HDMI Diff. Impedance

[Karamel]

Hi,

I am working with pcb design which has hdmi connector and hdmi transmitter IC and also, my pcb has 4 layer. (Signal, GND, Power, Signal)

I have read something about diff. pair calculation but, I didn't catch any of  how can I calculate diff. pairs impedance with these specifications. 

[Karamel]

I found some calculator in internet http://www.fedevel.com/welldoneblog/2011/08/pcb-impedance-calculator-single-ended-differential-pair/

I understood that, there are some important variations, such as, pcb thickness, dielectric meterial thickness, wires thickness or number of pcb layers etc. and I think, pcb manufacturing process is so important, because, for example if dielectric thickness change a little bit mistakenly, impedance changes too much. 

Have you ever had an experience about this situation?

[T3sl4co1l]

Easiest:

1. Pour solid copper polygons/planes on the inner layers.  This gives a foundation for the signals to work over.
2. Route high speed traces only over the outer layers.  And preferably, only on same layer as connector (no layer change -- vias).
3. Trace width depends on impedance, outer dielectric thickness, and dielectric constant.  Trace spacing (spacing between P/N in the diff pair) isn't very critical, but does affect it as well.

Typical 4-layer boards are built inside-out.  So, a "core" PCB (say 1mm thick) is etched with VCC/GND, then more PCB laminate is placed on either side, and the outer copper foils, and this is pressed and cured.  Then the outer copper is etched, holes are drilled and plated, and so on.

The added laminate is your dielectric thickness.  Usually 5-10 mils (0.13-0.26 mm) each, giving an overall thickness of 1.6mm or whatever.

The exact dimensions are specified in the layer stackup drawing.  If you don't provide one, or you're using a PCB proto service, you'll simply get whatever the PCB fab uses by default.  To find out what this is, find the information on their website.

Finally, use a microstrip or differential microstrip trace impedance calculator to find what trace widths you need.

You also need to match the trace lengths, most critically for P/N of each pair.  The lengths of all pairs don't need to be very well matched, but it may help.

One final trick:
4. If the trace lengths are very short (much less than the signal's risetime, say < 1 cm), the widths and lengths don't matter very much.

If you don't know any better (or you can't afford any better, such as putting the circuit on a cheap 2-layer board), place the PHY chip right up against the connector, as close as you can route it, including whatever support components (bypass caps, termination resistors?) are needed.

(The dielectric thickness for a 2-layer board is the entire thickness of the board.  So, you need very wide traces, ~0.8mm, to get useful impedances.  You can't even route a TSSOP component with traces that wide!  So for a 2-layer PCB, you have no choice but to make them short.)

Tim

[Karamel]

Dear T3sl4co1l,

Thanks for all informations  they are so clear, but I must ask one question to you because, I didn't understand second article.

This must be a suggestion, am I right? Because, I had seen some design which have diff pair lines in inside layers. Vias or pads must have an impedance? or must be change line impedance? So, How can I calculate all lines impedance with vias or pads? Do Pcb softwares, such as Altium, support this situation?


Addition:

I will exactly take this range less than 1cm (HDMI encoder chip <> HDMI connector) But I am asking these for learning.

[T3sl4co1l]

Vias are short, so do not contribute much to the trace length.  It is still best to avoid them.  Designs which use them, use as few as possible.

Tim