Differential pair design

[David6B]

Hello, these are HDMI high speed differential pair channels. i can see some things i don't like so much but i don't have enough practical experience to know if they are relevant.
Can anyone see any problem?

Thank you so much.

[blackfin76]

Well I see a couple of things that are not optimal. First of all the way the length matching is done is common for single ended signals but for differential signals you don't use this methode. Second thing is the differential pairs should be couples together with a minimal amount of trace separation to route around via's. Preferably route the whole differential pair around any obstacles. Also try to minimise cross talk with other differential pairs by increasing the physical separtion as large as possible.

[David6B]

thank you, do you think that those mistakes are big enough to have a real impact in the signal?

[blackfin76]

Well that is a good question, I can't give you the answer to that. There are many factors that contribute to things like skew, reflections and cross talk and they all add up. If the rest of the transmission path is very good you may have a lot more margin in your PCB design. Most 'guidelines' for high speed routing have tolerances that allow for a certain amount of error to make things work guaranteed. To find out how this design inpacts the system you can do measurements or simulations. You can also simply test the system the way you are going to use it and just see if it works. Personally I prefer to stick to the standards design rules. You can find lots of information on the internet about routing HDMI signals.

[T3sl4co1l]

Carefully controlled diff pair separation is largely a lie, and also largely unnecessary*.

Just because you routed another wire, doesn't magically absolve you of the duty to ensure the signal is in the correct common mode range for the receiver, or to keep noise low enough that the receiver does not misbehave.

The only thing you get: the signals are routed through the same locations, at the same times.  Time being relative to when the intended signal was launched down each trace -- in other words, the trace length from the transmitter.  Therefore, if the two traces always cross another trace (on an adjacent layer), or a gap in a split plane, at the same length-from-transmitter, then the induced noise will be balanced (common mode), and subtracted out by the receiver as long as it's still within its range.

For HDMI specifically, there ought to be a common mode impedance spec (I don't know specifically; I do know USB has such a spec, for instance), and this should be followed within the PCB.  If the traces have to split up, like shown here, that's not terrible, as long as the normal mode impedance is still followed; more important is just to keep the lengths matched, because that prevents common to differential mode conversion.

Most of all, high speed interfaces are designed to deal with bad cables and bad layouts.  You can do some pretty awful things, and still get good performance.  I don't recall that HDMI is as robust as, say, Ethernet, but you still have quite a large margin to exceed (i.e., somewhat less than the 50% logic threshold) before digital data is just completely toast.  The consequence is, using up more margin within the PCB leaves less margin for crappy cables.  So maybe you will later find you need a better-than-bargain-basement cable, or that it works with, say, 6m cables, but is unreliable with 8m cables and doesn't work with 15m cables.  That's the most likely result.

*Large in terms of the number of units built for a particular purpose.  HDMI TVs and monitors are everywhere, and it doesn't matter there.  Places where it is absolutely critical to performance, like femtosecond-jitter clocks in kilobuck FPGA boards, are not common!

Tim

[T3sl4co1l]

Well that is a good question, I can't give you the answer to that. There are many factors that contribute to things like skew, reflections and cross talk and they all add up.

I can give you the answer to that.

The coupling between adjacent traces within a layer, is typically small, less than 30%.  (I have to use "typical" here, because the board stackup is not specified.  If stackup, material, and trace width measurements were provided, the equivalent circuit could be solved for.)

So, if one trace has a full logic step, even if it's directly adjacent to another, the amount of induced interference is only about that much -- 30% of the full step, or whatever.

Crosstalk drops rapidly with separation, so that, say, 20 mils away from a 7 mil trace, in a 10 mil stackup, will be more like, uh, 5 or 10% I think.  (I don't have the numbers handy -- I'm pulling these out of my ass -- but they are easily solved for with a coupled-line calculator.  Search for one! )  That's enough to upset timing in a critical interface (you wouldn't want to run your RF synchronizer clock through here), but well within the capability of a typical commodity serial bus!

And as I said above, length matching is the more critical factor -- if a pair is routed from point A to point B, and ends up going through a few bends, the innermost trace will have less length than the other, and so must make a small loop somewhere to take up that difference.  Preferably, this happens at the corner, preserving the condition I gave above (lengths matched throughout the route).

Interference is also a length-dependent thing.  A length-tuning feature nearly touching another trace won't introduce much interference, it's probably a small fraction of the wavefront (the length of the wavefront being, the signal's risetime as it appears in space, moving at the speed of light).  If they were routed poorly so that there's a long stretch of proximity, there will be much more crosstalk, up to the full coupled amount (give or take frequency content, because of resonant effects of coupled lines).

So no, for almost all cases, don't worry about it, prioritize the other things.  Don't ignore these aspects, of course, but don't compromise higher priority aspects!

Cheers,
Tim

[blackfin76]

I agree with most of what you said but... I know the coupling between the two traces is not very large and therefore consider both signals as a single transmission line.  Routing both signals as a pair has the obvious advantage that both signals are influenced in a simular way and thus have a simular influence on the common mode signal path. The second benefit is that it's easy to check by simply looking at the art work and it also looks 'nice'.

[T3sl4co1l]

I agree with most of what you said but... I know the coupling between the two traces is not very large and therefore consider both signals as a single transmission line.  Routing both signals as a pair has the obvious advantage that both signals are influenced in a simular way and thus have a simular influence on the common mode signal path. The second benefit is that it's easy to check by simply looking at the art work and it also looks 'nice'.

You might've missed:

if the two traces always cross another trace (on an adjacent layer), or a gap in a split plane, at the same length-from-transmitter, then the induced noise will be balanced (common mode), and subtracted out by the receiver as long as it's still within its range

Agreed that it looks better.  Sad that good looking structures aren't always good E&M structures, oh well.

[David6B]

Thank you all for the replies. My concerns are on those red spots where one trace is much closer to another differential pair than to its complementary. Is that enough to ruin the signal?

[T3sl4co1l]

I wouldn't think so.  But there is a ton of space to move them around, which I would do just because it looks better.

Tim

[David6B]

Tks for all the help. will do.

David

[Deridex]

I'm surely no expert at routing high-speed-signals, but im pretty sure that meanders with 90° turns are no very good idea.
I would try to get em to 2x 45° or make em round.

[Gibson486]

Well I see a couple of things that are not optimal. First of all the way the length matching is done is common for single ended signals but for differential signals you don't use this methode. Second thing is the differential pairs should be couples together with a minimal amount of trace separation to route around via's. Preferably route the whole differential pair around any obstacles. Also try to minimise cross talk with other differential pairs by increasing the physical separtion as large as possible.

Can you elaborate? If it is a single ended signal, why would you need to match length? I am not challenging, i am just curious. Perhaps I have some semantics messed up and (even more likely), I have not encountered such things in my designs.

[Rerouter]

Ok, For example routing to a microSD card, all the signals are single ended, but they are defined by 1 clock signal, now those lengths need to be within a certain deviation from that clock signal to make sure they are sampled at the correct time.