Connect with us

PSPICE: Transmission line / Microstrip components

Discussion in 'CAD' started by Mikal, Jun 1, 2005.

Scroll to continue with content
  1. Mikal

    Mikal Guest

    Is it possible to simulate microstrip components in pspice? i.e.
    quarter wavelenght stubs as bandpass filters... Open ended stub would
    be a series resonant short, grounded end would be a parallel resonant
    open.
     
  2. Jim Thompson

    Jim Thompson Guest

    Yes, but RTFM. I have a stripline part placed in my personal library
    by a Garmin engineer, back when I was doing GPS chip designs, but I
    don't know how it works.

    ...Jim Thompson
     
  3. Robert

    Robert Guest

    I have a vague memory of them being a problem in TRAN simulations. Something
    about the required (small) step size causing very slow simulations. But that
    might have been just for Pulse waveforms.

    Robert
     
  4. Joel Kolstad

    Joel Kolstad Guest

    If you're using it as a "one port" device (i.e., the other end is terminated
    in a known impedance, including an open or a short), sure -- just compute the
    input impedance of the line as a function of s (that is, j*omega). The
    closed-form expression for a terminated transmission line is slightly messy
    (it's in any book covering transmission lines -- download
    http://oregonstate.edu/~kolstadj/Transmission Lines (Chipman).pdf if you don't
    already have such a book), but most simulators today will accept generic
    "Laplace blocks" where you stick in the function you're after. For the
    special case of short- and open-circuited lines, the general expression just
    turns into a tangent or cotagent function -- simple enough.

    If you won't be having to sweep over a wide range of frequency, figure out the
    input impedance at a nominal figure and equate that to an equivalent R, L
    and/or C -- it'll be an OK narrowband approximation. In the case of 1/4 wave
    stubs for bandpass filters, synthesis sizes the lines such that they're
    equivalent to a given inductor or capacitor anyway; the results end up being
    slightly (but not significantly) difference than keeping the L and C's fixed
    components.

    Simulating lossless transmission lines in SPICE is easy, because for transient
    analysis they're just a time delay whereas for AC analysis they're just a
    phase delay (proportional to frequency). Simulating lossy transmission lines
    is not at all easy, and you can find many papers that advocate different
    approaches. Most of the fancier simulators have lossy transmission line
    models built in, and it's best to use those unless you have a LOT of time on
    your hands.

    There are several free programs out there such as Elsie and the AADE Filter
    Designer that will simulate ladder networks consisting of lumped elements and
    transmission lines for you, if you goal here is just to perform simulations
    and you're not sold on SPICE. I believe they use ABCD networks to perform the
    analysis -- programmatically, this is about the simplest way to implement it
    (something like designing and analyzing a bandpass filter built from
    microstrip lines using your own Matlab, MathCAD, etc. routines is a very
    common homework problem in university classes).

    ---Joel Kolstad
     
  5. Jim Thompson

    Jim Thompson Guest

    That's true for IDEAL lines. I'm pretty sure that there is a
    dissipative model in there as well.

    ...Jim Thompson
     
  6. Pspice has lossy and lossless transmission lines.

    BTW, a one time there was a bug, not sure if it has been fixed.
    Basically if you set up a lossy transmission line circuit, ac
    analysis, sweep length and plot signal at some F vs length, then you
    see a discontinuity, a sudden change in slope. Reltol needs to be set
    much smaller (/100?) which then fixes this. Plot is then smooth as
    would be expected. Reltol doesn't affect ac compute time AFAIR.

    --

    Malcolm

    Malcolm Reeves BSc CEng MIEE MIRSE, Full Circuit Ltd, Chippenham, UK
    (, or ).
    Design Service for Analogue/Digital H/W & S/W Railway Signalling and Power
    electronics. More details plus freeware, Win95/98 DUN and Pspice tips, see:

    http://www.fullcircuit.com or http://www.fullcircuit.co.uk

    NEW - www.CharteredConsultant.co.uk - The Consultant A-List
     
  7. The basic problem was how to not miss transitions when you have
    transmission lines, one of the solutions was to reduce the max step size
    to one half of the shortest tline delay. If you had really small
    tlines, then this could really increase the simulation time...

    Charlie
     
  8. Joel Kolstad

    Joel Kolstad Guest

    The reason there are numerous lossy transmission line models out there is that
    some of the early ones had problems in that they were non-passive. In such
    cases, if you choose the right terminations (just R's, L's, and C's) you can
    create a non-stable system and get oscillations out of "nowhere." Later ones
    would include passivity at the expense of accuracy and presumably these days
    there are very good models available that are both stable and passive... but
    I'm not at all up to date on the models used in any particular simulator.

    I would be wary of anyone's simulator that doesn't tell you whose lossy
    transmission line model they're using!

    ---Joel
     
  9. AFAIR it is in one of the manuals - all greek to me though :). AFAIR
    each end of the lossy transmission line is a volt and current source
    pair. These model the line impedance, voltage, current, black box
    style. Maths links the two ends. This does mean that the two ends
    are floating so you need to 0V reference each end which of course is
    different to a real circuit.

    P.S. Sorry for emailing you Joel - I clicked the wrong button - DOH!

    --

    Malcolm

    Malcolm Reeves BSc CEng MIEE MIRSE, Full Circuit Ltd, Chippenham, UK
    (, or ).
    Design Service for Analogue/Digital H/W & S/W Railway Signalling and Power
    electronics. More details plus freeware, Win95/98 DUN and Pspice tips, see:

    http://www.fullcircuit.com or http://www.fullcircuit.co.uk

    NEW - www.CharteredConsultant.co.uk - The Consultant A-List
     
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

-