Take the 2-minute tour ×
Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It's 100% free, no registration required.

I have a 4-layer PCB, designed in Eagle CAD 6.5. The stack-up is:

  1. Signal
  2. GND (ground)
  3. DVDD (digital power)
  4. Signal

GND and DVDD are solid planes, with vias connecting them to layers 1 and 4.

I have 4 PCBs. Three PCBs are bare - unpopulated, fresh from the fabricator.

In the bare boards (and the assembled one) there is a short between GND and DVDD. It could be a manufacturing defect, but since all 4 boards are bad, it's more likely it is a design problem.

I've manually examined the gerbers in gerbv to see if there are vias that connect to both GND and DVDD, but did not see any. But there are a lot of vias, so I could have missed one.

I've done an Electrical Rule Check (ERC) and Design Rule Check (DRC) - to look for problems. I get no unapproved errors. I've examined all the approved errors to look for problems - there are no overlaps.

How do I find the source of the short circuit?

share|improve this question
5  
Run lots of current through it until it explodes. –  dext0rb Jan 26 at 7:53
    
@dextorb: how will making it explode show the source of the connection? Will it burn through at the short circuit? –  Adam Jan 26 at 8:07
    
@dextorb: I think you meant that as a joke, but it's not far from what I've actually seen done. See my answer. –  Olin Lathrop Jan 26 at 14:15
    
Thanks everyone for the great help! If I have the same problem on a future PCB, I will try out some of the other answers! –  Adam Jan 26 at 16:31
add comment

6 Answers 6

up vote 7 down vote accepted

Do you have any unplated holes or slots in the PCB's? I've previously specified some unplated holes on a similar layer stack, and found that the supposedly unplated holes were in fact plated and the plating was creating a short between the power and ground planes. A round file and a few minutes work quickly sorted the problem out.

share|improve this answer
    
This was the problem! I thought I specified some unplated mounting holes, but all the mounting holes came back plated. I used a mini-drill and abrasive bit to grind off all the plating inside the milling holes, and the unpopulated PCBs no longer have the short! –  Adam Jan 26 at 16:31
2  
I always use plated holes for mounting - and include surface pads the same diameter as the mounting hardware. The padstack ensures that the inner planes are kept away from the hole, and the surface pads ensure that tracks won't be run under the hardware, where they might be damaged (or worse, over the hole, leaving mystery open circuits.) –  Peter Bennett Jan 26 at 21:23
    
Peter - thanks, on the next rev I will put in pads for the mounting hardware! –  Adam Jan 27 at 2:40
1  
@PeterBennett Yes, I learnt my lesson re "unplated" holes; I generally connect the pads to ground as well, for extra case groundage. –  markt Jan 27 at 4:04
add comment

Try the poor man's IR camera: Spray the board with cooling spray so you have the whole thing covered with tiny white ice crystals. Then run a high current through the short (plane to plane). Often you can see a spot melting where the short is - assuming the short has higher resistance than the planes (very likely).

Higher resistance => more heat (P = U*I = R*I^2).

No cooling spray in the lab? Turn the air spray can upside down - what comes out is also very cold.

share|improve this answer
add comment

Use a good volt-meter and a power supply that supports current-limiting.

Drive a decent current between DVDD and GND, ideally 100mA + up to an amp or two if the traces are decently sized.

Then, using the voltmeter, measure between closely spaced points on the DVDD and GND net, until you find the smallest delta. Your short will be close to that point.

Alternatively, drive several amps or more through the short, and look at the board with a thermal camera.

Lastly, audit your gerbers (not the board file, the exported gerbers) in a separate piece of software. There may be a problem during the gerber export.


Note that all of the above (except checking the gerber files) are techniques to locate a manufacturing defect, such as layer misregistration or similar. If you have a design error, I don't know what to tell you, aside from the fact that if the DRC isn't catching it, and the schematic is correct, you're probably doing something wrong.

share|improve this answer
    
This is the method I use. You can tell when you're off on a branch that doesn't have the short because there is no gradient as the travel down the branch. –  Spehro Pefhany Jan 26 at 14:15
add comment

At my first job out of school at HP in New Jersey, my tech had a standard solution for this. Another part of this division of HP made power supplies, including 5 V 200 A supplies for electroplating. The tech would connect the two shorted parts of the board to one of these supplies. The resulting smoking hole gave you a real good idea what was shorted. It's a good idea to put on goggles before trying this. You also usually want to solder decent size wires to the two nets on the board that are shorted. That makes it easier to connect the high-current supply.

This may sound like a flippant answer, but this was back in the days of manual board layouts, and we got some useful information like this a couple of times. Sure, the board you run the test on is toast, but then again it wasn't of any use in the first place. You are getting use out of it, which it to tell you where the defect is.

If the defect was in manufacturing the board, then the connection is usually a thin bit of copper, and this method will actually fix it. If it's a design error, the connection will be more solid and you get the smoking hole.

share|improve this answer
    
An old electronics tech that I used to do design work for had a similar trick with boards that had manufacturing-induced shorts - he'd hook a 12V SLA battery across the short, and the copper whisker would promptly vapourize. It worked surprisingly well but it did make me nervous, especially the first time! –  markt Jan 27 at 4:02
add comment

Use a Groan-ohm (sorry, Tone-ohm) if you have access to one. The newer ones are very fancy and unbelievably expensive but with luck and persistence you can find an older one like the 700 dirt cheap on eBay.

They sometimes go cheap because they look like a simple continuity tester so the unwary don't notice them - and they are continuity testers - but with the twist that the probes are Kelvin connections and the pitch of the "beep" varies with impedance. Your ears are amazingly sensitive to pitch changes so you can resolve milliohm changes easily; simply move the probes around listening for the highest pitch.

Unbelievably intuitive to use, but annoying as hell to anyone else in the lab!

If it's on an inner layer you then have an interesting drilling or machining job ahead of you, but that's another story.

share|improve this answer
add comment

How big are the boards? First I would file the edges to make sure there is not a short from the milling or scoring in the wrong place. Then solder ohm-meter leads to the shorted layers and start drilling out vias and other thru-hole patterns till you jump from 0 ohm to near-infinity. Assuming the short isn't of another sort, like overlapping pads, you should find the offending spot.

share|improve this answer
add comment

Your Answer

 
discard

By posting your answer, you agree to the privacy policy and terms of service.

Not the answer you're looking for? Browse other questions tagged or ask your own question.