| Nice board, looking forward to seeing your next one. A little feedback, helpful I hope: A "via" is basically just a wire stuck right through the whole board top-to-bottom. (Okay, it's not really a wire. They drill a hole and then chemically grow a layer of copper that fills the hole.) You can connect the copper pattern on any layer(s) to that "wire", so it's often used to route a signal from one layer to the other. But you already have a real wire going through the board: the GND header pin! So no via is necessary; just connect directly to that pin on each layer (kicad probably did this for you automatically). This trick works with all thru-hole pins. For RF or high-current applications, sometimes you cover a board with a grid of vias, just making redundant connections between the planes all over the place, "stitching" them together. But careful, add too many vias and the PCB shop will bill you extra. Putting a GND pour on the top layer is a good idea. It's lower-impedance than individual skinny traces, and takes less/zero effort to route. The GND trace you manually routed isn't necessary; you can see by the transparent-red shape that kicad already has copper there. However, you ended up with a little "island" of dead copper between R2 and C2, which is the real reason you needed the via. A better approach would be to use the bottom layer for +3.3V power instead of a redundant ground pour. This gets rid of the +3.3V traces (BTW, best to use a single, thicker one instead of 2x side-by-side) and unifies the island into the ground pour. Even though this is a micro-power application, playing the traveling-salesman game with long scraggly power traces is never a good idea. You would still need vias to connect each top-layer +3.3V SMD pad to the bottom-layer power plane, but the signal-integrity benefits of a plane make this worth it. Maybe the absolute best is an uninterrupted GND plane on the bottom and a +3.3V pour on the top. Putting SMDs on the bottom side makes the board cost more, so good call leaving them all on top, but putting traces on the bottom layer is free. So you can even move signal traces between layers to avoid cutting up your planes too much. It's "fun" with big complex boards, like untying a giant knot... You are very miserly with your +3.3V global net symbols in the schematic! You can place as many as you want to optimize the schematic's readability. Especially near the CSB pin, the 4-way solder dot looks like some intermediate signal in a voltage divider, but it's actually just +3.3V. Same suggestion with GND -- basically, it's more informative to read "this pin is GND, and this pin is GND" than "these two pins are connected, I wonder what they're doing...oh, it's all GND". Pull-up resistors are usually oriented vertically, too, so they graphically pull "up"! Anyway...I hope you don't mind all my constructive criticism. It's nice to see something on HN I know about! |
Note that without a plated through hole (vias are small plated through holes, those designed for component legs are bigger) the solder will only adhere to one side. For mounting large components where vibration may be a problem this will make the pad weaker & more likely to lift off. A plated through hole lets the solder flow through & bond to pads on both sides. So you sometimes do need plated through holes.
Otherwise I agree. These days 4-layer boards are so cheap it's often worth just dedicating an entire layer to ground, and one to power. E.g. Signal, ground, power, signal. All your ground connections become vias. Most of your power connections are vias to a lower inside plane. Your signal traces are available to probe & rework easily. You get a bit of distributed capacitance from the power & ground planes.