ESP32 PCB & Schematic Review: Is there anything wrong?

[AndrewEE]

Hey everyone! This is my first time posting, not sure if this belongs in the beginner section (but as I am a newbie, thought I might post it here).

I'm looking for a review on my schematic and pcb layout using KiCad. This is my first PCB, I've tried to follow datasheets and rules I've picked up by looking at other people's boards (and guides). This is a 2 layer board that I am going to hand solder (with all basic required tools) without a reflow oven or hot air gun.

The project uses a laser sensor to measure distance and sends those readings to the ESP32 that then transmits it over Wi-Fi to my phone (going to try to make multiple different uses).


Here are the components on the board:
ESP32-WROOM-32E module
CH340C USB to UART converter (running in 3.3V mode)
AMS1117-3.3 regulator
USB-C 16 pin connector
VL53L0X distance sensor module connected via a 1x06 header

Resistors and capacitors are 0805 size, transistors are SOT-23 NPNs. Power traces are 0.5mm, signals are 0.2mm, and there are ground pours on both top and bottom layers.

A few specific things I want to ask:
- Are the decoupling capacitors wired correctly for all the components (ESP32, CH340C, AMS1117)? And are they close enough?
- Is the auto download circuit with the two NPN transistors wired right to EN and IO0 correct? I found a schem online using it, but also a lot of people use push buttons.
- Is this layout going to be okay to hand solder with my tools? I picked up good tools, but the only soldering I've ever done before was for keyboard switches.
- I placed some random vias throughout as I found online (I'm assuming it helps connect the ground fills on both sides properly). Is that fine?
- I'm getting two silkscreen violations (one for the USB and one for the MCU) but from my basic research I don't think they matter. Also, not exactly sure why the usb isn't rendered properly...
- I've added some testpoints, based on feedback from others' boards. Is this good?
- Does the routing and overall layout look fine or are there any obvious mistakes? I attached images of the schematic and the pcb.

Thank you for any help provided! Any advice is appreciated.

Updates:
a) In future projects, I will be using newer ESP32 MCUs (ones that don't need the USB to UART converter + its capacitors & NPN transistors).

 

[PGPG]

You're very close to having no wires in your schematic al all. This will make it even more difficult for people to read.

[AndrewEE]

I'm sorry, would it be better formatted to not split up the schematic using labels then? And instead direct wires? Please clarify your feedback.

Thanks.

[orzel]

You're very close to having no wires in your schematic al all. This will make it even more difficult for people to read.

I (respectfully) disagree. I kinda like it this way and find it very readable.

[ledtester]

- I would connect pins 5 and 6 of J2 to some GPIO pins. Even if they are not used by the VL53L0X they might come in handy when interfacing with another device.

- I would redraw the DTR/RTS part of the schematic as it is done here:

https://electronics.stackexchange.com/questions/473443/esp32-dev-board-dtr-rts

It's a bit easier to follow and others might recognize it as the canonical way to interface those signals to the ESP32 and it will make it easier to verify.

- Comparing your board with other ESP32-WROOM-32E modules, it looks like the WiFi antenna will be hanging off the end of the pcb - in case that's an issue.

Edit: Just saw your last pic - guess you already know about the antenna point.

[paulca]

You might want to round the corners  (right click the edge cut rectangle, shape modifications, fillet.

When drawing power symbols, it is "convention" for "VCC" or "5V" to be "Upwards", but it does not mean you need to do silly little U Turns with it either.  Both are equally jarring.  "Vcc pointed down" vs.  "Vcc doing a U bend to point up then Vcc label".

You can turn the test point symbols upside down, so the lead points up.

Personally... others will disagree, but I just use horizontal ones when it's difficult to be "oritientated" properly.  Like headers having --> 5V pointing out the side and/or --->GND

Silkscreen.  Its not there because someone said it has to be.  You can delete it all if you want.  So consider how it might help you.  What is TP3?  If you needed to look at the schematic... go edit the silkscreen put it on there, save yourself the lookup!  Another example.  Do you really care that it's C4?  Would you rather not know, "Oh, thats a 10u".  Sometimes the value is MORE useful to the person reading the silkscreen.  Note.... as you are building this board, thats YOU.

Put yourself into your future seat.  The board has arrived.  You have to solder it.  How?  How are you holding it down? What size is it realy?  What does it look like if I put a 3D model of my soldering iron tip in frame?  Can I even get between those components to solder it?  Look at C1 and C2.  How are you getting the point of your iron in there to solder them?  You'll have to do them before the IC!  Just be aware.

Your BOM includes about 4 different R values and about 4 or 5 diferent C values. 

USB CC pulls, 5.1k - probably taken from a datahseet.  Compared with the I2C pull ups, 4.7k - probably  basic convention for a "Medium hard pull on a transmission line", but I don't think it would make the sligestest difference if you just used 5.1k on the pullups too.  I doubt USB-C Would care about them being 4.7ks either.

The CH340 is showing as having electrlytic.  But I think you mean ceramic.... but it depends as it's an AMS1117.  Personally I would just put 1u ceramics on everything, 10us on the reg pins and call it done. 

Even one less tape to handle, one less component to "ping" across the lab or get blown off with the hot air... one less headache.  In digital electronics (RC circuit aside), you can get a LOT done with 10K, 4k7, 10u and 1u.  EDIT:  If you want it assembled... that figure right there... "Unique tapes to load", is direct tooling cost you pay.

[PGPG]

You're very close to having no wires in your schematic al all. This will make it even more difficult for people to read.

I (respectfully) disagree. I kinda like it this way and find it very readable.

Reading from top-left (I expect it being standard way in most countries were you write from left to right):
Do Q1 and Q2 functions are really clear for you?
Schematic suggests that Q1, Q2 emitters are the pins with the highest voltage. Are they? If yes then which way?
Looking at Q1, Q2 schematic part you expect RTS and DTR being RS232 interface lines so ±12V and -12V being send (in some situations) to EN and IOD nets.
If they will be connected with wires Q1, Q2 functions would be much clear (at least for me).
I gave up at that point and didn't went farther in schematic.

[Analog Kid]

General rules of thumb for easily-read schematics:

• Signal/logic flows from left to right
• Power goes from plus to minus (Vcc/Vdd to ground) top to bottom, unless circuit uses a negative supply
• All one drawing, please, connected as much as possible rather than separate little boxes

These aren't hard and fast rules, but most people find these give the most readable diagrams.

[kjr18]

This schematic is not that much complicated, you easily could connect everything with wires, only flags left would be power and ground, it is easier to follow connections and spot errors. As for Q1 and Q2 transistors if you need board space you could use something like UMH3N, that way you could reduce component count by replacing both transistors and their base resistors with single small SOT363 package.

If you really need to split schematic to parts, make their function broader, in this example split them to two blocks, one esp32 and TOF sensor connector in one block, and everything else on another. that way you only have four connections between both blocks (rxd, txd IO0 and EN.

[paulca]

Personally in almost all causes I prefer labels to wires.

Why?

When you have a wire, what do you do with it?  You follow it to were it connects and read that label... why bother with 2 steps when 1 is available?

The exception is when the two components are right side by side in the schematic or when they NEED to be side by side in real worlk for a reason.  eg. crystals, specific decoupling caps etc.  However, and just my way, if wires have to cross.... its back to labels.  I just cannot stand birds nests.

[PGPG]

Personally in almost all causes I prefer labels to wires.

Are you human or AI?

When you have a wire, what do you do with it?  You follow it to were it connects and read that label...

What label? If the wire connects one thing with another than what for labels.
For example from input you have transil to GND (power symbol) and 4k7 pull-up to 5V (power symbol) than resistor to transistor base and also resistor and capacitor from base to GND, emitter to GND and collector to uC input (internal pull-up). You can have no label on the whole that way (except power symbols at top and bottom of this circuit).
This connection is not as simple as elements side by side so you suggest to separate it into several parts using some labels?
It is how the transistors were connected in the schematic from the first post.

When you have wires you see what is connected to what. With labels you have to search whole sheet to find second label and you are never sure if the label is not used also somewhere else. If you find 3 such labels you are not sure if you should search for the next one and so on. If wire doesn't go any more you know that you see whole connection.

But the human mind is inscrutable and there are people who can spot all the labels at a glance (like in the movie "Rain Man").

[kjr18]

When you have wires you see what is connected to what. With labels you have to search whole sheet to find second label and you are never sure if the label is not used also somewhere else. If you find 3 such labels you are not sure if you should search for the next one and so on. If wire doesn't go any more you know that you see whole connection.

But the human mind is inscrutable and there are people who can spot all the labels at a glance (like in the movie "Rain Man").

If it is as searchable pdf you can at least search for labels, good luck with pictures. Not everyone in the world is genius, or have perfect memory. We are human after all.

For many people it's easier to follow signals with wires. And it helps with pcb layout tracing.

As for any other tips I think you should add a bit more area connected to 3.3V. Maybe with some via's connecting to other side of board. That way you will have more heatsink area.

[JustMeHere]

Those copper pours and the slots in them are going to cause some noise. 

You should consider do this type of work with a 4-layer board.  A little more expensive but WAY easier to route.

Putting slots in your ground plane will cause noise with any signal that needs to cross the slot.  It doesn't have to be a high frequency signal....just a signal with a fast edge.

Also, I'm not seeing any TVS or fuses on your USB input.

Consider mounting holes...and put them on a 10x10mm grid (project box mounting plates are allegedly aligned to this, but I haven't had a chance to prove it to myself.)
Consider through hole test points.  The hole makes it easier to rest a probe.  You can also buy little test point clips for dirt cheap and stick them in the holes during testing (https://www.digikey.com/en/products/detail/keystone-electronics/5001/255327  -- get the right ones for the hole size you choose)

Personally in almost all causes I prefer labels to wires.

Yeah, I find giving up a little on the schematic with more labels, makes the actual routing easier because all nets have human names and can be found on the schematic.
And when you ask AI to "proof read" your board, it doesn't get hung up on crossed wires.  (Yeah, it does help a bit.  It can catch mistakes...and make mistakes.  But that's nature of "paired-programming")  These clips effectively give you more "hands" as you can use a "witch's hat" instead of the probe pin to test.