First SMD Board - Please Critique / Suggest / Help Me Improve - Page 1
Forum section: electronics / general

author: algorhythm
author_rank: Contributor
timestamp: April 28, 2016, 12:23:39 pm
content: Hello EEVBlog.I'm a novice getting into surface mount design. This project is a little clock with an Atmega328, Maxim DS3234, and Avago display. I have no experience with pcb design/layout and would really benefit from some expert advice about what should be fixed or changed to make a better board.I'd love to hear any critique, suggestions, tips for improvement, etc...Thanks everyone!

author: T3sl4co1l
author_rank: Super Contributor
timestamp: April 28, 2016, 12:28:07 pm
content: Ew, square trace routing! 1985 called, they want their autorouter back!I see traces joining pads laterally. This looks bad. Typically the soldermask doesn't bond well (it's too narrow) and the trace gets covered with solder. Which looks like a short. If you don't know that those pins are supposed to be connected, it looks like bad soldering (or bad PCB design).Looks like a lot of floating copper, too. Stitch the top and bottom pours together with vias!Tim

author: algorhythm
author_rank: Contributor
timestamp: April 28, 2016, 12:39:00 pm
content: Haha, I suppose there's no accounting for taste. No autorouter was used but I guess 1985 wants my traces back.More seriously though, you're talking about the lateral traces between the DS3234 pads? Would it be better to make a trace in front of them all and connect to that?I didn't know if the top pours should be connected to ground or not. I'll put in some vias. Is it ok to have some things grounded to the top pours and others to the bottom, or should everything ground to the bottom, and the top is just stitched in? Should I make the top pour part of the GND signal?

author: cowana
author_rank: Frequent Contributor
timestamp: April 28, 2016, 12:46:47 pm
content: Quote from: algorhythm on April 28, 2016, 12:39:00 pmYep - much better as it allows you to see the traces going to each pin separately.Quote from: algorhythm on April 28, 2016, 12:39:00 pmUnless you're trying to do something specific (such as star grounding to stop noisy ground loops), there's no harm in liberally applying vias everywhere stitching the two planes together, then ground to any connected pour. In general you're aiming to decrease inductance by reducing the loop area of the power pins.

author: algorhythm
author_rank: Contributor
timestamp: April 28, 2016, 12:52:10 pm
content: Ok, great.I made the top part of GND but haven't added any extra vias yet, however, it looks like most of the existing GND vias tied in most of the top pour.I also moved the DS3234 lateral traces (which are grounded pads btw), but when the top pour became part of GND, eagle added them back.

author: ruffy91
author_rank: Regular Contributor
timestamp: April 28, 2016, 12:54:05 pm
content: Free advice: place some mounting holes. The're always useful if there is room for them. Also use thicker traces for power supply where possible.

author: Brutte
author_rank: Frequent Contributor
timestamp: April 28, 2016, 01:02:05 pm
content: Floating copper. Move the tracks, or just connect that floating copper to something (GND, VCC or something DC, preferably).The negative battery contact might not get in contact when it is surrounded by soldermask.I would also increase the clip's solder pads to improve that mechanically as there is a serious force that pushes it out. You know, the copper for pads is separated from copper pour with thermal relief because of a reason - it eases manual soldering to heat up faster. This is not made for esthetical reasons. So doing the same trick for reflow oven or when the aim is to improve heat transfer is pointless. Although it might ease the job for rework. Same applies when you have to manually solder a huge battery clip or a TO220 - a beefy soldering iron and heavy tip is needed, thermal relief won't help here.IMHO your TQFP pads are too short for manual soldering. Ok for reflow.And there is no NRESET routed to the connector - this tiny cannot be debugged without this pin so the board would be useless for development.

author: algorhythm
author_rank: Contributor
timestamp: April 28, 2016, 01:35:33 pm
content: Quote from: ruffy91 on April 28, 2016, 12:54:05 pmThanks. This isn't the final board so I didn't include a mounting hole, but it's a good idea and there's one in now. The power traces are now 16mil as well.Quote from: Brutte on April 28, 2016, 01:02:05 pmI'm not happy with this battery clip either and I'll probably use a through-hole battery clip on the final board to save a little space and increase strength. I've been putting a little blob of solder on the ground pad to make it stick up a bit above the solder mask, but it's not ideal.Eagle seems to automatically include thermal isolation wherever anything connects to a pour. Perhaps you know how to turn of the thermal isolation on individual pads? I'd love to know.Soldering on this tqfp footprint hasn't been a problem for me.The reset connection should be visible on pin 5 of the 2x3 icsp connector. Am I missing something here? Usually I burn the arduino bootloader via icsp then use the 1x6 ftdi header to develop and debug.

author: Brutte
author_rank: Frequent Contributor
timestamp: April 28, 2016, 06:16:13 pm
content: Same remark about pads applies to USB receptacle - those micro and mini USB SMD vesions are hopeless for PCBUse THT version if you want that to last longer than one insertion. Or preferably use angular USB-B (beefy ones as in USB printers).The blob on a negative CR battery contact is not a good idea as it might short the battery while inserting it. Just make pad bigger and also make sure you won't scratch soldermask and short something.As for NRESET - that looks ok but you would have to disconnect FTDI while debugging/programming as there is a capacitor involved.The AVCC is shorted to VCC and that is not what datasheet recommends.There are vias under TQFP - not sure about you but I always etch a PCB and test it before I order a final version. Drilling and soldering vias under TQFP is PITA. You can usually overcome that with ugly jumper wires but I always try to move via "outside" first, if possible.

author: algorhythm
author_rank: Contributor
timestamp: April 28, 2016, 09:01:48 pm
content: Thanks for the helpful input everyone! The board is off to Osh Park.Cheers.