I gathered as much. You were just a bit blunt and direct, but all advise is greatly appreciated. I’m 30 minutes into the video and it helps a lot. I’m working with I2S so if I’m not mistaken, the signal is already into the MHz range so the things Rick’s saying about how the fields form absolutely apply. Thank you for your help.
I mean mounting by hand, no stencils, paste, reflow oven or hotplate. The number and complexity of the boards shown is well below the hassle to manage all that.
Just tweezers, a good iron, flux and solder braid.
Never used a stencil in my life for simple prototypes (but usually i do much less, 2 or 3 max, even much more complex than the one shown).
I’m hand soldering this. It’s a second revision of my first PCB design. Until now I’ve only done prototype boards. I’ve done quite a few of those, but they were all low frequency. This board has I2S. The first revision works but I get noise in the I2S microphone signal if I ramp up the WiFi signal too high. The second revision has a dedicated LDO close to the mic. That should help a lot.
I’m using 0805 SMD components where I can. Soldering those by hand were fine. I’m worried about the LDO though for the new board. It’s a TLV70033_SOT23-5 and it looks really small. I don’t have it yet but I’ll see how that goes soldering it by hand. I wasn’t planning on using soldering masks or hot guns or whatnot.
SOT23-5 is no problem hand soldering without stencil. Even at my age.
0804 is clumsy. 
Good flux, good tweezers, better light.
Increases assembly cost so I’m not using it.
I don’t accept.
QFN uC packages with thermal pad at their bottom forces me to 4 layers as I can’t go with VCC under them and connect from there to all its VCC pads and going with VCC track 3/4 around footprint perfectly bothers other connections.
If so you will be interested in links I have posted here long ago:
In 90s we have done 3 steps. First from THT to 1206, second from 1206 to 0805 and third from 0805 to 0603. So since 25+ years our standard is 0603 (and SOT323 for transistors and dual diodes) I see no problem with hand soldering them.
From time to time I use 0402. Mainly 100nF blocking capacitors. If you have no other choice it is possible to hand solder 0402 but I have done it only few times.
At PCB I shown previously there are 6 0402 100nF around main uC (just follow VCC track and you will find them. The row of resistors to the left are also 0402.
SOT323 is no problem. SOT23-5 is no problem.
SOT353 is more problematic.
For prototypes and one-offs soldering without a stencil, then it does not matter much for the soldering whether you have footprints on both sides.
If you also have at least one THT part (maybe just a connector) then the bottom is not flat anyway. One thing I have considered it to add a footprint for a relatively thick SMT diode in each corner of the PCB. Diodes are cheaper then mechanical feet and they also get the job done. You can use such diodes in your circuit, or just don’t bother at all and just have unconnected footprints. For mechanical stability it’s better to put a few vias though any pad that is used for mechanical strength. Especially for SMT connectors. SMT pads without vias are quite easily ripped of a board without such via’s.
EMC concerns and signal integrity is another reason to go to 4 layers. With a 4 layer PCB, you usually have a core of around 1.2mm thick, and the prepreg between the inner layers is around 100um thick. Much thinner then the PCB core, and this improves signal integrity.
The video was very helpful in understanding why the board needs to be redesigned. This is what I ended up with:
I’ve changed the pads for the ESP32 and amplifier board to SMD pads. Continuous ground plane at the bottom, ground pour at the top. Power is routed at the top and there are no signal lines at the bottom. I’ve added a bunch of vias to connect the ground pours at the top to the bottom ground plane. I’ve also moved the GND line in the connector to be close to the I2S signal lines. I’ve updated the board settings with the help of this thread: Board setup - design rules for Pcbway and other questions. I’m unsure how many vias to place. I placed them close to ground pads and in islands.
I think I got everything. Feedback is greatly appreciated.
The other board I’m working on:
(it’s upside down; don’t ask)
It connects to the first board. I know I also have a problem with the cable I’m using to connect the boards. I’ve put the GND cable close to the high frequency I2S signal cables, but the cables really should be shielded. I’m still trying to figure out how to solve that.
Can you suggest good flux and good tweezers? A shot would be nice already 
.
That PCB looks a lot better. I still have some doubt about the smallish cutout around the antenna. My guess is this is the absolute minimum, but I guess your gadget has a longer range when there GND plane is further away from the antenna.
For the amount of via’s, they look adequate, but I would either remove thin copper slivers that are only connected on one end, or add a via at the other end to. For example near U1 pad 3.
Off-board wires / cables always need extra attention if you want to do it properly. For DIY emc conserns are not such an issue, but for a proper design it’s common to add filters, series resistors or ferrite beads. I still remember long rows of Pi filters near the connector of a parallel port printer I took apart for parts. And that was back in the '80-ies. With modern microcontrollers, you often have some way to set the drive strength or slewrate of output pins, and this is also a factor that helps.
And about your version number… Why already V2? Normally V1 is the first viable product ready for production, so this being V0.2 would be more logical. I have completely given up on version numbers, they don’t mean much to me. Instead I simply use the date (Indeed in ISO_8601 format as a version number, and also as an sort of UUID for my projects. I put on the date that I send Gerbers to the fab as a “version number”, but never two projects with the same date, so a project may have yesterday’s or last weeks date.
I’ve put some signal wires closer together to limit the number of small copper pour slivers. There was one lef between pin 1 and 2 of U1. I put a zone rule there. Is that the way to do this? I tried increasing the minimum width of the zone, but that prevented the area in U2 to be filled.
I have 33 Ω series resisters at the source side of the signal lines already. R1 and R2 on this board, and one on the sending end on the other board. You’re thinking it’s good to also add ferrite beads? Do you have suggested reading/watching material for this?
I based the cutout for the WiFi solely on the cutout on the ESP32 board. I’m gathering I shouldn’t have. Any advise on how big I make it? I’m limiting the cutout to stay within the area of the pads, but that maybe isn’t necessary? Would it be advisable to add a larger exclusion zone with just “Keep out zone fills” checked?
I’m worried about EMI in as far as that I’d like this device not to cause havoc in my home. I’m building quite a few of these.
The version number is anything but serious 
. The first PCB had no text on it at all. My ESP32 app uses the Git hash as a version number. That’s by far the best option I think. I’m not too worried about it in this design.
For DIY you don’t have to be too concerned. Just having a good GND plane, and proper decoupling already gets you a long way. It’s for commercial products that have to go though formal EMC testing that you need to dive deeper into details.
Well, I have not seen the schematic.
I always put an inductor and filtering for the power input to my projects. I have even some ferrite beads in the power cable I use for my breadboards. I leaned this the hard way, as inductors and ferrite coils are the only parts that keep microcontroller circuits on breadboards and matrix boards (note: no GND plane at all) from spurious resets. I used to use a low frequency transformer based halogen desk lamp for testing, but alas, that lamp also failed at some time. CFL lighting with such an old fashioned laminated metal choke coil are also good EMI generators for testing.
For the signal wires. SMT chokes cost next to nothing and are easy to mount, but I don’t know how effective they are. It’s easy to put some footprints for (various?) filters on a print. Then you can do some simple tests and experiment whether you see any difference. KiCad also has footprints for solder jumpers (both NO and NC). 33 Ohm series resistors seem sensible, those also give some limited (extra) protection against ESD events.
If you’re serious about designing electronics, you can’t get around learning more about EMC, but you don’t have to do that right now. A good place to start for a test setup for EMC is to make something resembling a LISN. Tekbox sells these things, but too professional and expensive for DIY, but good for their documentation. You can build something simpler for DIY needs. You don’t have to overthink EMC. Unless you start building Tesla coils, your gadget is extremely unlikely to cause interference on other stuff. For suceptibility from external sources you can do tests. An EMI generator can be build with an NE555, a relay and an old fashioned EI transformer. Adding something that triggers the relay at an adjustable phase angle is recommended, this has a lot of influence of the EMI such an transformer generates. (I.e. only primary coil is used, secondary can be “whatever”, or open).
Using a git hash as a version number is swell for PC stuff, but not human recognizable, and too long to print on a PCB (unless you use a QR code). I use the date because it’s human readable, and in chronological order. It also automatically logs the time frame of old projects.
Here an example of the effects of the cutout’s size
1 Like
For tweezers, I like my “Sandvik Belzer 5544 AM”. But as I found out, they are now Bahco and this exact type no longer exists. The most similar one is this: https://www.bahco.com/de_de/smd-pinzetten-zum-positionieren-und-loten-von-bauteilen-bis-1--mm-breite--greifwinkel-45---pb_5547am_.html Treat them with care and respect, don’t abuse them and they will last for decades.
Flux I use Edsyn FL 22, but expensive. When I’m running out of it, I’ll try Amtech that has a good reputation.
Would you mind posting your project here? I’d like to make some suggestions to placement and routing. But I’m to lazy to describing them in words. If you don’t want, you could also send me a private mail.
1 Like
Thank you. The project is here:
The version I’m showing in this thread is in a separate branch. The URL should get you to the right branch and folder.