[feedback] My first PCB. Felt pretty easy... what am i missing? - Page 1
Forum section: electronics / projects

author: ID_739762
author_rank: Newbie
timestamp: April 26, 2025, 07:51:13 pm
content: Hey forum,i never thought i would touch that black magic called pcb design ... but for several art projects i need to make some "breakout boards" with a keyboard switch and 2812 LED's. It needs to be compact and every switch to be on its own board (i want to do different shapes and maybe one odd switch in the wall or something). I thought for prototyping and experimentation that would be nice. The switches will be read via a mux and the LED's to be handeld like a ws2812 led strip with FASTled lib, daisychaining the modules.Did i do it right? I followed the datasheet wireing example. Im not much of an electrical engineer... :smiley:It would be nice if someone could take a look at it and tell me if i goofed up :smiley:Thank you!

author: CurtisSeizert
author_rank: Regular Contributor
timestamp: April 27, 2025, 07:27:48 pm
content: Ultimately, if it does what you want it to do, then you're OK. The demands on this are not very stringent, so it will probably be fine. That said, there are a couple things I would recommend here.(1) Make GND a plane, say on the bottom, and do all the routing on the other side. This will help with signal integrity.(2) Think about return currents. All the current that flows in to V+ (or elsewhere) is returning via GND. Large changes in current can create voltages between different points in your GND net. Especially be wary of sharing GND return paths between signal (data) lines and higher current lines (e.g., LED supply). Often, it is trace inductance, not resistance that is the issue. Point (1) helps to minimize inductance.(3) When I place some active part on a PCB, the very next thing is placing decoupling caps. These should be as near to the power pin as possible, and this is generally a high priority.(4) For readability, use power symbols in your schematic rather than global labels. Naming your nets at the schematic design stage is helpful when you're laying out the PCB.(5) It is probably inevitable that your first PCBs will not be good, and that is fine. Do the layout as well as you can, and take the time to diagnose issues when they come up so you know what changes to make.(6) Put a name, date, and revision on the PCB so you know what it is.Assuming you will be assembling this yourself, get a syringe of tack flux. Solder bridges, especially to power or ground pins, are not fun to debug if you don't see them. There are a lot of bridged pins on gull wing parts that I tried to desolder and resolder when I was starting out. Now, if I see something like that, I hit it with a dollop of flux, touch it with the soldering iron, and surface tension does the rest. Flux pens just don't work as well. I hope this helps.

author: Ice-Tea
author_rank: Super Contributor
timestamp: April 27, 2025, 07:57:02 pm
content: In addition to the above: how many of these do you want to daisy chain? You'll find that the amount of current adds up pretty quickly, with your current layout you're also likely to find there's something called "fusing current" for traces on a PCB. In other words: you need to run that 5V trace much, much thicker.Also not sure where you got 104nF as a value. You might be able to get it, but the standard is 100nF.Not sure what that multiplexer is supposed to do but I'm guessing it can't read the state of the switch if you don't bias it somehow.

author: pcprogrammer
author_rank: Super Contributor
timestamp: April 28, 2025, 05:40:50 am
content: Quote from: Ice-Tea on April 27, 2025, 07:57:02 pm104 is possibly the notation used on a capacitor to indicate that it is 100nF. 10 with 4 zeros in pico Farads.About the switches and using an analog multiplexer, yes it will work, but it is from a microcontroller point of view more efficient to do it digitally. Depending on the number of switches one can use a scan matrix to reduce the number of pins or a digital multiplexer if the switch count is low.For this it is also needed to de-bounce the switches, either in software or hardware. When using a digital multiplexer a capacitor to ground and a pullup to vcc, with the switch in parallel on the capacitor will do the trick.When using a scan matrix, the switches need diodes in series to allow multiple to be pushed at the same time.Another issue might be the serial data connection of the LED's. Depending on the data rate, the length and type of the wiring, it might be needed to add small series resistors to maintain data integrity.

author: Solder_Junkie
author_rank: Frequent Contributor
timestamp: April 28, 2025, 09:41:20 am
content: A couple of basic issues when designing print boards for “home” construction:1. The datasheet pad layouts are generally for factory assembly, if hand soldering you need an extra millimetre, or so, of pad width in order to solder by hand.2. Check with the actual switch that it doesn’t foul other parts on the board.Both issues can be checked by printing the board on paper and placing the part(s) on the paper.PCBs are incredibly low cost from JLCPCB, but it still helps to get things as near as possible before sending off the files.

author: TheBereavingBee
author_rank: Newbie
timestamp: May 14, 2025, 04:59:59 pm
content: For a first attempt you are doing great. I'm only going to talk about the layout for this board. It does look like you are missing a via connecting C2.I would recommend avoiding via-in-pad by pulling the vias out of the pads and connect with a trace. Having a hole in the middle of the pad can cause solder starvation during assembly as the liquid solder wicks into the hole.You can lower the cost of this board by increasing the trace width of these connections. Its easier to fabricate a board with larger traces and larger spaces in-between traces. Usually specified by a the fab house as something like "5/5 space and trace on 1 oz copper" which means 5 mil traces with a 5mil gap between them. This is related to the copper weight or thickness of copper on the board. A higher weight copper board will need a wider trace width and larger space to keep the cost down.If you can avoid right angles on your traces then you should, this will radiate less than a 45 degree elbow. It wont make a difference on this board but its good to start with best practices early.Pouring a ground plane can help with heat dissipation and EMI as well.Good luck and keep it up!

author: bson
author_rank: Unknown
timestamp: May 15, 2025, 08:07:24 pm
content: As you've noted, it really doesn't have to be that complicated.Most comments would be minor stylistic suggestions, for example to use global power symbols in KiCad instead drawing wires for power rails. And use "GND" instead of "GND IN" (because power isn't really conceptually directional like signals, although it is). For the PCB, use the fattest traces you can fit - or at least like 30 mil or something. Thin traces are more fragile, but realistically it makes no difference. Just about lining up all factors in your favor, even tiny remote ones like if you drop the PCB and just happen to nick one of those traces.This is why when people talk of autorouting simple boards we collectively roll our eyes here...

author: eugene
author_rank: Frequent Contributor
timestamp: May 16, 2025, 01:36:21 pm
content: I haven't completely verified your design, but as others have said, if it works then it works. My major suggestion is as follows.Having separate GND in and GND out as well as 5V in and 5V out is a good idea if you're planning to run separate wires in and out. However, you can simply connect both GND pins together right at the connector. Likewise both 5V pins. Your design has both running all around the board from in to out. There's no need for that and it means that all of the current powering all of the boards needs to go through all of those skinny traces on the first board. Just connect the pins on the connector together with traces that are as fat as you can reasonably fit without heroics.Others have offered the suggestion of putting a ground pour on the bottom side. In some applications that makes good sense. In some it's virtually required. But in this case I don't think it's necessary if you connect the GND and PWR pins at the connector and fatten up all of the traces. Fat traces cost the same as skinny ones (except really skinny ones might actually cost more in some cases.) In fact, the fab house generally prefers to leave more copper on the board and etch away less.

author: JamesE
author_rank: Newbie
timestamp: May 18, 2025, 10:13:30 pm
content: Generally I'd just recommend keepingabovethe manufacturing minimum specifications unless absolutely necessary. If the manufacturer states a minimum of 0.2mm trace width, go for 0.25mm or 0.3mm if you've got space. Whatever the minimum margin is between holes and traces, allow even more space with your routing.I did a keyboard PCB a while ago and from my example, you can see how I steered well clear of the minimums. It's just a guarantee that it can be manufactured easily and traces are more resistant to damage.