PCB Review Request

The premise for this PCB is rather simple, I want a PCB that shows my initials and can be controlled either with the WLED app or custom Arduino code. The PCB is two layers with the front copper as a power plane (5V for the RGB Leds) and the back copper acting as GND. Power traces are at 0.5mm, with signal traces at 0.3mm, and a differential pair for the USB D+ and D- lines. I actually attempted to make this project a few months prior with an MCU instead of an ESP-32, and am hoping that this is an improvement from my previous design. My previous design can be found here :https://www.reddit.com/r/PrintedCircuitBoard/comments/x8ox5y/pcb_review_rgb_sign/

The current version is as follows:

PCB - Back Copper.pdf (66.2 KB)
PCB - Front Copper.pdf (85.1 KB)
DR Sign 3.0.pdf (178.8 KB)

Any feedback is greatly appreciated.

Hi, the first thing that sticks out to me is the placement of the ESP32 module and the ground plane. If you look on the ESP32 datasheet there is very specific instructions as to the best placement and proximity to other elements on the pcb.


A cosmetic one only, but I’d hide JLC order number somewhere under the ESP32 instead of placing it at the bottom of the board. And if I’m right it has to be JLC x4 (12 letters in total), but you have x3 (9 letters).


Which page of the datasheet mentions placement and proximity? Can’t seem to find it on the specific Esp-32 I’m using or the ESP-32 Series datasheet.

Yes, you are correct the JLC order number is 12 letters in total not 9, never realized that thank you.

Well, which datasheet are you using? :slight_smile: Note that you have a module, not just a chip.

1 Like

I was referring to this datasheet: https://www.espressif.com/sites/default/files/documentation/esp32-wroom-32e_esp32-wroom-32ue_datasheet_en.pdf and also checked the series datasheet: https://www.espressif.com/sites/default/files/documentation/esp32_datasheet_en.pdf

page 15 (or 20 of the pdf)

1 Like

Ahh I see, I’ll read the entire pdf and make the changes as necessary thank you!

Okay, so I read the datasheet which was very helpful btw, and looking in regards to the layout it seems that I have to have the antenna portion either sticking off of the PCB or on the PCB but with no copper, traces, or components and a 15mm clearance. The pdf also suggests for two layer boards that the top layer should be for traces and components, while the bottom layer is for the ground plane where no traces or components should be connected.

If this is the case, then wouldn’t it mean I have to basically redesign the entire board? Right now I have a lot of components and traces on the back which I’m assuming interfere with the wifi and bluetooth capabilities. Was just wondering if I needed to start from scratch in terms of the layout before I actually commit to anything.

In general it does not matter much which of the layers is the GND plane. Most often the bottom is used because that has no (or far less) footprints, and the pads of the footprints would already make holes in the GND plane before even the routing starts.

In your case, I would put the GND plane on the front and then push all signals to the back. If you put the VIA’s under the LED’s you won’t see them and the front is just an uniform color. You can also put all the decoupling capacitors on the back so you don’t see them.

But it’s mostly a visual thing for this design anyway. Keeping a clearance around the antenna is important, and using decoupling caps too, but apart from that there is not much critical stuff on this PCB, and any “decent” GND plane will do.

You can consider hiding the USB connector on the bottom too, or just add some SMT pads on the back and connect it with a dab of glue and some short wires.


Thanks for the tips, I originally had the USB connector on the back of the PCB, but was having trouble routing the D+ and D- lines as they were crossing when I tried to route from the USB connector to the USB to serial converter.

And I see what you mean by swapping layers, by placing the GND plane on the front and moving the signal layers to the back that would clean up some of the routing that is on the front, I wanted to put the decoupling caps on the back as well, however because of some of my component placement on the back it would interfere with other pads or traces.

You didn’t tell about the use cases, environment etc. when your gadget is used. If you for example use only WiFi under 10 meters it probably doesn’t matter almost at all how the device is designed. If you want to use Bluetooth from the next room it probably matters.


Good point, was planning on using this device in the same room through wifi, wasn’t really concerned with having it work from a long distance.

If this is the case, then is my design good to order as is?

What I said was just something to consider. You have to decide yourself. I would at least try to keep the antenna area clean.

1 Like

Do you want to risk RF communication problems from quite easily avoidable causes? If you mess up the clearance around the antenna there is no prediction of how bad it gets. I also have a thorough dislike for bad RF connections.

1 Like

No, I’d rather avoid that, I’ll make the changes as necessary then.

Ok so I started making some slight adjustments based on the hardware guidelines pdf, I moved the ESP-32 to the top right corner, not sure if I should move the other components closer as well as I’m worried the long traces could potentially act as antennas.
image (1)

You still have not implemented those other suggestions. You still don’t have a decent GND plane (with no interruptions), and a 3x jlc string instead of 4 x jlc. (If you put that string under the esp8266 you won’t see it at all after assembly).

I do not like the location of C20, C21 R24 and D20 so close to the mountinghole. When you put in screws, there is not much room for the screw head, and it may deform the PCB a bit locally and those brittle ceramic parts may break.