Generation of rational model based SPICE circuits for transient simulations
Nobby Stevens
*
and Tom Dhaene
**
*
Agilent Technologies Belgium, EEsof EDA, Kortrijksesteenweg 1093b, 9051 Gent, Belgium
**
Ghent University – IBBT, Gaston Crommenlaan 8 bus 201, 9050 Gent, Belgium
nobby_stevens@agilent.com
Tom.Dhaene@UGent.be
Abstract
In this paper, we present an efficient and compact circuit
netlist formulation for rational models. It is shown how to
implement the method for several commercially available time
domain solvers. Finally, an example is given describing the
flow and procedures to follow in order to obtain a reliable and
stable transient simulation.
Introduction
Designing a circuit with analog, digital and/or active
components requires a rigorous analysis in the time domain.
Especially with regard to signal integrity issues such as cross-
talk and signal degradation, it is crucial to have a good
quantitative knowledge of these effects during the design
phase. As of today, a number of SPICE simulators are
commonly used for transient simulations. Note however that
most electromagnetic simulators and measurement tools
perform in the frequency domain.
The conversion from frequency domain to time domain is,
from a numerical perspective, a delicate procedure. Here,
rational macromodeling comes into play. Once a passive
mathematical rational model of the frequency data is
constructed, a last and important step to take is the realization
of a compact SPICE-like circuit using lumped components,
that can be efficiently processed by a time-domain circuit
simulator (such as e.g., Hspice and Spectre).
Equivalent SPICE realization
Consider the scattering matrix S of a Linear Time-Invariant
system (LTI), with b and a respectively the column vectors of
the reflected and incident waves:
a S b = (1)
Suppose that for this system, a broadband passive rational
model has been constructed by use of the Vector Fitting
technique [1-3] or the direct interpolation scheme [4]. For
each element S
kl
of the scattering matrix, one can write:
∑
=
−
+ =
kl
M
1 m
kl
m
kl
m
kl kl
p s
c
d S (2)
where, the
kl
m
c are the residues and
kl
m
p are the
corresponding poles. They both are real, or occur in complex
conjugate pairs. Note that the order
kl
M may depend on the
dynamic behavior of each individual element. Also a set of
common poles can be used, or each element can have its own
set.
We obtain the following relationship between the reflected
and incident wave of an N-port system:
∑ ∑
= =
−
+ =
N
1 n
n
M
1 m
kn
m
kn
m
kn k
a
p s
c
d b
kn
(3)
Realization of vi/ab transformation
SPICE circuit simulators work with port voltages and
currents. The relationship between the reflected wave b
k
and
incident wave a
k
and the corresponding port voltage v
k
and
port current i
k
is given by (Z
0
is the reference impedance):
0
k 0 k
k
Z 2
i Z v
a
+
=
(4)
0
k 0 k
k
Z 2
i Z v
b
−
=
(5)
Using these relations, we can see the incident wave as a
(scaled) virtual voltage and the reflected wave as a scaled
virtual current:
k 0 k 0 k
b Z 2 i Z v + = (6)
k
0
0
k
k
i
2
Z
Z 2
v
a + = (7)
From a network point of view, this can be represented as in
Figure 1. (CCVS stands for current controlled voltage source
and VCVS for voltage controlled voltage source.) This way,
no negative resistors are introduced as in the work by
Lamecki [5] and Neumayer [6]. Some SPICE simulators may
have difficulties with negative resistor values.
Realization of rational transfer function
At this point, equation (3), which describes the relation
between incident and reflected waves, must be reformulated as
a circuit equivalent network. The form of the rational
representation (2) is particularly interesting for transient
simulations since the inverse Laplace transform of each term is
known. Recent versions of commercially available SPICE-like
circuit simulators make use of this fact and actually support
the rational presentation as defined in equation (2).
978-1-4244-2318-7/08/$25.00 ©2008 IEEE SPI 2008