PCB review request - ESP32-WROOM-32

[Inappropriate name removed by admin]

Looking for feedbacks on this project ive been working on, so roast me all u can on design, component placement and routing that i need to improve

[Kim Christensen]

I don't think you can put the ESP32 in the middle of the PCB like that. That would severely limit the WIFI/BT range.

As per manufacturers documentation.

[PlainName]

so roast me all u can on design

Schematic:
Why aren't the switches placed to the left of the ESP? If they were you could just, like, connect the wires and not have floating labels that go who knows where.

Why not continue the current sensor wire up another inch or so and connect them to the pins without floating labels that go who knows where? Really, what's the point of that inch or so break when the things are point in the right direction and in the right location anyway? Just makes it harder to see what goes where and does what to whom.

[Gribo]

Put the antenna on the board edge (The module's antenna PCB edge should align with your board's edge). Make sure there is sufficient clearance, Do not place any parts or ground plane under the antenna. Look at Espressif's layout guidelines.

[RiZsho]

Schematic:
Error #1: U4 A and B aren't really connected anywhere
Readibility #1: On the "Current sensor" section you have vertical wires going from Opamps and horizontal text. Make lines horizontal
Readibility #2:  RS485_EN label on ESP has no wire. Sure it's connected but it looks weird and unfinished

[Batang]

Biggest issue is having the ESP32 in the center.

The ESP32 antenna should be at the edge of the PCB and have lateral clearance as well.

There should be no copper pour under the antenna!

[ANTALIFE]

What's going on with the footprint/3d model for CN1?

[amaschas]

I can give some general feedback, though since I don't know what this thing is supposed to do it's a bit difficult.

I would echo what others have said about the ESP32 placement. I recommend reading this document, particularly the portions about placing the ESP32 module on a PCB: https://docs.espressif.com/projects/esp-hardware-design-guidelines/en/latest/esp32/esp-hardware-design-guidelines-en-master-esp32.pdf

I am not a professional PCB designer by any means, but I have done several board layouts with the TSP5430 in conjunction with an ESP32. Here's the TSP5430 layout and schematic from a recent design for a 7-12V -> 5V DC/DC converter. The actual design for the circuit was taken directly from TI's webbench power design tool, which I find pretty handy for DC to DC regulators.





I would note the continuous ground plane that connects the circuit grounds, solder pour and arrangement of parts that touch the PH net, the lack of long traces generally. Everything is as close together on the PH net as I could make it since that's where all the switching is happening. I'm trying to keep the loops where current flows into the circuit and then back to ground as small as possible. I also think the bulk input capacitance is generally better supplied via ceramic capacitors due to ESR concerns, so the electrolytic capacitor at C3 is a concern. Note that I have 3 big 1210 47uF ceramic capacitors in parallel on my design to reach the desired input capacitance.

[mengfei]

...just curios what name did he/ she used 

[Kim Christensen]

Alternate name for a cat or woman's bits + a verb. 
They may be confused trying to relog with the new username. 

[mengfei]

shouldn't those be flagged during registration   

[Kim Christensen]

I seem to remember that he substituted 55 for the letters ss to fool the naughty word filter bot.