Am I on the right track with this PCB design? - Page 1
Forum section: electronics / beginners

author: pwnell
author_rank: Regular Contributor
timestamp: September 07, 2022, 12:27:24 am
content: Continuing from my thread herehttps://www.eevblog.com/forum/beginners/how-to-replace-momentary-button-with-timed-circuit/,I have tried to create my first PCB design. Since I have never created a custom PCB I am very new to all of this. I would greatly appreciate it if someone could just peek at it and let me know if I have missed anything or messed something up.Some general remarks:1. This is a very low speed circuit so I know my traces are not efficient, however keep in mind this basically just generates a 13 second pulse to two relays, alternatively, on each push of the push button.2. I will wire in the connections to the switches, power and push button at the spots where I placed through hole pads - my idea was just to solder the wires to the board.3. I made the bottom plane the ground plane, and used some vias to help connect the ground tracks to the bottom.4. I had to use a fake resistor (R8) as a jumper as I could not see a way to connect U3 pin 4 and U3 pin 1 any other way. I will either get a 0 ohm 1206 resistor or use a wire.5. The funny shape is due to the limits of the case I am using - I have two holes which I will use to mount it to the case's standoffs.

author: mariush
author_rank: Super Contributor
timestamp: September 07, 2022, 01:25:44 am
content: Sigh ... could probably replace 2 thirds or more of the components with a single 50 cents microcontroller ... like ATTiny10 -https://www.digikey.com/en/products/detail/microchip-technology/ATTINY10-TS8R/2271065- or PIC10F222 -https://www.digikey.com/en/products/detail/microchip-technology/PIC10F222T-I-OT/1015544As for the layout ... as you still have through holes for the relays and power input, I'd recommend just using through holes for the diodes ... generic 1n400x are cheap, don't see why you have to use surface mount stuff there.align the components, rotate them if needed .. ex the capacitors at the top (c4, c6, c3) ... pcb is big enough you don't have to get them so close to edge and risk something hitting them.if you use vias to ground for some components maybe be consistent and use a via to ground (on bottom layer) for all components. Will simplify the layout.consider using same footprint for all resistors, for example 0805 - you'd still be able to solder 0603 resistors on it but it's wide enough and big enough to even solder leaded resistors to the pads. Don't see why R5 must be such small footprint.if you want to keep everything single sided, it may be easier to have a thicker 5v trace go through the middle of the pcb (between the relays and going all the way to power the U2 and U3 chips.There's a few resistors that can jump over that thicker power trace, especially if you use bigger footprints (ex 0805)... at a brief look I see R3 , R4 and R6 having to jump over the 5v voltage rail.

author: gamalot
author_rank: Super Contributor
timestamp: September 07, 2022, 01:34:37 am
content: I didn't take a close look at the layout, but the outer profile of the board has two "concave" right angles that could cause trouble in production. Sorry for my English, hope you understand what I'm talking about.

author: fourfathom
author_rank: Super Contributor
timestamp: September 07, 2022, 01:53:04 am
content: Quote from: mariush on September 07, 2022, 01:25:44 amYes. Look at the ground on U2 (Pin 7). It goes a very long way before it connects to the common ground. Just drop a via at pin 7.And there's no shame in running a few traces on your ground layer, especially in a slow design. You don't want to break up a ground-plane path that is carrying a lot of current or fast edges, but a few short traces using vias to jump under an obstructing trace can make the job much easier and cleaner. In fact, it might be useful to run portions of your +5V net on the ground-plane side of the board.Finally, don't be afraid of four-layer boards. Some fab houses (JLCPCB for example) charge virtually the same for four-layers as they do for two. Your design obviously doesn't *need* four layers, but it's always something to consider. If you are etching the board at home then yes, use two layers.

author: MarkF
author_rank: Super Contributor
timestamp: September 07, 2022, 02:20:59 am
content: Just a few comments:I would try to avoid running traces right on the edge of the PCB. This helps protect them from physical damage.Don't be afraid to run traces on the ground/power plane. Just insure the plane stays intact (i.e. no isolated areas that need connectivity.) Replace R8 with a trace.Avoid running traces at 45ofrom the inside corners of SMD resistors/capacitors/diodes/etc. I also avoid running traces under these SMD components.I took the liberty to illustrate re-arranging the components around the ICs. Pardon me if things are wired just right. Also, insure you have space for soldering (or a placement order) if you intend to hand-solder.I used all 1206 parts.

author: golden_labels
author_rank: Super Contributor
timestamp: September 07, 2022, 04:21:48 am
content: pwnell:If you are having so much free space, I would use larger capacitors. Tiny MLCC caps come at the cost of reduced capacitance under DC bias. There is no reason to suffer that here. Unless there are some constraints I am not aware of, like price or already having smaller parts in stock. These are mostly decoupling caps, so the exact value is not that important, but it’s still a pointless loss that gains nothing.

author: onsenwombat
author_rank: Contributor
timestamp: September 07, 2022, 08:31:58 am
content: Pretty much parroting others, whatever you do with this particular design is likely not going to be any sort of issue.The caps/resistors in general look a bit funky both in terms of their placement and routing (the upper part esp). This is probably the thing I'd emphasise most here. On this design you got space left and right, but you got parts all over the place to boot. Some other time you might not have the luxury. Learning the skill and habit to optimise the real estate usage, and usually as the result - the visual side of things, will come in handy if/when you proceed to more advanced designs.No clue what levels of currents you have running there, but for educative purposes might consider beefing up some of the nets at least so that you familiarise yourself with this, if for nothing else.Ground vias should be as close as possible to the component leads.Would not run ground tracks on the top side in the first place as you've got the whole bottom plane for this.Don't place anything close to board edges unless you have to do it for whatever reason. Same applies for the routing. You've pulled the GND plane back nicely, but there's that odd track running beyond it.Doesn't matter in this kind of design, but consider copper pours on all layers. If and when you do this, remember to stitch those planes together in generous enough manner.

author: MarkR42
author_rank: Regular Contributor
timestamp: September 07, 2022, 09:00:59 am
content: Edit: answering your question, yes.I think 10uF is probably too much for a decoupling capacitor (it will still work)For strict "correctness" probably you should put decoupling capacitors on all the chips, maybe a much smaller value 1uF or something.But I think it's very likely that it will work in the current configuration, especially as everything is low speed, mostly digital and the chips are probably not very fussy about power smoothness.

author: pwnell
author_rank: Regular Contributor
timestamp: September 07, 2022, 02:03:37 pm
content: Thanks for all the feedback - I will see if I can improve the design. @mariush the point of this design was not to use a microcontroller but to learn how to interconnect these fundamental blocks, and design a PCB which would have been much easier with a single microcontroller and some bypass caps. Trying to learn here - so thanks again for all the comments.