A New Spice-Oriented Frequency-Domain
Optimization Technique
Masayoshi ODA † , Yoshihiro YAMAGAMI † , Yoshifumi NISHIO † , Junji KAWATA ‡ and Akio USHIDA ‡†Dept. of Electrical and Electronic Engineering, Tokushima University, 770-8506, Japan
E-mail:{masayoshi,yamagami,nishio}@ee.tokushima-u.ac.jp‡Dept. of Mechanical and Electrical Electronic Engineering, Tokushima Bunri University, 769-2193, Japan
E-mail:{kawata,ushida}@fe.bunri-u.ac.jp

Abstract— There are many kinds of optimization techniques
for designing high-performance RF circuits. In this paper, we
propose a new frequency-domain Spice-oriented optimization
algorithm using the steepest descent method. We have developed
a simulator executing the frequency-domain analysis based on
the harmonic balance (HB) method, where all the nonlinear
devices such bipolar transistors and MOSFETs are replacedby the equivalent HB modules. The objective functions in theoptimization are estimated by the DC analysis of the modified
HB circuits.
On the other hand, our steepest descent algorithm is realizedby equivalent circuit model. Thus, the optimum solution is stably
found by the transient analysis of Spice. We show the formulationof HB circuits in section II, the Spice-oriented optimization
algorithm in section III and the interesting examples in section
IV.

I. I NTRODUCTION
There have been proposed many kinds of optimization
algorithms for designing analog integrated circuits [1-5]. Especially, the frequency-domain optimization method is very
important for designing the high performance RF circuits andthe communication systems. Our algorithm is combined withfrequency-domain harmonic balance (HB) method for solving
nonlinear circuit and the optimization technique based on thesteepest descent method.
The Volterra series methods [6-8] are widely used for theanalysis of nonlinear circuits in the frequency domain, which
can be also easily applied to design the circuits [3,5-6],
because they can get the solutions in the analytical forms.
Although the algorithms are based on the elegant bilinear
theory, it is not so easy to derive the higher order Volterra kernels. Furthermore, the applications are difficult for large scale
systems containing many nonlinear elements [6-7]. Remarkthat the methods can be only applied to the weakly nonlinear
circuits such that the nonlinear devices are modeled by power
series. The convergences to the strong nonlinearities are notguaranteed.
The HB method is also widely used for solving nonlinear
circuits [10-13] in the frequency domain. It has such a property
that it can be stably applied even to the strong nonlinear
circuits having bipolar transistors and/or MOSFETs. On theother hand, they need many troublesome tasks for getting thecircuit equations and the applications of HB method.

0-7803-9390-2/06/$20.00 ©2006 IEEE

Therefore, we have developed a Spice-oriented algorithm
based on the HB method using Analog Behavior Models(ABMs), where all the nonlinear devices are replaced bycorresponding HB models, and linear inductors and capacitors
are transformed into the corresponding HB elements coupledwith the controlled sources [11]. Once these device modules
such as bipolar transistors and MOSFETs are stored in ourcomputer library, a given circuit is easily transformed into
the HB circuit. Thus, the frequency-domain analysis such as
frequency response curves can be easily obtained by solving
the circuit with DC analysis of Spice. We show our HB method
and the device modules of nonlinear devices in section II.
These solutions from HB circuit are used in the following
frequency-domain optimization techniques.
Now, let us discuss our optimization algorithm in thefrequency-domain. First, we define the objective function as
follow,
Φ(x, y), x ∈ Rn , y ∈ Rm ,(1)wherex:circuit variables such as voltages and currents,
y:parameters (ex., L, R, C, voltage and current sources).
We want to minimize or maximize the function (1) byadjusting y, where x are obtained from the HB circuit
1. Although there are many optimization techniques [15], we use a well-known steepest descent algorithm using
Spice. Although the descent direction is generally decided
by the sensitivity analysis [2], we find it with the numericaldifferentiation techniques because our modified HB circuithas very complicated structures. Then, our Spice-orientedoptimization algorithm is realized by the equivalent circuit,and the optimum point can be found by the equilibrium pointin the transient analysis. From our many simulation results, wecould find out the optimum point stably when it has uniquepoint.
We show our optimization algorithm and the equivalentcircuit model in section III, and interesting examples in section
IV, respectively.
1 Note that the problem of maximization is reduced to the minimization
when we change the sign of Φ in (1). Hence, we will only discuss here theproblem of minimization.

3694

ISCAS 2006

II. H ARMONIC BALANCE CIRCUITS OF NONLINEAR

Then, we have

DEVICES

Analog integrated circuits are usually composed of manykinds of nonlinear devices such as diodes, bipolar transistors
and MOSFETs, whose Spice models are described by theseveral special functions such as exponential, square-root,
piecewise continuous functions and so on [14]. The Fourierexpansions in these devices cannot be described by analyticalforms. On the other hand, these devices in our HB circuits
are replaced by the equivalent circuit models using ABMs ofSpice which execute the Fourier expansions. To understandour ideas, we consider a two-terminal element described by
i = fˆ(v).

(2)

Assume the input and output waveforms as follows;
v(t) = V0 +Mk=1Mi(t) = I0 +k=1,

I1 = f1 (V0 , V1 , · · · , V2M ),·········

I2M = f2M (V0 , V1 , · · · , V2M )I2k =1π

 2π 0f (v) cos kωtdt

f (v) sin kωtdt0






B. Parasitic inductor
In the same way, we assume current-controlled inductor asfollows;

iL = I0,L +φL = Φ0,L +⇒ vL =(4)M
k=1,qC = qˆC (vC ) .

(5)

M


(I2k−1,L cos kωt + I2k,L sin kωt) .

(10)

k=1



(Φ2k−1,L cos kωt + Φ2k,L sin kωt) kω (−Φ2k−1,L sin kωt + Φ2k,L cos kωt) (6)(7). (11)In this case, the nonlinear device model consisted of theresisters and inductors are realized by the equivalent circuitswith the current-controlled voltage sources given by (4) and(11).
Thus, 3-terminal bipolar transistors modeled by Ebers-Mollmodel and/or Gummel-Poon model [14] are schematicallyrealized as shown in Fig.1. The corresponding device modelto MOSFETs is shown in Fig.2.
CWe assume the capacitor voltage as follow;(V2k−1,C cos kωt + V2k,C sin kωt) .

M
Then, we have

C0B

C2M-1

B0Fig. 1.

E0

E2M-1

E2M

(c) Mth cos-component(d) Mth sin-component

HB module of the bipolar transistor.
D0B

B2M

(b) DC-component

DG

C2M

B2M-1

E
(a) BJT

Now, assume that a nonlinear capacitor is the voltagecontrolled given by

k=1

(9)

k=1

A. Parasitic capacitorM. (8)Thus, the nonlinear device models consisted of the nonlinear
resistors and capacitors are realized by the equivalent circuitswith the voltage-controlled current sources given by (4) and(8).

where k = 1, 2, · · · , M . The formulas can be applied to any
kind of function even to the piecewise continuous functions[14]. The integrations can be numerically calculated using thetrapezoidal integration formula, and that they are realized with
ABMs of Spice, schematically [13]. Since bipolar transistors
and MOSFETs also have the parasitic capacitors and/or inductors, we need to take account of these elements in the devicemodules.

vC = V0,C +kω (−Q2k−1,C sin kωt + Q2k,C cos kωt) (3)where the Fourier coefficients can be numerically calculatedby the following formulas;
 2π
1


I0 =f (v)dt
2π 0 

π
1
2π

k=1

k=1

We assume the inductor current as follows;

where M denotes the higher harmonic component to be taken
account in the analysis. The output Fourier coefficients aredescribed as follows;I0 = f0 (V0 , V1 , · · · , V2M ) I2k−1 =⇒ iC =M(Q2k−1,C cos kωt + Q2k,C sin kωt) 

φL = φ̂L (iL ) .

(V2k−1 cos kωt + V2k sin kωt) (I2k−1 cos kωt + I2k sin kωt) 

qC = Q0,C +M


G0

D2M-1

B0

G2M-1

D2M

B2M-1

G2M

B2M

S

S0

S2M-1

S2M

(a) MOSFET(b) DC-component(c) Mth cos-component(d) Mth sin-component

Fig. 2.

HB module of the MOSFET.

Note that the HB circuit consists of (2M+1)-subcircuits
corresponding to the DC, the fundamental and up to the M thhigher harmonic components.
Once these device modules are installed in our computer
library, we can easily formulate the HB circuits, and carry out
the frequency-domain analysis.

3695

III. O PTIMIZATION ALGORITHM
Now, we consider our frequency-domain optimization. Generally, the objective function (1) may be composed of the several requirements such as the maximum output, low distortion,phase margin, and so on. The ratios of requirements pk should
depend on the subject, in advance. Thus, the object function
is described as follow;
Φ(x, y) =K


pk φk (x, y),

(12)

k=1

are obtained as the voltages at the capacitors in our simulator
which satisfyΦ1 − Φ0 dy1

=−C1


dt
∆y1


Φ2 − Φ0 dy2


=−C2
dt
∆y2.
(17)

·········Φm − Φ0 dym


=−Cm
dt
∆ym
Note that the capacitor values play to improve the convergence
ratios in our optimization.

where the signs of pk should be chosen properly,|pk | < 1,(13)and K is a number of requirements. In this case, x is thecircuit variables such as node voltages and/or currents which
are estimated by the solutions from the HB circuit in section
II, whose circuit equation is given as follows;
F (x, y) = 0, F (·, ·) : Rn → Rn .

IV. I LLUSTRATIVE EXAMPLES
To understand the ideas of our optimization algorithm, let us
consider a simple problem to find out the optimum capacitanceand inductance giving the maximum power consumption at RL
in Fig.4.

(14)

R0LThen, the optimum point satisfies the following relations;∂Φ= 0, (k = 1, 2, · · · , m).
∂ykE +
ȁ -(15)

When we use the steepest descent algorithm, the descent∂Φ< 0, (k = 1, 2, · · · , m) indirection is given by − ∂yk
the parameter space y ∈ Rm . Although we can apply thesensitivity analysis to find the direction of steepest descent,our HB circuit containing bipolar transistors and MOSFETs
are too complicated for the sensitivity analysis. Therefore, weapply the numerical differentiations to the calculation of thedescent directions. Namely, we have for a variable s,Φ1 (x, y1 + ∆y1 , y2 , · · · , ym ) − Φ0 (x, y) ∂y1=−∂s∆y1Φ2 (x, y1 , y2 + ∆y2 , · · · , ym ) − Φ0 (x, y) 
∂y2Fig. 4.

L=A simple optimization problem.

1
1RL (R0 − RL ), C =ωωR0

R0 − RLRL(18)Now, let us find the values with our optimization approachshown in Fig.5.
ȁLILsILc+-=−EcȁCVCs+VCcȁLILc

RL

Ǟ0(C,L)CǞ1(C+ǍC,L)ILs-(Ǟ1-Ǟ0)/ǍC

I1
C1

I1+-+-ȁCVCc VCs-

The flowchart of our optimization algorithm is shown inFig.3.

LRL
Ǟ2(C,L+Ǎ.)(a)HB circuits-(Ǟ2-Ǟ0)/ǍL

I2
I2

C2(b)Optimization circuit

Fig. 5.

Optimization circuit,ω = 1rad/s, Ec = 1V, RL = 1Ω, R0 = 3Ω.

㱂0䋽㱂(x,y1,y2,䊶䊶䊶,ym)㱂1䋽㱂(x,y1+㰱y1,y2,䊶䊶䊶,ym)-(㱂1-㱂0)/㰱y1

㱂2䋽㱂(x,y1,y2+㰱y2,䊶䊶䊶,ym)-(㱂2-㱂0)/㰱y2㱂m䋽㱂(x,y1,y2,䊶䊶䊶,ym+㰱ym)-(㱂m-㱂0)/㰱ymFig. 3.

RL

They are theoretically given as follows;. (16)∆y2·········
Φm (x, y1 , y2 , · · · , ym + ∆ym ) − Φ0 (x, y) ∂ym
=−∂s
∆ym∂s

C

I1 C 1Fig.5(a) shows the Cosine and Sine subcircuits [13] in ourHB circuit. Since the circuit is driven by EC cos ωt, theCosine circuit has a DC source EC . C and L are replacedby the controlled sources, respectively. The objective function
is defined by+y1-I1
I2 C 2+y2-I2Im CmIm22.
+ ILs
Φ (C, L) = RL ILc+(19)ym-Flowchart of our steepest descent method.

The objective function Φ0 (x, y) is estimated by the circuitvariables x and the parameter values y. The parameters yThen, the optimization circuit shown in Fig.5(b) consists of 3
subcircuits Φ (C, L), Φ (C + ∆C, L), Φ (C, L + ∆L), where
C and L are given by the voltages of capacitors C1 and C2 ,respectively The result with the transient analysis of Spice isshown in Fig.6. The values C and L are exactly equal to thosevalues from (18).

3696

1.640L
Vout [mV]201.2

cos-comp
pow[µW]

00.8
C-200.4

sin-comp

power
0-40

01020Fig. 6.

3040[sec] 50

10Spice simulation results,

98Fig. 8.

1010[rad/sec]

10

Frequency response curve,

ICC = 1mA, RL = 36.22Ω, vin = 0.1 cos ωt.

∆C = 0.001, ∆L = 0.001.

40
RL[Ω]
pow[µW]

30
Vout[mV]

Next, we consider a high frequency RF power amplifier
shown in Fig.7 which is used in mobile-phones [5], where Lg s
are the parasitic inductances. We want to optimize the circuit
parameters in such manner that the output power consumption
at RL becomes maximum by adjusting RL and ICC . We
first modeled the transistors with Gummel-Poon model, andobtained the HB modules, where we consider up to the third
higher harmonic components.

201000Fig. 9.

1234[sec] 5

The result of our steepest descent method.

VCCICCFor future problem, we need to extend our algorithm to theproblems with the multiple optimum points.

T2C1R EFERENCES

T1
Rb1
Rb2
VCC

Vbb

VCCLg
L1L2RbC3T3C4T4C2Vin

RL+-LgFig. 7.

Lg

RF power amplifier,

L1 = L2 = 0.1mH, LG = 10nH, C1 = C2 = C3 = C4 = 1nF, VCC = 3V,Vbb = 3V, Rb1 = Rb2 = 1Ω, Rb = 1Ω.

We have calculated the frequency response curve in theregion ω = 108 − 1011 . The waveform is nearly sinusoidal,
and the amplitudes are exactly equal to the result fromtransient analysis. In our optimization algorithm for getting themaximum output power, we have changed the current sources
and the load resistor in the region ICC = 1mA − 7mA, andRL = 0.1 − 70Ω, respectively. Thus, we can stably find out
the optimum point as shown in Fig.9.
V. C ONCLUSIONS AND REMARKSIn this paper, we have proposed a new Spice-oriented
frequency-domain optimization technique, whose objectivefunction can be obtained from the HB circuit. We first transform the nonlinear devices such as bipolar transistors andMOSFETs into the corresponding HB modules. Our optimization technique depends on the steepest descent algorithm
which is realized by the equivalent circuit. The optimum point
is given as the equilibrium point the transient response, which
can be stably solved by the transient analysis of Spice.

[1] R. K. Brayton and R. Spence, Sensitivity and Optimization, Elsevier
Scientific Pub. co., 1980.
[2] G. D. Vendelin, A. M. Pavio and U. L. Rohde, Microwave Circuit Designusing Linear and Nonlinear Techniques, John Wiley and Sons, Inc.,
1990.
[3] J. Wood and D. E. Root, Fundamentals of Nonlinear Behavior Modelingfor RF and Microwave Design, Artech House, Inc., 2005.
[4] D. Leenaerts, J. van der Tang and C. Vaucher, Circuit Design for RFTransceivers, Kluwer Academic Publishers, 2001.
[5] H. Floberg, Symbolic Analysis in Analog Integrated Circuit Design,
Kluwer Academic Publishers, 1997.
[6] P. Wambacq and W. Sansen, Distortion Analysis of Analog IntegratedCircuits, Kluwer Academic Publishers, 1998.
[7] D. D. Weiner and J. E. Spina, Sinusoidal Analysis and Modeling of
Weakly Nonlinear Circuits with Application to Nonlinear Interference
Effects, Van Nostrand Reinhold, 1980.
[8] L. O. Chua and C-Y. Ng, “Frequency-domain analysis of nonlinear systems: formulation of transfer functions”, IEE Trans. Electronic Circuits
and Systems, vol.3, no.6, pp.257-269, 1979.
[9] K. S. Kundert, J. K. White and A. Sangiovanni-Vincentelli, SteadyState Methods for Simulating Analog and microwave circuits, Kluwer
Academic Publishers, 1990.
[10] A. Ushida, T. Adachi and L. O. Chua, “Steady-state analysis of nonlinear
circuits based on hybrid methods”, IEEE Trans. on Circuits and SystemI: Fundamental Theory and Applications, vol.1, pp.649-661, 1992.
[11] A. Ushida, Y. Yamagami and Y. Nishio, “Frequency responses ofnonlinear networks using curve tracing algorithm”, ISCAS 2002, vol.1,
pp.641-644, 2002.
[12] R. J. Gilmor and M. B. Steer, “Nonlinear circuit analysis using themethod of harmonic balance- A review of the art. Part.1. Introductoryconcepts”, Int. Jour. of Microwave and Millimeter-Wave Computer-Aided
Eng., vol.1, no.1, pp.22-37, 1991.
[13] R. J. Gilmor and M. B. Steer, “Nonlinear circuit analysis using themethod of harmonic balance- A review of the art. Part.2. Introductoryconcepts”, Int. Jour. of Microwave and Millimeter-Wave Computer-Aided
Eng., vol.1, no.2, pp.159-180, 1991.
[14] R. L. Geiger, P. E. Allen and N. R. Strader, VLSI: Design Techniquesfor Analog and Digital Circuits, McGraw-Hill, 1990.

3697