Sumorobot circuit design help. - Page 1
Forum section: electronics / general

author: digitalundernet
author_rank: Contributor
timestamp: October 07, 2013, 06:20:43 am
content: I'm sorry if this is in the wrong section I'm fairly absent sometimes. I've got to build a sumobot for class and I was wanting to design my own board to go with it. I'm worried with how my board layout is going. Its my first time trying to do SMD and only my 4th board. I've got two pictures here, one of the board as a whole and one with the AVR. Everything in me screams what I'm doing for bypassing on the AVR is wrong. Can someone please give this a look and tell me how bad it is?

author: kizzap
author_rank: Unknown
timestamp: October 08, 2013, 04:57:19 am
content: A number of things that I would change:Don't use the top layer as your +5V layer; keep both copper pours as ground.I can see a number of vias that don't seem to be on the same grid reference as the trace they are connected to, I would consider moving them around.Speaking of Vias, I can see a couple that will cause the board to fail any DRC checks, I.E. there is one for the crystal that is almost touching the trace next to it. I use octagonal vias (just a personal preference)Some of the traces that I can see there seem way over specced for whatever signals are going through them. Most people love to try push down to a 8/8 mil spec for smd stuff, however with a recent board I have designed, I have easily gotten away with 16mil traces throughout, with only one trace slightly larger to "gild the lily". A perfect example is the two SMD components bottom right, they have a thin trace heading to them, yet the trace going to the via is as wide as the component will be.You have a number of SMD components both on top side and bottom side. This isn't too bad an issue really, however if you can fit them top side (and looking at the board space you should have no issue here) you should try to, it will make troubleshooting and routing just that little bit easier.There is a lot of blank board space there being wasted. surely you could make the board smaller?I've taken the liberty to show a board that I am working on atm. I would never say that I am the best at PCB layout, but I am proud as to the OCD neatness that I have with this board.You will note that I have the majority of the SMD stuff on the rear. this helps with routing, as I can run longer straight traces to where I need them, and keep them grouped together. The exception to this naturally is the LED/resistors mounted on the front which are indicators, therefore needed. You will also note that I have a lot of the components that are part of the same function grouped together, to help with troubleshooting.I have also made the grid visible, which helps a lot in getting things looking good.I have tried to limit, where possible the protrusions caused by the height of some components on the rear, namely with the SMD capacitors next to the shrouded header connector, as they both will be standing a fair amount off the board.I hope this gives you some ideas as to what to look at.-kizzapEdit: GAH! Can't believe I forgot the most painfully obvious one too, which I believe even Dave has eluded to in his videos. Keep all your interconnects to one board side!!! so if you need to troubleshoot it is easy to simply flip out the board!

author: digitalundernet
author_rank: Contributor
timestamp: October 08, 2013, 05:42:37 am
content: Thanks for the suggestions! They help a lot.I've been tinkering on the board myself while waiting on a reply and started to do most of what you mentioned. I didnt realize its a bad idea to do 5v top pour. I've fixed that and started to make all trace sizes uniform (no idea what I was thinking there really). I've never worked with SMD before so the size and lack of any space is a bit frightening. Hopefully it'll force good habits though. I can haven't flipped the caps on the crystal back to the top pour but I plan on it tomorrow. Finish routing the 5v lines and what do you think of this? Any other changes I should work on? I might chop off some width to save cost.All interconnects will be on the top. Simple screw terminals

author: kizzap
author_rank: Unknown
timestamp: October 08, 2013, 06:23:50 am
content: Looking better alreadyI spy some traces that aren't at a multiple of 45 degrees (just a general tidyness thing- I'm way too OCD for my undiagnosed comfort).I don't mind the rows of connectors with the +5V and GND connectors, just ensure that they cannot short each other out, maybe change the part to have octagonal pads? Also keep the +5V trace on that connector a little larger, just in case you end up pulling more power then you think from there. If you are clever, you could have them only 0.1" spaced, so that you could use a three pin header to connect to them.Are you sure you have the correct pin spacing for all the interconnects? most screw terminals have a pin pitch larger the 0.1"You could also easily scoot the MCU, and especially the interconnects to the left, and have a ton of space to bring the motor controller down.-kizzap

author: digitalundernet
author_rank: Contributor
timestamp: October 09, 2013, 04:48:10 am
content: So I took a look at the motor/power connectors after you mentioned they looked small. You were totally right. I was using the wrong component all along. I've since replaced the parts but got a "Forwards/backwards annotation" error, tried to fix it by replacing the parts and got no joy. Finally it got so bad it said every part was wrong.After much cursing at wasting nearly a week on this I re started my design. It's a bit smaller and still have a ways to go but I hope this will work. Thanks for the help Kizzap. I was a bit scared to post here because I'm way over my head.

author: walshms
author_rank: Regular Contributor
timestamp: October 09, 2013, 05:57:29 am
content: One more suggestion for you.Try to keep your clock source symmetrical; in other words, keep trace lengths identical, as short as possible and put the capacitors as close to the crystal as possible. For what you're doing it's not critical, but it's good design practice.

author: senso
author_rank: Frequent Contributor
timestamp: October 09, 2013, 12:03:56 pm
content: The annotation error es/was because you edited the components present in the board with the schematic closed, you can correct that, adding the components to the schematic it would correct the error, happened the same to me a days a go.