Please verify that I laid out this PCB correctly

Question

I have done Arduino for almost two years now, but I'm new to making PCBs. I have a circuit with a lot of wires and buttons and I need some help verifying it's correct.

Answer 1

Consider using the internal pull-ups as suggested in comments (tutorial), which will save you board space. When drawing circuit diagrams, it's really good practice to make it as uncluttered as possible, without crossing lines unecessarily or having it be confusing. There are good introductions to this here.

Your partial circuit is something like this, which when it's laid out like this is really easy to understand -- a set of switches, each of which pulls a single CPU pin to ground when pressed.

Which leads naturally to a board layout somewhat like the following. Note it's usual to show the board from the top side, where the components usually are. The colours vary in different CAD packages, but in KiCAD (which you appear to be using), red is top (not used here) and blue is bottom copper.

The usual way to do a board is

1. set the size and outline
2. fix anything with a specific location (LEDs, switches, connectors)
3. then do the tracking

Note that it's extremely common to move items around from one CPU pin to another just for the convenience of the PCB. Also most switches of these kinds have two pins for each side of the switch, and you only need to connect to one of each pair of pins. Again, this is for convenience in laying out the board.

It's also very common to lay things out, resize the board, move everything around and really try it lots of different ways.

Obviously these are only starting suggestions. Make sure you point your Arduino in a suitable direction so you can get at the USB socket or 6-pin ISP conveniently. Consider putting switches on one side and Arduino on the other -- it all depends on what you're making.

Answer 2

Not to detract from the prior answer which is quite good, here is my rendition using the copper ground pour concept, (sometimes referred to as "Filled Zones"). Note that all the ground connections are automatically made by the common pour (in green). You do need to assign the pour (or zone) to a node for that to work properly. To complete your design you may need to add additional traces, (your prior design included a 12 pin connector at the side), so using the ground pour idea may help simplify any other routing requirements. This layout includes the Nano on the opposite side as you mentioned. Finally, on your last routing design you didn't connect the extra ground on the Nano at pin 29.
[Later edit to better show ground to pad connections]

Answer 3

Comments are apparently not abided, so.

In short, needs more work. To start with, you're leaving a GND pin unused? Don't. While this is passive board with only some switches, better get used to the fact that GND is sacrosanct. Use the ground pour example from Nedds example and expand it with some stitching vias, i.e., add vias that connect ground to ground between top and bottom layer to keep the ground flowing across traces.

You're also positioning the switches in a fairly haphazard manner. OCD or not, arranging switches in rows and columns looks so much tidier and actually saves space and makes it easier to use them, you can use honeycomb pattern if that's preferable, which is often most space efficient.

Don't forget a millimeter is sort of small distance in real life, although it's nice and big on the layout designer. Think about how much space your fingers need to operate the buttons comfortably, maybe print pcb assembly image 1:1 to give something to poke your finger at, as it were.

There's no prize for doing things one - layer, that's challenging for vets and gets into territory of using parts as jumpers. If you're having PCBs made, there's nbig difference between 1 and 2 layer and usually 2-layer is the default for pooled proto boards.

Oh, and tag the switches. Silkscreen if you have it, copper if not. You can use copper for text, just remember to blank solder resist over it.