# PSPICE: Transmission line / Microstrip components

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

1. ### MikalGuest

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 ThompsonGuest

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. ### RobertGuest

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

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
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

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).

5. ### Jim ThompsonGuest

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

...Jim Thompson

6. ### Malcolm ReevesGuest

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. ### Charlie EdmondsonGuest

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

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. ### Malcolm ReevesGuest

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