Electronics > RF, Microwave, Ham Radio

Help with fixing cross talk and some other issues on my board

(1/7) > >>

I have been working on a 4 channel SDR to attempt to do phase based direction finding for wildlife telemetry transmitters.  My first version was very basic, and was just to make sure I understood some really basic concepts of RF front ends, and that I could get the SI5351 working as an LO.  My second version (attached image with all SMA jacks on the left) integrated band pass filter, LNA, and op amps to boost signal into ADC.  Everything works, but I am getting horrible cross talk that affects the phase of each channel.  Inputs range from 148-152Mhz, and are mixed down to less than 10khz.  PCB is 4 layers, 2nd layer is ground, 3rd is 3.3V power plane.  I am going to list out my issues/questions, and hope I give all needed information in one go :)

1. If I hook my signal generator up to only one input, I can read the signal with FFT on my scope at -15dbm.  Without moving the cable, if I probe the next connector over, I can still see the signal at -20dbm.  Can that much cross talk be happening from from the signal radiating back out as EM, and getting picked back up by the traces, or is there something wrong with my circuit/layout that is causing the signal to just travel over to the other channel.  The 3rd connector down seems to affect the other channels down more than all others.  Are all the input, BPF, and LNA circuits just too close together, or possibly the issue in #2

2. The output of the mixers goes through a via to the back side of the board to goto the pins connecting to the ADC input of the various dev boards I am playing with (Uno R3 compatible pins outs).  I didn't think much of it at first, because I told myself it's only a 5khz signal, so low frequency, and I only recently thought about the fact that the mixer is also dumping out a 300ish mhz signal as well.  I assume that's going to cause some issues.  I figure I can rearrange the board as shown in the mockup (2 connectors each side), and put the low pass filters right after the mixer, so that the high frequencies will get filtered before going into the via, and under everything.  Is a 20khz signal going under it still going to cause it to radiate back into the LO traces and other places?

3. Assuming that's still a problem, I had considered putting through hole SMA connectors on the board, instead of the edge connectors, but wasn't sure if the right angles in the connectors would affect the input signal.  I have read and seen videos that talk about avoiding right angle turns in traces, and wasn't sure how much that applies to the SMA jacks.  If I can use through hole connectors, I can put them a bit further in on the board, and then route the output of the mixer around the outside of the board to the pins on the top layer, to avoid it going under anything.

4.  If there is a ground plane directly under all these signal traces, would via fences help any more?  The main things that could have them are the traces for the LO from the SI5351 to the mixers, and the output of the mixers to the ADC pins.
 I have also seen suggestions to put vias to ground just in a grid all over the PCB, but haven't seen an explanation as to why that helps.

5. Would shield cans help cross talk, or is that mainly to avoid EMI from the board affecting other devices?

6.  How much does the topology of a BPF affect signal integrity?  In order to save space, my BPF currently has a  U shape to it (marked in green on the V2 PCB image).  The first two shunts aren't highlighted, but when it goes through the second cap and inductor I have it make a hard turn, and then out of the inductor into coupling cap with another hard turn.  Would it help anything to straighten out the path the signal takes?

7. The various controller boards I am using (STM32 mainly, but also and ESP32 board, and Arduino Uno for some testing), have a lot of noise on the 3.3V pin.  I initially thought that since I had caps at the Vin pins of the LNAs and the SI5351 that it wouldn't matter, but since I decided the board, I have learned a bit more about current loops and how they can cause more EMI to be radiated.  I assume some caps at the 3.3V pin to ground would help to avoid there being large current loops over the width of the board.

8. The op amp circuit is one I found on stack exchange as I was learning a lot of this.  it didn't have a cap on the power input of the op amp, so I didn't put a cap on the power input of the op amp.  The guy went through a nice detailed description of what ever component did in the circuit, so I didn't think much of it.  The noise on the 3.3V power plane really affects the output of the op amp though, if I put the caps at the 3.3V pin for the whole board, would it hurt to still have them right at the op amp?

Not using standard stripline techniques?  Yes, signal path best dead straight, or at most 45 degree bends.  I don't understand your grounding - the top layer appears to have grounded parts without a via to ground.  Or if its a ground plane where are the stitching vias down the internal groundplane?  Bad grounding will leak RF everywhere.


--- Quote from: MarkT on February 05, 2024, 09:05:15 pm ---Not using standard stripline techniques?
--- End quote ---

Define standard techniques.  I do know I messed up the trace width for 50ohm impedance.

--- Quote ---I don't understand your grounding - the top layer appears to have grounded parts without a via to ground.  Or if its a ground plane where are the stitching vias down the internal groundplane?  Bad grounding will leak RF everywhere.

--- End quote ---

Top layer gets filled, and the pads get connected to the fil, which connects to the GND pin, and also do some GND vias.

Stripline is normally straight, perhaps 45 degree bends if necessary, use SMT parts ideally of the same width as the line for series components, and for components to ground they go off at 90 degrees, spaced apart from each other.  Topside ground plane needs to be a consistent clearance from the stripline, with stitching vias all along the edge.  No breaks in groundplane under the stripline.  And above all get the impedance close to 50 ohms (you may need to experiment, or get this info from the PCB manufacturer).

The RF filter design does not look realistic to me. It looks like you assumed the lumped components behave ideally at RF, but they don’t, specially those 560nH inductor.

The crosstalk may also come from the limited RF to LO isolation and the complete lack of isolation at the LO distribution network.

I would change the IF low pass filter to a diplexer to properly terminate the IF port at LO frequency into 50ohm and avoid LO-IF leakage reflection going back into the mixer and degrading its performance.

BTW, what about image rejection with so low IF frequency?


[0] Message Index

[#] Next page

There was an error while thanking
Go to full version
Powered by SMFPacks Advanced Attachments Uploader Mod