Confusion between single ended and differential ended impedances for HDMI

[tom66]

I'm designing a board with a HDMI input - this board will be used as part of my Ambilight project. I'm using an ADV7611 as my HDMI decoder and will be using OSHPark with the following specifications: 1.6mm board thickness, 35um copper, and relative permittivity of 4.6. I have been told that these parameters are reasonably well controlled. This will be (if possible) a 2-layer board.

The HDMI specification is 100 ohm ±15% differential-mode trace impedance... but they don't specify a common-mode trace impedance.  But, in order to get 100 ohms differential impedance my common mode impedance must be about 50 ohms, unless my traces were very close to each other. Does this sound right?

What trace width and impedance should I use? I used this calculator, among many others:
http://www.mantaro.com/resources/impedance_calculator.htm#differential_microstrip2_impedance

I calculated 8mil space between traces of thickness 116mil.

Well that doesn't make any sense! Not only would that make the layout virtually impossible, it doesn't match up with anything else I've seen before. HDMI traces are usually thin, and routed on top copper. I've seen them routed on two-layer boards as well, so I don't believe this is a 4-layer board issue. And the QFP the traces are being routed into has very little space to support such large traces.

I am a complete newbie to high speed digital design, so please excuse any errors in my calculations. I am sure I must be making some error here, but I don't know what it could be.

[bktemp]

100 ohm on a 2 layer board is practically impossible. The main difference between a 2 and a 4 layer board is the distance to the ground plane: On a 4 layer board the typical distance between the outer and inner layer is around 0.4mm. If you put that into the calculator, you will get much more practical values for the trace width.
If you keep the traces short, it will work even if the impedance is wrong.

[AndyC_772]

Agreed. If you're dealing with signals as fast as HDMI, you need a 4 layer board with a proper ground plane.

It's a subject I could prattle on about for ages, but here's a more practical tip. Head on over to http://speedingedge.com/ and buy Lee's book, or if you ever get the opportunity, go on one of his training courses. You'll learn more about high speed design than your brain can handle, and may come away (as I did) believing that nothing you ever design that's "fast" is ever likely to work.

But: you'll produce some very well designed products indeed just by trying.

[georges80]

As others have stated, you'll need to go 4 layer (or 6 depending on complexity of the rest of the design). If you want to control the impedance you will need to specify the layer stack and specify the required impedance for your trace width/separation to the PCB house so they can control the stack up thickness of the prepreg & layers or tell you to change your trace width/separation to meet their capabilities.

A trick to minimise EMI is to make the variation trace pair lengths DIFFERENT (you have quite a leeway within the HDMI spec) to 'spread' the energy to different times when it hits the connector. Read and learn about minimising stub lengths at the connector. Tie the ground pads of the connector at BOTH ends of the pad to reduce stubs.

Do NOT cut the ground plane (the one paired to the layer with the HDMI signals) anywhere under the HDMI traces. Do not switch layers for the HDMI differential pairs. Hopefully the IC you are using is pinned out to feed cleanly to the HDMI connector. Use soft/rounded corners if possible to route the differential pair traces.

Calculate your upper frequencies and put fencing vias all around the PCB perimeter (google and learn).

There's a LOT more to learn and implement if you want a good design (that is solid and doesn't radiate like a radar installation) versus one that sort of works... And 2 layers is not good in this case.

cheers,
george.

[tom66]

Thanks for the info so far from everyone.

4-layer is possible, but would be more expensive for a small run, this is for an internal prototype only - at least for now - so I would like to keep it on 2 layers if possible.

So, I am looking at the datasheet for the ADV7611 and it specifies that it is usable with 2-layer design. (http://www.analog.com/static/imported-files/data_sheets/ADV7611.pdf 1st page) (Yes the IC is optimised to route directly into a HDMI connector.)

Is this for some kind of theoretical super-slim 2-layer PCB?

I only need about 20mm between my HDMI connector and my IC. Could I use the 1/10 transmission line rule of thumb? (165MHz TMDS, wavelength ~1m in FR4, therefore anything under 100mm should be possible with minimal reflection issues)

If I am using 2 layers, are there any good rules on the trace width/length, spacing between TMDS pairs and each part of the pair, or does it not really matter that much?

[AndyC_772]

A trick to minimise EMI is to make the variation trace pair lengths DIFFERENT (you have quite a leeway within the HDMI spec) to 'spread' the energy to different times when it hits the connector

One of us is missing something here...

If you have a perfectly balanced differential pair, then at a given point along the transmission line, a positive going edge on one signal coincides exactly with a negative going edge on the other.

Therefore, the electric and magnetic fields due to one signal are exactly equal and opposite to those which are due to the other signal.

Therefore, the net field, as picked up by the receiving antenna in the EMC lab, is zero.

In practice, of course, the field is non-zero, but that's because of practical limitations. The P- and N-channel drivers aren't perfectly matched, the traces are slightly separated in space, there's common mode noise that's the same on both traces, and:

If the two signals are slightly skewed in time, then instead of cancelling out, the signal from one trace precedes the equal-and-opposite signal from the other.

I appreciate that, provided the skew is small compared to the wavelength of the highest harmonic frequencies that are present in the edges, then it's unlikely to have a major effect. You can usually get away without matching lengths to within fractions of a millimetre.

This is the first time, though, that I've ever heard anyone suggest that a length mismatch can have any kind of positive outcome.

Perhaps I've misunderstood, or am missing something. Can you elaborate please?

[AndyC_772]

So, I am looking at the datasheet for the ADV7611 and it specifies that it is usable with 2-layer design.

HDMI = consumer product, therefore = cheap, and they've tried to make it so that you can physically lay it out on a cheap PCB. That doesn't mean it's ideal from a signal integrity point of view, though.

The IC may well include drivers that have well controlled slew rates, which will tend to reduce the high harmonic content of the switching edges and minimise the harmful effects of an impedance mismatch, but that doesn't mean the design is 'right'.

If it's for a prototype, which will be used in a lab with short cables and known equipment, then it may be a non-issue. To heck with the impedance, just keep the traces short, and if it works, then that's great. Consider putting sites for small resistors in series with the HDMI signals, or perhaps even a small capacitor across each pair. They won't make the design "right", but with a given combination of layout, cable and connected device, they might make the difference between a board that works in the lab and one which doesn't.

Seriously, though... Lee's book. It's worth it.

[georges80]

I probably wasn't clear. I meant to say:

1) closely match the 2 trace lengths in ONE pair of HDMI differential signals.
2) do NOT match the length of one pair with another pair.

HDMI allows quite a skew between pairs and you can use a little of that to make the pair lengths different. This becomes more helpful with multiple channels (a recent design I did had 4 HDMI channels on the same board).

This hint was provided by an RF engineer that works in a large company as the EMI guru. His reasoning to me was to help spread the instant that the signals reach the connector, which though meant to be a good impedance match to the traces/cable will in practice have some mismatch.

cheers,
george.

[AndyC_772]

Ah... yes, OK, good idea. Spreading out one pair with respect to another pair, means you have a reduced overall signal amplitude at any given instant in time because the slightly mismatched edges don't coincide.

Makes sense, I like that idea. I wonder if it works with Gbit Ethernet too, which is notoriously bad for radiated EMI, but has 4 pairs that could be skewed w.r.t each other.

Anyone have the spec to hand?