4 layer PCB stackup for better EMC

Question

I want to design a PCB with few "low dropout linear voltage regulators", which would be used to power some sensors we are building. None of the parts on the PCB is expected to do any high speed switching. The sensor is on a separate board, and the power from the PCB is routed through SMA cables to the sensor. (The power requirements are low ~mW, and SMA is used just as an additional shielding). Sensor operates at 10 MHz, and I need the supply to be clean upto few 100 MHz. The regulators will be decoupled by low ESR capacitors and will be powerd from batteries.

I wanted the PCB not to pickup any external interference and was suggested a 4 layer design, where the stack was 1-GND, 2-Signal, 3-Signal, 4-GND. But, many online forums reccomend against this, and they prefer the reference planes at the layers 2 and 3.

1. Can someone experienced in this field give their views on this? I dont mind if reworking the board would be impossible.

2. Should I add a grounded copper pour on the layers carrying the signals?

3. How closely should the via stiching be done? (Some of the major noise sources I get are at 2 MHz, 100 MHz-FM and 555 MHz).

Please let me know if further informaton is needed. Thanks.

Answer 1

I know you want the board to not pick up external interference but don't forget the board itself can generate interference if your layup is not great. Which it won't be if you have broken ground planes. From your comment about how cutouts in the ground plane for components might affect the shielding, it seems you are completely focused on shielding and giving no thought to the presence (or lack thereof) of an unbroken ground plane.

I suppose if you have solid plane underneath the components and literally only have cutouts for the pins you might get away with it if your components are few since it would largely be like a regular plane with vias going through it. But the devils is in the details.

Also remember that the signal layers in that layup do not share the same reference plane and you will need to accommodate for that when signals move between the signal planes or else you will just generate more EMI.

This is from Henry Ott's book EMC Compatibility:

You may be interested in these for comparison:

But man, it feels nasty.

Answer 2

In most cases a stack-up with two GND planes should be superior to any other stack-up without two GND planes from an EMC perspective. Whether your GND planes are on L1+L4 or on L2+L3 doesn't make too much of a difference anymore in many cases.

One additional benefit of having GND on L1+L4 is that you can stitch them together around the periphery of the board to create a Faraday cage. Then again signals on outer layers with a close-by GND plane shouldn't be very good antennas anyway (receiving or transmitting). So the actual difference in EMI performance might be negligible.

Personally I always default to GND being on L2 and L3 on four layer boards, unless their is a strong compelling reason to do otherwise.

I wouldn't bother with GND pour in the signal layers. What you can do is pour power on the signal layers. Maybe in a way they overlap so you can connect them with vias. But that depends a lot on your application.

Regarding stitching vias the most important thing is to have a close-by return GND via for every signal via, if practicable. This is probably enough stitching so you might not need any additional GND vias.