Fresh set of eyes—PCB short

[CountChocula]

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

[GARTHWILSON]

When loading the files into the gerber viewer, I get a ton of error messages saying "unknown RS-274X extension found %TF%", so I tried to look up the code in my RS-274X book, and it's not there. The files do load, so I suppose there's something that just doesn't get interpreted along with the rest. Right away however I find a ton of design-rule violations, with only .0035" trace & space. The cheap board houses usually don't guarantee anything below .006", maybe .005". If there's any inaccuracy in the etching, I suppose you could get shorts (or, going the other way, super-narrow traces will get eaten away). One reason they're so cheap is because they don't give us any human attention to flag potential problems. Whatever we send in the files is what they make, whether it'll work or not.

Your antipads ("moats") should be much smaller. Having them so big won't cause shorts of course, but will contribute to AC-performance problems. The ground plane should go between all the DIP pads, so the return current for traces that go between doesn't have to go all the way around the end of the IC. I'd recommend making them only about .016" larger than the pads, ie, .008" per side.

[plasmo]

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

[CountChocula]

GARTHWILSON wrote:

When loading the files into the gerber viewer, I get a ton of error messages saying "unknown RS-274X extension found %TF%", so I tried to look up the code in my RS-274X book, and it's not there. The files do load, so I suppose there's something that just doesn't get interpreted along with the rest. Right away however I find a ton of design-rule violations, with only .0035" trace & space. The cheap board houses usually don't guarantee anything below .006", maybe .005".

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

Quote:

Your antipads ("moats") should be much smaller. Having them so big won't cause shorts of course, but will contribute to AC-performance problems. The ground plane should go between all the DIP pads, so the return current for traces that go between doesn't have to go all the way around the end of the IC. I'd recommend making them only about .016" larger than the pads, ie, .008" per side.

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

[CountChocula]

plasmo wrote:

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, 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!

[gfoot]

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!

[CountChocula]

gfoot wrote:

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

[GARTHWILSON]

CountChocula wrote:

GARTHWILSON wrote:

When loading the files into the gerber viewer, I get a ton of error messages saying "unknown RS-274X extension found %TF%", so I tried to look up the code in my RS-274X book, and it's not there. The files do load, so I suppose there's something that just doesn't get interpreted along with the rest. Right away however I find a ton of design-rule violations, with only .0035" trace & space. The cheap board houses usually don't guarantee anything below .006", maybe .005".

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

(It's 3.5 mils, not 35.) That's impressive. I guess the technology keeps marching on, and I need to review all the capabilities anew. Hole aspect ratios also have increased (for other manufacturers) but I still have trouble trusting them to get reliable thru-plating on holes with aspect ratios over 4.

[speculatrix]

CountChocula wrote:

plasmo wrote:

That mounting hole was clearly not rendered at all in the inner layers.

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.

[CountChocula]

speculatrix wrote:

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 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!