First PCB design - seeking wise counsel - Page 1
Forum section: electronics / projects

author: sentry7
author_rank: Regular Contributor
timestamp: October 02, 2015, 10:49:34 pm
content: Hey guys,As the title says, I'm designing my first PCB; I'm just a bit into the routing process. Before I go any further, I want to get some opinions of the board as far as board dimensions, component placement, and routing is concerned. Below, I have some shots of the design. In order, they are bottom layer, top layer, silkscreen, and all layers.As of right now, the board dimensions are 6" x 4".

author: KL27x
author_rank: Super Contributor
timestamp: October 02, 2015, 11:26:00 pm
content: Some of your thin traces look kinda lonely. Say, the trace between C19 and R18, for example. When the board etches, thin traces can get overetched if they aren't protected by other traces or planes. Which brings up another point. You might be able to significantly simplify your routing if you use ground planes, top and bottom, and using planes takes care of this problem, automatically.The traces on the left side of the top image also look pretty lonely. Personally, I try to bundle them together tighter, in between the points where they diverge to run between pads, unless inductance or timing is a concern.Mind, if you're making just one or two, this isn't a concern. But if you are making a lot of these, this kind of thing can change your yield/cost in the long run. Making things easier for your board manufacturer never hurts. Maybe keep that in mind for your next project.

author: tautech
author_rank: Super Contributor
timestamp: October 03, 2015, 12:06:26 am
content: Not too bad.Component polarity and DIP pin 1 both signified with a square pad.The one thing that strikes me is the very thin annular ring on all DIP pins.Yes, thicker one do make it harder to route traces in between, but that's a price you must pay for ease of rework. Thicker pads don't come adrift like skinny ones do.

author: sentry7
author_rank: Regular Contributor
timestamp: October 03, 2015, 12:19:03 am
content: Quote from: tautech on October 03, 2015, 12:06:26 amYeah, the IC pads have an outer diameter of 56 thous with the holes being 29 thous, so the ring width is 56 - 29 = 27 thous. What ring width would you recommend?

author: sentry7
author_rank: Regular Contributor
timestamp: October 03, 2015, 12:28:22 am
content: Quote from: KL27x on October 02, 2015, 11:26:00 pmThanks for input, KL27x. So you're suggesting I bring the traces in tighter to one another in areas like the one marked?

author: KL27x
author_rank: Super Contributor
timestamp: October 03, 2015, 12:35:32 am
content: Well, I would just throw in a ground plane and call it a day.But if you do not want to use one, I start thinking about trace "shading" when traces are 12 mil and smaller on a 1 oz board. This is very conservative, but it ensures the board can be banged out in high yield by a bottom dollar manufacturer, if that's the route I go.In the top half of your outlined area, you could just make your traces as big as you want.In the bottom half, that's where, in absence of a ground plane, I would try to bundle the traces tighter if they're thin. I usually shoot for a gap between traces to be the about the same thickness as the traces.For the thru hole pads, if you want to make the board really bullet-proof, one thing to consider is using oval pads to create large bonding surfaces while leaving room for routing signals.

author: sentry7
author_rank: Regular Contributor
timestamp: October 03, 2015, 12:48:08 am
content: Quote from: KL27x on October 03, 2015, 12:35:32 amI absolutely agree with the use of a ground plane. The signal traces are 10 mil and the power lines are 50 mil. I still have a lot of routing left to do. This is a single board computer, so I have plenty of buses left to wire. I'm actually afraid that my components are too close together and that I may run out of routing space. Looking at the silkscreen, what do you think?

author: tautech
author_rank: Super Contributor
timestamp: October 03, 2015, 12:49:15 am
content: Quote from: sentry7 on October 03, 2015, 12:19:03 amI make all DIP pads 100 x 60 oval except pin 1 and then you can still get fine traces in between if needed.All other TH passives 100 mil/thou.All polarized components should have 2 different pads. (no need to keep refering to the top overlay for + or cathode etc)Home etching is not quite as accurate as commercial made PCB's (under-cutting etc) so I err on the larger sizes.

author: sentry7
author_rank: Regular Contributor
timestamp: October 04, 2015, 10:14:01 pm
content: OK, here is what the final board looks like (with possible minor adjustments). I just want to run this by you guys for a quick review.Question: I have now realized that a lot of my pads for discrete components are on the top layer. I know that soldering some components on the top layer may be difficult (ICs, not so much). Is soldering top layer components too difficult? Should I do some rerouting?

author: JoeB83
author_rank: Regular Contributor
timestamp: October 05, 2015, 07:30:41 am
content: Quote from: sentry7 on October 04, 2015, 10:14:01 pmI'd increase the pad size for all of your through-hole components, and maybe widen the 10 mil traces to 15-20mil, if it's possible.And, as others mentioned, try a ground plane, it may de-clutter things a bit.Edit: are the caps next to the ICs decoupling caps? If so, maybe try to get them as close to the power pins as possible. (Of course, making sure your parts will fit, especially if you're going to use sockets for the ICs!)

author: sentry7
author_rank: Regular Contributor
timestamp: October 05, 2015, 07:49:08 pm
content: Quote from: JoeB83 on October 05, 2015, 07:30:41 amI'll see what I can do.Quote from: JoeB83 on October 05, 2015, 07:30:41 amThere is actually a hidden ground plane in my layout; I will upload it in the next revision.Quote from: JoeB83 on October 05, 2015, 07:30:41 amThose caps are decoupling caps, and I am using IC sockets but I will try to get the caps a bit closer to the power pins.

author: homebrew
author_rank: Frequent Contributor
timestamp: October 05, 2015, 08:32:45 pm
content: Well, the board might perhaps run but overall I think you could do far better. Some minor remarks:1) From the position of power and ground on U2 I assume you are building some Z80 system. U3 and U4 would be RAM/ROM. I would suggest putting these chips together as the data/address bus is largely the same. Keep the bus as short as possible.2) In general I would either put some ground planes in place (on both sides and use a lot of vias to stitch the planes together) or run a fat (32mil) trace of both VCC and GND underneath each IC ensuring small loop areas in the power section. (improves EMI-protection)3) Your voltage regulator circuit doesn't look that nice as well... I assume it is a 7805 or the like. These devices need bypass capacitors (100n) as close as possible to the In- and Out- pins to operate stable. Also a diode in reverse across the regulator will protect it if the input has less voltage than the output side (i.e. in the instant when powering off the device and the caps are still charged). Capacitance seems to bee too less in general. Put at least 470 uF at the input. Ah yeah, do yourself a favor and add a diode in series with the power jack to have some protection against wrong polarity. A fuse would also be nice...In general I would highly recommend an in system programmable device (Atmel/PIC or the newer 8051 derivates) as it is sooo much more productive. But that ain't my business :-)