Critique my circuitboard layout - Page 1
Forum section: electronics / projects

author: MattHollands
author_rank: Frequent Contributor
timestamp: October 13, 2015, 10:29:23 pm
content: Hi! I'm trying to design a tiny, keyring mounted TV IR remote. Currently nicknamed, "remoteli".Almost all of the electronics will be mounted on one board, and I was hoping I could get some feedback on my board layout. I've never done SMT board design before, and I've never had a board professionally made either. I am planning to get it made by OSHPark.The board is 18x39mm in area. There will be a top board which sandwiches in a CR1616 battery and connects the ground side to the bottom board.I've attached a few pictures, explaining what components are and also showing top and bottom layers. Feedback would be appreciatedMatt

author: trophosphere
author_rank: Frequent Contributor
timestamp: October 13, 2015, 10:51:33 pm
content: Your traces exiting out of the QFN footprint reminds me ofthis hackaday article.

author: MattHollands
author_rank: Frequent Contributor
timestamp: October 14, 2015, 12:00:47 am
content: Wow. That's an odd pad... Good shout. I'll adjust the traces slightly so that even if this pad is there, it won't short. Thanks

author: singapol
author_rank: Frequent Contributor
timestamp: October 14, 2015, 01:26:20 am
content: Have you considered the physical size of the mounting screw heads ( minature screws) ? The clearances may not be optimal, too close for the traces at the top and bottom for the battery ( may short to ground) seeing that it's 1mm grids?

author: MattHollands
author_rank: Frequent Contributor
timestamp: October 14, 2015, 04:21:41 am
content: @blueskullI think that's down down to the rubbish resolution I uploaded. Sorry. My design rules are set to minimum 0.102mm solder mask expansion. Good shout though, I had to check.@singapolThe screws will be coming up from the bottom side. Ie, the screw heads will be on the bottom side. Therefore they shouldn't touch anything because the solder mask will protect from connection, and if anything they will connect to ground.

author: MattHollands
author_rank: Frequent Contributor
timestamp: October 14, 2015, 04:55:04 am
content: Circuit Maker!!When submitting to OSHPark, the preview for the bottom silk screen look reversed (attached).... If anyone has used OSHPark, should I mirror it, or is this the view from above, looking through the board? Sorry, being dumb, there's a fully rendered image showing it the correct way around! It's getting late.

author: JoeB83
author_rank: Regular Contributor
timestamp: October 14, 2015, 04:57:48 am
content: Quote from: MattHollands on October 14, 2015, 04:55:04 amI was going to comment on your bottom silk screen, but you worked that out.......so, just thought I'd like to pass on that OSHPark is great, I use them for all of my hobby PCBs.

author: MattHollands
author_rank: Frequent Contributor
timestamp: October 14, 2015, 05:08:04 am
content: I'd heard they're good! I've placed an order, so now we waitThanks for all the feedback so far

author: Naeldasazor
author_rank: Newbie
timestamp: October 14, 2015, 08:23:53 am
content: The bottom solder pad of the attiny1634 should be connected to the ground but i can't see the connection between the pads and your ground plane/wire.Reference:http://www.atmel.com/images/atmel-8303-8-bit-avr-microcontroller-tinyavr-attiny1634_datasheet.pdfPage 2.

author: con-f-use
author_rank: Unknown
timestamp: October 14, 2015, 05:12:31 pm
content: The only problem I have with OSH park is that their logistics company ships really slowly. It takes 5-7 weeks till they get stuff to my location. Quality at that price and quantity is pretty unbeatable. If you want 10 or 11 rather than 3 boards, you might want to considerdirtyPCBs. They let you choose the color of your soldermask. Otherwise they are basically the same.

author: MattHollands
author_rank: Frequent Contributor
timestamp: October 14, 2015, 06:10:47 pm
content: @Naeldasazor. Doh. I redid that pad the other day and forgot to reconnect itI was planning on getting more made anyway since this is a prototype. It can be fixed with a bodge wire for this board while I develop the software etc. Good spot.@con-f-useIt said that delivery for me should be 3-5 days, so I was hoping it would come within two weeks... I hope it doesn't take that long

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 14, 2015, 08:06:18 pm
content: Disclaimer: I'm guessing you're not doing anything the least bit critical, so as long as you have bypasses around the MCU, none of this will matter in the slightest.That said, as best practices go:It looks like you've got some top side ground traces, which are pretty long. These could stand to have multiple vias in them, or just pour the top side with a ground pour as well. And you can stitch the ground pours that way, which will make it even quieter.Speaking of ground, it doesn't look like the MCU's center pad connects to anything? Even if they don't say the pad connects to anything internally, always ground it (or if it is specified, as something other than ground, then do that thing).Mind the pad exits -- especially for very small parts (like 0603 and smaller chip R/C's, TSSOPs, QFNs, etc.), these trace widths should be at least a little smaller than the pads, and exiting straight with the pad axis, or at worst, diagonal in a corner.On that topic, I see a number of diagonal pad exits, around the pushbuttons for example, which is perfectly fine.Try to avoid unbalanced pad connections (>3x total trace/spoke widths connecting to one pad, and not the others, of an e.g. chip R/C, or SOD or SOT package).If this is for hand assembly, try to add extra pad lengths, even for QFNs. You can actually hand solder a QFN; the best way is to use a relatively large (50mil+?) via to access the exposed pad (you can't really verify that it's soldered properly, just fill it up with enough solder and heat to hope it's been done), and get long enough pads around the edges so you can more or less drag solder it like any leaded component. (Which reminds me of something else: some "QFN" style parts are actually LGAs, with no pads wrapping around the corners -- get a magnifier and inspect them carefully! FT232R is one such part that's bitten me before.)If you're doing reflow (and, if you ever need to rework it at all, then hot air as well), you can make the pads much more modest in size (the IPC calculator should handle this just fine).That "TSOP" part (what a terribly confusing name, in the context of PCB layout!) looks like it has suspiciously small pads, so that comes to mind.http://www.vishay.com/docs/82434/tsop572.pdffor others wondering. Be especially careful of the bizarre exposed pad on that little bugger. I'd suggest shopping for a different, easier to use part, just because that footprint is a mess!Tim

author: MattHollands
author_rank: Frequent Contributor
timestamp: October 15, 2015, 02:25:24 am
content: Thanks for a thorough review!I think you're correct that most of these things won't matter for this application, but they're definitely good points for general design.I looked into trying to find a better IR detector, but nothing is shallow enough for my application. I think I'm just going to have to try my best with what I've got.I'm planning to do reflow with a hot air gun, but it's my first time, so slightly wary.The centre pad was a stupid mistake