Envelope Simulation by SPICE Compatible Models of Electric ...

1Envelope Simulation by SPICE Compatible Modelsof Electric Circuits Driven by Modulated SignalsSam Ben-Yaakov * , Stanislav Glozman and Raul RabinoviciDepartment of Electrical and Computer EngineeringBen-Gurion University of the NegevPOB 653, Beer-Sheva 84105, IsraelTel: +972-7-646-1561; Fax: +972-7-647-2949; Email: sby@ee.bgu.ac.ilWeb site: www.ee.bgu.ac.il/~pelAbstract - SPICE compatible equivalent circuits were developedto facilitate the analysis and envelope simulation of electriccircuits driven by modulated signals. The circuits are based ona novel complex phasor domain transformation. The proposedmethod facilitates simulation of any general linear circuitdriven by a modulated signal such as AM, FM or PM.Simulation time by the proposed envelope simulation is muchfaster than the full cycle-by-cycle simulation of the originalcircuit and excitation.I. INTRODUCTIONModulated signals play an important role in PowerElectronics. For example, Frequency or Phase Modulation(FM, PM) is related to resonant power converters [1] andelectronic ballasts of discharge lamps [2]. Furthermore,Amplitude Modulation (AM) plays an important role indetermining the stability of high frequency electronicballasts for discharge lamps [3,4]. In these systems, the lampis driven by a high frequency source in series with aninductor which controls the current (Fig. 1). Power level isnormally regulated by shifting the frequency of the sourceand thereby increasing or decreasing the current. Hence,current level can be closely controlled by a feedbacknetwork connected to a controlled oscillator that feeds thepower stage. It should be noted that when the FM signalpasses through reactive elements it would be translated to anAmplitude Modulated FM signal. Direct analysis of theresponse of such an electrical circuit to a modulated carrieris thus complex while cycle by cycle simulation of such asystem is very lengthy due to the presence of the highfrequency component.The method proposed in [5] is based on a phasortransformation by which the original circuit of the highfrequency modulated carrier is transformed into anequivalent circuit of the low frequency modulation signals.In this transformation, the resistance components areequivalent to themselves but the equivalent circuits of thereactive components include the component itself plus an''imaginary'' resistor element. This technique was applied inlimited studies for specialized cases, e.g. when the carrierfrequency equals the resonant frequency of the circuit underexamination [3,4]. Still lacking thus far is a method thatwould facilitate envelope simulation by SPICE basedgeneral purpose circuit simulator such as PSPICE(MicroSim Inc. USA).3RZHUFig. 1.(OHFWURQLF'ULYHUFreqΣ 9UHIFMinputsignalFeedback, lamp9 lampFluorescent lamp, driven by a high frequency source in series withan inductor which controls the current.* Corresponding author

2In this study we developed a complex phasortransformation approach that was then used to derive aSPICE compatible model transparent to the high frequencycarrier. The proposed method facilitates envelope simulationof any linear electric circuits by any general purposesimulator. This approach differs from earlier solutions toenvelope simulation which rely on specialized computerprograms [6].II. COMPLEX PHASOR TRANSFORMATIONAPPROACHAny analog modulated signal (AM, FM or PM) can bedescribed by the following general expression:u(t)= U1(t)⋅cos(ωct)+ U 2 (t) ⋅sin(ωct) (1)where U1(t) and U 2(t) are the modulation signals and ω c isthe angular frequency of the carrier.Expression (1) could also be written as:or as:u(t)= Re[(U1(t)− j⋅U 2 (t)) ⋅exp(jωct)] (2)[ exp(arg(U(t)) ⋅exp(jωt) ]u(t)= U(t) ⋅ Rec (3)−1⎛ − U ⎞where 'arg(U(t))' is⎜ 2 (t)tan⎟ .⎝ U1(t)⎠Expression (3) implies that the modulated signal in thetime domain u(t) can be represented by a generalized phasorthat both its magnitude and phase are time dependent. Theexpression of the complex phasor U &(t)is:&U(t)= U1(t)− jU 2 (t)The magnitude:&2 2 1/ 2U (t) = [U1 (t) + U 2 (t)]is equal to the modulation envelope of the original signalu(t) (eq. (3)).As will be shown next, the complex phasor&representation U(t)= U1(t)− jU 2 (t), introduced here, canbe used to drive the low frequency equivalent circuits thatrepresent the envelope behavior of the system withoutinvolving the high frequency carrier. This would shortensimulation time considerably since the time domain analysisdoes not include the high frequency component. Theequivalent circuit is obtained similar to [6] by a phasortransformation of the electric components L, C, and R. Aninductor L in the original circuit becomes an inductive(4)(5)component L in series with an imaginary resistor jω c L in theequivalent circuit, a capacitive component C becomes acapacitor C in parallel to an imaginary resistor 1/(jω c C), anda resistor component R is equivalent to the same resistorcomponent R. Therefore, the equivalent circuit in thegeneralized phasor domain will consist of inductors,capacitors, and resistors in series or in parallel to''imaginary'' resistors. Such a circuit is not compatible withSPICE simulators and consequently an additionaltransformation is needed to permit simulation by commoncircuit simulators. This additional step is described in thefollowing section.III. SPICE MODELS FOR CIRCUITS WITHIMAGINARY RESISTORSThe proposed methodology is demonstrated byconsidering an L, R circuit (Fig. 2a) driven by a generalizedmodulated signal:v(t)= V1 (t) cos( ωct)+ V2(t) sin( ωct)(6)The equivalent circuit in the generalized phasor domain(Fig. 2b) can be described by:&& & dI(t) &V(t)= RI(t) + L + jωcLI(t)(7)dtYW9M9 5i(t)(a)5 /(b)5 /9 I ,M, 5 /9 I (c)/j*ωc*L-I*ωc*LI *ωc*LFig. 2. SPICE model for a circuit with an ''imaginary'' resistor: (a) originalR, L circuit driven by a modulated voltage source; (b) theequivalent circuit of (a) in the generalized phasor domain; (c) crosscoupled equivalent circuits based on (11) and (12) that replace (b).

3where the last term could be interpreted as an "imaginary"resistor of the 'value' jωcL. V & &(t)and I(t)are the complexphasors that prevail in the equivalent circuit of Fig. 2b:&V(t)= V 1(t)− jV2(t)&I(t)= I1 (t) + jI2(t)Applying (8) and (9), (7) can be rewritten as:V1− jV2= R(I1+ jI 2 ) +d(I1+ jI 2 )+ L + jωcL(I1+ jI 2 ) (10)dtTo facilitate analysis by general purpose circuitsimulators we divide the complex equation (10) into real andimaginary parts:dI1V1 RI1+ L − ωcLI2dtdI2− V2 = RI2+ L + ωcLI1dt(8)(9)= (real) (11)(imaginary) (12).The two equations, (11) and (12), can now be emulatedby two interconnected circuits (Fig. 2c). Notice that thisrepresentation does not involve imaginary resistors and thatlast terms in (11) and (12) are emulated by cross-coupleddependent voltage sources (a voltage source whosemagnitude is a linear function of the current in the crosscircuit). The newly developed equivalent circuits of Fig. 2ccontain only conventional electric components and aretherefore SPICE compatible. A similar but dual thinking canbe followed for a capacitor in parallel with the ''imaginary''resistor. For example, the equations for a capacitor C inparallel to a conductance G, fed by a current sourcemodulated signal, will be:dV1I1 GV1+ C − ωcCV2dtdV2I2 = GV2+ C + ωcCV1dt= (real) (13)− (imaginary) (14)Following this approach, SPICE compatible circuitscould be developed for more involved circuit configurations.The usefulness of the proposed simulation method isfurther demonstrated by considering the case of phasemodulated (PM) voltage source driving the circuit of Fig. 2a.The source is assumed to be of the form:v(t)= A cos[ ωct+ m p sin( ωmt)](15)Therefore, the equivalent circuit of Fig. 2b is driven bythe generalized voltage phasor:&V(t) = A cos[m p sin( ωmt)] ++ jA sin[m p sin( ωmt)](16)Consequently, the SPICE compatible equivalent circuitsof Fig. 2c are driven by the sourcesV1 = A cos[m p sin( ωmt)](17)− V2 = A sin[m p sin( ωmt)](18)The circuits of Fig. 2c were fed to a PSPICE simulator(evaluation version 8) via the Schematics Capture front endby using the appropriate symbols (dependent voltage sourceare represented by EVALUE symbols). The simulation wasrun for the following values: R= 10Ω, L= 7 mH, A= 200V,f c = ωc/2π= 40kHz, m p = 10, f m = ωm/2π =2kHz.Fig. 3a shows the original current i through the circuitof Fig. 2 (upper trace) and the envelope of the current,obtained by the circuits of Fig. 2c and applying (5) (lowertrace). Fig. 3b compares the results of cycle by cyclesimulation and envelope simulation. Fig. 3c depicts thevoltage phasor components V 1 and -V 2 , while Fig.3d thecurrent phasor components I 1 and I 2 . The spectrum of thecurrent of the original circuit (Fig. 2a) is shown in Fig. 4awhile the spectrum of the reconstructed current is given inFig. 4b. The reconstruction was calculated by:i(t)= I1(t) cos( ωct)+ I 2 (t) sin( ωct)(19)applying the original carrier frequency and the envelopecomponent (I1, I2) of the SPICE simulation results based onFig. 3c. It is evident that both the envelope signals (Fig. 3)and the spectra (Fig. 4) obtained by the proposed simulationmethod are identical to the original ones.IV. THE GENERAL CASEConsider a general R, L, C circuit that is driven by amodulated carrier u(t). The matrix state space equation of thesystem is:x = A ⋅ x + B ⋅ u(20)By expressing u as the complex excitation (4), insertingit in (20) and breaking the resulting complex state spaceequation into real and imaginary parts one obtains: (21)X1 = A ⋅ X1− A1⋅ X 2 + B⋅U1 (22)X 2 = A ⋅ X 2 + A1⋅ X1− B⋅U 2where X1, X2 are the complex state variables of the phasordomain circuit, U1, U2 are the source complex phasors and

4P$P$(a)$P$$P$(b)$PVPV7LPHPV$N+]N+])UHTXHQF\N+]P$(a)Fig. 4. Signal spectra: (a) current in the original circuit (Fig. 2a); (b)reconstructed current spectrum . See text for details.P$$99 9PV7LPH(b)PVPVA1 is the matrix of the imaginary resistors, jωcL associatedwith each inductor and 1 jω cCassociated with eachcapacitor (ωc is the carrier frequency). The cross coupledterms A1X2 in (21) and A1X1 in (22) can be represented asdependent sources: voltage source in the inductor case andcurrent source for the capacitor case. Original resistors areleft as is. Equations (21) and (22) can now be simulated astwo circuits that include dependent sources that are afunction of the state variables of the cross circuits. Note that(21) and (22) include only the low frequency componentwhile the high frequency carrier is present only as analgebraic coefficient (ωc).999 99P$, $P$P$PVPV7LPH(c), $P$PVPV7LPH(d)PVPVFig. 3. Simulation results on the circuit of Fig. 2: (a) current i through theoriginal circuit of Fig. 2a (upper trace) and envelope of the current,obtained by envelope simulation based on Fig. 2c (lower trace); (b)traces (a) zoomed and superimposed; (c) voltage phasorcomponents V 1and -V 2; (d) current phasor components I 1and I 2.V. IMPLEMENTATIONPreparation of (21) and (22) for analysis by generalpurpose analog circuit simulator can proceed by translatingthe equations into equivalent circuits. Matrix 'A' is that of theoriginal circuit, whereas ' A 1' is new matrix representing thecoupled dependent sources. Here we describe a directmethod that bypasses the need for constructing the newmatrix. Starting with a general R, L, C circuit (Fig. 5a) thatis driven by a modulated carrier v(t), we first replace thereactive elements by dependent sources. An inductor Li isreplaced by a current source i Li and a capacitor Ci isreplaced by a voltage source v Ci (Fig. 5b). The magnitudeof the dependent sources is linked to auxiliary circuits thatemulate the behavior of the elements. That is, the auxiliarycircuit for Li comprises a dependent voltage source v Li thatforces the in-circuit voltage on the inductor Li. The currentgenerated in the auxiliary circuit is then fed back to the maincircuit by the dependent current source i Li that representsthe inductor. In a similar way, dependent voltage sourcesv Ci replace capacitors in the main circuit. This separationstep is not crucial but is used to streamline the structure ofthe equivalent circuits that will later evolve and allowautomatization of the process.

5Fig. 5.Derivation of phasor equivalent circuits. (a) Original circuit. (b)Replacing reactive elements by dependent sources. (c) Real part ofphasor equivalent circuit. (d) Imaginary part of phasor equivalentcircuit.The next step applies the transformation of the circuitinto two phasor circuits per (21) and (22). Now we apply thetwo phasor sources V 1 and − V2(as shown in Section III)and implement the dependent sources A1X2 and A1X1.These are shown schematically in Fig. 5c (real part) and Fig.5d (imaginary part) for a specific inductor Li and a capacitorCi.The state equations that represent an original inductorL (Fig. 5a) are thus for the real part (Fig. 5c):iv(t)v(t)99/Lv Li&Lv C i5Lv R iv L iv C iv R i9/L9&L95L9/L9&L95L5Li L ii C ii R i(a)i L ii C ii R i(b),/L,&L,5L5L(c),/L,&L,5L5L(d)v L ii C i/L9/L,&L/L9/L,&L/L&L9&L&L9&L&L,/L,/Li L iv C i,/L/L ω c9/L&L ω c,/L/L ω c9/L&L ω cCidV1Ci= I1Ci+ V2Ci⋅ ωc⋅ Cidt⋅ (25)and for the imaginary part (Fig. 5d):CidV2Ci= I 2Ci − V1Ci⋅ωc⋅Cidt⋅ (26)The equivalent circuits of Figs. 5c and 5d are nowSPICE compatible. They include the original R, L, Ccomponents and dependent sources. It should be noted thatthe dependent sources are a function of the signals in thecross circuits. That is, the dependent sources in the realsection ( − I2Li⋅ ωc⋅ Li, − V2Ci⋅ωc⋅Ci, Fig. 5c) depend onthe corresponding signals in the imaginary part (Fig. 5d) andvise versa.The circuits of Figs. 5c, 5d are compatible with anymodern circuit simulator. In the followings we present anexample that was run on PSPICE (MicroSim Inc., USA,evaluation version 8), but any other simulator will do.VI. EXAMPLEWe demonstrate the technique outlined above byconsidering a resonant circuit (Fig. 6). It is assumed that thecircuit is driven by PM modulated carrier of the form givenabove (15). The circuit was transformed according to theguidelines given above and the equivalent circuits (a total of6 independent circuits) were run on PSPICE. The phasordomain sources are (17) and (18). For purpose of illustrationwe chose the carrier frequency ( fc= ωc2π) to be40.55kHz equal to the circuit resonant frequency 1 2π LC .In the first run to be illustrated, the modulation parameterswere: A=200V, f m = ωm2π= 100Hzand mp=20.Once the time domain simulation is done, any of theenvelope signals can be displayed. For example, theenvelope of the capacitor voltage (VC) is reconstructed bythe expression:2 2V C (V1C) + (V2C)= (27)LidI1Li= V1Li+ I2Li⋅ ωc⋅ Lidt⋅ (23)and for the imaginary part (Fig. 5d):LidI2Li= V2Li− I1Li⋅ ωc⋅ Lidt⋅ (24)9FThe state equations that represent an original capacitorC (Fig. 5a) are for the real part (Fig. 5c):iFig. 6.Illustrative circuit.

6where V1C and V2C are the envelope simulation resultsobtained for the real and imaginary parts, respectively. Thedegree of matching between the real signal and the results ofenvelope simulation (Fig. 7a) demonstrate the agreementthat is obtained. The perfect match is illustrated in thezoomed portion (Fig. 7b). Furthermore, the originalspectrum of the signal and the one reconstructed from theenvelope simulation results are identical (Fig. 8a). Thesimulation time for envelope simulation was 0.5 sec ascompared to 300sec when full simulation on circuit andmodulated carrier. The CPU used was a 333MHz Pentium.Envelope simulation offers large flexibility and accessto a wealth of information in a short simulation time. Forexample, the effect of the sweep speed on the capacitorvoltage was explored by parametric simulation in which themodulating frequency was stepped from 50Hz to 200Hz in50Hz steps while keeping the depth of modulationm p ⋅ f m = 4000 constant (Fig. 8b). Simulation time for thisrun was 10sec (on the same PC).N99N99N9N9N+]N+])UHTXHQF\(a)N+])P +])P +])P +])P +]N+]9PVPV7LPHPVN9(b)9N9Fig. 8.Simulation results: (a) Spectrum of original circuit (uppertrace) and reconstructed from envelope simulation (lowertrace). (b) Envelope simulation of capacitor voltage (Fig.6) for various modulating signals.VII. DISCUSSION AND CONCLUSIONS9N9N99PVPVPV7LPH(a)PV7LPH(b)PVPVPVPVFig. 7. Simulation results: (a) Real component of capacitor voltage (Fig. 6)(upper trace) and envelope as obtained by envelope simulation(lower trace). (b) Zoomed portion of (a).The general and systematic approach developed hereoffers a simple and straightforward procedure for generatingSPICE compatible phasor equivalent circuits of any R, L, Ccircuit driven by any modulated signal. The proposedequivalent circuits that were obtained by introducing thecomplex phasor representation are SPICE compatible andcan thus be run on any general purpose circuit simulator.Since envelope simulation involves only the low frequencycomponents, simulation time will be much shorter than thefull signal simulation. The time speed up will depend on thecomplexity of the circuit. For the simulation shown here aspeed up factor of about 1000:1 was observed. Althoughillustrated for the PM modulation case, FM and AM can beeasily implemented as well. The FM case can be consideredas a scaled case of PM while the AM case is a truncated v(t)signal including only a real partV1 = Vm⋅[1+ m ⋅cos(ωmt)] . Note however that even in thiscase the imaginary equivalent circuit is still needed but withV2=0. It should be noted that the proposed simulationapproach is not limited to sinusoidal modulation.

7Fig. 9.9(a)9N9(b)9N9(c)9JWPVPV7LPH9FW F\FOHE\F\FOH9FW HQYHORSHPVSimulation results: (a) Arbitrary modulation function. (b) Capacitorvoltage (Fig. 6) obtained by cycle by cycle simulation. (c) Capacitorvoltage (Fig. 6) obtained by proposed envelope simulation.The proposed method is applicable to any modulationfunction g(t). To illustrate this, we run a simulation on sameresonant circuit (Fig. 6), but with an arbitrary modulationfunction (Fig. 9a). Matching between cycle by cyclesimulation (Fig. 9b) and envelope simulation (Fig. 9c) wasagain excellent. The speed up factor was similar to the othercases (about 1000:1).The systematic method for generating the auxiliarycircuit is based on simple rules that can be easilymechanized to fully automate the transformation.It can thus be concluded that the proposed envelopesimulation is very efficient in terms of computer time. Itshould be noticed that the method, as presented here, isapplicable only to linear circuits.REFERENCES[1] R. L. Steigerwald, "High-frequency resonant transistorDC-DC converters," IEEE Transaction on IndustrialElectronics, Vol. IE-31, No. 2, pp. 182-190, May 1984.[2] B. C. Pollard and R. M. Nelms, "Using the seriesparallel resonant converter in capacitor chargingapplications," Proceedings of IEEE Applied PowerElectronics Conference, pp. 731-37, 1992.[3] E. Deng, "I. Negative incremental impedance offluorescent lamp," Ph.D. Thesis, California Institute ofTechnology, Pasadena, 1995.[4] E. Deng and S. Cuk, "Negative incremental impedanceand stability of fluorescent lamp," Proceedings of IEEEApplied Power Electronics Conference, pp.1050-1056,1997.[5] C. T. Rim and G. H. Cho, "Phasor transformation andits application to the DC/AC analyses of frequencyphase-controlled series resonant converters (SRC),"IEEE Trans. on Power Electronics, v. 5, no. 2, pp.201-211, April 1990.[6] D. Sharrit, "New Method of Analysis of CommunicationSystems," IEEE MIT Symposium WMFA: NonlinearCAD Workshop, June 1996.