Mikal said:
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.
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