[SI-LIST] Re: how to simulate with S parameters
- From: "Dohn V. Salvador" <dohns@xxxxxxxxxxxxxxx>
- To: hassan@xxxxxxxx, Giovanni.Guasti@xxxxxxxxxx
- Date: Mon, 03 Mar 2003 10:21:18 -0800
Hello,
It's true that some SPICE simulators can read Laplace models or even S
parameters ( - the current HSPICE only supports S parameters in AC, but not
transient simulation). You can even convert S parameters into Laplace
models as outlined in your email. But, the simulators are only as good as
your input data.
The frequency-table format of HSPICE Laplace models rarely worked
properly
in the transient (and even AC) simulation. The analytic format of HSPICE
Laplace models is better, but many algorithms are needed to ensure that the
equations are stable, and satisfy the passivity and DC conditions.
As for those simulators that read S parameters directly - the simulation
can either diverge or give wrong results if the input S-parameter data
violate passivity (due to the measurement or EM solver's errors, for
example).
Optimal Corp.'s WideBand Spice addresses the above two issues by
generating
passivity-corrected Laplace models or S-parameter Touchstone files for all
simulators (that either read or not read S parameters directly).
Best regards,
Dohn V. Salvador
dohns@xxxxxxxxxxxxxxx
www.optimalcorp.com
Tel. No. 408-363-6300 x122
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of Hassan O. Ali
Sent: Sunday, March 02, 2003 9:50 AM
To: Giovanni.Guasti@xxxxxxxxxx
Cc: 'si-list@xxxxxxxxxxxxx'
Subject: [SI-LIST] Re: how to simulate with S parameters
I asked this question before and I received a lot of good info. The info
even cleared some of the things I was clueless about. Here are a few
tips pertaining to HSPICE:
1. You can use the S element (N-port linear element) in HSPICE 2002.2.
Read more about the S element from page 6-66 of the "True-Hspice Device
Models Reference Manual, Release 2002.2".
The general syntax is:
Sxxx n_1 n_2 n_3 ... n_N <n_ref> mname=Smodel_name
n_1 ... n_N are N signal nodes
n_ref is the reference node
mname is the name of the .MODEL statement of type S.
The S model syntax is as follows:
.MODEL S_model_name S
+ [FQMODEL=sp_model_name | TSTONEFILE=file | CITIFILE=filename]
+ <TYPE =[S|Y|Z]> <FBASE=base_frequency> <FMAX=maximum_frequency>
+ <Zo=[50 | vector_value] | Zof=ref_model>
You have to RTFM to understand the parameters above.
For example, if you have your 2-port S-parameter model in a file
"cable.s2p" in Touchstone format with 50ohm reference, the S element and
.MODEL statements can be as follows:
S1 n1 n2 0 mname=cable
.MODEL cable S TSTONEFILE=cable.s2p
That's it!
I think it's better to use HSPICE's SP file format (it has more control
parameters). For better transient accuracy, you have to supply enough
S-parameter data to cover the frequency bandwidth (BW) of interest
(starting from DC). A general rule of thumb for NRZ signal, BW =
0.35/tr, where tr is the rise time. The higher the BW the more accurate
the transient simulation would be.
It's better to make the number of frequency points a power of 2 e.g.
256, 512, 1024, etc, to simplify HSPICE's inverse Fourier
transformation. If you need a time resolution, dT, in your transient
simulation, then the n'th frequency point, f_n, would be determined by
the formula:
f_n = n/(N.dT) , n=0, 1, 2, ..., N-1
where N is the number of frequency points such that N.dF is
approximately equal to the BW, and dF is the frequency interval in your
S-parameter data file. I use the above formulas to determine a frequency
step and highest frequency to set in a field solver such as HFSS.
The time resolution, dT, for example, can be determined by the number of
time points per risetime. A risetime of 100ps resolved in 5 time points
would make dT=20ps.
Field solvers and network analyzers won't give you S-parameter values at
DC but you can use any curve-fitting tool (e.g. Excel) to extrapolate
S-parameter curves to DC (0 frequency) and add the data in the
S-parameter file. In Excel, I plot the first 10 to 30 points (too many
points would confuse curve-fitting) and add a 6th order polynomial
trendline. In Trendline Options I extrapolate the trendline Backward to
0 frequency and I choose to display the equation on the chart and read
the DC value as the constant in the displayed equation.
2. You can also use the G element which I think is supported by all
SPICE's (certainly supported by HSPICE). Here is what Thomas Beneken
<beneken@xxxxxxxxxxxx> mentioned about it:
====================
If you obtained the S-parameters of a device, e.g. from VNA
measurements,
You can build up a SPICE subcircuit that represents the (linear) device
in
simulations.
S-parameters describe waves in 50 Ohm systems, but you need voltages and
currents for SPICE. So first to do is to convert S-parameters into
y-parameters:
y11=((1-s11)*(1+s22)+s12*s21)/d
y12=-2*s12/d
y21=-2*s21/d
y22=((1+s11)*(1-s22)+s12*s21)/d
d=((1+s11)*(1+s22)-s12*s21)*Z0
Z0=50 Ohms
Next step is to build up the SPICE subcircuit following this template:
.SUBCKT MyDevice IN OUT GND
RIN IN GND 1E20
ROUT OUT GND 1E20
G11 IN GND FREQ {V(IN,GND)}=
+(<f>,<y11dB>,<y11deg>) ... this line repeated for all frequencies
G12 IN GND FREQ {V(IN,GND)}=
+(<f>,<y12dB>,<y12deg>) ... this line repeated for all frequencies
G21 IN GND FREQ {V(IN,GND)}=
+(<f>,<y21dB>,<y21deg>) ... this line repeated for all frequencies
G22 IN GND FREQ {V(IN,GND)}=
+(<f>,<y11dB>,<y22deg>) ... this line repeated for all frequencies
.ENDS
If You are lucky You have the y-parameters analytically expressed in s
(=
j*2*PI*f). For instance this subcircuit describes a directional
transmission
line matched to 50 Ohms with a delay of 100 picoseconds:
SUBCKT MyDelayline IN OUT GND
RIN IN GND 1E20
ROUT OUT GND 1E20
G11 IN GND LAPLACE {V(IN,GND)}={1/50}
G12 IN GND LAPLACE {V(OUT,GND)}={0}
G21 OUT GND LAPLACE {V(IN,GND)}={-2*exp(-s*1E-10)/50}
G22 OUT GND LAPLACE {V(OUT,GND)}={1/50}
.ENDS
Hope it helps,
Thomas
=================================
Hope that helps.
Regards.
Hassan.
Guasti Giovanni wrote:
>
> Hi All,
> I would like to make some transient and ac simulation of a lossy cable,
> modeled with frequency Scatter parameters.
> Does anybody know the right way to do it? Does Hspice permit it? Could you
> indicate some interesting lectures to me?
> Thanks in advance.
>
> Regards,
>
>
>
> Giovanni Guasti
> giovanni.guasti@xxxxxxxxxx <mailto:giovanni.guasti@xxxxxxxxxx>
>
--
Hassan O. Ali Email: hassan@xxxxxxxx
12-2159 Elmira Drive Tel/Fax: (613) 721-9047
Ottawa, Ontario
CANADA K2C 1H3 WWW: http://www.glcom.com/hassan
------------------------------------------------------------------
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:
