FEDEVEL
Platform forum

Astral Master , 11-22-2025, 05:02 PM

EEG pcb. 4 layers, signal, ground ground, signal. no cuts in ground planes. Very sensitive analog. Please let me know if you notice anything drastically wrong with my design. I got it as good as I can but Im not a professional

tomas.kaplan , 11-25-2025, 02:22 PM

Hey there. Power supply traces looks pretty thin to me, but i expect this device does not draw a lot of current. Since you have a lot of space, you can make it wider. What caught my attention is RF trace for your 2.4 GHz connection. Did you calculate the needed trace width and ground clearance based on your PCB stackup? For 50 Ohms it looks pretty thin to me.

Regarding the power supply decoupling of your sensitive analog input chip. Your decoupling is on the bottom side of the board and your via positioning is not optimal. I would recommend to follow Example layout from the datasheet - see the picture.



Your TVS diode could be moved right into the trace and be closer to the battery connector.

tomas.kaplan , 11-25-2025, 02:27 PM

I think that your STlink connection is missing RESET signal. Check that too. From my experience with STM mcus, reset was needed.

Brego , 11-25-2025, 05:32 PM

First thing that I saw was a TVS diode at the connecor. You should rotate it so the ground connection is shorter. Also you should avoid making stubs (I circled it with red). Instead, connect trace directly into the pad.

QDrives , 11-25-2025, 09:12 PM

What a crap layout example from TI.

QDrives , 11-25-2025, 09:21 PM

1) Remove the 'acute angles'
2) Do not place traces between traces
3) Connect your exposed pad
4) Remove the silk screen, especially on the RF part.
5) Your power supplies will screw all measurements with the noise

tomas.kaplan , 11-25-2025, 09:36 PM

Yea, as i look at it more closely, its not that nice. 🤔

QDrives , 11-26-2025, 02:23 AM

'Bridges' between pads (green).
Vias shared (red arrows)
Vias far away from components
Decoupling capacitors far away from components.

QDrives , 11-26-2025, 02:32 AM

And this is the kind of shorts you get.
When you are troubleshooting, you will spend some hours 'fixing' the shorts.
Always go outside or inside to make the 'short'.

QDrives , 11-26-2025, 02:33 AM

The middle one is acceptable as it is also shown outside as a short.

tomas.kaplan , 11-26-2025, 07:10 AM

I have to admit, that if two neighbor pins are power supply on the same voltage rail, I short them right at the pins too since I dont expect the pcb cutting during debugging at that spot. But if its something different, its very wise to short it outside.

tomas.kaplan , 11-26-2025, 07:13 AM

Astral Master , 11-26-2025, 06:18 PM

Astral Master , 11-26-2025, 06:18 PM

are you saying to connect pins like that instead of the green line?

Astral Master , 11-26-2025, 06:19 PM

the lm27762 has a 2mhz swithcing charge pump i am concerend about rise time noise getting into my outputs on the ldo i can figure out what the loop is of those rise time lines

QDrives , 11-26-2025, 08:18 PM

The left encircles connection may give you problems in the future when you get a board that does not work.
The other two are 'visibly' shorted

QDrives , 11-26-2025, 08:23 PM

Have you simulated what happens when you intermittently draw 10mA more due to RF on the analog rails?
If you want to measure uV level signals, you need power noise (ripple) close to that or lower.

Astral Master , 11-26-2025, 11:06 PM

Astral Master , 11-26-2025, 11:06 PM

Check that out

Astral Master , 11-26-2025, 11:06 PM

I knew it was gonna be a problem

QDrives , 11-27-2025, 02:31 PM

https://www.signalintegrityjournal.com/articles/573-designing-power-for-sensitive-circuits

Sniper2 , 11-27-2025, 09:05 PM

interesting most oscilators i deal with dont mention any power supply parameters

Sniper2 , 11-27-2025, 09:06 PM

only had to deal with clean supply with a PLL that wante like 20 mV pk ripple

Sniper2 , 11-27-2025, 09:06 PM

not crazy for 3v3

Sniper2 , 11-27-2025, 09:07 PM

hardest part was keeping the probes steady in contact with the cap pins

Astral Master , 11-27-2025, 10:40 PM

do you guys recommend hot air rework or soldering iron for 0402 components on pcb?

QDrives , 11-28-2025, 02:25 AM

It is an ADC and op-amps.

QDrives , 11-28-2025, 02:26 AM

I prefer soldering iron, but somebody mentioned that the stress on the component is probably higher then when using hot air.

Sniper2 , 11-28-2025, 02:19 PM

soldering iron since this way i dont mess up other things as bad + I can still hold the board after