[SI-LIST] Re: (no subject)
- From: "Raj Raghuram" <raghu@xxxxxxxxxxx>
- To: <si-list@xxxxxxxxxxxxx>
- Date: Tue, 10 Dec 2002 15:20:06 -0800
Mick, Ege, Hassan, and others,
As mentioned, there are primarily two approaches to do SPICE type transient
simulations for components described in S-parameters.
(1) Convert S-parameters to certain forms, either equivalent circuit
representations or certain table lookup format, from which SPICE engines can
read and run.
(2) Enable a SPICE solver to read S parameters directly. The SPICE solver
will then internally do the things in (1), or do convolution directly which
can be quite demanding for computer resources for large number of such
circuit components.
While it may appear more attractive to have the time domain circuit
simulator directly read in and use the S-parameters, deficiencies in the
representation used are not then easily seen. Often the original
S-parameters or the circuit model representing them may not be stable,
causal, and passive. Also, extrapolation of the S-parameter data to DC is
often a problem and separate DC values may be needed.
It is technically very challenging to have accurate and reliable transient
simulations from S-parameters of complicated responses. There are quite a
number of tools out there. A tool that is claimed to have such a
capability, either through (1) or (2), does not necessarily mean it can do a
good job.
One of the major issues, in time domain simulations by a SPICE circuit
solver, is whether the circuit really behaves in the way it should behave,
as characterized by its original S parameters.
Here is a way to check whether the tool really does the job it is supposed
to do. Assume you have a two-port circuit described by S parameters.
You have a SPICE equivalent circuit of the two-port network or your solver
can directly read-in S parameters. Connect port one with a time-varying
voltage source Vs(t) and a 50 ohm resistor, connect port 2 with a 50
resistor as shown in the following graph. Run the SPICE engine to get the
transient voltages V1(t), V2(t) and Vs(t).
50 ohms --------------
|-------| | |
|-----| |------o| |------|
| |-------| + | | + |
--- | | ---
Vs(t)|+| V1(t) | |V2(t)| | 50 ohms
|-| | | | |
--- - | | - ---
|--------------------o| |------|
----- | |
--- --------------
-
Take Fourier transforms of Vs, V1 and V2; then the S parameters of the
two-port circuit can be extracted as follows:
S11 = (V1(f)-Vs(f)/2)/(Vs(f)/2)
S21 = V2(f)/(Vs(f)/2)
One can find S22 and S12 in a similar way by moving Vs to port 2.
The S parameters extracted from the above procedure represent the actual
S-parameters of the two-port circuit in transient simulations; the amount of
their deviation from the original S-parameters reflects how accurate the job
is done.
The above tests are fairly easy to do with any SPICE solvers. I have some
netlist templates available and I would be happy to provide you if you are
interested.
Best Regards,
Raj Raghuram
Sigrity, Inc.
"Achieve what others can't"
raghu@xxxxxxxxxxx
http://www.sigrity.com
4675 Stevens Creek Blvd. , Ste 130
Santa Clara, CA-95051
PH: 408-260-9344 x116
CELL: 408-390-7614
FAX: 408-260-9342
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
