PCB Review Request - RGB Initials Mini sign - Page 1
Forum section: electronics / projects

author: dreece2498
author_rank: Contributor
timestamp: January 14, 2023, 07:06:15 pm
content: This PCB is a direct follow up to the PCB I posted a review on a few months back which can be found here:https://www.reddit.com/r/PrintedCircuitBoard/comments/x8ox5y/pcb_review_rgb_sign/After realizing the design was garbage, I decided to do a complete redo with an ESP-32 instead. The idea is to control the RGB leds using the W-LED app, that way I can have numerous options for different animations and such. The PCB is a two layer board with the front copper as power (5V for the RGB Leds) and the bottom acting as a ground plane. I made sure that no copper or traces were near the antenna on the ESP-32, as I know that can cause numerous issues. Power traces are 0.5mm, signal traces are 0.3mm, everything but the CP2104 will be hand-soldered. I tried to keep the board as small as possible, and only use parts that were needed, as I found with previous designs I was adding stuff that just wasn't necessary.The schematic can be found here:https://www.docdroid.net/0aathMx/dr-sign-30-pdfSome questions that I have concerning my design:I'm aware that MCUs often have to be bootloaded in order to program them, what exactly do I have to do with the ESP-32 in order for it to work with the W-LED app? This is my first time using it so I am unfamiliar with how it works.Is hand-soldering an ESP-32 difficult, or should I pay JLC to solder on the part for me?Is there anything missing in my circuit that I would need for the design to work properly?Hoping for this to be a big improvement from the design I made back in August. Any help is greatly appreciated.

author: mariush
author_rank: Super Contributor
timestamp: January 14, 2023, 08:47:38 pm
content: Ugh ... that trace on the back that cuts all that ground fill...If you insist on using those addressable RGB leds...You can probably move the small decoupling capacitors for each led on the other side and just have vias going to each leds Vcc and VssThis way it would look nicer on the front.Could probably not have those traces go through the middle of the D. Consider adding some 0 ohm resistor as jumper links (to jump over traces on other side) inside of using vias and messing the look in the front.. Maybe try moving your usb stuff towards the corner of the pcb, or maybe rotate the esp32 90 degrees and move it above the usb connector so that those traces that need to go around the chip don't need to cut the ground so much.You have D34 and D43 oriented differently on the pcb and their cap is on the other side of the led.

author: CountChocula
author_rank: Unknown
timestamp: January 14, 2023, 09:16:19 pm
content: Howdy! Took a look at the schematic—some random notes, in no particular order:Are you sure you calculated your current budget correctly? Looking at the datasheet for the LEDs you use, they need up to 12mA each, and the ESP32 can take big gulps of 100-200mA, especially when WiFi is on, so you could pull 400mA or more, and that's without accounting for the regulator and serial chip. You might end up exceeding 500mA total consumption, which could result in your USB supply current limiting you and causing glitches when your LEDs are all on at maximum brightness.Similarly, if you want a fuse, 2A seems way too high to me…There is a LED_OUT label in both the regulator section and the ESP32 section; as it is, I think D20 may effectively be tied to R10, which is probably not what you want. I'm not sure, though—perhaps labels don't carry across sheets, but I would not use the same for both nets, just to be safe.What is the purpose of R23? I don't think it's necessary.The ESP32 comes with its own bootloader; as long as you have a proper serial connection, you shouldn't have any problems. However, I would not bother adding a USB to serial interface on the board unless you expect to program the chip very often (and even then, I would probably suggest you use OTA updates). I would consider simply routing out the serial pins and using an external FTDI breakout likethis one: they're cheap, they don't take up board space, and someone has already done the legwork of figuring out how to make them work. If you absolutely need the serial chip… you would probably be better off just using an off-the-shelf ESP32 breakoutIt's not hard to solder the ESP32 to a PCB; the castellated connections require a little more care than a THT component, but they're not a big deal. On the other hand, it might be good to have JLC mount at least the LEDs; their PNP machine will position components much more accurately than you can if you assemble the board by hand, and the end result will look much neater. Consider having them also assemble all the passives—that way, you can use smaller components that can save board space. For example, I've attached below a picture of a board they assembled for me, and it looks a million times better than the prototype I had soldered by hand (I soldered the ESP32 here, but they did the LEDs and passives). As I recall, it was pretty inexpensive to have 5 fabricated, and it looks good enough that several friends have one in their living rooms.Good luck!—CC

author: dreece2498
author_rank: Contributor
timestamp: January 14, 2023, 11:30:12 pm
content: Thanks for the feedback, I'm assuming the trace your talking about that's cutting the ground fill is from Q30 to pin 3 of the ESP-32. Which side of the RGB led do you recommend moving the decoupling caps too? The trace connecting from VDD to the cap probably isn't necessary since I have a power plane on top. What parts do you recommend that I add the 0 ohm resistors as jumpers? And wouldn't these still need vias to connect to these resistors if they are on the back copper (I'm probably misunderstanding what your saying here)? Good catch on D34 and D43 I will change that accordingly.

author: dreece2498
author_rank: Contributor
timestamp: January 14, 2023, 11:35:35 pm
content: Thanks for the feedback, if that is the case in terms of current consumption then I'm better off switching to a regulator that can withstand up to an 1A instead of just 500, as for the labels since they are net labels and not global labels, they do not carry over although they should not be the same name so I changed that. R23 was used as a resistor for the signal line of leds, which was recommended by sparkfun here:https://learn.sparkfun.com/tutorials/ws2812-breakout-hookup-guide?_ga=2.18477049.1505323406.1673739193-1196797627.1659886592&_gac=1.256994169.1673739193.CjwKCAiAwomeBhBWEiwAM43YIDyLdJ2Ws7F7peS2Wsp9LHnN63pHf_JvaCZHBoJwuP5HjQ09lLm_4BoCwUcQAvD_BwE since the led I'm using is essentially a clone of that one. The 2A fuse can also get lowered to 1A as well.In terms of the CP2104, I wanted to use it originally because I didn't want to use any breakout boards and wasn't sure if it was needed in order for the ESP-32 to be able to communicate with the W-LED app.

author: bidrohini
author_rank: Regular Contributor
timestamp: January 21, 2023, 07:56:25 am
content: You can also post your design tohttps://www.pcbway.com/project/questionpublishMany experienced PCB designers are there. They also may give some valuable opinions.