Impedance matching on the pcb.

Discussion in 'The Projects Forum' started by Olek, May 22, 2014.

  1. Olek

    Thread Starter New Member

    May 20, 2014
    2
    0
    I would like to clarify how to design pcb differential pair transmission line geometry to match cable impedance on one side and how to terminate the pair of traces on another side.
    Question#1:
    Are the following methods correct for designing pcb differential pair?
    For the example sake, I’m designing 90 Ohms pcb differential pair.
    I plan to use simple differential and single ended impedance calculators available online.

    Case “A”: Differential pair traces are routed close one to another (there is a coupling between them).
    Procedures:
    Use differential impedance calculator to determine transmission line geometry for given differential impedance Zdiff=90 Ohms (impedance seen between two lines of a pair).
    Value of Zo calculated by impedance calculator is not relevant here.
    Terminate far end of the pair with 90 Ohms resistor (it is odd mode
    termination).

    Case “B”: Differential pair traces are routed apart one from another (so that there is no coupling between the traces).
    Procedures:
    Use impedance calculator to determine traces geometry for single ended mode impedance Zo=45 Ohms.
    Differential impedance of the pair will be Zdiff= 2 x Zo=90 Ohms ( I do not need the calculator to get this value)
    Terminate far end of the pair with resistor Rt=Zdiff= 90R (it is odd mode
    termination).

    Question #2.
    Is common mode termination necessary to maintain signal integrity?
    I mean here termination for common mode signal or even mode termination.

    Aleksander
     
  2. MuPlusSigma

    New Member

    May 22, 2014
    13
    0
    #1 - Cases A and B are correct, although I don't know why you'd choose case B over case A. You want the traces close to each other so they see the same noise and cancel out cross talk. By odd mode termination, I assume you mean a resistor from one trace to the other. Put this resistor as close to your receiver as possible.

    What you have here sounds fine, but I can't promise it will work. You still need a good layout, etc...

    #2 - Your "odd mode termination" should be sufficient for signal integrity. If you're worried about the range of voltages the receiver sees, you can add some locations for thevenin style termination that you'd install if needed.
     
  3. AnalogKid

    Distinguished Member

    Aug 1, 2013
    4,546
    1,252
    What is the signal and what is the bandwidth? Full or micro stripline?

    Case B is frought with danger. Small mismatches in trace length can generate skew errors at the receiver. Also, as noted, you lose all common mode noise rejection. Plus, you create a condition that is more susceptible to differential mode noise.

    Separate from all of that, keep in mind that pcb traces are very thin. You can think of the sides of the two traces acting as plates of a long distributed capacitor. Long but not tall at all. The total plate area is tiny compared to the coupling to the ground plane(s). For the best signal integrity, it is the impedances from the traces to ground that must be the more tightly controlled.

    ak
     
  4. Olek

    Thread Starter New Member

    May 20, 2014
    2
    0
    Thanks for the replays.

    Why case 'B"?
    According to Lee Ritchey (from Speeding Edge) side by side routing doesn't guarantee common mode noise rejection and intoduces ditructive coupling.

    I want ro route USB differential pair trace using either stipline or microstrip line.

    Currently, I'm just learning high speed pcb design and I wanted to clarify some isues.

    Aleksander
     
  5. MuPlusSigma

    New Member

    May 22, 2014
    13
    0
    For Case B, you say that “pair traces are routed apart one from another”. This made it sound to me like they could take completely different routes. Now I think you mean routed next to each other, but just far enough so that the impedance is double the single ended impedance. That’s much more reasonable. If you had, for instance, two 8 mil traces with 17 mil spacing and 8 mil dielectric, I’d consider that Case A and perfectly fine, but you might put that under Case B.

    I skimmed Ritchey’s “A Treatment of Differential Signaling and its Design Requirements” from his website. I’m certainly not going to say that this expert is wrong about anything, but I do observe that this paper focuses quite a bit on what it considers to be misconceptions. There are always exceptions to otherwise good general rules. Instead of explaining these general rules and showing where there are exceptions, this paper "disproves" these rules by showing special cases where they do not hold. I suppose that if one is selling their expertise, a way to show one’s quality is to demonstrate how conventional wisdom and guidelines of other experts is wrong when taken out of context.

    Yes, side by side routing doesn’t guarantee common mode noise rejection. But it has good common mode noise rejection if you don’t do anything silly like route one differential line equally close to an unrelated signal trace as to its tightly coupled differential partner. I didn’t see anything about destructive coupling from Ritchey, so I don’t quite know what you mean.

    Use a stripline if you can. That’s better if you already have a stackup with interlayers. And if the impedance is very important, you’ll have to pay extra for an impedance controlled board.

    All of these guidelines become more important as the frequency increases. Also, good luck getting your drafter to follow them. Sometimes the hard part is deciding if you can live with what your drafter has produced.
     
Loading...