Are my PCB and schematic OK? Am I missing something?

Question

this is my first time designing and ordering a PCB, so I'm quite nervous about this. So I thought you guys could have a look, since you are more experienced than me by far.
The PCB is for an enclosure I already picked out, and it will function as a CAN bus controlled relay controller.
I will use it in our EV conversion for the taillights. I designed it to be able to handle 5A, with appropriate external fuses.
The ADC pins are to measure the bulb resistances, to give a blown bulb light or not. I started another topic about the PSU unit, so I don't know much about this part.

Also, does anyone have an idea what's best to do with the GPIO0 pin on the ESP32?

I've made some changes, so here's the EasyEDA project: https://oshwlab.com/pol.peerboom/patrol-lcu

The schematic, now with upload header, all grounds connected and updated layout:

all pin 4's on the relays are the output lights in dutch, and all ADC nets are the voltage measurement for the resistance.

And here the updated board so far:

thanks so much!

Answer 1

A few things I can see...

1. As per comments, NUD3160 avalanche MOSFETs have S/D swapped

2. AO3401A high-side P-channel MOSFET has S/D swapped

3. AMS1117 has GND missing.

4. AMS1117 10uF ceramic on the output does not guarantee stability as per datasheet. Suggest a series 2Ω resistor between the cap and 3.3V. Or switch to a tantalum.

5. Bypass cap near the CAN transceiver.

It would be easier to follow the schematic if higher voltages were on top and power/signals flowed from left to right. Most of that schematic is opposite.

I'll let others comment on the layout, but I'll add images to the question.

Answer 2

The grounding plane on the bottom layer has issues. Only 10-20 mil of copper (if that) exists on the current return path from the relays. The grounding system needs to be near continuous, and if you have a thick trace for VCC to carry current you also need the same thickness at least for the ground.

Remember that copper traces and planes have resistance, the smaller you make the traces the more resistance they will have. This will create problems with large currents so make sure that you look at the current return path from each device back to the ground pin of the power supply. You can even estimate the amount of resistance with a PCB Trace calculator

Answer 3

Just some stylistic comments on the schematic:

• Try drawing your ground symbols always pointing downwards.
• In general, try drawing bigger voltages above lower voltages. It's the other way round under U9, which makes it unnecessarily difficult to understand what's going on. Being consistent here also makes it less likely to screw up polarity of certain devices.
• Also try sticking to a left-to-right signal flow.
• You are using both ground symbols and signal references for your GND net, for example. Don't use signal references for supply nets.
• Please try to avoid "label hell". Tidy little boxes and a lot of on-page references may look "nice" from a distance. But it's really hard to understand what's going on. Try drawing complete wires whenever practicable instead of labels everywhere. You need to put a little effort into arranging your sub-circuits, of course.
• Maybe you don't need pin 1 dots on schematic symbols. That's more common on layout symbols.
• In many places there are junction dots on wires where there is apparently no junction (at pin 3 on K8, for example).
• The part names of your relays obfuscate the net labels which are connected to pin 5.
• P-channel FETs like Q1 are usually drawn horizontally with the incoming voltage on the left. Also double-check if that FET is really doing what you expect it to. If the FET is turned off, the body diode will still be conducting.
• It's not obvious what net the wire connecting C6 and C7 is connected to. I suppose it's GND. If not, the circuit won't work.