1
\$\begingroup\$

I have designed a few PCBs for one of my projects. The PCB is picking up FM radio signals. I can see this as spikes in the spectrum where each radio station is broadcasting.

I tried covering the PCB with a grounded aluminum foil (many layers) to act as a Faraday cage. Although it reduced the signal's amplitude a little, the suppression is minimal.

The PCBs have highly sensitive sections where this amount of noise cannot be tolerated. The PCB has its ground connected to the copper pour.

Can anyone suggest ideas on how to get rid of this noise?

I am attaching an image of the noise spectrum.

Spectrum

A schematic of the PCB is attached below.enter image description here

We are seeing RF interference on every conductive material, not necessarily on the PCB. Hence, any general techniques typically used in such situations would be useful. I have included a ruler to enable scale measurements.

\$\endgroup\$
15
  • 3
    \$\begingroup\$ How is it picking up these signals? Does your pcb have RF circuitry on it? It could be your circuitry promotes the reception, so no amount of shielding is going to help you. Without knowing the details of your circuit we can’t conjure up any magic solutions. \$\endgroup\$
    – Kartman
    Sep 13, 2022 at 6:28
  • 4
    \$\begingroup\$ 'covering the PCB with foil' is unlikely to create an effective Faraday cage, the devil is in the detail. Your use of the qualifier 'grounded' foil supports that, grounding the foil does nothing to stopping radio reception via a Faraday cage. It needs to surround the circuit entirely, topologically equivalent to a conductive sphere around the circuit. Now obviously DC has to go in, and signals need to enter and exit. You manage this through filtered penetrations of that sphere. The design of the that filtering is what sets a successful Faraday screened circuit apart from an unsuccesful one. \$\endgroup\$
    – Neil_UK
    Sep 13, 2022 at 6:36
  • \$\begingroup\$ @Kartman, The PCB does not have any RF circuitry. One of the PCBs, which is a power distribution board, also is showing noise at the ground terminals. Just by probing the ground terminal with a scope, I can observe the noise. Even when using a BNC cable with one end connected to the scope and the other end open, I can see similar spectra (with a reduced amplitude). Any general ideas typically done in such scenarious would be helpful. \$\endgroup\$
    – user32335
    Sep 13, 2022 at 7:06
  • \$\begingroup\$ @Neil_UK, For testing purposes, no DC connections were going in or out (eventually they have to). The PCB was covered fully with the foil. The only connection going out of the foil was a BNC cable to the scope. The ground of the BNC cable was connected to the aluminum foil. \$\endgroup\$
    – user32335
    Sep 13, 2022 at 7:15
  • 1
    \$\begingroup\$ What is the length of the trace you are measuring those signal on? Could you please provide a schematic or at least a picture of your PCB? It's not rare for a long trace, to pickup many signals. A trace will start picking up signal when it's length is superior to Lambda/30 of the frequency for example. \$\endgroup\$ Sep 13, 2022 at 8:47

1 Answer 1

0
\$\begingroup\$

Okay, thank you for the PCB.

There is many things to take into account when designing a board which should be resilient to EMF radiation. One may be tempted to wrap the thing into aluminium foil, or in a big metallic box. This is not the right direction to start.

Big metalic shielding boxes are hard to design and very expensive i.e. Farday cages

When you want to shield your thing in a box you have to :

  1. Make sure there isn't any slot in the resulting assembly. Because EM radiation can enter them pretty easily.
  2. So if you want an opening you will have to put some contacts fingers, which have to make electrical contacts between pieces to cut the slot. For that you have to put special contacts, with special materials so oxidation don't electrically open those contacts.
  3. And finally, you will want wire in and out, so take care in shielding.
  4. Basically this list goes on forever, it's exhausting and expansive.

So what do I do? Start by bullet proofing your board In this regard, your design as a few mistakes :

  1. Many GND vias everywhere: to ensure GND coherence. Meaning your GND should be at the same potential everywhere. What distance appart? (Lambda/30) your problem is at 100MHz so let's take 110Mhz (wavelength shorter) this means your problematic wavelength is 270cm so your via stitching should be no further than 9cm appart. This is big way to big so we ditch the thumb rule, and something around 0.5cm appart should be great. The goals is to have no copper tongue left, image 1. And this shielding will be important for the following point, so you want to fence yours signals with vias close alongside them.

  2. You have very long traces on your PCB, which act as antennas, I mean, they literally collect EMF radiation. A wire become an antenna from an EMC perspective when it become bigger than.... You guessed Lambda/30, so your are clearly in this range. "But what do I do have to take this signal from point A to point B?" You could use a 4 layer PCB, yes it's more expansive, but burying your signal between two GNDs will shield it from the outside. And as you added GNDs vias everywhere, the signal will not have any slot left on the PCB sides to couple to your trace.

  3. Shunt the parasitic signal to the GND Using a low pass filter, with Ksim (KEMET capacitor simulator) I was able to find a capacitor value able to shunt the 100MHz region while, not harming the signal of interest in the MHz region (image 2). The curve is a S21 in shunt configuration, so you inject frequencies at side 1, and see what is left at side 2, with the capacitor in the middle. This capacitor could be placed at either side of the trace, or simply at the measuring side. The simulated capacitor is a 2nF capacitor, so it shouldn't mess with the SOI.

Grounding copper tongues Capacitor selection

\$\endgroup\$
1
  • \$\begingroup\$ Thank you for the detailed reply. I'll try out the suggested techniques. \$\endgroup\$
    – user32335
    Sep 13, 2022 at 19:13

Your Answer

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

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