High-Speed PCB layout challenges - Learning the dark art the hard way.

[Rerouter]

Well i did the math, for a 5ghz resonance you only need 1.45nH of inductance, which i would say is in the right ballpark.


That resonance also has a wavelength within 10 times your trace length so tansmission effects are out to play, (60mm)

From the looks of things, the edge only rings twice, then stops, while at the same time those first 2 rings decay only a tiny amount impling to me that the termination is sending off a decent reflection,

When i do the math that 700fF probe capacitance is almost 50 ohm loading at that 5Ghz resonance, which lines up with what we are seing, the fast signal meets with a 25 ohm load, kicks off an ugly reflection, its phase inverts, destructivly adds and kills the ringing.

So it would appear that yes this one is mostly down to impedance errors.

The probe is likely both adding the resonance and adding the spike aplitude,

[Rerouter]

You can actually use this info to your advantage, if you pull up some charts showing overshoot vs impedance difference and subtract out the probes contribution you should be able to say how close to the mark you hit on the traces

[T3sl4co1l]

Remember what frequency and impedance means:

5GHz and 100 ohms is equivalent to 0.318pF and 3.18nH is equivalent to 2.5mm and 50ps.  (That would be 1/4 wave at 5GHz, and the length assumes unity velocity factor: the maximum possible length in any medium.  Microstrip gives about 0.7-0.8 times length.)

The culprit can be nothing other than a geometric feature with these dimensions!

Tim

[rx8pilot]

The culprit can be nothing other than a geometric feature with these dimensions!

Tim

I wish I could fully grasp that - what am I missing? If the trace was a little longer it may not resonate?


I did a quick measurement that was helpful to see. A short 12 inch piece of 75 Ohm coax was connected to the signal source and I roughly terminated the end of the coax with a single 0402 75 ohm resistor (like I said, rough). I wanted to compare the signal from the source and the output of the DUT with the exact same test fixture. The scope has EQ and clock recovery built in which makes this quite a bit easier. Looking at the DUT output on the end of the cable is not nearly as bad as what I see on the 100 ohm differential traces. There is still some ringing, but not the worst I have ever seen. Maybe some of the 5Ghz ring is simply filtered due to bandwidth limitations of my makeshift test fixture. sure wish I had a 3Ghz and 6Ghz signal source - but I have to wait for that.

The screen shots have some erroneous traces and the cursor data is meaningless.

[Rerouter]

Hmm, still 5Ghz ringing, under quite a different setup. could you try changing your termination value with this setup, to say 120 ohms, again the scope loading will be  quite high, and this can let you isolate it out.

[rx8pilot]

Is the probe loading really that severe? It seems it would be useless if it loaded high frequency circuits that much.



Sent from my horrible mobile....

[Rerouter]

3.125Ghz with a 700fF capacitor is 73 ohms of impedance, in reality being a square wave the frequency it will be far lower impedance, but as those higher frequencies are already lower in amplitude its not as much of an issue.

[T3sl4co1l]

I wish I could fully grasp that - what am I missing? If the trace was a little longer it may not resonate?

It's so obvious, it could only be impossible to understand.

Presumably, you have an unterminated or mismatched stub somewhere.

The length of the stub is inversely proportional to the resonant frequency.

There cannot be any longer transmission line segments that produce that ringing.

So, on the list of suspects, the long PCB traces are right out.

IC interconnects (trace taper/neckdown/fanout, if applicable; pad and bondwire equivalent circuits) could plausibly be on the list, but hopefully are taken care of by the manufacturer (pin models and internal terminations designed to tune that out), and are still on the short side (< 2mm).

Also, the impedance of the suspected stub should be fairly high, since the amplitude of the ringing is much less than the total height of the transition.  (Or fairly low, if it's a series stub, but that would be harder to explain.)

The common element in all of this: the probe itself.  Which looks like it has dimensions, and RLC equivalent specs, plausibly similar to the observed effect.

You should drop the probe (not literally, that would be expensive~) and use a direct wired approach as your gold-standard reference.  This will show if it is indeed the probe itself.  Standard RF techniques apply: build a microstrip resistor divider/attenuator alongside the trace, to tap off some signal and route it to a coax cable.  Use a wideband balun to resolve differential mode waves specifically (or matched lengths of cables and difference it at the scope -- precision matching probably not being required due to delay adjust in modern scopes).

Tim

[AndyC_772]

I'm afraid I can't offer any further insight right now, but one very good thing has come out of this.

You've learned that a whole host of PCB features, which may have been non-optimal, actually don't matter nearly as much as you might have thought!

There's hope for us all here 

[BrianHG]

The scope has EQ and clock recovery built in which makes this quite a bit easier.

Q: Are you using a fixed EQ to compensate for your probe?  This is OK.
If you are dynamically equalizing the source signal, then what you are looking at is not what's truly going on at the PCB trace level.  It's being filtered to get the best possible eye opening.  Equalization like this may also hide a lot of fine issues with layout and all the testing/scope shots you've done to date may be faulty.

[rx8pilot]

Good point to bring up. I only used the EQ in a fixed mode on the scope to get an idea of how well the data can be recovered after being launched into the coax cable.

I was examining traces as an un-processed signal which shows me everything. Since I have little experience measuring signals this fast, I am looking at them in a variety of ways to build some intuition about the task. When I started down the path of power electronics a couple of years ago - I was seriously humbled at the difficulty of measuring those systems in a way that delivers useful information. Looks like high-speed digital will slap me in the face a few times.



Sent from my horrible mobile....

[rx8pilot]

3.125Ghz with a 700fF capacitor is 73 ohms of impedance, in reality being a square wave the frequency it will be far lower impedance, but as those higher frequencies are already lower in amplitude its not as much of an issue.

I looked closer (as much as I am able) at the probe loading and what you (and Tim) have been saying is starting to make sense. The probe manual has some solid data to go by and I clipped the impedance plot for reference. It shows that the impedance drops to a min of 220 ohms as the frequency goes much above the Gigahertz range. This, as mentioned, can certainly disrupt a differential trace and create the ringing. The question I end up with is how do you measure a differential trace as I am trying to do? Maybe it is not possible to directly probe it in circuit? Maybe an indirect measurement of the trace impedance like a TDR and a test coupon? Maybe removing the reciever chip and terminating the line with an appropriate value to combine probe loading and have a 100ohm load in the end? Keysight provides the SPICE model for the probe and the tip which makes it fairly easy to make a simple simulation to better understand what is happening.

Hmm, still 5Ghz ringing, under quite a different setup. could you try changing your termination value with this setup, to say 120 ohms, again the scope loading will be  quite high, and this can let you isolate it out.

It appears that 120ohm termination plus the probe should be rather close to the Z₀ of 75 ohms. It is easy to try.

Presumably, you have an unterminated or mismatched stub somewhere.

The BNC launch is questionable for sure. I am still planning to have Samtec help me get those launch structures dialed in. One known issue is that I am launching on the top side of the board and the recommendation of Samtec is to launch on the bottom with the connectors I am using. I was not confident in a bottom launch and then having to transit a via to get to the signal side of the PCB. Physical restrictions of the intended mechanical housing create this challenge. The stub is leaves maybe be enough at 2-3mm to cause a problem. The quick test is for me to trim the center pin of the BNC to remove the stub and see if it makes an appreciable difference. Samtec offers a custom service for connectors where they trim the center pin to allow launching on the top of the PCB. I would rather learn how to successfully use a via to avoid custom connectors if it is needed.

At the moment, I am hypothesizing that there are issues with the design and the measurements - but closing in on a workable solution.

[Pitrsek]

Actually going trough via is better than keeping stuff on one layer and having a THT stub on the connector.
If you go trough via, it behaves like a transmission line - with appropriate ground vias around it can be  made +- correct impedance. If you do not travel trough the via, via behaves like a small capacitor. That's reason why are connectors back-drilled. More info in L.Ritchey books and most probably in some papers as well.  Do you have a spare PCB sample so you could back drill the connector center pin?

EDIT: Soldering the connector from the other side is probably way easier than back-drilling 

[rx8pilot]

Actually going trough via is better than keeping stuff on one layer and having a THT stub on the connector.
If you go trough via, it behaves like a transmission line - with appropriate ground vias around it can be  made +- correct impedance. If you do not travel trough the via, via behaves like a small capacitor. That's reason why are connectors back-drilled. More info in L.Ritchey books and most probably in some papers as well.  Do you have a spare PCB sample so you could back drill the connector center pin?

EDIT: Soldering the connector from the other side is probably way easier than back-drilling 

Back drilling definitely seems like the long road to the solution. All I need is some more learning and confidence to use a via properly in this case. I do have plenty of PCB's but not enough of the chips to make another board - only had two samples of each part. All layers were cutout on the PCB design except the top signal layer. I can trim the pin back on the assembled PCB to about 30mils of the top layer to see what difference it makes.

To eliminate the probe artifacts - I connected the signal source directly to the 50ohm input on the scope with a 75 Ohm BNC cable. This is a 75ohm source and cable going into a 50ohm load, but for comparison of source and DUT, is not a terrible idea. Both ends are BNC which eliminates the need for any adaptors to physically connect them. If all was perfect, the DUT output would look identical to the original signal source.

The signal source looks quite reasonable considering the mismatch. Looking at the DUT output - and it has a relatively small ring. Not nearly as much as we saw with the active probe on the differential PCB traces. Does this mean that maybe I am not as far off as I thought or is the cable simply acting as a low-pass filter that has the appearance of improvement?

In the image - the blue trace is the signal source and the orange is the DUT output. A single pulse using the same cable and scope input.

[BrianHG]

Once again, your output signal rises and falls much faster, even more now than before, than your source.  This is to be expected of a re-clocker (this is the purpose of the re-clocker, make a clean new square wave, clocked cleanly to a new synthed PLL clock, remove timing discrepancies from long transmition cables, rise and fall as fast as possible).  I bet if you place a series 25 ohm resistor, or series ferite/inductor to match slow down your output to match your source, I bet the ring will be almost completely gone.

[Someone]

The question I end up with is how do you measure a differential trace as I am trying to do? Maybe it is not possible to directly probe it in circuit? Maybe an indirect measurement of the trace impedance like a TDR and a test coupon?

Well you can TDR the board with or without the chips in place, but what you are looking for and how to correct the eye is then relying on experience and understanding of the design. Lots of pretty pictures and some good information here:
http://www.keysight.com/upload/cmc_upload/All/Download1.pdf
But the link seems brittle, its a presentation titled 'Measuring “Hot TDR” and Eye Diagrams with an Vector Network Analyzer?'

But going back around again, once you know the probe loading you can put it back into simulation and see how its affecting the data/eye. Getting a probe with lower loading you'll soon run up against its limitations anyway so its back to simulation and modelling, or paying big money for automated de-embedding. In the end the only interesting parameter for your customer is the signal they receive at the end of the cable, so you can ignore a lot of the intermediate measurements and concentrate on what arrives at a properly terminated receiver having passed through cables.

[T3sl4co1l]

The twiddle in the waveform may be mismatch at the join between cables.

Ringing due to mismatch of long cables (>> 1mm) can only manifest as ringing at correspondingly low frequencies (many cycles!).

Tim

[Rerouter]

There are actually differential probes out there with as low as 35fF of capacitance, these are what come out when you want minimal loading.

However i expect it to cost as much as a house.

In both cases, you use the difference between measuring styles to figure out the difference caused by the probes,

To really hit the nail on the head you can follow approches like the following link, you would test each output with only the probe and matching circuit loading it.
digitizers/impedance_and_impedance_matching

Once you see that the signal is clean and the inpedance of the trace in spec, so long as the termination is correct within the reciever you can have a good idea on what the signal actually resembles

[rx8pilot]

Once again, your output signal rises and falls much faster, even more now than before, than your source.  This is to be expected of a re-clocker (this is the purpose of the re-clocker, make a clean new square wave, clocked cleanly to a new synthed PLL clock, remove timing discrepancies from long transmition cables, rise and fall as fast as possible).  I bet if you place a series 25 ohm resistor, or series ferite/inductor to match slow down your output to match your source, I bet the ring will be almost completely gone.

Yes, it is faster rise time for sure. The slew rate is limited at 1.485Gbps and will be faster at 3G and 6G when detected. At that point, the ringing would likely be faster than I can see. If I slow it down externally, it may cause problems with the faster slew rates when they are applied. Do you suppose the value of the inductors on the return loss network may need some re-considering? The output path is a 75ohm resistor in parallel with a small 4.7nH inductor just before the AC coupling cap. I have a slightly larger value and a slightly larger value but they both made things quite a bit worse. (did not grab any shots of that).

I also back drilled the center pin of the BNC up to about 30mils of the top signal layer - that did not appear to change much. It may have helped, but compared to the bump I am looking at it was contributing very little.

Well you can TDR the board with or without the chips in place, but what you are looking for and how to correct the eye is then relying on experience and understanding of the design. Lots of pretty pictures and some good information here:
http://www.keysight.com/upload/cmc_upload/All/Download1.pdf
But the link seems brittle, its a presentation titled 'Measuring “Hot TDR” and Eye Diagrams with an Vector Network Analyzer?'

But going back around again, once you know the probe loading you can put it back into simulation and see how its affecting the data/eye. Getting a probe with lower loading you'll soon run up against its limitations anyway so its back to simulation and modelling, or paying big money for automated de-embedding. In the end the only interesting parameter for your customer is the signal they receive at the end of the cable, so you can ignore a lot of the intermediate measurements and concentrate on what arrives at a properly terminated receiver having passed through cables.

Big money seems to be very helpful testing electronics  Automated de-embed, RF sim software, and various other tools are still in dream territory right now. I love watching the various marketing videos from Keysight and Rode - and then I discover the amazing piece of gear they are showing is about $300k and I move on the the next best thing: Guessing 

Seriously though, I am looking at how to take advantage of the SPICE model provided by Keysight of the probe. I have only used SPICE for much more basic simulation, so that would be yet another software learning curve  I have never tried to effectively de-embed a probe (or fixture) from a measurement. What is the magnitude of effort needed to accomplish what you are talking about for someone that has never done it?

The twiddle in the waveform may be mismatch at the join between cables.

Ringing due to mismatch of long cables (>> 1mm) can only manifest as ringing at correspondingly low frequencies (many cycles!).

Tim

Just for reference - I am going to try various cables to see how they may be different. I have a variety ranging from short/good to long/bad and quite a few in-between.

[rx8pilot]

There are actually differential probes out there with as low as 35fF of capacitance, these are what come out when you want minimal loading.

However i expect it to cost as much as a house.

Yikes! I would be rather happy to have a second one of my 'low end' 700fF probes 
Hopefully, I will have a 3G and 6G signal to try soon - very curious how the system will respond to faster rise/fall times.

[BrianHG]

The output path is a 75ohm resistor in parallel with a small 4.7nH inductor just before the AC coupling cap. I have a slightly larger value and a slightly larger value but they both made things quite a bit worse. (did not grab any shots of that).

Arrg, an added inductor in a microwave speed signal path with a capacitive load....  Can you please draw a diagram of your output path filter, with the location on the PCB (just painting the probe points on your PCB screen capture would be fine).  This can easily generate signal ring & if it is part of the manufacturer's recommended output, it may be there to limit or enhance the fine edge of the signal.  You may just need to tune the inductor value to trim out your PCB's characteristics.

[rx8pilot]

The output path is a 75ohm resistor in parallel with a small 4.7nH inductor just before the AC coupling cap. I have a slightly larger value and a slightly larger value but they both made things quite a bit worse. (did not grab any shots of that).

Arrg, an added inductor in a microwave speed signal path with a capacitive load....  Can you please draw a diagram of your output path filter, with the location on the PCB (just painting the probe points on your PCB screen capture would be fine).  This can easily generate signal ring & if it is part of the manufacturer's recommended output, it may be there to limit or enhance the fine edge of the signal.  You may just need to tune the inductor value to trim out your PCB's characteristics.

Here is the data sheet and my layout. The data sheet clearly states the inductor values are a guideline only and need to be adjusted to compensate for the characteristics of the actual PCB. I am not sure how to know how to go about that. I went a little up and little down on each one and the result was worse. At the moment I have the datasheet values in the DUT. I only have 3 values available to me right now - 6.2nH, 4.7nH, and 2.7nH. On my next DigiKey order I will throw in an inductor range that allows finer steps.

[T3sl4co1l]

Try 0402 resistors and inductors (assuming the resistor power dissipation isn't a problem), and squash them as close together as possible.  Keep trace width constant, rather than necking up and down all the time.

Tim

[BrianHG]

Arrrg, you are driving the +&- balanced output to 2 different track lengths...  You do realize that the a balanced load on each output on the IC make a balanced equal load on the IC's power supply as well, canceling out internal the IC's VCC&GND current consumption equally making a flat consistent DC load on the die.  The timing error you create by un-balancing the output perfectly will add a ring or bounce to both outputs as the designed neutral load no longer exists.  Now, this is if you want the penultimate perfect signal achievable with the IC, this doesn't mean what you have done wont still create a great SDI signal.

Next step, test: Short out 2.7nH to 0 ohm and re-scope & post images.

Also, when doing your next PCB, the pullup inductor/resistors network with +/- outputs should match in physical size and structure being mirror like right up at the IC.  This once again goes towards both the positive and negative outputs having a perfectly matching drive and load.

[rx8pilot]

Arrrg, you are driving the +&- balanced output to 2 different track lengths...  You do realize that the a balanced load on each output on the IC make a balanced equal load on the IC's power supply as well, canceling out internal the IC's VCC&GND current consumption equally making a flat consistent DC load on the die.  The timing error you create by un-balancing the output perfectly will add a ring or bounce to both outputs as the designed neutral load no longer exists.  Now, this is if you want the penultimate perfect signal achievable with the IC, this doesn't mean what you have done wont still create a great SDI signal.

Next step, test: Short out 2.7nH to 0 ohm and re-scope & post images.

Also, when doing your next PCB, the pullup inductor/resistors network with +/- outputs should match in physical size and structure being mirror like right up at the IC.  This once again goes towards both the positive and negative outputs having a perfectly matching drive and load.

Ya know - that was not even considered at all but makes sense. Thanks!

Try 0402 resistors and inductors (assuming the resistor power dissipation isn't a problem), and squash them as close together as possible.  Keep trace width constant, rather than necking up and down all the time.

Tim

The resistors are already 0402, but the L's are 0603. I was split on the tapered traces until I found an app note that specifically compared the various track geometry on a VNA. I am going to post it to see if anyone has an opinion on the information.