Review 2 layer Digital only PCB design in KiCad 5.1 - Page 1
Forum section: electronics / beginners

author: lukasz.kostka
author_rank: Contributor
timestamp: October 14, 2019, 08:18:01 pm
content: Hi.I'd like to learn how to design PCB boards. I've decided to go for something simple and designed a LCD controller. My goal is to make myself familliar with PCB design and ordering boards. I'd like to ask someone to review my board design. I've went with a 2 layer board with GND plane on back.Myrepositorywith files.Fab housespecsfrom where I will order boards from.I am asking for a review of how I've placed traces, GND plane, vias. I've already checked with my fab house specs and all is fine.

author: MarkF
author_rank: Super Contributor
timestamp: October 15, 2019, 12:00:19 am
content: You will get better responses if you post pictures of each layer for those who do NOT use KiCAD.

author: lukasz.kostka
author_rank: Contributor
timestamp: October 15, 2019, 12:09:12 am
content: I've attached screenshots.

author: LaserTazerPhaser
author_rank: Regular Contributor
timestamp: October 15, 2019, 02:37:01 am
content: You can shorten traces with free angle traces instead of typical 90/45 degree traces. Traces can be a wider to match TQFP pads.

author: TheHolyHorse
author_rank: Regular Contributor
timestamp: October 15, 2019, 07:31:00 am
content: Quote from: LaserTazerPhaser on October 15, 2019, 02:37:01 amNot using 45 degree angles will make some flipBut electrically it doesn't matter.

author: mariush
author_rank: Super Contributor
timestamp: October 15, 2019, 08:43:48 am
content: I'd make an effort to not break that ground fill under the chip. You have room on the circuit board to route the traces so you won't break that.Maybe move the IC half an inch or so lower, towards the center of the board.Also, I'd try to get all traces come out straight from pads and then curve, not how you have MISO, SCK, D2 and D3.I'd try to have a thicker Vcc trace on the top and not go with VIA around those traces. I'd probably either use a jumper wire (or zero ohm resistor) or route the 4 data traces on the bottom of the board breaking the bigger ground fill for a short distance.The capacitor at the top on Vcc and GND could be rotated counterclockwise 90 degrees so VCC pad would be above the GND pad of the ceramic cap, and the GND pad right above the GND pin of the chipThis way you may have room for those traces on the left and not have to go to the bottom layer to route them. You'd still have to make the connection between the Vcc pads (ceramic cap and header) but that could be a short thicker trace on the bottom, if you bring all the header traces closer together on the top

author: homebrew
author_rank: Frequent Contributor
timestamp: October 15, 2019, 05:51:52 pm
content: How about flipping the controller to the other side of the board?Routing then gets MUCH easier ...

author: lukasz.kostka
author_rank: Contributor
timestamp: October 15, 2019, 06:51:45 pm
content: Quote from: homebrew on October 15, 2019, 05:51:52 pmGreat. Thanks. Haven't thought about it. I will give it a try with even smaller board.

author: mariush
author_rank: Super Contributor
timestamp: October 15, 2019, 06:53:15 pm
content: Yeah, that would work quite nicely.I'd move those two traces going to D3 and D4 to the left near the D2 trace, to eliminate one via on the VccI'd also rearrange the vias under the chip so that the ground fill (or whatever) isn't completely cut in half as it is now

author: lukasz.kostka
author_rank: Contributor
timestamp: October 15, 2019, 07:58:16 pm
content: I've shrunk whole board and flipped components on the other side. Now it is much better.

author: Kasper
author_rank: Frequent Contributor
timestamp: October 16, 2019, 05:50:51 am
content: Vcc trace: make Vcc wider and try to have star layout instead of all Vcc in series.Decoupling caps: it is best to have decoupling cap between Vcc and IC. Remove trace between pin 18 and 4 of the IC. Assuming the 10 pin connector is power input; connect Vcc from 10 pin connector through decoupling cap then into IC pin 18.Ground pours: probably doesnt matter for this but for good practice for high frequency and emc compliance, each piece of ground should have atleast 2 vias or should be removed. Each piece should have vias near each corner. Like stitching down a piece of fabric, dont leave any corners unstitched to flap around. In other words don't leave peninsulas or else they can act as antennas.

author: Kasper
author_rank: Frequent Contributor
timestamp: October 16, 2019, 05:57:18 am
content: Add mounting holes and test points if you think you might want them.Silkscreen labels to the headers and test points can be handy.Run DRC (design rules check) it should catch things like the unconnected net 'CON' near the south east corner.

author: Kasper
author_rank: Frequent Contributor
timestamp: October 16, 2019, 06:09:25 am
content: The rings on your vias look a little thin. Drill holes sometimes dont go exactly where you want. If the ring is not much bigger than the hole and the drill is a little off then it can cut the connection between track and via. Think of the ring as the tolerance you are giving to the drill bit.If you have space for extra tolerance, larger via holes and larger rings, use it. Not only is it easier and less risk for manufacturer, larger vias makes it easier for you to add wires to your board if you need to do mods or add test leads later.It is good to have as few different drill sizes as possible. That means less drill bit changes for manufacturer.

author: lukasz.kostka
author_rank: Contributor
timestamp: October 16, 2019, 01:18:45 pm
content: Ok. What about now ?I do not want to change VCC to be wider since it is impossible to route it between pins.I've enlarged via pads.Can't figure out a way for pin 4 VCC on atmega to go to a star point. IMO it is good enough since there will be little current.

author: Twoflower
author_rank: Frequent Contributor
timestamp: October 16, 2019, 01:43:32 pm
content: Quote from: Kasper on October 16, 2019, 05:50:51 amWhy? The solution now is that both VCC pins might have a reasonable big voltage difference between both VCC pins. Yes a split power plane isn't the best, but I think much better than routing the supply all over the place and open a big loop to catch up lots of noise. And there are no traces/signals crossing the area that could be affected.If you want to prevent the ground-plane split you can rout the VCC trace close to the solder pads; preferably on the left side around.The VCC for the upper connector: Route the signal from pin 2 to pin 15 on the back-side. If you do this, you might be able to stay on top layer with the SS signal. You can easily split the VCC above pin 5 to make space. This seems to be a digital circuit. So a strict star routing isn't necessary.If you want to keep the VCC at the lower side of the PCB: You should remove the long finger on top-layer between the VCC and SS. Such traces might act as antennae. At least do some ground-stitching there.An no one forbids you to use two or more trace-widths on one trace. But if the current on the traces is not that high that's probably OK as it is.

author: lukasz.kostka
author_rank: Contributor
timestamp: October 16, 2019, 03:06:43 pm
content: Thanks. For input. Now I will design a analog board. Will create a new topic for that.

author: Kasper
author_rank: Frequent Contributor
timestamp: October 16, 2019, 03:36:26 pm
content: Quote from: lukasz.kostka on October 16, 2019, 01:18:45 pmThat looks better but I would still aim for wider Vcc. If you move south edge further south that will make room for it. Its better to have it neck dock through a tight spot and be wide elsewhere than it is to have it skinny the whole way.

author: lukasz.kostka
author_rank: Contributor
timestamp: October 16, 2019, 03:43:36 pm
content: It is fine. I have a 0.4 mm wide trace with 0.035 thick. It can carry 1.2 A which is way more than I need.

author: Kasper
author_rank: Frequent Contributor
timestamp: October 18, 2019, 03:28:24 pm
content: It probably is fine but heat is not the only reason to make wider traces. If you want to learn PCB design beyond this one project, learning how to route power could be useful.I was once tasked with finding and fixing false detection problem in 1000 motion sensors. The PCB designer thought a skinny shared trace was fine. He caused a huge problem for a small business that could barely afford it. All because he thought it'd be fine to make the PCB 1mm smaller than it should have been.