Custom USB Hub PCB: I cannot find the error. - Page 1
Forum section: electronics / projects

author: jb82
author_rank: Contributor
timestamp: January 28, 2025, 11:47:51 am
content: I've designed a PCB that contains two functionalities:A two channel USB hub in the lower area of the PCBA temperature controlled switch for a fan in the upper areaAnd, as the title says, it's not working.The error is actually quite simple: When you measure between +5V and GND, there seems to be a short. My PC confirms this by reporting an overcurrent event when connecting it. However, I can't seem to find it's origin.I'd appreciate it if someone could have a look at this. Maybe it's just one of these stupid mistakes which can only be spotted by an uninvolved observer. Then again, I'm self-educated and might have made a more stupid mistake. Anyway...The board has four layers with stackup Signal/GND/PWR/GND. Below, you'll find:The schemaThe PCB layers from left to right and front to backFront and back of the soldered PCBThe full KiCAD projectKiCAD project:https://www.dropbox.com/scl/fi/vifsk1yzzz8nw8g45lf8q/USB_Hub_cam.tar.gz?rlkey=velfqg913r854xvwaiirya7px&st=xflipqzz&dl=0Some additional remarks:I've soldered the board myself.The QFN package of the USB hub was my first suspect for accidentially creating a hidden short. However, desoldering it did not change anything.Measuring between +5V and GND on an empty board also produces a short.The pin CRFILT of the USB hub has to be connected to Vss instead of Vdd, I've just spotted this, but I don't think this could cause the observed behaviour, especially not with the hub desoldered. Side question: Is there a reason some manufacturers call their ground pins Vss instead of GND? After hours of browsing through all kinds of funky pin names it's very easy to confuse Vdd with Vss.Thanks in advance

author: xvr
author_rank: Frequent Contributor
timestamp: January 28, 2025, 01:42:01 pm
content: Check the blocking capacitors - sometimes they can fail and short out the power supply.

author: fchk
author_rank: Frequent Contributor
timestamp: January 28, 2025, 02:25:33 pm
content: 1. Never put vias into pads except for thermal pads on QFN etc. Reflow soldering will fail otherwise since the solder pase escapes through the via hole.2. Standard USB Pinout is 1=VCC 2=D- 3=D+ 4=GND. You are supposed to keep it exactly this way.3. The voltage divider on VBUSDET needs to go to VBUS on the upstream port, not to 3.3V.4.Vss is the rail where the MOSFET source connections are connected. (usually GND)Vdd is the rail where the MOSFET drain connections are connected. (usually supply voltage)Same with bipolar circuits:Vcc: bipolar transsistor collectors railVee: bipolar transistor emitters rail

author: eleguy
author_rank: Regular Contributor
timestamp: January 28, 2025, 02:29:33 pm
content: Quote from: jb82 on January 28, 2025, 11:47:51 amYou might be out of luck in this case. Something has to be then quite wrong, right? What has happened to me few years back is that I forgot to refill zones in Kicad before creating gerbers. And hahaa... yes. I had moved one via just a little and short was indeed the outcome. The fab house does not check this kind of problem. Good that it was just an development batch which I was able to fix by drilling the broken via away and soldering some rework-wire instead. Not fun but I learned my lesson. I think nowadays Kicad refills zones automatically...

author: Ice-Tea
author_rank: Super Contributor
timestamp: January 28, 2025, 02:34:16 pm
content: - Hook up the 5V to a bench PSU.- Turn the current up little by little.- Whatever starts to smoke is probably your short.

author: jb82
author_rank: Contributor
timestamp: January 29, 2025, 05:42:42 pm
content: @xvr Sadly, the error also shows on an unsoldered board, as mentioned at the end of my post (On hindsight, this makes the shots of my soldered board useless, but I couldn't think straight anymore that day).@fchk Thanks for the tips. They won't solve my current problem but may safe the next batch... As for point 1, I heard a lot of different opinions, but looking at my board, I can confirm that the solder on the via pads seems to be less. I'm gonna fix this too, thanks again.@Ice-Tea Would also be worth a try. I keep this in mind if nothing else helps.

author: globoy
author_rank: Frequent Contributor
timestamp: January 29, 2025, 06:04:08 pm
content: Quote from: Ice-Tea on January 28, 2025, 02:34:16 pmIf you've ever thought you might want a thermal imaging camera, this is your opportunity to justify it to yourselfBefore the board smokes, it will get hot and the camera is a great way to see that spot.

author: ealex
author_rank: Frequent Contributor
timestamp: January 29, 2025, 06:11:58 pm
content: Some of the vias seem to short multiple planesFor example - on the DN1 connector you have 2 vias, one for GND and the other for VCCOn the bottom plane it looks like both vias are connected straight to it.The same for DN2 and maybe other places.Also, The VCC vias seem to stop - they're not present on the 4'th layer - maybe you intended something special but the board house drilled them trough all the stack ?(Also - via in pad is not a great idea if the board house can't plug the holes - it will wick solder from the pad and even worse, it can create bubbles and push the part.You can see the wicking effect on your boards - R2 and C3 - the pads with vias have almost no solder on them.It works for big parts / when you hand assemble the parts and you can manually add enough solder to those area.)

author: jb82
author_rank: Contributor
timestamp: January 29, 2025, 06:17:17 pm
content: Thanks again for all tips, but I think I found it, thanks to the help of in3otd via PM.As @ealex wrote too, the manufacturer seems to have turned my blind into through vias. They offer a direct upload of KiCAD projects without the detour of generating your own gerber files, that's probably where it happened.

author: janoc
author_rank: Super Contributor
timestamp: January 29, 2025, 08:46:23 pm
content: Congrats to finding the problem - but all those ERC errors (those orange and red arrows in the schematic) don't bother you?

author: thm_w
author_rank: Super Contributor
timestamp: January 30, 2025, 12:46:53 am
content: Is there a reason you thought you needed to use blind vias?The cost increase is significant.