[SI-LIST] Re: (no subject)
- From: Matthew Herndon <mherndon@xxxxxxxxx>
- To: "'si-list@xxxxxxxxxxxxx'" <si-list@xxxxxxxxxxxxx>
- Date: Fri, 10 Jan 2003 14:25:47 -0800
Hi, everyone -
I really enjoyed the recent thread with subject "(no subject)" (it was
about using s-parameters in SPICE-like simulators and about dispersion
and loss). So I wrote a summary for my own notes. It occurred to me
that others on the list might find the summary useful, so I've included
a shortened version of it below. If anyone wants the full version,
contact me offline. If more than, say, 10 people request it, I'll post
it to the list.
Thanks to everyone who participated in this very interesting and
informative discussion!
Happy reading!
-matt
Matthew K Herndon, PhD
ECAD Group
Apple Computer, Inc.
Cupertino, CA.
The original question was submitted by Mick Zhou of Agere on Dec 6,2002
[1]:
Has "anybody successfully generate broadband (DC-20GHz) SPICE model
from S matrix for complex structures using the SPICE generator in
ADS?"
Responses indicated that the following additional simulators have this
capability; there was various discussion of accuracy, speed, ease of
use, bugs, etc:
Fullwave SPICE (Ansoft)
IConnect (TDA Systems)
Nspice (Apache)
Broadband Spice (Sigrity)
At this point, we split into two sub-threads: generating SPICE models
without frequency-dependent lookup tables, and the relationship between
dispersion and loss.
Spice models without frequency-dependent sources:
=================================================
In theory, one can create such models. In practice, one needs to
overcome a few difficulties, especially for broadband simulation and for
long lines: it is hard to model dispersion accurately [6].
There are two approaches to simulating S-parameters in SPICE-like
simulators (the following quotes and summarizes [26]):
(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. 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.
The equivalent circuit (using lumped elements, usually RLC)
approach does work well in some situations; and converges for the same
reason that the Fourier transform converges [8] (Note: I would like to
know more about this analogy). We don't have to know anything about
the dielectric properties other than what is implicitly contained in the
measurements. The only assumption is a linear, time-invariant system
It takes a lot of lumped elements to (perfectly) match the measured
s-parameters. One calculation came up with 400K elements. So "curve
fitting" approximations are used. Questions then arise about how many
elements are needed. Apparently, 40 is a "typcial" number in some
cases. Clearly it
depends on the complexity of the shape of the S-parameters curve. And if
you happen to drive the circuit at frequencies where the curve-fit is
poor, you can get erroneous results (imagine a single sinusoid at a
point where the curves are far apart).
Dispersion and loss
===================
Dispersion means that the velocity of spectral components of a signal
depend on frequency, effectively scattering or "dispersing" the arrival
times of the signal wavefront. This effect is not the same as loss,
either skin effect or dielectric loss. Dispersion happens when Er varies
with frequency (so therefore velocity varies with frequency), as in a
prism.
However, if dispersion is caused by the dielectric material (the most
common situation in SI), there must also be loss; the Kramers-Kronig
relationship (aka causality) states that the real and imaginary parts of
the dielectric constant are related to each other [15]. So in this
sense, you can say that if a MEDIUM is "dispersive" it must also be
"lossy".
[40] FR4 is non-linear (?), non-uniform and has significant changes in
Er across frequency (e.g., 4.2 to 4.0 over the range 0.5 to 5 GHz). Real
air exhibits some change in Er with frequency due to humidity; pure
(dry?) air does have a flat response and extremely low losses. Likewise
some other materials, e.g., Rogers and some PTFE (teflon) and ceramic
materials.
Dispersion will (always?) occur if the medium non-homogeneous, e.g.,
microstrip.
SI-list postings quoted directly:
[6] From: Yu Liu <yu_liu@xxxxxxxxxxxxx>
Date: Fri Dec 6, 2002 9:31:32 PM US/Pacific
[8] From: Steve Corey <steven.corey@xxxxxxxxxxxxxx>
Date: Mon Dec 9, 2002 11:05:10 AM US/Pacific
[15] From: Steve Corey <steven.corey@xxxxxxxxxxxxxx>
Date: Mon Dec 9, 2002 4:44:28 PM US/Pacific
[26] From: Raj Raghuram <raghu@xxxxxxxxxxx>
Date: Tue Dec 10, 2002 3:20:06 PM US/Pacific
[40] From: Scott McMorrow <scott@xxxxxxxxxxxxx>
Date: Wed Dec 11, 2002 10:45:28 AM US/Pacific
On Friday, December 6, 2002, at 11:42 AM, Zhou, Xingling (Mick) wrote:
>
> Hello,
>
> Did anybody successfully generate broadband (DC-20GHz) SPICE model
> from S
> matrix for complex structures using the SPICE generator in ADS ? Or any
> other alternatives. I know Ansoft fullwave SPICE does the work.
> Unfortunately, some circuit simulators do not support the frequency
> dependent lookup table sources. We can definitely use [S] directly,
> but some
> users still prefer SPICE models. Any experience to share ?
>
> Thanks,
>
> Xingling(Mick) Zhou, PhD
> Signal Integrity Technologist
> Agere Systems
>
> Tel: 610-712-7462
> Fax: 610-712-4081
>
> ------------------------------------------------------------------
> 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
>
>
------------------------------------------------------------------
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:
