2
\$\begingroup\$

I'm trying to create my very first PCB and before wasting my money on ordering non-functional PCB, I'd like to ask your advice.

Background: I have WS2815 LED strip, controlled by ESP32 which uses two touch buttons as an On/Off/ChangeMode signal source. This strip is powered by 12 V and have 5 V data signal input. ESP32 is 3.3 V controller as well as touch buttons, so I have to use level shifter for data line and DC-DC regulator for powering ESP32 and buttons. I already have ESP32 programmed and everything wired in place (soldered using hunging wires from here to there between adapter boards), but this is a bit of mess. My current setup:

  • Notebook PSU with 12 V and 5 V (USB port) output, powerful enough to power my setup
  • ESP32 soldered on adapter board
  • 74HCT125D soldered on adapter board
  • AMS1117-3.3 soldered on breadboard power supply (I've soldered wires directly to the AMS1117 pins while it still soldered to this board, keeping the board as it is except for the added GND, 3v3 and 5v wires)
  • two TTP223 touch buttons hidden in places
  • WS2815 led strip itself (3m of strip, 60 LEDs/m, 180 LEDs in total if this matters)

I have PCB drawn using easyeda.com which is appears to be (mostly) identical to my setup, but I'm not sure if I did it correctly.

EDIT 2: With all suggestons below I've made another attempt which looks like final to me (I'm not going to make industrial-grade product, this is just a PCB for my humble DYI, so I'm already happy with results which are much better than I was able to achieve by myself).

Decoupling capacitors are finally close to the inputs (not as close as they are supposed to be, but as close as I could achieve).

Unused inputs on 74HCT re no more floating and design allows to cut the traces when I need to use them and solder the wires back when I no longer need them.

There is no more GND plane on top side which decreases the possibility of isolated GND islands and (in theory) decrease the possibile cross-talk.

I'm going to stuck to LM1117MPX-3.3 which should have TAB conected to Vout (3.3 V in this case), so this allowed to simplify the traces routing.

5 V pin on debug pin headers still not connected, but again, if I would really need it I'll solder wire to it.

Updated pictures are below.

Schematics:

Schematics

PCB layout with copper areas shown:

PCB with areas

PCB layout with copper areas hidden (for readability):

PCB without areas

PCB 2D preview (top side):

PCB 2D top

PCB 2D preview (bottom side, flipped horizontally):

PCB 2D bottom

PCB 3D preview in case if anyone wondering:

PCB 3D

Some points regarding decisions made while I've drawn this PCB:

  • PSU itself, LED strip and buttons are located separately, therefore not present here, it will be soldered using pins and/or pads
  • components are chosen based on elements I already have (PSU, buttons, LED strip), elements that are on the way to me (couple other ESP32 MCUs for this and other projects), and components which are available in the local stores (for example, 74AHCT125 appears to be better because it is faster, but I only have 74HCT125 available in my area, ordering it somewhere else would be really expensive just because of delivery costs with no visible benefit)
  • I'm not really experienced with soldering and the only iron I have is TS100 with BC2 tip which makes it hard to solder small elements, this is why capacitors are 1206 - I won't be able to deal with smaller ones, this size is my absolute minimum at this moment
  • I'm pretty sure that I will either modify this later (add new button/sensor/whatever) or do something wrong while soldering this one, that's why I left some spare pins and connection pads on the board (so I'll be able to cut wrong trace and solder wires to correct this)
  • PCB thickness is a key. It will be hidden behind furniture so it should be as thin as possible (that's why pins are 90 degrees, for example)

Some questions I'd like to clarify:

  • Should I alter traces somehow? It was autoroute with some manual post-routing adjustment (several traces went through via holes to the other side and back with no reason, while small manual traces replacement solved this). Currently it is set to 0.382 width with 0.254 clearance, but I could mess with clearance during manual adjustment.
  • Is it ok to have footprint for pull-up/pull-down resistors like this?
  • Any advice on the components used here? Unfortunately not every replacement option is acceptable due to component limitations in local stores, but any advice would be appreciated.
  • Any general advice?
\$\endgroup\$
16
  • 1
    \$\begingroup\$ Please place the decoupling capacitors next to the circuit or IC you are trying to decouple. Don't stack them all in one corner and route power from there. Avoid slicing up your bottom side ground plane with long routes. \$\endgroup\$
    – winny
    Commented Dec 9, 2021 at 15:33
  • 1
    \$\begingroup\$ I suggest you review the Hardware Design Guidelines for the ESP32. You have components in the (strongly recommended) keepout zone of the PCB antenna \$\endgroup\$
    – TypeIA
    Commented Dec 9, 2021 at 16:44
  • 1
    \$\begingroup\$ And what @Justme said earlier doesn't seem to have been fixed: you should never leave CMOS inputs (such as the inputs to any 74(A)(H)C(T) or 4000-series chip) floating! This will cause the chip to generate noise as random noise is picked up by the floating inputs and amplified by the circuitry on the chip, and it can interfere with functions of the chip if you, for instance, connect two of the three inputs to a 3-input OR gate and leave one floating. Just connect unused inputs to ground or Vcc, whichever keeps the circuit working as intended. \$\endgroup\$
    – Hearth
    Commented Dec 11, 2021 at 19:25
  • 1
    \$\begingroup\$ @OlegButrimov This is a problem with the non-ideal behavior of CMOS logic (more generally, of high-impedance inputs): they're extremely sensitive to noise. Random noise on the inputs gets amplified to random noise on the outputs, and that output swinging back and forth at high speed between vcc and ground is going to waste power and re-radiate even more noise. The functional diagram doesn't say anything about this because the functional diagram is about the ideal characteristics of the device. \$\endgroup\$
    – Hearth
    Commented Dec 11, 2021 at 21:10
  • 1
    \$\begingroup\$ Take a look at the image here: forum.kicad.info/t/footprints-for-decoupling-capacitors/18698 and compare that to where you have placed your decoupling capacitors. \$\endgroup\$
    – winny
    Commented Dec 11, 2021 at 22:09

2 Answers 2

Reset to default
2
\$\begingroup\$

AMS1117 is junk. It has a very slow transient response and needs a large output capacitor like 100µF, otherwise when the micro draws current pulses due to wifi, with a regulator this slow, voltage will drop, it will occasionally crash, and you'll waste time. And it will also burn if you short the output, no matter what the datasheet says about "short circuit protected". But hey it costs 4c, it's okay if someone else has to desolder it when it dies, but if you'll be the one to fix it, better invest 50c more...

The other options are okay. However these LDOs are not designed for use with ceramic caps only. LM1117 datasheet says:

The ESR of the output capacitor should range between 0.3 Ω to 22 Ω.

So basically, you need an electroytic output capacitor on top of your ceramics. You can spend 30 minutes picking the right tantalum cap with just the right value... or just you put a 10 cents electrolytic with way too many µF, like 100-330, and you'll save 30 minutes.

You have a nice ground plane on the back, so there's no reason to flood the top with copper. There are a lot of unconnected bits between traces which serve no purpose besides increasing crosstalk. In addition, if you use one of the cheap manufacturers, the soldermask looks nice but it isn't very tough. If you insist a bit with the soldering iron, it can scratch off and expose the copper. When that happens, soldering a SMD pad next to it without making a short becomes quite the challenge! So since you have a ground plane, why not just use one via on every ground pin?

Also when you use a copper flood, the software thinks everything it touches is perfectly connected to ground with zero ohms, even if the resulting path is a zig zag through the whole pcb with a 0.2mm neck between two pins... the software will proudly tell you "no unrouted nets!" but the board won't work. That's another reason to use vias, you can see where they are and what path the current takes to return to ground.

Make sure you triple check the pinouts on these switches, they're treachrous.

ESP32 needs some pins set to specific levels to boot in the correct mode, so make sure you check which ones.

If you have buttons at the end of wires, consider using a 100nF capacitor to ground and a stronger pullup than the one provided by the micro, to avoid noise pickup.

\$\endgroup\$
4
  • \$\begingroup\$ You could also use a small resistor in series with a ceramic capacitor to satisfy the ESR requirement. \$\endgroup\$
    – Hearth
    Commented Dec 11, 2021 at 21:11
  • \$\begingroup\$ Wow, that gives a lot of info to think of, thank you a lot! Thanks for pointing out possible issues with ground plane on top side, will look at board without it (isolated islands was one of the reasons for adding vias, btw). The buttons I have are matching the schematics here, but I'll surely will triple-check it before soldering, noted. ESP pin levels at boot time are checked, I didn't broke it (yet). Buttons noted, thanks 10uF tantalum capacitor is ok or bigger is better (locally available 10uF is smd_B, 22uF is smd_C)? Should I add it in addition to or instead of ceramic ones? \$\endgroup\$
    – Oleg Butrimov
    Commented Dec 11, 2021 at 22:21
  • \$\begingroup\$ In addition to the ceramics. \$\endgroup\$
    – bobflux
    Commented Dec 12, 2021 at 7:32
  • \$\begingroup\$ If you don't care about height, standard aluminium electrolytic is cheaper and has more µF though. \$\endgroup\$
    – bobflux
    Commented Dec 13, 2021 at 14:17
2
\$\begingroup\$

Unused CMOS inputs are floating and no bypass caps near it.

\$\endgroup\$
3
  • \$\begingroup\$ Sadly, I'm very new to the electonics so I could be wrong, but I assume that mean that I should add something like 0.1uF capacitor next to each output (except VCC and GND maybe) to ESP32 and 74HCT as close to the pin as possible (as per comment from @winny), so one pad of the capacitor will be connected to pin and another to GND. Is it safe to add capactors to the pins that are in use already or it is enough to just have the pads to place capacitors in case if this pin will not be used at some point in future? Will try to do so and update my PCB in topic then \$\endgroup\$
    – Oleg Butrimov
    Commented Dec 9, 2021 at 16:19
  • \$\begingroup\$ No, you have it the opposite way; bypass caps are for power supply pins and unused input pins must be set to high or low depending on what is the idle state if it is important to have some specific idle state \$\endgroup\$
    – Justme
    Commented Dec 9, 2021 at 17:12
  • \$\begingroup\$ Oh, so capacitors on power supply line, like it already done, but I should move them to the component which receives this power (pair on 3.3 V line close to ESP32 and pair on 5 V line close to 74HCT. TTP223 touch buttons outside the PCB appears to already have their own capacitors). As for inputs - does that means that I need to figure out for each unused pins should be high or low then use appropriate resistors (quick googling says that 10k is nice, but will check it more precisely) to pull it to 3.3 V and GND accordingly? \$\endgroup\$
    – Oleg Butrimov
    Commented Dec 9, 2021 at 18:01

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.