIA among friends, anyhow?

Is it possible you forgot to rerender the fills before outputting. When using KiCad I keep hitting the B key like it’s some kind of nervous tic.

_________________
I like it when things smoke.
Blog – Zolatron 64 project

I usually have automatic refilling turned on in the plotting dialogue, but what happened this time around is that I used a plugin to render the gerbers, and perhaps it didn't run a fill command. I don't think I will be using it again

In any case, I followed George's suggestion and drilled the plating out of the mounting hole, and that seems to have done the trick—no more shorts. On to the next fault!