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

[psyon]

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?

[MarkT]

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.

[psyon]

Not using standard stripline techniques?

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

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.

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

[MarkT]

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).

[eb4fbz]

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?

[Marsupilami]

The level of crosstalk is not normal. Something is shorting or you're not even measuring what you think you're measuring.

You said the probe reading of the input is -15dBm. Is that what you're sending into the circuit? How are you probing it? Are you touching on the center pin of the SMA or are you looking at the output of your board? Where is the probe ground connected? Is your scope and also your signal generator in 50Ohm mode?
You have to isolate where the problem is. What if you remove the first parallel LC section of the filter, then probe the connector? Next, populate the filter, but remove the series 22p cap to the LNA. Probe. Are you getting the expected response from your filter? Etc.
You can also try removing absolutely everything non-crucial and replacing things with 0ohms or solder shorts. E.g. remove the filters and the LNA. Does your mixer give the expected response?

Your grounding is not good, but it still should probably work better than to give you 5dB isolation, assuming that's the only issue. Biggest problem is that if you consider your layer 2 ground plane as the reference, wherever components interact with ground there should be a gazillion vias connecting to that layer.
The closest ground via to the input connector is under the mixer. It doesn't matter if you put copper under the connector if it can't conduct current, because it's not connected anywhere near. Try to draw a full current loop on your circuit, mapping out the return path.

I wouldn't be concerned by the U shape in the filter or 90 degree turns for this design.
Make sure you can test and evaluate sections of your circuit individually, and that your measurements make sense. Get your grounding (return paths) right and as others said make sure you account for component parasitics in your filters.

HTH

[psyon]

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.

In what way wouldn't they be behaving idealy?  The filter values are from the design tool on rf-tools.net.  I did initially have issues with the 560nH inductor, because the ones I initially bought had an SRF of only 115Mhz.  It was causing the signal to be attenuated by around 30db or more.  I replaced them with inductors with a SRF of 500Mhz, and the signal strength improved.  What else might I need to be looking at?

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

Are you talking isolation into the mixer, or trace isolation on the board?

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

We pick the frequencies used for the wildlife transmitters, and can space them as needed.  We generally space them 20Khz apart at a bare minimum, but on sites with less animals tracked, they are generally 100Khz apart or more.  Why specifically does a low IF frequency affect this more?  It seems it could be an issue at any IF I use.

You said the probe reading of the input is -15dBm. Is that what you're sending into the circuit?

No, the signal generator says 0dBm, but I don't know what it's basing that on.  It's an AD9910 arduino shield.  I have a limited budget so trying to make it work.

How are you probing it? Are you touching on the center pin of the SMA or are you looking at the output of your board?

Touching the center pin of the SMA connector.

Where is the probe ground connected?

The metal of the SMA connector.

Is your scope and also your signal generator in 50Ohm mode?

generator is.  My scope doesn't have a 50Ohm mode.  I do have some 50Ohm pass throughs, but I was not usin them in this case.  I wasn't taking the -15dBm value as an accurate value, I was just looking at it relative to other locations I was probing.

You have to isolate where the problem is. What if you remove the first parallel LC section of the filter, then probe the connector? Next, populate the filter, but remove the series 22p cap to the LNA. Probe. Are you getting the expected response from your filter? Etc. You can also try removing absolutely everything non-crucial and replacing things with 0ohms or solder shorts. E.g. remove the filters and the LNA. Does your mixer give the expected response?

I will give this stuff a shot, but not looking forward to it.  I have found I have very shaky hands and have been struggling with hand soldering the smd components.  Getting better, but need more practice.  Probably doesn't help how close I put everything either.

Biggest problem is that if you consider your layer 2 ground plane as the reference, wherever components interact with ground there should be a gazillion vias connecting to that layer.

Is it better to do the ground pour on layer one with a lot of vias, or  leave it only layer 2 poured and just have vias to GND where needed?

The closest ground via to the input connector is under the mixer. It doesn't matter if you put copper under the connector if it can't conduct current, because it's not connected anywhere near.

The top layer is poured, so the ground of the input connector is connected to that, which is then connected to pin 6 of the P1 header.  it does have to take a wild ride to get there though along the top layer.  This goes back to the question above.

Try to draw a full current loop on your circuit, mapping out the return path.

That's what I have been doing for the last few days since I posted. 

Make sure you can test and evaluate sections of your circuit individually

I've been trying too.  My tools are limited though.  I was told I should have put RF test points on it, but I didn't have the fore thought on the first too versions.  I have a NanoVNA that I have been trying to use to test the BPF, but not getting great results by trying to calibrate it with a probe (not a scope probe) attached.

[Marsupilami]

No, the signal generator says 0dBm, but I don't know what it's basing that on.  It's an AD9910 arduino shield.  I have a limited budget so trying to make it work.

That's hopefully at least close. Try disconnecting it from your hardware and probing the output of it. If you have a 50Ohm SMA terminator put that on the output and probe the pin of the output SMA connector with your scope in HiZ. You should see a ~0.63Vpp signal at the nominal 0dBm output. Without termination the voltage should read about 2x as much.

My scope doesn't have a 50Ohm mode.  I do have some 50Ohm pass throughs, but I was not usin them in this case.  I wasn't taking the -15dBm value as an accurate value, I was just looking at it relative to other locations I was probing.

That's fine, but I think you should figure out at least within a factor of 2 what's going on. If there's such a high difference between what you should be reading and what's on the scope it can be that you're only picking up radiation with your probe ground lead loop of something along those lines.

I will give this stuff a shot, but not looking forward to it.  I have found I have very shaky hands and have been struggling with hand soldering the smd components.  Getting better, but need more practice.  Probably doesn't help how close I put everything either.

Make sure you have decent tweezers (don't have to be expensive at all), get yourself a Pinecil ($25) or a TS100 or alike lightweight iron, tacky flux and use leaded solder to make it easier to melt.
If you're not that very young anymore you might want to get some magnification too. A headband magnifier or a cheap ($30) USB microscope should be plenty.
I'm sorry, I don't mean to give you an off topic lecture, but I do RF boards for a living and this is a very important part of the trade. Enable yourself and get good at it.

Is it better to do the ground pour on layer one with a lot of vias, or  leave it only layer 2 poured and just have vias to GND where needed?

I would do the 2nd option. The solid ground plane on L2 is the easiest and safest option. The L1 ground pour will not do very much for you in this case over it. When you're looking at RF boards you see a lot of top layer copper pours, but there are other reasons for that too than just straight return path. In your case and freq range an inner plane ground should be enough. Put at least 1 via at every component pad connected to ground, as close as possible. 

The top layer is poured, so the ground of the input connector is connected to that, which is then connected to pin 6 of the P1 header.  it does have to take a wild ride to get there though along the top layer.  This goes back to the question above.

That's not necessarily a deal breaker, it's just making it a lot harder to figure out what's going on, why and where. Rely on your L2 ground plane.

I've been trying too.  My tools are limited though.  I was told I should have put RF test points on it, but I didn't have the fore thought on the first too versions.  I have a NanoVNA that I have been trying to use to test the BPF, but not getting great results by trying to calibrate it with a probe (not a scope probe) attached.

Yes, that can be a tough problem. I would get one of these boards for the purpose. https://a.co/d/akz1yUq At your frequency range you can even leave the u.fl connectors on and just touch the pad next to it with the probe. Failing that, at this frequency you can do open load short whichever way you can. Open, leave the probe be, short, short the tip to the ground contact, load, take a 50Ohm smd resistor and hold it between the probe tip and the ground lead. This should be good enough to give you some helpful readings.
Get the short springy wire ground contact for the probe though instead of the alligator lead and make sure you touch ground with it as close as possible.

[psyon]

Are you using a ground clip with a lead or a short metal wire twisted around the scope/VNA lead? It might matter at ~100 MHz.

Clip.

Are you calibrating your nanoVNA on each run?

Yes.

[psyon]

Make sure you have decent tweezers (don't have to be expensive at all), get yourself a Pinecil ($25) or a TS100 or alike lightweight iron, tacky flux and use leaded solder to make it easier to melt.
If you're not that very young anymore you might want to get some magnification too. A headband magnifier or a cheap ($30) USB microscope should be plenty.
I'm sorry, I don't mean to give you an off topic lecture, but I do RF boards for a living and this is a very important part of the trade. Enable yourself and get good at it.

I don't mind being off topic, I can use all the input I can get.  25 years ago I taught myself programming by just picking a project, and just jumping in and making it.  That's what this has become.  Any extra things I can be told along the way are great.  I am not very young, but my eyes are fine.  The shaky hands may be nerves.

Yes, that can be a tough problem. I would get one of these boards for the purpose. https://a.co/d/akz1yUq At your frequency range you can even leave the u.fl connectors on and just touch the pad next to it with the probe. Failing that, at this frequency you can do open load short whichever way you can. Open, leave the probe be, short, short the tip to the ground contact, load, take a 50Ohm smd resistor and hold it between the probe tip and the ground lead. This should be good enough to give you some helpful readings.
Get the short springy wire ground contact for the probe though instead of the alligator lead and make sure you touch ground with it as close as possible.

Just to make sure, I know how to use the VNA and use it to measure antennas for the same telemetry.  The board though would help me know that I can getting good reads with the probes I am using to try to measure my board, correct?

Overall, thanks for all your input so far.  I have asked for help in many places, and this is the best responses I have received. 

[Marsupilami]

Just to make sure, I know how to use the VNA and use it to measure antennas for the same telemetry.  The board though would help me know that I can getting good reads with the probes I am using to try to measure my board, correct?

Overall, thanks for all your input so far.  I have asked for help in many places, and this is the best responses I have received.

Yes, you need to calibrate the VNA to the point it connects to the device under test. With the connection being a piece of coax, it's trivial to use the common sma cal kit. Your board however doesn't have SMA test point, not surprisingly, so your connection will be the the probe tip and ground lead. If so that is where you have to calibrate. You could just touch the probe to the SMA standards, but that's difficult to do reliably.
In a professional setting the same is happening just with dedicated RF probes. E.g. https://www.packetmicro.com/Applications/rf-probing.html  For these setups there is usually a piece called a calibration substrate, that contains planar cal standards to be touched by the probe for calibration. This principle works up to 100s of GHz, the scope probe and some cheap standards should work reasonably well for your application. It's not going to be super accurate. I wouldn't try to characterize the filter phase response based on this for example, but to give you an idea about magnitudes here and there it should be fine.

I'm glad I can help. This is what we're here for. 

[DavidAlfa]

Very poor ground for a RF circuit.
Use top/bottom ground planes, add via stitching every 5mm or so.


Shield each RF trace individually, don't place them too close.
Those traces are quite ugly, avoid sharp corners in RF as they radiate, most PCB design SW can route smooth/round traces.


Interestingly, this paper states the 45º corners are worse than 90º ones:
https://speedingedge.com/PDF-Files/90degbrooks.pdf

[psyon]

So how do you test for shorts when the inductors on the filters are shorts to ground when testing with a meter?

[psyon]

That's fine, but I think you should figure out at least within a factor of 2 what's going on. If there's such a high difference between what you should be reading and what's on the scope it can be that you're only picking up radiation with your probe ground lead loop of something along those lines.

When I hook the signal generator to scope through 50ohm pass through, it's 630mVpp, as it should be when I set signal generator to 0dbm.  When I hook the cable back to my board though, and touch probe to center pin on connector, with spring ground lead to metal of connector, it's 110mVpp (which is the -15dbm I said before) without the 50ohm pass thru.  I wondered if it could be the scope attenuation signal, because it's an SDS1104X-E that I unlocked for 200MHz, but at 100MHz it's still around 110mVpp.  At 10Mhz it's only 10mVpp and very very noisy.  Assuming I have learned something along the way here, the signal attenuation of the 10Mhz signal at the connector is because the 5.1nH inductor on the filter, is only 320mOhms of impedance to 10Mhz, so allowing the current to pass thru like a short, causing the voltage drop.  But, if I am understanding that right, that means the 150Mhz signal should only have 4.8Ohms of impedance, which actually does match up, and woudl cause a voltage drop to around 110mVpp.   But... the capacitor would also have that same impedance at 150MHz, so shouldn't it be like it's 2.4Ohm?  So, first, I am realizing I don't understand the math in a second order filter.  But second... what I am reading with the scope is what my math says it should be even though simulation says it should be the 630mVpp and not the 110mVpp.

The fact is I am seeing 110mVpp on all four connectors.  If I had some short due to bad soldering or something, I don't think I would see it consistently on all four.  Hopefully the VNA test board will show up, and I can test with that soon.

[Marsupilami]

You said you have a NanoVNA, right? Have you measured the input impedance of your board with it? That should be a good indication if it's loading your siggen incorrectly.

[Marsupilami]

Also be careful directly probing your circuit with a passive scope probe to a HiZ input.
The typical probe lead length in case is in the same magnitude as the wavelength of your signal of interest. That can cause all kinds of weird stuff with the measurement and how the circuit, especially a filter behaves meanwhile.
Cal your NanoVNA to the end of a pair of SMA cables and do a full 2-port measurement between 2 of the SMA connectors on your board.
The most interesting thing will be S11 and S22 responses. It will tell how close to 50Ohm your filter is. Also The S12/S21 should give an indication if there's leakage between the two channels early on in the signal chain.

[psyon]

You said you have a NanoVNA, right? Have you measured the input impedance of your board with it? That should be a good indication if it's loading your siggen incorrectly.

  I had been so focused on measuring the S21 by trying to use a probe on the board just before the PGA-103+, that it hadn't even occured to me to just measure the input impedance.   It's definitely off.  NanoVNA does not measure S12  though.

I used rf-tools.net to design the bandpass, it's supposed to be matched for 50Ohm.  The PGA-103+ should also be 50Ohm.  I guess I don't know at this point if I have a design/layout issue, or a component issue.  I mentioned somewhere, possibly in a different post, that the first 560nH inductor I used had an SRF of only 115MHz, and when I replaced that with one with a higher SRF, things did improve substantially.  SRF of the 5.1nH is a 5GHz.  Digikey doesn't list SRF for capacitors, nor do the datasheets for the ones I have checked, so I wasn't sure how much that would come into play.

[Marsupilami]

This looks... well... not good, but also not terrible. S21/S12 doesn't matter, that should be the same here and apparently you still have at least 20dB isolation between the two channels, which is good.
Also around 128MHz S11 is not absolutely terrible, so maybe you can tweak your original design with ideal component to a target of 150MHz and that way replacing one or two components could get you to something kinda working at 140.
Component parasitics are often not listed for generic purpose passives. Either you build enough margin into the design to be able to work with whatever or you need to get the more expensive special kinds that has defined characteristics. E.g. https://www.mouser.com/new/kemet-electronics/kemetcbrmlccs/

[psyon]

Also around 128MHz S11 is not absolutely terrible, so maybe you can tweak your original design with ideal component to a target of 150MHz and that way replacing one or two components could get you to something kinda working at 140.

Not sure if I am misunderstanding something, because the component values were already picked to target 150Mhz.  Well,  specifically the pass band is supposed to be 140-160MHz (The reality is that the frequencies we use are between 148MHz and 152MHz).  The tool on rf-tools.net gave those values, and when I simulate the filter with KiCad, it shows the correct passband.   

[Marsupilami]

Sorry, I thought your center was supposed to be 140. In this case try the designer tool to spit out something centered around 160 or 170.
Clearly your realization is off and until you figure out exactly which parasitics or other issues are causing the difference you can experiment easily with just adjusting the design to empirically fit real life better.

[psyon]

Sorry, I thought your center was supposed to be 140. In this case try the designer tool to spit out something centered around 160 or 170.
Clearly your realization is off and until you figure out exactly which parasitics or other issues are causing the difference you can experiment easily with just adjusting the design to empirically fit real life better.

Am I wrong in thinking I should redo the board to fix grounding issues and such first, and then as long as I have the right topology on the board, I can tweak components from there to dial it in?  Maybe when I put together the next revision, I can calculate the values for 160-180MHz, and then tweak from there.  Cross talk is my biggest issue at the moment.  Nothing else really matters if I can't get good isolation on each channel so I can do phase comparison without them interfering with each other.

[Marsupilami]

I can't rule out that that's going to help, but this is a very big assumption. Again looking at your S21 results between 2 ports you apparently have 20dB isolation.
When I have such a case ("what the flying f is going on with this board?!"), which is quite often, I try to experiment until ruled out as many potential causes as possible and try to find the root cause. This is mostly because a board spin is usually expensive, both in money and time and while it might not be the most fun tinkering with a clearly faulty revision there's often more things there to learn.
In your case it might make sense to just get a new board and hope that by fixing the grounding that takes care of all perceived issues. Maybe you can even add more diagnostic features. You have to do your own risk analysis on this

[psyon]

Again looking at your S21 results between 2 ports you apparently have 20dB isolation.

That's only looking before the mixer.  Please pardon the horrible images I am attaching.  With how I have things mounted right now, it's hard to get all four scope probes hooked up to the outputs.  The photos show the screen on my development board that my board plugs into.  Each channel is rendered from Channel 1 on top, to Channel 4 on the bottom.  FFT on left, just raw signal on right.  Raw signal being the output of the mixers, put through the low pass, and run through an op amp.  Input for this was -25dBm to avoid the output being clipped, but it is a bit on some of the pics.  The signals are drawn to scale.  The first pic (strongest signal on Green), is when the signal generated is hooked up to Channel 1, and no others.  You can see there is cross talk to channel two, but it looks a bit more than 20dB, but I could be wrong.  Second pic is when plugged into channel 2, and the signal strength on channel 1 is definitely more than -20dB from channel 2.  Channel 3 is the oddest one, since all channels show equally.  When plugged into channel 4, I get the best isolation from all other channels.  Everything on the front end is uniform, but the traces after the mixer are different, and wonder if that's why the cross talk varies so much depending on where I am plugged in.   VNA gives the same results no matter which input I test.

When I do hook up my scope probes, I see the same thing as I do when I use my own program to render them on the LCD.

[Marsupilami]

You can't be sure this is happening after the mixer.
The VNA measurement mostly checks only before the LNA. But let's say apart from the filter response being off we're good up to the amp input.
Is your LNA output biasing section correct? That's a likely culprit because all four tied together apart from the inductor holding off the RF. If that doesn't work well for some reason that's a problem.

[psyon]

Is your LNA output biasing section correct? That's a likely culprit because all four tied together apart from the inductor holding off the RF. If that doesn't work well for some reason that's a problem.

Bias point is correct on the output of the LNA.  Everything I read said that when using an inductor as an RF choke, you want the SRF to be as close to the frequency you are blocking as possible.  I was able to find one with an SRF of 150MHz.

https://www.digikey.com/en/products/detail/taiyo-yuden/BRL2012T4R7M/1788954