Actions
Forum Thread Details
  • Replies 36 replies
  • Subscribers 113 subscribers
  • Views 2866 views
  • Users 0 members are here
Related

Let's talk about Crosstalk !

battlecoder

I've been a member for a long time, but this is my first time posting.

I guess it's a bit too late for a presentation, but I'm a software engineer with a fascination for electronics; It's been my hobby for more than 20 years, and I keep learning new things almost every day.

I recently became interested in frequency domain analysis. I know it has countless applications in the Ham/radio world, but I was thinking about more general-purpose use cases; like identifying cross-talk or interference on a PCB design.

I know that's a huge topic and there's some well known general advice and practices to reduce this, like ground planes and decoupling capacitors, and filters... but I wanted to check how bad it could be, if absolutely no sane advice or practice was followed.

So I came up with this ugly PCB as my ultimate test-bed:

image

This is honestly not far from a PCB I would have designed when I was starting in electronics. I liked having nothing but the tracks on the board.

For a first test, I injected two signals from a signal generator on the left side of the PCB, both very stable and clean. One of them a 7 Mhz sine wave, and the other one a 10 Mhz square wave. I picked two relatively close frequencies to see how easy (or hard) was going to be telling them apart later.

Both traces start very far from each other on the left side of the PCB on big pads, and then they get closer together near the center, just to take on their own separate paths again as their approach the right side.

I'm monitoring the "output pad" on the right side for both waveforms on an oscilloscope, and while I was initially watching both on the screen of the scope, the one that I think looked more interesting was the output of the "sine wave" trace:

image

That's one messed up sine wave. For the record; without the square wave signal connected (or with the signal turned off), that wobbly sine-wave becomes a very clean, proper sinusoidal wave, so this was clearly the influence of the other signal.

I'm sure it's possible to use the FFT on the scope to dissect the frequency content of that signal,but I wanted to explore none-invasive methods. Something that I could use for a quick inspection and that didn't require probing around test points or component pins. Something that could potentially identify higher-frequency content outside of the range of my scope. And for that  I went for a cheap "near field" probe, connected to a TinySA Ultra Spectrum Analyzer. You can actually see the near field "probe" hovering over the tracks in the first picture.

This is a capture from the TinySA:

image

I was honestly amazed at how well this worked. The probe captured perfectly the two main components of the coupled signal (both a 7 and a 10 Mhz component) even without touching the PCB. Because I zoomed tightly on the frequency range of both signals there's no harmonics from the square wave in sight.

The results were pretty exciting to me, but this left me curious about a couple of things. And I thought this forum was the perfect place to ask::

How often is this kind of debugging needed in real life? How frequently is this kind of analysis required? (other than when performing EMI emissions testing). Is there an area in electronics where cross-talk issues are more of a problem than in others? (for example is this problem worse in high-frequency applications?)

If any of you have an anecdote or story where cross-talk has been an issue, a mystery, or a lesson well learned, I'd love to hear it!

  • I don’t have an answer but it’s an interesting experiment to post about.  Are you sharing the ground paths between the two signals?  What happens if you don’t?  What happens as the frequencies get further apart / closer together?

  • One area where this becomes a pain is when you have a mixer on a board and although you may have chosen an adequate filter to block the LO, it still manages to couple its way across the board so that a 'substantial' portion appears at the output.  I put substantial in quotes because on one hand you might kick yourself if the LO is 40dB below the carrier inspite of your filter, but at the same time 40dB means that it's only only 1/10,000 the power.

  • One way this problem can be solved, can be seen by looking at Ethernet cable. There, the signals are close to each other, but the coupling is reduced heavily by having each signal wire and its return twisted together (there are balanced signals there, but the point still remains), allowing 100m lengths to be supported.

    Similarly, on PCBs, it's a good reason why the ground plane is so necessary to reduce the loop area to a minimum. You'll see an improvement if you can replace that ground trace with a ground plane, although you may find the close parallel lines will still pick up some energy from each other, since the ground plane isn't so close compared to the distance between the lines.

    Other techniques are used too, e.g. try not to run wires closely like this on the PCB, and maybe even have a ground trace between the signals, if they are really sensitive, to reduce electric field impact too.

    Sometimes, parallel lines are actually deliberate; that's how some RF couplers work (at higher frequencies), one use-case being that it's handy for sampling a signal without extracting too much energy from it.

    EDIT: One more point; although the SA is a very suitable instrument for this, the H-field probe can be connected to the 'scope too, if the SA was not available, since these signals are likely still of sufficient power for resolving by the 'scope's FFT. Ideally needs 50-ohm termination at the 'scope end though (e.g. T-piece and a BNC 50-ohm load). 

  • The perfect storm:

    • several low level analog sensor signals (20 mV full scale)  where you need accurate waveform capture up to 1 MHz  with <0.1% error
    • the analog circuitry has a lot of high impedances to keep power consumption down
    • a microcontroller that is communicating over several digital serial channels plus rf channels.
    • all on a very dense and small PCB

    By the time you get this working well, you will have developed a lot of knowledge, design practices and tricks to manage noise and crosstalk.

  • in reply to Andrew J

    I think it's that lower trace in the photo, which is the ground path. Actually, one more experiment the OP could do, is swap the probe and croc-clip connections to make that ground path become the central trace instead of the lower one. Might improve things a bit, but really needs a ground plane.

  • in reply to shabaz

    I think the OP is just experimenting to MAKE crosstalk and see how bad it is, rather than asking why.  There's also the top unused trace.  

    I thought it could be interesting to create a PCB that had a variety of paths, e.g.

    • As per the OP: two signal paths that converge/diverge with a common ground
    • two signal paths that converge but have a  separate return between them
    • two signal paths that converge but have a separate return on the bottom side that lie directly under the signal path
    • two signal paths that converge but have a single (common) ground plane underneath them.
    • two signal paths directly over each other with a separate ground plane on the inner two layers (requires a 4 layer PCB)

    I suppose there are a number of combinations but it would be easy to experiment to see how signals are affected with these layouts at different frequency distances.

    As for the OPs original questions, I don't know as I don't have any experience to draw on.

  • If the question is how often this sort of troubleshooting is done with a H-field probe, I think the answer is mostly for EMI testing, simply because it's a crude method, it's hard to see fine signal quality detail. You can get finer probes, might need a preamplifier too. So, I don't think it replaces observing signals with a normal probe., mostly using time-domain view (e.g. eye diagram), but, more and more, using spectral analysis to see the finer detail that's not possible in time domain view. It would be unexpected to have extremely severe crosstalk because people would be using ground planes etc. So the measurements for crosstalk need to be more subtle, and test for longer! for instance bit error tests.

  • Great demo on cross-talking signal probes. One version of answers from my projects to you: cross-talking from such dirty PCB layout could cause a lot of challenges for SW/FW debugging.  If the traces are for high speed SPI buses, can you image that the SPI packages delivered from such lousy traces will make SW/FW folks' life easier? It it just for medium high speed communications. If the projects are for PCIE/SATA/SAS signal lines, cross-talking issue is one of main tasks for HW/FPGA designers to overcome even before SW/FW folks jump into the projects. In general, signal integrity process can help designers to get a solid design to avoid such bad cross-talking issues. However, SW/FW might be the first one to find the issues after bring the board up into running, Then HW/FPGA designers might use the demo flow you presented here for HW trouble-shooting.

    In summary, cross-talking analysis can happen more likely at higher speed signals/differential signals and high density PCB boards than lower speed and low density PCB boards.

  • Long ago I was developing a high-speed data collection system that contained both analog (Op-Amps and A/D converters) and digital (75Mhz DSP, large CPLD, multiple banks of RAM and a USB transceiver). I used large, flooded ground and power planes throughout the PCB.  In initial testing it became very clear that there was a lot of crosstalk in the design, with very clear signs of the digital signals being superimposed on the analog signals.  In analyzing the design, there were significant digit signal runs over large areas of the power and ground planes.  I started doing a lot of reading about grounding techniques and decided to minimize ground and power flooding, in exchange for a more purposeful routing, with a more star like routing.  That and forcing and high-speed signal to cross power/ground traces at a perpendicular path.   The effects were absolutely amazing.  I went from a huge crossover issue to a drastically reduced occurrence. up to the point that it was not visible in scope tracings or in the collected data.  

  • in reply to Andrew J

    You are correct! bottom trace is ground in the test setup. I also added a top trace in case I wanted to experiment with adding a second ground path at top. Using one of the middle traces as ground is another completely valid experiment, but as Andrew mentioned, I first tried to make crosstalk happen, which is also the reason why I didn't add a ground plane to begin with.

    I like the idea of creating a PCB with variety of paths. Like a sort of cross-talk educational board!