Connect with us

Propagation delay in PCB traces

Discussion in 'Electronic Design' started by [email protected], Aug 18, 2008.

Scroll to continue with content
  1. Guest

    Hey gang,
    Time for another difficult question.
    How can I figure out a tolerance across different PCBs for a given
    electrical length?
    Suppose I tuned a trace to have +200 ps, how will this 200ps vary
    across
    temperature, process variation, time, one batch to the next?
    Anyone know where to start? I've asked around and all I got was
    "measure it".
    There has to be some sort of theoretical base to start from.
    TIA
     
  2. Guest

    Thanks John. It is on a Rogers material. I am looking at Appcad now,
    it is quite nice. Never heard of it before.
    A well kept secret of pros, I guess.
    I will read up on all relevant parameters of Rogers and see where this
    leads me.
     
  3. TT_Man

    TT_Man Guest

    And you're going to put 75A down a PCB track?
     
  4. Guest

    Uh, what? Wrong thread maybe?
     
  5. Tom Bruhns

    Tom Bruhns Guest

    RFSim99 is another freeware program that's useful for playing with
    things like this; it has a built-in microstip and stripline
    calculator.

    You didn't elaborate on just why you care, but I'd suggest that for
    most things, it's not going to matter much at all, and if you want
    things to be seriously stable, you should probably in any event
    arrange to have board effects cancel out in some way:
    autocalibration, use of matched traces so it's the differential that
    matters, not the absolute propagation, or things like that.

    But at the same time, the physics helps out some: propagation
    velocity depends on the effective permittivity that the fields are
    traveling through, and propagation velocity varies as the square root
    of that. Not only that, but the dielectric for microstrip is
    partially air, which doesn't vary much. So for example, nominally 50
    ohm microstrip on er=5.0 substrate yields about 1.56e8 m/sec
    propagation velocity; er=4.5 makes that 1.64e8, and 4.0 makes it
    1.73e8. (Different calculators will yield slightly different answers,
    but the variation as a percentage should be very close.) So a 20%
    reduction in er made for about a 10.9% increase in velocity. That was
    for a trace width that stayed constant; if the trace width is adjusted
    to keep impedance constant, the percentage in propagation velocity is
    slightly less. For stripline (embedded in a constant er), the
    velocity variation over the same er range is about 11.8%.

    Note also that there is some variation in velocity as a function of
    frequency...it's not huge, but it's there.

    It will help a lot if you specify a particular substrate material.
    "FR4" doesn't cut it; "Isola 370HR" (for example) will get you much
    more consistent results, and you can search for substrate materials
    which are particularly stable and whose manufacture is well
    controlled. Consult with your board fab house about this!

    Cheers,
    Tom
     
  6. Guest

    Thanks, in any case the widest swing seems to come from the
    variability of the Er of the material, which is 3.36 +- 0.05, about +-
    1.6% ( I think).
    I don't know what causes the +-0.05 change though. Things like thermal
    expansion of the board seem to have a negligible impact, if my home-
    brewed spreadsheet is to be believed.
     
  7. Tom Bruhns

    Tom Bruhns Guest

    Yes, that should be the case. If the transmission is embedded
    entirely in a dielectric of relative permittivity, Er, and the
    magnetic permeability is the same as freespace, and the line is run in
    TEM mode, then the propagation velocity is 1/sqrt(Er) times the
    freespace propagation velocity. It doesn't matter what the dimensions
    are (so thermal expansion has no direct effect), or what the line
    impedance is. For microstrip, the fields aren't completely inside the
    Er of the substrate; some are in the air above the board. Thus the
    propagation velocity is slightly faster, the mode isn't true TEM, and
    there's some dispersion. See, for example,
    http://www.microwaves101.com/encyclopedia/dispersion.cfm, for more
    info on this.

    I'd expect Er to vary with temperature, with frequency, with absorbed
    moisture, ... (Note: Er of air is slightly greater than 1, and
    changes with pressure, temperature, humidity, ..., enough to be
    noticeable if you are monitoring part per million changes in
    capacitance of air-dielectric capacitors.)

    Cheers,
    Tom
     
  8. One tough application I ran into is doing PCB's
    for radar detectors, you know those do-dads
    speeders use to detect cop radar.
    In place of 90 degree track turns is a curved
    radius to prevent radiation. I suppose at a 1 cm
    wavelength track length needs to be accounted
    for too, because of phase.

    I think I'd start with a computer (numerical analysis)
    sim, and see how it works. You can build in provision
    for slight tweaking to refine it.
    Ken
     
  9. Tom Bruhns

    Tom Bruhns Guest

    On Aug 20, 9:40 am, "Joel Koltner" <>
    wrote:
    ....
    Do you really think it's going to be practical to tune the equivalent
    of an inch or two of propagation with something like a "fat blob"
    that's small enough to not mess things up at a few GHz?

    How about some line sections in a binary sequence of lengths that
    could be patched in or out, depending on where shorts were placed?

    Or maybe just design things so the effect can be calibrated out...

    Cheers,
    Tom
     
  10. Hi Joel,
    Judging from your post, betcha you're a sharp engineer
    who knows his stuff, including Maxwell's Eqs, but I
    won't go to math unless you want.

    Ok. Agreed the 90 can be considered as an LC.
    If the LC (Inductance capitance) causes a loss
    of power apart from a resistive component that
    power is assumed to be radiated, IMHO.
    A rose by any other name.
    Well my guess is a solder blob would set-up a
    reflection (is that what you mean by "return loss",
    I'll assume so.)

    Another method may be to put jumpers over the trace,
    two jumpers with approapriate spacing can null the
    impedance and reflection but put in a propagation delay,
    (I'm certain you know the theory of ferrite beads).

    So that would LC store the energy and then reradiate
    it along the trace, does that sound good?
    Off hand I think 1/4 wavelength spacing would work??
    Ken
    PS:I got started on this stuff by installing TV antenna's
    in the late 60's. There was a procedure to splice that
    old flat 300 Ohm lead wire, that required each side of
    the line to be spliced (pig tailed, NOT soldered) a few
    inches apart to reduce ghosting and reflection.
     
  11. Tom Bruhns

    Tom Bruhns Guest

    OK, well, go and simulate the effect of what you're imagining as a
    blob. But note that the width of a microstrip trace has much greater
    effect on its impedance than on its velocity factor. Do you really
    want to keep reflections low??

    If you really want to significantly affect the propagation delay, you
    should probably be milling out dielectric so it's replaced with air,
    and adjusting the trace width (widening it) to maintain constant
    impedance. It honestly doesn't sound very practical to me. I suppose
    if you want to electrically lengthen a trace, you could do it by
    milling out under it, narrowing the trace as well, and replace the
    board dielectric with something with a higher dielectric constant.
    (I'd be laughed out of here if I even hinted at putting something like
    that into production!)

    Let's say you change the net er around a section of microstrip from
    2.5 to 8 (something like alumina...). In the er=2.5 section,
    propagation is at 5.27psec/mm, and in the er=8 section, it's 9.43psec/
    mm. So to adjust over a 200psec range, you need a 48mm length of
    line. Ouch. I just can't imagine doing that with a Dremel tool.
     
  12. Tom Bruhns

    Tom Bruhns Guest

    Hmmmm...well, "us guys" here have always been into things like
    continuous autocalibration that happens in the background while
    measurements are running, and even very significantly improves the
    measurement beyond the calibration effects. ;-)
    I was thinking er=10 alumina, and WAGging that it would give a net
    around er=8. If you're going to all that trouble, you _could_ pile
    alumina over the top of the trace, too, so it's embedded
    microstrip... (Eeeechhhh.) But you're right -- the effective er over
    er=10 alumina is only about 6.5. For plain microstrip over er=2.1
    solid Teflon, ATLC tells me that a 50 ohm line will be about 3.1 times
    as wide as the substrate thickness and have net er=1.79 and 4.46ps/mm,
    and 50 ohms over er=10 alumina will be about .95 as wide as the
    substrate thickness, net er=6.52, and 8.52ps/mm. So to get 20ps
    adjustment and keep the impedance constant, you'd have to considerably
    narrow a 5mm length and completely fill under it with different
    dielectric. There's gotta be a lot easier way... And if you don't
    narrow the trace but leave it the same width that gives 50 ohms over
    er=2.1 substrate, you have a section of 25 ohm line...

    And this doesn't all sound terribly impractical to you??? ;-)

    Cheers,
    Tom
     
  13. Hi Joel.

    Let me agree with you, cuz we're close to splitting
    hairs, with the caveat that reflection can be
    constructive or destructive, such as in an antenna,
    or radar dish.
    Dang, that's a tough one.
    Likewise, I shall now return to my lurking state
    until the next full moon.
    Ken
     
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day

-