Layout / Schematic review - reference design

Please can someone review and suggest any improvements??
I will follow up this post with the final design and or confirmation of if it worked or not, it should serve as a good reference design.

I have clamped the TX/RX pairs to AGND and 3V3A using IC21 IC22. Its a very noisy environment…
I’m not sure if I have clamped the RXP/RXN correctly… Should C106 and C107 be on the LEFT hand side of the clamp??

Don’t copy anything here until I have has a chance to follow up…

NEW REVISION (More seperation between twisted pairs. Moved caps. Some layers not shown (see above for missing layer…)

Why making things complicated? You did not explain why you add these devices to the circuit.

Its a network controlled 40KV PSU. When we do short circuit tests - the interconnecting cables physically jump. There’s a lot of EMI generated, hence my mention of a ‘noisy environment’.
The risk is that the STM32F303 or W5500 state machine resets when this occurs - which is equally as problematic as hardware damage…
Ultimately, at a few pence each and already used elsewhere on the board, its looks good in the ‘risk mitigation’ column of the spreadsheet! They can be no fits if not needed.

Hi jnewcomb.

Is IC21 and IC22 TVS Diode?

The TVS diode protects against external EMC shocks. And C106 and C107 are connected to the left.

Is your equipment too noisy?

It is recommended to adjust the values ​​of R142 ~ R145.

And avoid crossing the TX / RX signal with the power signal as much as possible.


1 Like

Is IC21 and IC22 TVS Diode?

No, they are clamping diodes connected to the RX/TX pairs.
(The IC has a TVS protecting the supply rail. See circuit symbol.)

Is your equipment too noisy?

very much… (See my post above)

And C106 and C107 are connected to the left.

OK. I will move the CAPS C107 and C106 to the left of the protection device.

It is recommended to adjust the values ​​of R142 ~ R145

Can you suggest a value? I take 33R from the recommended schematic.

What is the maximum capacitance (to ground) I can put on the TXP TXN RXP RXN pins on the W5500 device?
I ask because I can use a different protection device. It is a unidirectional 3.3V TVS diode (Tranzorb). It has a capacitance of 30pf (to ground). The diode clamp has 4pF.

Thank you…

I can’t work out how to edit my original post, so I’ll append a reply here…
The board works perfectly - but only if I use the J0012D21NL connector from Pulse
However - my BOM called up J0011D21BNL which has a different pinout!! So… 3 signal lines need to be swapped because the RJ45 footprint is incorrect.
Pin1 - Should connect to: TX-
Pin2 - Should connect to: RX+
Pin3 - Should connect to: TXC

Check the footprint of the connector you use, its a minefield…

I have also changed R155 to a 10nf CAP

Remember to keep R130, R131, R132, R146 close to the micro. The rest (Including R145, R144, C111) should be a close as possible to the RJ45 connector.

The two clamp ICs may be no-fits and the circuit will still work. I only have them due to the nature of the environment our product works in. For you it may be overkill.

Note: A good resource for RJ45 connections is here

I have an updated schematic. The final connector I used was the PulseJack J0011D21BNL
This schematic is tested and works…
Note: the USBLC6 is not required for low EMI environments. If you wish to include it the data sheet hints you should not connect pin1 to 6 and pin3 to 4…
Don’t take the 3.3V off board… use a cheap linear like a LD1117S33TR to power the micro and nearby digital peripherals. DONT take 3.3V off board or share it too far.

ONE last note… The USBLC6-4 can also be exchanged with the USBLC6-2 device.
If you want you could use a single USBLC6-4 package for both RX and TX twisted pair… but the tracking may be a bit more tricky… When I designed the circuit I mixed up the -2 and -4 parts… but shorting IO1 to IO4 and IO2 to IO3 means it works anyway! Opps…

What does the finished board look like?
And does it work as you imagined?