Mor M. Peretz Power Electronics Laboratory Department of Electrical and Computer Engineering Ben-Gurion University of the Negev, ISRAEL

Size: px

Start display at page:

Download "Mor M. Peretz Power Electronics Laboratory Department of Electrical and Computer Engineering Ben-Gurion University of the Negev, ISRAEL"

Jasper Perkins
5 years ago
Views:

1 Mor M. Peretz Power Electronics Laboratory Department of Electrical and Computer Engineering Ben-Gurion University of the Negev, ISRAEL [1]

2 Advanced Applications This part will focus on two PSpice compatible advanced applications. The applications described in this chapter emphasize the viability of the modern circuit simulators, especially when dealing with nonlinear circuits and systems. In this chapter we will use our knowledge in circuit modeling that was gained in previous parts (especially behavioral modeling) to present elegant solutions for two non-trivial simulation challenges: Non-linear passive components Analysis of Modulated-driven systems Innovative thinking, good engineering practice and the powerful, yet simple, models provided by PSpice can cause system analysis to be much easier. [2]

3 : Outline 1. Function dependent components a. Overview b. Methodology c. Examples: non-linear Resistor, Capacitor, Inductor 2. Envelope simulation a. Background and rational b. The approach c. Large-signal d. Small-signal e. RLC circuit implementation [3]

4 Function dependent components Simulation based analysis of a system is particularly useful when dealing with a non-linear behavior that might be difficult to handle analytically. There are many types of (passive) components which their values depend on the circuit parameters or operation, such as: non-linear magnetics, voltage-controlled capacitors, thermistors, etc. Here we present the methodology of developing a simple, PSpice compatible behavioral model for non-linear passive components. Reference: Ben-Yaakov, S., and Peretz, M.M., Simulation bits: A SPICE behavioral model of non-linear inductors, IEEE Power Electronics Society Newsletter, Fourth Quarter, 9-1, [4]

5 Function dependent components Modern simulation packages include models for non-linear component model that is based on conventional modeling methods (e. g. Jiles-Atherton for magnetics). However, unless the vendor already provides a model for a given device, developing your own model for a specific application may prove to be a tedious chore if not practically impossible. The modeling methodology presented is easy to apply using either manufacturer s data (which can be drawn from datasheets of App. Notes) or by a simple set of laboratory measurements. [5]

6 The method The basic idea is to reflect the behavior of a linear component (PSpice R, L, C) via a non-linear transformer E1 G1 V I pr sec 1 K = = I pr V sec In X' out Ipr Vpr G1 E1 + - Isec Vsec Norm. value The impedance of the original component is: The impedance reflected to the primary: X' = V I pr pr = X = K V I V I sec sec sec sec = K X [6]

7 The method The actual component value in terms of K is: ( R or L or C )' = K ( R or L or C) If K is made dependent on the circuit parameters, then the model will emulate the non-linearity of the device. Using PSpice, one may use ABMs in which the dependence of K on the parameters can be defined as an expression (EVALUE) or table (ETABLE). The dependence of the component can be defined by either the voltage or current thru it, or by sensing other parts in the circuit. The dependent sources of non-linear transformer my be inverted, that is, in-voltage out-current. Depends on the application. [7]

8 Example - Thermistor demo18 Here we demonstrate an application for a temperature dependent resistor. The temperature is sensed using external circuitry and coded into voltage 1C=1V. The resistance variance with the temperature was drawn from manufacturer datasheet and inserted into an ETABLE. Since now a resistor needs to be emulated, the transformer V5 Vsec sources are inverted. R2 Model for all non-linear components is compatible with all basic spice simulations (AC, DC, TRAN) res_in res_out Vdc E2 1u R4 1u PARAMETERS: temperature = 4 V(temp) IN+ OUT+ IN- OUT- ETABLE E1 OUT+ IN+ OUT- IN- EVALUE k V(x) {temperature} GVALUE IN- IN+ G1 temp V3 OUT- OUT+ I(V5)*V(k) 1Vdc Vdc V4 x R3 1 R1 1 res_in res_out [8]

9 Example - inductor The inductance value may change by either of the following: 1.The DC current that flows thru the inductor 2.Bias current A Ibias inductor Bias windings L Lr Ibias Several detailed applications of a non-linear inductor can be downloaded from: and in the course website: [9]

10 Example inductor, parametric modulation in_ind out_ind E3 R7 1u R13 1u pr+ pr- IN+ OUT+ IN- OUT- EVALUE (v(pr+)-v(pr-))/v(func1) IN+ OUT+ IN- OUT- EVALUE i(vsweep)*13/8 Conversion unit Inductor model G1 OUT+ IN+ OUT- IN- GVALUE i(vsec) sw 1meg R9 E1 secondary func1 Vsec Vdc R1 1u 1 2 L1 1 Expression (pwr(n,2)*4*3.14*pwr(1,-7)*1.72*pwr(1,-4)/.1)* (sqrt(((pwr(125,2))-56.18u*pwr(125,3)*v(sw)+14.3p*pwr(125,4)*pwr(v(sw),2)) /(( u*125*v(sw)+62.1n*pwr(125,2)*pwr(v(sw),2))))) Inductor model used for simulation [1]

11 Example inductor, parametric modulation out IOFF = IAMPL = 1m FREQ = 1k I3 R1 1k in_ind out_ind VOFF = 2.5 VAMPL = 2.4 FREQ = 5 mod V2 R14 1 Vsweep Vdc Modulation Circuit Modulating signal Performing modulation on the input signal by changing the circuit parameters. [11]

12 Example inductor, parametric modulation 4.mV Modulating signal (inductance value) 2.mV V 2.V V V(func1) Output signal -2.V s 1ms 2ms 3ms 4ms 5ms 6ms 7ms 8ms 9ms 1ms V(OUT) Time On course website you can find a presentation which gives a detailed methodology for non-linear inductor model development and background [12]

13 Envelope simulation Various types of electronic systems are based on resonant networks that are often exposed to modulated signals. Envelope simulation by a SPICE compatible model could be used to simplify the circuit analysis and in the extraction of the smallsignal transfer function which is due to modulation. Here presented a unified model for both large and small signal analyses using envelope simulation. V ref Modulator Resonant network Load β Envelope detection [13]

14 Approach large signal Any analog modulated signal (AM, FM, PM) can be described by the following expression: u () t = U ( t) cos( ω t) U ( t) sin( ω t) 1 c + U1 and U2 are modulation signals (in-phase and quadrature), ωc is the carrier frequency. The expression can be rewritten in a complex form: Or u u () t = Re[ ( U1( t) ju2( t) )] r r () = () arg( U() t t U t Re e ) e Where: r U jω r U c t 2 () t U () t ju () t, arg U() t 2 () t = U () t + U () t c r 1 U ( ) 2( t = ) tan = 1 2 U 1 () t [14]

15 Approach Consequently, any modulated signal can be represented by a generalized phasor with time dependent magnitude and phase. The PSpice compatible envelope simulation circuit can be developed by the following stages: 1.Duplicating the circuit to create the real and imaginary parts. 2.Replacing reactive elements as will be shown into the real and imaginary parts of the circuit. Resistors are left as-is. 3.Placing two excitation sources, one for each part but exluding the carrier. 4.Adding an ABM expression block to calculate the square root of the sum of squares of the Re and Im output signals. Lineykin, S., and Ben-Yaakov, S., A unified SPICE compatible model for large and small signal envelope simulation of linear circuits excited by modulated signals. IEEE Power Electronics Specialists Conference, PESC-23, , Acapulco, Mexico, [15]

16 Approach The replacement of reactive elements by equivalent circuits for envelope simulation: Re L i L_im 2 π fc L + - i L_re i L Im L i L_re 2 π fc L + - i L_im C V C_re Re Cross-coupled elements to describe Re and Im. The carrier frequency is present only as an algebraic coefficient. V C Im V C_im 2 π fc C C V C_im V C_re 2 π fc C [16]

17 Approach sources AM modulation is exemplified. The AM signal with carrier is described by: u t = A 1 k A sin ω t cos ( ) ( ( )) ( ω t) c + a The excitation for the time domain analyses needs to be separated into Re and Im parts and excluding the carrier. U t = A 1+ k A sin ω t U 1 2 m m ( ) c( a m ( m )) () t = For DC analysis, steady state, the simulation is repeated for number of carrier frequencies. That is, the modulating signal, Am, is zero and the carrier is constant. U U 1 2 ( t) = () t = A c c [17]

18 Approach small signal Small-signal analysis can be obtained by either of the following: 1.Using several runs of TRAN analysis for different modulating frequency. This method is tedious!!! 2.Replacing the time dependent sources by phasors. Since the circuit is linear, it will be left as-is after linearization obtained by the simulator when applying AC. The sources (AM) are: U U 1 2 ( t) Ac( 1+ ka ) () t = A ~ m A ~ = m Is the excitation source Other modulation types and their application in the basic analyses are detailed in: Lineykin, S., and Ben-Yaakov, S., A unified SPICE compatible model for large and small signal envelope simulation of linear circuits excited by modulated signals. IEEE Power Electronics Specialists Conference, PESC-23, , Acapulco, Mexico, [18]

19 Example RLC, AM modulated demo19 E6 IN+ OUT+ IN- OUT- EVALUE in_trn L3 1 2 {Lr} {Ac*(1+Ka*Am*sin(6.28*fm*time))*cos(6.28*fc*time)} Cycle-by-cycle circuit C7 {Cr} out_trn R8 {Rm} Real Part in_re I_re Vdc L1 1 2 {Lr} C1 a b {Cr} E1 OUT+ OUT- EVALUE {-I(I_im)*6.28*fc*Lr} IN+IN- IN+IN- {-(V(c)-V(d))*6.28*fc*Cr} GVALUE OUT+ OUT-G1 R1 {Rm} PARAMETERS: fc = 45k Lr = 7m Cr = 2.2n Rm = 1 Am = 1 Ac = 1 Ka =.2 fm = 2 E4 in_re IN+ OUT+ IN- OUT- EVALUE {Ac*(1+Ka*Am*sin(6.28*fm*time))} TRAN source IN+IN- {(V(a)-V(b))*6.28*fc*Cr} GVALUE OUT+ OUT-G2 E5 out IN+ OUT+ IN- OUT- EVALUE sqrt(v(b)**2+v(d)**2) R7 1u I_im Vdc L2 1 2 {Lr} Imaginary part R4 1k OUT+ OUT- IN+IN- C2 c d {Cr} E2 EVALUE {I(I_re)*6.28*fc*Lr} R2 {Rm} [19]

20 Example RLC, AM modulated demo19 4mV V Output signal -4mV 2. V V(out_trn) V( o u t ) V Input signal SEL>> -2.V 2ms 25ms 3ms 35ms 4ms V( i n _ t r n ) V( i n _ r e ) Ti me [2]

VARIOUS power electronics systems such as resonant converters,

VARIOUS power electronics systems such as resonant converters, IEEE TRANSACTIONS ON INDUSTRIAL ELECTRONICS, VOL. 53, NO. 3, JUNE 2006 745 Unified SPICE Compatible Model for Large and Small-Signal Envelope Simulation of Linear Circuits Excited by Modulated Signals