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

Ray Anderson (raymonda@radium.eng.sun.com)
Thu, 2 Sep 1999 11:42:38 -0700 (PDT)

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 majordomo@silab.eng.sun.com. 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 ****