IEICE TRANS. FUNDAMENTALS, VOL.E89–A, NO.3 MARCH 2006

764

PAPER

Analysis of Reactance Oscillators Having Multi-Mode Oscillations
Yoshihiro YAMAGAMI†a) , Yoshifumi NISHIO†b) , Members, and Akio USHIDA††c) , Fellow

SUMMARY
We consider oscillators consisting of a reactance circuit
and a negative resistor. They may happen to have multi-mode oscillations
around the anti-resonant frequencies of the reactance circuit. This kindof oscillators can be easily synthesized by setting the resonant and antiresonant frequencies of the reactance circuits. However, it is not easy toanalyze the oscillation phenomena, because they have multiple oscillations
whose oscillations depend on the initial guesses. In this paper, we propose a
Spice-oriented solution algorithm combining the harmonic balance methodwith Newton homotopy method that can find out the multiple solutions on
the homotopy paths. In our analysis, the determining equations from theharmonic balance method are given by modified equivalent circuit models
of “DC,” “Cosine” and “Sine” circuits. The modified circuits can be solved
by a simulator STC (solution curve tracing circuit), where the multiple oscillations are found by the transient analysis of Spice. Thus, we need not
to derive the troublesome circuit equations, nor the mathematical transformations to get the determining equations. It makes the solution algorithms
much simpler.
key words: oscillator, multiple oscillations, harmonic balance method,
Newton homotopy method, SPICE

1.

Introduction

Analysis of oscillator circuits is very important for designing communication circuits such as modulators and mixers.
Generally, oscillators have both zero amplitude unstable solutions and non-zero amplitude stable and/or unstable orbits.
In the analysis, it is very diﬃcult to find out the multiple
oscillations, because the oscillations depend on the initial
guesses in the transient simulation. Furthermore, the transient analysis sometimes becomes very time-consuming especially for high Q oscillators. Nowadays, many kinds ofcoupled oscillators have been proposed [1]–[3], which have
many interesting phenomena such as multiple oscillations,
quasi-periodic oscillations, chaos and so on. Thus, in order to analyze these phenomena, it will be useful to develop
simulators to find out the multiple oscillations.
For circuits having a unique non-zero amplitude oscillation, there are Newton-like shooting algorithms [4]–[7]Manuscript received April 7, 2005.
Manuscript revised August 8, 2005.
Final manuscript received November 30, 2005.
†
The authors are with the Department of Electrical and Electronic Engineering, Faculty of Engineering, University of Tokushima, Tokushima-shi, 770-8506 Japan.
††
The author is with the Department of Mechanical and Electronic Engineering, Faculty of Engineering, Tokushima Bunri University, Sanuki-shi, 769-2193 Japan.
a) E-mail: yamagami@ee.tokushima-u.ac.jpb) E-mail: nishio@ee.tokushima-u.ac.jpc) E-mail: ushida@fe.bunri-u.ac.jp
DOI: 10.1093/ietfec/e89–a.3.764

solving the following relation;
F(v(0), T ) = v(0) − v(T ) = 0,(1)

where v corresponds to the state-variables of the circuit, andT is the period to be determined. Since the algorithms are
based on the Newton-Raphson method, we need to start
the iterations from a suitable initial guess. The convergence is guaranteed only when the initial guess is locatednear the steady-state solution. W. Ma, L.J. Trajkovic and L.
Mayaram [7] have proposed an elegant algorithm combining
a homotopy method with the above shooting method. The
approach has a global convergence property, so that it can besafely applied to find out the solution satisfying (1). However, it is still diﬃcult to choose a suitable initial guesses
converging to the multiple oscillations.
In this paper, we propose an elegant Spice-oriented harmonic balance method for solving multiple oscillations. We
apply it to an oscillator consisting of a reactance circuit coupled with a negative resistor. At first, the circuit is designedby specifying the resonant and the anti-resonant frequencies
of a reactance circuit such as Cauer or Foster circuit. After then, the oscillator is realized by introducing a negative
resistor. We found that the oscillations may happen aroundthe anti-resonant frequencies [8].
Now, we will outline our solution algorithm as follow:
1. For a given reactance oscillator, the waveform of thenegative resistance is assumed as follows;
v(t) = V0 + V1 cos ωt +M[V2k−1 cos kωtk=2+ V2k sin kωt]

(2)

Note that we can set V2 sin ωt = 0 in (2) because of anautonomous system [11], and ω is chosen as an additional variable.
2. The current of negative resistor is given byMi(t) = I0 (V) + [I2k−1 (V) cos kωt +I2k (V) sin kωt] (3)k=1where I0 (V), I1 (V), I2 (V), . . . , I2M (V), are functionsof V = (V0 , V1 , V3 , . . . , V2M )T . Thus, each frequency
component (I2k−1 (V), I2k (V)) is described by the nonlinear voltage-controlled current sources in our harmonic balance method.
For the linear inductances, they are transformed into

c 2006 The Institute of Electronics, Information and Communication Engineers
Copyright YAMAGAMI et al.: ANALYSIS OF REACTANCE OSCILLATORS HAVING MULTI-MODE OSCILLATIONS

765

the linear current-controlled voltage sources, and thelinear capacitances into the linear voltage-controlledcurrent sources. These transformation algorithms using
ABMs (Analog Behavior Models) of Spice are shownin Sect. 3. This modified equivalent circuit corresponds
to the determining equations of the harmonic balancemethod.
3. Introducing the Newton homotopy method, the modified circuit is solved by a transient analysis of Spice. In
Sect. 2, we propose an solution algorithm to find out themultiple oscillations which consists of a curve tracing
algorithm based on the arc-length method [9].
Thus, in our method, we need not derive any troublesome circuit equations, determining equations of the harmonic balance method nor the Jacobian matrices to solve theequations, which makes the solution algorithm much easier.
We will show an interesting illustrative example of a Cauer
oscillator in Sect. 4.
2.

Harmonic Balance Method Combining with Newton
Homotopy Method

In order to show the ideas of our solution algorithm, let us
consider a reactance oscillator having a negative resistor as
shown in Fig. 1. Assume that the circuit equation of reactance oscillator is written byh(v, ẇ, w) = 0, h(., ., .) : R2n+1 → R2n+1 ,(4)where v is the nonlinear resistor’s voltage, and w ∈ R corresponds to the circuit variables of the linear reactance circuit.
Now, let the nonlinear characteristic of the negative resistor
be described in the following form;ni = ĝ(v).

(5)

We assume the voltage waveform of v as given in (2). Applying the harmonic balance method to the circuit equation (4), and eliminating the variables from w, the determining equations for the harmonic components can be describedas follows;f0 (V0 , V1 , V3 , · · · , V2M , ω) = 0 · · · DC





f1 (V0 , V1 , V3 , · · · , V2M , ω) = 0 · · · cos ωt





f2 (V0 , V1 , V3 , · · · , V2M , ω) = 0 · · · sin ωt

, (6)


........................................................





f2M−1 (V0 , V1 , V3 · · · , V2M , ω) = 0 · · · cos Mωt f2M (V0 , V1 , V3 , , · · · , V2M , ω) = 0 · · · sin Mωtwhere the fundamental frequency component “ω” should
be determined as an additional variable, and M denotes thehighest frequency component. Thus, the determining equations are described by a set of algebraic equations, which
consist of (2M + 1)-equations and the same number of variables. However, it is not easy to solve the equations, because
they may have the multiple solutions.
For simplicity, we set the relations (6) as follow;
f(V) = 0, V ∈ R2M+1 , f(.) : R2M+1 → R2M+1 ,where V = [V0 , V1 , V3 , · · · , V2M , ω]T . Applying the Newton
homotopy method [9] to solve (7), we have the following
relation;F(V, ρ) = f(V) + (ρ − 1)f(V0 ) = 0,

where s denotes the arc-length from a starting point. Equation (9) is a set of nonlinear algebraic-diﬀerential equations,and their circuit models can be realized by the use of ABMs
(analog behavior models) of Spice [12]. The circuit diagram
is shown in Fig. 2(a) and (b), where “VCCS” is a voltagecontrolled current source. The current sources fˆi (V, ρ) andI s , Iρ in Fig. 2 are given by†††

Circuit diagram of the Newton homotopy method.

The solution curve satisfies the relation (8).
Spice [10] has many useful analog behavior models, so we caneasily realize the current sources fˆi (V, ρ). In this circuit, V2 = 0 is
realized by setting K = ∞.
††Reactance oscillator.

(8)

where ρ is an additional variable, and V0 is the initial guess.
Then, the homotopy path† starting from (V0 , ρ = 0) satisfies
the relations (6) at ρ = 1. In this way, we can find out
the multiple solutions on the paths, whose curves can beeﬃciently traced by the application of the arc-length method
as follows;
F(V, ρ) = 0








2M+1
2

 dVi 2


dρ

+
=1 
,
(9)


ds
ds



i=1




i2

Fig. 2

Fig. 1(7)

IEICE TRANS. FUNDAMENTALS, VOL.E89–A, NO.3 MARCH 2006766

fˆi (V, ρ) = Fi (V, ρ) − Vi , i = 1, 2, . . . , 2M + 1, 





for V2 = 0








2M+1
2

 dVi 2

dρ
(10)

Is =
, Iρ =
.



ds
ds




i=1




i2
The second term of (10) is realized by STC (Solution Curve
Tracing Circuit) as shown in Fig. 2(b), where RD is a suﬃciently large dummy resistance to avoid the L-J cut set. Furthermore, f1 (V0 ), f2 (V0 ), . . . , f2M+1 (V0 ) in Fig. 2(a) denotethe initial guesses. Thus, we can easily trace the homotopy
path starting from an arbitrarily chosen initial guess (V0 ).
The circuit shown in Fig. 2 is solved by transient analysis of
Spice, and the multiple oscillations are found at ρ = 1 on
the homotopy paths.
3.

Fig. 3

Fourier transfer circuit model.

Equivalent Circuit Models

3.1 Fourier Transfer Circuit Model
Oscillator circuits usually consist of many linear and/or nonlinear reactive and resistive elements. When the harmonicbalance method is applied to the analysis, the determining
equations are described by a set of algebraic equations asshown in Sect. 2. Firstly, we need to expand the responses
of nonlinear elements into the Fourier series. Let us assume
the input and output waveforms as follows;

M




[V2k−1 cos kωt + V2k sin kωt] v(t) = V0 +





k=1
(11)

M






i(t) = I0 +[I2k−1 cos kωt + I2k sin kωt] 
k=1

where M denotes the highest harmonic component to takeaccount in the analysis. The output Fourier coeﬃcients aredescribed as follows;
I0 = g0 (V0 , V1 , · · · , V2M ) 
I1 = g1 (V0 , V1 , · · · , V2M ) 

(12)


...............................

I2M = g2M (V0 , V1 , · · · , V2M )In this case, these coeﬃcients can be given by explicit forms
only if the nonlinear characteristics are described by power
series. For general nonlinear elements, we need to introduce
some other techniques for the Fourier transformation. Whenthe input-output relation is given by
i = g(v),(13)

the Fourier coeﬃcients are calculated by the following formulas;



1 T


g(v)dt
I0 =



T 0


 T

T
.
2
2


I2k−1 =
g(v) cos kωtdt, I2k =g(v) sin kωtdt 



T 0
T 0



k = 1, 2, . . . , M(14)Now, let us apply the trapezoidal integration formula to (14)given as follow;
 bhg(v)dt = (g0 + gn ) + h(g1 + g2 + · · · + gn−1 ),2a(15)
where the step-size of the integration is h = (a − b)/n for “n”
divisions. Then, the truncation error is given by g(2) h2 /12n.
Using this formula, we can realize the equivalent circuit
model satisfying (15) with the ABMs of Spice. To understand the circuit model, we assume that the input is givenby (11) with θ = ωt. Then, the Fourier transfer circuit
model for calculating the Nth higher harmonic component
is shown by Fig. 3. 2K + 1 blocks calculate the Nth components (I2N−1 , I2N ) in (14). On the other hand, the integrationinterval [0, 2π] for θ = ωt is divided by 2K sections using the resistors, so that the kth input voltage of the ABM
blocks is given by kth term in (15) with ωt(= θk = 2πk/2K)
at the kth node, and the values (14) are calculated by the useof ABMs of Spice. Thus, the resultant outputs are givenby {g(V, θk ) cos Nθk , g(V, θk ) sin Nθk , k = 0, 1, 2, . . . , 2K}.
Summing all of them and dividing by 2K, the outputs areequal to the coeﬃcients of cos Nθ and sin Nθ, respectively.
To investigate the numerical accuracy, we first calculate
a modified Bessel function as follows; π1
IN (x) =e x cos θ cos Nθdθ.
(16)
2π −π
The simulation results with h = 2π/20 are shown in Fig. 4.
The value I1 (10) = 2761 for N = 1, x = 10 is exactly equal
to the result from the Table of Bessel function [13]. Remarkthat Fourier expansions for exponential functions are very
important to the analysis of the circuit containing diodes andbipolar transistors [12]. Next, we apply the transfer circuit
to the Fourier expansion of MOSFET, whose characteristic
in Spice model is described by a piecewise continuous functions [12] as follows:
1. Linear region: (VGS > VT , VGS − VT ≥ VDS > 0)

YAMAGAMI et al.: ANALYSIS OF REACTANCE OSCILLATORS HAVING MULTI-MODE OSCILLATIONS

767

Fig. 4

Fourier transformation for modified Bessel function.

Fig. 6Equivalent “Cosine” and “Sine” circuits.

MφL (t) = ΦL,0 +ΦL,2k−1 cos kωt+ΦL,2k sin kωt . (19a)k=1

Diﬀerentiating φL (t), we haveMvL (t) = kω −ΦL,2k−1 sin kωt + ΦL,2k cos kωt . (19b)k=1

Fig. 5 Fourier transformation for MOSFET. VDS = 3 [V], K
3.87 [µA], λ = 0.01605, W = 2 [µm], L = 2 [µ], VT = 0.827 [V].

ID =

KW
VDS
(VGS − VT ) −VDS
L2(1 + λVDS ).

=VL,2k = −kωΦL,2k−1 , VL,2k−1 = kωΦL,2k ,k = 1, 2, . . . , K,
(17a)

2. Saturation region: (VGS > VT , VDS > VGS − VT )ID =KW(VGS − VT )2 (1 + λVDS ).
L

(17b)

The result of Fourier expansion for an input VGS cos ωt isshown in Fig. 5. Thus, the Fourier transfer circuit model
given by Fig. 3 can be eﬃciently applied to any kind of circuit elements contained in analog ICs.
3.2 Fourier Expansion of Linear and Nonlinear Inductors
Let an inductor flux be the current-controlled as follow;
φL (t) = φ̂(iL )Thus, “Sine” and “Cosine” components for the kth higher
harmonic components are respectively given by(18)

If the characteristic is described by a power series, theFourier coeﬃcients will be described in explicit forms. Otherwise, we need to use the Fourier transfer circuit model
given in Fig. 3. Thus, the Fourier expansion is described in
the following form;(20a)

Thus, the inductor is replaced by the coupled currentcontrolled voltage sources as shown in Fig. 6.
For a linear inductor, we havedidt
⇒ VL,2k = −kωLIL,2k−1 , VL,2k−1 = kωLIL,2k (20b)vL = L

3.3 Fourier Expansion of Linear and Nonlinear Capacitors
Let a capacitor charge be the voltage-controlled characteristic as follow;
qC (t) = q̂C (vC )(21)

The Fourier expansion can be carried out with the same
technique as the inductor.
qC (t) = QC,0 +M[QC,2k−1 cos kωt + QC,2k sin kωt],

k=1

Diﬀerentiating qC (t), we have

(22a)

IEICE TRANS. FUNDAMENTALS, VOL.E89–A, NO.3 MARCH 2006

768

iC (t) =Mkω[−QC,2k−1 sin kωt + QC,2k cos kωt],

(22b)

k=1

Thus, “Sine” and “Cosine” components for the kth high harmonic component are respectively given by
IC,2k = −kωQC,2k−1 , IC,2k−1 = kωQC,2k ,k = 1, 2, . . . , K,

(23a)which means V2 = 0. Although the equivalent circuit inFig. 7 is composed of 2M + 2 sub-circuits, one of themcorresponds to the V2 sin ωt = 0 or V2 = 0. Therefore,
the solution of the circuit decides the 2M + 1 variables{ω, V0 , V1 , V3 , . . . , V2M−1 , V2M }. The modified circuit shownin Fig. 7 can be eﬃciently solved by the Newton homotopy
method shown in Sect. 2 and STC (Solution curve Tracing
Circuit).

For a linear capacitor, we havedv
iC = C ⇒ IC,2k = −kωCVC,2k−1 ,dt
IC,2k−1 = kωCVC,2k

4.
(23b)

Thus, each capacitor is replaced by the coupled voltagecontrolled current sources as shown in Fig. 6.

An Illustrative Example

Consider a reactance Cauer oscillator having a negative resistor as shown in Fig. 8, whose nonlinear characteristic isgiven byiG = −C1 vG + C3 vG3 , C1 = 1. C3 = 1.

(26)

3.4 Equivalent Circuit Model of the Determining Equations

Assume the resonant and ant-resonant frequencies as follows;

All the reactance elements in the linear reactance circuit andnonlinear resistors can be replaced by the equivalent circuit
models in the table of Fig. 6. Thus, the reactance oscillator
shown in Fig. 1 is transformed into the “Cosine” and “Sine”
circuits as shown in Fig. 7, where we assume the voltage andcurrent of nonlinear resistor as follows;

Anti-resonant frequencies : ω10 = 1, ω30 = 4, ω50 = 6
Resonant frequencies : ω20 = 2, ω40 = 5v(t) = V0 +M[V2k−1 cos kωt + V2k sin kωt]

(24a)[I2k−1 cos kωt + I2k sin kωt]

(24b)

k=0

i(t) = I0 +

M

k=0

For the analysis of autonomous systems, the time origin canbe arbitrarily chosen satisfying a relation “V2 sin ωt = 0.”
The equivalent circuit model is shown by Fig. 7(a); namely,
V2 − ω = −ω

(25)

(27)
Then, we have the circuit parameters as shown in
Fig. 8, where we have added a small resistor (r = 0.05) toeach inductor.
It is well-known from the experimental results [6],[14], [15] that, when a weakly nonlinear resistor (26) has
a symmetric characteristic to the origin, the resultant waveforms will have only odd number of the higher harmoniccomponents. Thus, we can setvG (t) = V1,1C cos ωt +M
[V2k+1,1C cos(2k + 1)ωt
k=1

+ V2k+1,1S sin(2k + 1)ωt],(28)

where the term V1,1S sin ωt in (28) was deleted because of
the autonomous system.
Now, we will develop “Cosine” and “Sine” circuits to
Fig. 8 which correspond to the determining equations of theharmonic balance method.
In this case, for linear inductors, we have
VL,2k = −kωLIL,2k−1 , VL,2k−1 = kωLIL,2k ,k = 1, 2, . . . , M.

(29)

For linear capacitors, we have

Fig. 7 Equivalent “Cosine” and “Sine” circuit models of the determining
equations. k = 1, 2, 3, . . . , M.

Fig. 8 Cauer oscillator. C1 = 0.1, C2 = 0.343, C3 = 0.439, L1 = 0.417,
L2 = 0.262, L3 = 1.058, r1 = · · · = r3 = 0.01.

YAMAGAMI et al.: ANALYSIS OF REACTANCE OSCILLATORS HAVING MULTI-MODE OSCILLATIONS

769

Fig. 9Equivalent circuit describing the determining equations.

IC,2k = −kωCVC,2k−1 , IC,2k−1 = kωCVC,2k ,k = 1, 2, . . . , M.

(30)

Thus, the inductors and capacitors in the modified “Cosine”
and “Sine” circuits are replaced by the simple coupled linear current-controlled voltage sources, and coupled voltagecontrolled current sources, respectively. Whole the circuit
configuration until the 3rd higher harmonic components isshown in Fig. 9. In order to trace the multiple solutions, italso contains the Newton homotopy sub-circuits denoted by{(ρ − 1) fi (V0 ), i = 1, 2} in the first two sub-circuits. Observethat each of the “Cosine” and “Sine” circuits has the same
topology as the original circuit shown in Fig. 8. It makes
easier to construct the equivalent circuits with the schematic
editor of Spice.
Combining STC (solution curve tracing circuit) shownin Fig. 2(b) with Fig. 9, we can trace the homotopy paths
starting from { fi (V0 ), i = 1, 2}, and the multiple solutions
are found at ρ = 1. We have traced both sides of the paths
by setting the initial conditions ρ̇(0) > 0, and < 0 of STC.
The results are shown in Fig. 10(a) for s < 0 and (b) fors > 0, where the solid line corresponds to ω-curve. Thus,
we have found 6 solutions at ρ = 1 as follows:
Stable solutions : ω1 = 1.0878, ω3 = 3.6770, ω5 = 5.722
Unstable solutions : ω0 = 0, ω2 = 2.0001, ω4 = 4.999
Observe that the amplitudes of oscillations at resonant
frequencies ω = 0, 2, 5 are all the zeros. It means that theFig. 10

Solution curves, (a) s < 0, (b) s > 0.

reactance oscillator does not oscillate at the resonant frequencies of the reactance circuit [8], and the non-zero oscillations will happen around the anti-resonant frequencies.
We found from Fig. 10 that the oscillator has totally 6 solutions, and that those around the anti-resonant frequencies
are stable† Next, we have calculated the steady-state waveforms starting from the initial conditions estimated by theabove harmonic balance methods. The results are shown in
Figs. 11(a), (b) and (c). The frequency spectra with FFT are
shown in Figs. 12(a), (b) and (c), respectively. The waveforms at ω = 1.0556 is largely distorted and contains manyhigher harmonic components.
We have confirmed from the results that, although
the Cauer oscillator happens to oscillate around the antiresonant frequencies of the reactance circuit, their frequen†
Although we can arbitrarily choose the initial guesses, it may
happen to trace all the solutions or some of them depending on theguesses. In this example, when we have traced both directions ofsolution curves of s > 0, s < 0 with ω0 = 6, most of our cases
found all of the solutions on the homotopy paths. It is known thatthe curve tracing algorithm [9] is failed at the point of rank(F(V)) <n for an n + 1 variables. However, it is impossible to know thegeometries of curves in n + 1-dimensional space. Hence, to find all
the solutions, we will recommend to choose many initial guesses
in the space around the expected solutions.

IEICE TRANS. FUNDAMENTALS, VOL.E89–A, NO.3 MARCH 2006

770

Fig. 11 The steady-state waveforms. (a) ω1 = 1.0556, (b) ω3 = 3.619,(c) ω5 = 5.68.

cies are little diﬀerent from the designed frequencies because of the nonlinearity of the resistor.
5.

Conclusions and Remarks

It is a diﬃcult task to analyze oscillators having multi-mode
oscillations, because each of the oscillations depends on thecorresponding initial condition. In this paper, we have proposed a Spice-oriented harmonic balance method, where thedetermining equations can be described by the equivalent“DC,” “Cosine” and “Sine” circuits. The modified circuits
are solved by the Newton homotopy method using Spice.
Thus, in our algorithm, we need not to derive any troublesome circuit equations, determining equations nor the Jaco-

Fig. 12 Frequency spectrum for Fig. 11. (a) ω1 = 1.0556, (b) ω3 =3.6191, (c) ω5 = 5.68.

bian matrices. As an example, we considered a Cauer oscillator having multi-mode oscillations which is composedof a reactance Cauer circuit and a negative resistor. We
found from the results that the oscillations happen to appear
around the ant-resonant frequencies of the reactance circuit.
The solution algorithm shown in this paper will be applied
to any kind of reactance oscillators.
The Cauer oscillators sometimes happen quasiperiodic oscillations depending on the circuit parameters.
We will also apply our algorithm to electronic circuits suchas Hartley and Colpitis oscillators. These are the future
problems.

YAMAGAMI et al.: ANALYSIS OF REACTANCE OSCILLATORS HAVING MULTI-MODE OSCILLATIONS

771

References[1] T. Endo and S. Mori, “Mode analysis of a multimode ladder oscillators,” IEEE Trans. Circuits Syst., vol.CAS-23, no.2, pp.100–113,
1976.
[2] S. Moro, Y. Nishio, and S. Mori, “On coupled oscillators networks
for cellular neural networks,” IEICE Trans. Fundamentals, vol.E80A, no.2, pp.214–222, Feb. 1997.
[3] Y. Nishio and A. Ushida, “Multimode chaos in two coupled chaotic
oscillators with hard nonlinearities,” IEICE Trans. Fundamentals,
vol.E79-A, no.2, pp.227–232, Feb. 1996.
[4] K. Kundert, J. White, and A. Sangiovanni-Vincentelli, Steady-State
Methods for Simulating Analog and Microwave Circuits, Kluwer
Academic Publishers, Boston, 1990.
[5] T.J. Aprille, Jr. and T.N. Trick, “A computer algorithm to determine
the steady-state response of nonlinear oscillators,” IEEE Trans. Circuit Theory, vol.CT-19, no.4, pp.354–360, 1972.
[6] K. Matsuo, T. Matsuda, Y. Nishio, Y. Yamagami, and A. Ushida,“Steady-state analysis of reactance oscillators having multiple oscillations,” Proc. ITC-CSCC 2000, vol.1, pp.203–206, 2000.
[7] W. Ma, L.J. Trajkovic, and K. Mayaram, “HOMSPICE: A
homotopy-based circuit simulator for periodic steady-state analysis
on oscillators,” IEEE ISCAS 2002, vol.1, pp.645–648, Phenix, Arizona, 2002.
[8] R.K. Brayton and K. Moser, “A theory of nonlinear networks,” I and
II, Q. Appl. Math., vol.22, pp.1–33 and pp.81–104, 1964.
[9] A. Ushida, Y. Yamagami, Y. Nishio, I. Kinouchi, and Y. Inoue, “Aneﬃcient algorithm for finding multiple DC solutions based on the
SPICE-oriented Newton homotopy method,” IEEE Trans. Comput.Aided Des. Integr. Circuits Syst., vol.21, no.3, pp.337–348, 2002.
[10] MicroSim, PSpice A/D Circuit Analysis User Guide, MicroSim Co.,
1995.
[11] A.H. Nayfeh and D.T. Mook, Nonlinear Oscillations, John Wiley &Sons, 1979.
[12] A. Ushida and M. Tanaka, Electronic Circuit’s Simulations, Korona
Pub., 2002.
[13] K.K. Clarke and D.T. Hess, Communication Circuits: Analysis andDesign, Addison-Wesley, 1971.
[14] E. Ikeno and A. Ushida, “The arc-length method for computationof characteristic curves,” IEEE Trans. Circuits Syst., vol.23, no.3,
pp.181–183, 1976.
[15] Y. Ueda, Some Problems on the Theory of Nonlinear Oscillations,
Nippon Printing, 1969.

Yoshihiro Yamagami
graduated from the
Department of Electrical Engineering, Anan
Technical College, Tokushima, Japan, in 1982.
He joined the Department of Electrical andElectronic Engineering of Tokushima University, Tokushima, Japan, in 1984. His researchinterests include computer-aided simulations of
nonlinear circuits and high-speed interconnect
circuits.

Yoshifumi Nishio
received B.E., M.E.,
and Ph.D. degrees in electrical engineering from
Keio University, Yokohama Japan, in 1988,
1990, and 1993, respectively. In 1993, he joined
the Department of Electrical and Electronic Engineering at Tokushima University, Tokushima
Japan, where he is currently an Associate Professor. From May 2000 he spent a year in the
Laboratory of Nonlinear Systems (LANOS) at
the Swiss Federal Institute of Technology Lausanne (EPFL) as a Visiting Professor. His research interests include analysis and application of chaos in electrical circuits, analysis of synchronization in coupled oscillators circuits, development of analyzing methods for nonlinear circuits and theory and applicationof cellular neural networks. He was the Chair of the IEEE CAS TechnicalCommittee on Nonlinear Circuits and Systems (NCAS) during 2004–2005
and is currently the Secretary of the IEICE Research Society of Nonlinear
Theory and its Applications (NOLTA). He is serving as an Associate Editor
for the IEEE Transactions on Circuits and Systems - Part I, for the area ofTheory and Systems. He is a member of the IEEE and the RISP.

Akio Ushidareceived the B.E. and M.E. degrees in Electrical Engineering from Tokushima
University in 1961 and 1966, respectively, andthe Dr. degree in Electrical Engineering from
University of Osaka Prefecture in 1974. He
was an Associate Professor from 1973 to 1980
at Tokushima University. From 1980 to 2003,
he was a Professor in the Department of Electrical and Electronic Engineering at Tokushima
University. Since 2003, he has been with the
Department of Mechanical-Electronic Engineering, Tokushima Bunri University. From 1974 to 1975, he spent one year
as a visiting scholar at the Department of Electrical Engineering and Computer Sciences at the University, Berkeley. His current research interests
include numerical methods and computer-aided analysis of nonlinear circuits. Dr. Ushida is a member of the IEEE.