measuring trace impedance

Discussion in 'General Electronics Chat' started by kubeek, Apr 21, 2012.

  1. kubeek

    Thread Starter AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    I have seven 3" differential microstrip lines with 90Ω diff. impedance, and I would love to verify their single ended and differetial impedances.
    I don´t have access to network analyzer, but I have 40Mhz dual channel scope and multimeter with LCR measurement. I don´t have any signal generator, but I could hack something together.

    What do you suggest?
     
  2. kubeek

    Thread Starter AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    Suppose I use build an XR2206 function generator, how would I measure the impedance?
    I suppose I would need some high frequency inverting amplifier to have a differential signal relative to ground plane. Could I then use 45ohm resistors in series with the outputs and measure voltage on them through a frequency sweep? Do I need to terminate the other end?

    Also any replacements for xr2206? I can´t find it in local shops.
     
  3. crutschow

    Expert

    Mar 14, 2008
    12,993
    3,229
    It is difficult to measure such a short trace impedance without high frequency response instruments, such as a network analyzer. The propagation delay on a trace is only about 1ns/ft.

    Why are concerned with this? What is the frequency of the signals going through the microstrip lines? Normally they are only used at microwave frequencies where a quarter wavelength is less than the line length.

    The 2206 maximum frequency output will be much too low to be of any use in this measurement.

    The only way I can think of is to measure the end-to-end inductance and the line-to-line or line-to-ground capacitance, and calculate the characteristic impedance from those values (Z =√(L/C). But it won't be easy to accurately measure such small values of inductance and capacitance, since the strays will likely exceed the trace values.
     
  4. kubeek

    Thread Starter AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    The signals will be high-speed usb, which is clocked at 480MHz.
    I have claculated what the trace impedances should be when I designed the board, but I wanted to check how much do the inconsistencies in ground plane affect the quality of those traces.
     
  5. crutschow

    Expert

    Mar 14, 2008
    12,993
    3,229
    Unless the signals have sub-nanosecond rise and fall times, three inches of trace will have little effect on the signal, even if there's an impedance mismatch. The rule-of-thumb for digital signals is that you only need to be concerned if the rise time is less than 1/2 the propagation delay of the trace path.

    So measuring the impedance is an interesting academic exercise, but it's not necessary to insure signal integrity for that signal frequency and trace length. ;)
     
  6. kubeek

    Thread Starter AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    Well, the USB specificasion sets the Rise Time (10%-90%) as 500ps minimum.
    What is the propagation delay in this case?
    Edit: some calculator told me 166ps per inch, which adds to about 500ps
     
  7. WBahn

    Moderator

    Mar 31, 2012
    17,718
    4,788
    With a clock period of just over two nanoseconds, the rise and fall times would pretty much have to be subnanosecond. If we use c in a vacuum, the delay of 3" would be about 0.25ns. I don't have any feel for what c in a microstrip line would be. What, perhaps c/3 to c/2. Let's pick c/3 to be conservative, meaning that the delay would become about 0.75ns and half of that would be 375ps. So it seems like 3" is probably about at the limit of where you have to be concerned.
     
  8. kubeek

    Thread Starter AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    I think c is usually a little lower than 200m/us, so that gives 10cm/500ps one way for the longer traces.
     
  9. crutschow

    Expert

    Mar 14, 2008
    12,993
    3,229
    So it does sound like you are on the margin for the trace impedance being important.

    But that still leaves the problem of how best to measure that impedance. I don't have any new thoughts on that.
     
  10. kubeek

    Thread Starter AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    Ok, I got one new thought, how fast scope would I need to obtain to try time-domain reflectometry? I guess I could measure it at school.
    I would still need differential signal though, that complicates things a bit..

    I am still thinking if this is even necessary. Even though the production of the boards will cost a lot, I think that if I stick to microstrip calculations and keep the ground plane mostly intact under the lines I should be ok (there has to be a 6wire bus crossing perpendiculary under the microstrips unless I go for 4 layer board, but hopefully ~1cm of missing ground plane won't wreak havoc on the impedances)
     
  11. crutschow

    Expert

    Mar 14, 2008
    12,993
    3,229
    Au contraire. "Hopefully" seldom works in engineering. ;) 1cm (or any break) in the ground plane will indeed play havoc with the trace impedance. The voltage pulse traveling down the microstrip is balanced by a reflected current pulse traveling down the ground plane. If this ground pulse has to find a longer path then that will appear as a significant disruption in the characteristic impedance and cause a large signal reflection at that point. You must have a continuous ground plane under all microstrip lines so if that requires a 4-layer board then that is what you will need.
     
  12. Ron H

    AAC Fanatic!

    Apr 14, 2005
    7,050
    657
    I second that. A break in the ground plane, or even an area where the signal line does not lie directly over ground plane, will have a negative effect on signal integrity.
     
  13. kubeek

    Thread Starter AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    Actually the bus is around 4-5mm wide. I understand that "hopefully" is not a terrific way of engineering, but still it is more economical to try it this way, and if it doesn´t work then find some other solution.

    Right now I can see two solutions to this: either I have 35 jumpers on each board jumping over the differential pairs which seems very unpractical, or I go for 4 layer board which costs about 3 times more than 2 layer.
     
  14. crutschow

    Expert

    Mar 14, 2008
    12,993
    3,229
    Alternately you could use a short differential-pair cable wire run on the PCB for the USB connection.
     
Loading...