# Re: [SI-LIST] : About the AC analysis with HSPICE

Dmitri Kuznetsov ([email protected])
Fri, 03 Sep 1999 10:49:41 -0700

Ray,

Here is a scheme to extract S parameters in a circuit simulator without
using .net.

___________
-----------| |---------------
Port 1 | A Circuit | Port 2
| |
-----------|___________|---------------

1. Run ac analysis of the following:

Rref ______________
------/\/\/\-------| |------------
| + | | + |
| V1 | The Circuit | V2 <
(Vin) | | > Rref
| - | | - <
-------------------|______________|-----------|

where Rref is the reference impedance (typically 50 Ohm).

2. Then:

S11 = (2 V1 - Vin) / Vin,
S12 = S21 = 2 V2 / Vin.

3. Repeat step 1 with Vin placed at port 2.

4. S22 = (2 V2 - Vin) / Vin.

You can use algebraics or controlled sources to do the math. This
technique is readily derived directly from the S-parameter definition
below.

a c
--> ___________ -->
XXXXXXX-----------| |---------------XXXXXXX
<-- |The Circuit| <--
b | | d
------------------|___________|----------------------

S11 = b/a for d = 0,
S12 = b/d for a = 0,
S21 = c/a for d = 0,
S22 = c/d for a = 0,

where a, b, c, and d are incident and reflected waves in the reference
system.

Due to the reciprocity property of linear networks, S12 = S21 (but only
if the same reference impedance is used for both ports). S11 = S22 if
the circuit is symmetric with respect to the test ports (e.g., a uniform
transmission line). S-parameters and other ac responses of transmission
lines are always oscillating because a transmission line with mismatched
terminations forms a comb filter. These oscillations are often mistaken
for a simulation problem.

Regards,
Dmitri Kuznetsov

=======================================================
Dmitri Kuznetsov, Ph.D.
Principal Engineer

ViewLogic Systems, Inc. e-mail: [email protected]
1369 Del Norte Rd. Tel: (805)278-6824
Camarillo, CA 93010 Fax: (805)988-8259
=======================================================

Ray Anderson wrote:
>
> Following up on my earlier post of a few minutes ago, I found the
> spice deck I mentioned (as well as a reference)
>
> The original work was published in the article:
>
> "S-Parameter Output from SPICE Program" (Goyal, R., IEEE Circuits and
> Devices, March 1988, pp.28,29)
>
> It was also published at a later date in one of the popular
> trade mags (which I still don't remember).
>
> Here is a simple spice deck which implements the method.
> Caveat Emptor, your mileage may vary and the rest of the usual disclaimers....
>
> -Ray
>
> S-parameter Measurement
>
> * derived from R. Goyals article"
> * "S-Parameter Output from Spice Program"
> * IEEE Circuits and Devices March 1988, pp. 28-29
>
> * Connect driving signal to node: input
> * Connect DUT to node: in
> * Measure S11 at node: S11
>
> vdrive input 0 ac 2
>
> * Measure S11
> Gin in 0 input 0 -0.02
> Rin in 0 50
> Eovr mix 0 in 0 0.4
> Edel mix s11 input 0 0.2
> Rmes s11 0 1
>
> * Device Under Test
> Rdut in 0 50
> Cdut in 0 20pF
>
> .option post
> .probe s11
> .ac lin 100 1MEG 1000MEG
> .end
>
> **** To unsubscribe from si-list: send e-mail to [email protected] In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****

**** To unsubscribe from si-list: send e-mail to [email protected] In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****