4
\$\begingroup\$

I want to be able to filter the 3V3 power line going out of the ESP32 MCU. Since this "may" have a frequency around 2.4GHz (Wifi or Bluetooth antenna). This may then affect other components that also need the 3V3 power from the same net. I have implemented the below circuit thus far:

schematic

I then simulated this on LTSpice:

enter image description here

I first choose a general ferrite bead with the below specs:

enter image description here

The results of the simulation are below:

enter image description here

enter image description here

My questions:

  1. Am I using the correct approach to simulate the ferrite bead?

  2. From the results the attenuation is not sufficient, is there a way to calculate the values for the inductance, capacitance, and resistance so I can manually enter these values for the ferrite bead?

Edit 1:

I realized the frequency to attenuate was 2.4GHz and not 2.4MHz

Here is the simulation with the 2.4GHz frequency.

enter image description here

enter image description here

This Ferrite bead seems to be doing the job (I just need to confirm the current).

Edit 2:

Simulation results with modeling the capacitor with ESR and series inductance.

enter image description here

enter image description here

Edit 3:

Capacitors used:

  1. 22pF:C0201C220K8GACTU (ESR=0.149, ESL=28.1p)

  2. 0.1uF: C1206C104J3GACTU (ESR=0.0089, ESL=19.8p)

  3. 1uF: C1206C105K3RACTU (ESR=0.0124, ESL=0.3p)

enter image description here

enter image description here

\$\endgroup\$
1
  • \$\begingroup\$ Generally speaking, the only way to reliably do this is to assemble a test coupon with the passive parts laid out same as they'll be in the product, with connectors for network analyzer installed. The connect the thing to a network analyzer, and determine exactly what the response is. Spice is garbage in = garbage out: the results are only as good as the device models supplied by the vendor. If you're not getting spice models from the manufacturer for each passive part that you're using, then you're at best doing guesswork. It'll be much quicker to test it and get real data. \$\endgroup\$
    – Kuba hasn't forgotten Monica
    Commented Apr 20, 2022 at 10:00

2 Answers 2

Reset to default
3
\$\begingroup\$

I want to be able to filter the 3V3 power line going out of the ESP32 MCU

Well, it seems to me that you have your ferrite bead in the wrong position; it should either be to the right of the 3 parallel capacitors or, form a Pi filter with another set of 3 capacitors to the far left. If forming a Pi filter then it works bidirectionally of course.

But also, you didn't run the AC response up to and beyond 2.4 GHz to see the effect of the ferrite bead (a limited effect I might point out): -

enter image description here

Simulated circuit: -

enter image description here

Whether the effect of the dip brings anything to the party I very much doubt. It seems to me that with the capacitors you have, the attenuation would be about 120 dB anyway.

However, if you need a better answer, you should model the capacitors including their self-inductance and resistance. You should also watch out for strong (and undesirable) resonance effects in the low to mid MHz. You should also model the effective loading on the lines in terms of resistance because this will affect the Q factor of resonant peaks (possibly causing device over-stress and maybe failure).

\$\endgroup\$
17
  • 1
    \$\begingroup\$ They should be the same basically but, the notable thing is that the FB (when properly operated as a FB) is not bringing much to the party; just that dip around 2.4 GHz. Its inductance however, is causing the 40 dB/decade slope from the low MHz to over 1 GHz and that by itself is doing pretty much what you might want it to. But, you must adequately model the capacitors. \$\endgroup\$
    – Andy aka
    Commented Apr 18, 2022 at 11:17
  • 1
    \$\begingroup\$ Yeah, it can become really tricky above 1 GHz. I also think that you need a parallel capacitance of about 22 pF as your smallest value i.e. 1 nF is too big as your smallest value. \$\endgroup\$
    – Andy aka
    Commented Apr 18, 2022 at 11:52
  • 1
    \$\begingroup\$ @JoeyB the smaller the capacitor, the lower its ESL will be and, the better job it will do at the higher frequencies however, it can't be too small or it becomes ineffective. \$\endgroup\$
    – Andy aka
    Commented Apr 18, 2022 at 12:07
  • 1
    \$\begingroup\$ Kemet 22 pF capacitor - use the kemet website because they have good graphs for many capacitors. \$\endgroup\$
    – Andy aka
    Commented Apr 18, 2022 at 12:35
  • 1
    \$\begingroup\$ Up to a point @JoeyB ("it can't be too small or it becomes ineffective"). \$\endgroup\$
    – Andy aka
    Commented Apr 18, 2022 at 13:24
0
\$\begingroup\$

Multiple parallel capacitors should be modeled with their parasitic inductance at the very least. One capacitor will resonate with the parasitic inductance of the next capacitor to produce amazing peaks and nulls in the total bypassing of the undesired noise.

Usually, the old adage of paralleling multiple capacitors of different value are likely to produce LESS, and very frequency dependent affects on the performance.

One trick is to add series resistance to each capacitor to De-Q the parasitic unwanted resonances.

\$\endgroup\$

Your Answer

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

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