Rev. Roum. Sci. Techn. Électrotechn. et Énerg., 52, 1, p. 3342, Bucarest, 2007 PSPICE SIMULATION OF POWER ELECTRONICS CIRCUIT [614960]

Rev. Roum. Sci. Techn. – Électrotechn. et Énerg., 52, 1, p. 33–42, Bucarest, 2007 PSPICE SIMULATION OF POWER ELECTRONICS CIRCUIT
AND INDUCTION MOTOR DRIVES
ADRIAN ȘCHIOP1, VIOREL POPESCU2
Key words: PSpice, Voltage source inverter, Induction machine.
This paper shows how power electronics circuits, electric motor s and drives, can be
simulated with modern simulation programs. The focus will be on PSpiceTM, which is
one of the most widely used general-purpose simulation programs . A simulation
example is presented, and the results are compared with those o btained with Power
System Simulation Tool based on SimulinkTM.
1. INTRODUCTION
Historically, simulation of transient phenomena related to powe r systems has
been carried on using the electromagnetic transients program (E MTP) [1] or one of
its variants, such as the alternative transient program (ATP) o r electromagnetic
transients for dc (EMTDC), which are all based on the trapezoid al integration rule
and the nodal approach. These software packages use fixed-step algorithms, which
yield excellent results for power systems free of any power ele ctronics devices.
However, the fixed-step algorithms do not adapt well to the pre sence of
discontinuities, which are cause d by the switching devices.
Spice is a general-purpose circuit simulation program, which wa s developed
at the University of California, Berkeley [2]. The Spice circui t simulation program
h a s b e c o m e a n i n d u s t r y s t a n d a r d . T h e m a j o r a d v a n t a g e o f u s i n g S pice in power
electronics is that, with the sam e software, a particular circu it can be designed and
analysed at different system and subsystem levels, i.e., at the levels of the power
switch, the converter circuit, and converter systems, including feedback control.
However, for higher levels of simulation, simplified models for the switch and the
converter must be implemented, in order to minimise convergence problems and
reduce the run times.
There are several commercial version of Spice that operates on personal
computer under several popular operating systems. One commercia l version of

1 University of Oradea, 5 Armatei Române 410087 Oradea; aschiop @uoradea.ro
2 University "Politehnica" Timiș oara, 2 Bd. V. Pârvan, 300223, Ti mișoara

34 Adrian Șchiop, Viorel Popescu 2

Spice is called PSpiceTM. It contains models for basic circuit elements (R; L; C,
independent and controlled sourc es, transformer, transmission l ine), switches, and
most common semiconductor devices: diodes, bipolar junction tra nsistors (BJT’s),
junction field-effect transisto rs (JFET’s), MESFET’s, and MOSFE T’s. PSpiceTM is
mainly applied to simulate electronic and electrical circuits f or different analyses,
including dc, ac, transient, zer o pole, distortion, sensitivity , and noise. SPICE uses
the nodal approach with a variable-time-step integration algori thm so that it can
correctly simulate switching powe r electronic circuits. Using t he analog behavioral
modeling (ABM) blocks facilitates the simulation of control sys tems in PSpiceTM
A/D (a commercial version of Spice by MicroSim). However, there are no specific
models for electrical machines, circuit breakers, surge arreste rs, etc. To simulate a
power system, the user has to build the needed models using SPI CE primitives and
basic elements.
Sometimes, users of PSpiceTM claim that the convergence problems are so
severe that its use for simulations of power electronics circui ts is just not possible
or worth the effort. However, this is absolutely not true and w i t h t h e p r o p e r
techniques of gate signal generation, we can simulate just abou t any given circuit
with little or no convergence problems. In addition, if converg ence problems are
avoided, simulations run much faster and larger numbers of indi vidual transitions
can be studied. This is achieved by generating gate signals tha t are slightly less
s t e e p t h a n i n r e a l c i r c u i t s u s i n g a n a l o g b e h a v i o r a l e l e m e n t s . T his gives a lot of
insight into the cycle by cycle as well as the system level beh avior of a power
electronics circuit. In this fashion, the function of an existi ng, as well as the
expected performance of a new, proposed circuit, can be studied . An excellent
application for these cycle-by-cycle simulations is the develop ment and
verification of control strategie s for the power semiconductors .
The aim of this paper is to present the capabilities of PSpiceTM in simulating
power electronics circuits, induction machines and induction mo tor drives. We
present PSpiceTM simulations of voltage source inverters with two levels, induc tion
machine fed by three-phase voltage source inverter and of vecto r control of
induction machine when exact mot or parameters are known. These examples
represent pure system level simu lations, which could have also been done using
programs like Matlab/SimulinkTM.
2. SIMULATION OF THREE PHASE VOLTAGE SOURCE INVERTER
WITH PSPICETM
To illustrate the capabilities of the PSpiceTM simulation program, we present
an example that shows a complete three-phase inverter bridge us ing six power
MOSFETs. This circuit is shown i n Fig. 1. Note that freewheelin g diodes are an

3 Simulation of power electronics circuit and motor drives 35

integral part of every power MOSFET and are not shown separatel y. The inverter
drives a three-phase load, which could represent an induction m otor for a singular
operating point. The load is connected to the inverter output t erminals with so-
called connection bubbles.

Fig. 1 – Circuit for a three-phase inverter.
Due to the number of elements involved, the circuit for the gat e drive signal
generation is contained in a hierarchical block named PWM_Gener ator presented
in Fig. 2.

Fig. 2 – PWM generation sub-circ uit for a three-phase inverter.
The interface ports named "1+", "1–", "2+"…"6–", provide the connection
between the subcircuit and the ports of the hierarchical block above. Here the

36 Adrian Șchiop, Viorel Popescu 4

connection is to the ports on the PWM_Generator block. The inte rface ports are
created by simply drawing a wire up to the boundary of the bloc k. The name of the
port is initially generic, "Px", where x is a running number, but can be easily edited
by double clicking on the generic name. After drawing a block a nd creating all the
ports, double clicking inside the box will open up a schematic page for the
subcircuit, which has all the appropriately named interface por ts already in it.
Additional details on hierarchical techniques can be found in [ 3]. Careful
inspection of the implementation of the soft-limiter element pr ovided in PSpiceTM
shows, that it uses a scaled hyperbolic tangent function. It ca n easily be seen that
the result of the soft limiter is an output signal with smooth transitions, which is
crucial to avoid convergence problems in PSpiceTM. The soft limiter used here has
an upper and limit of ± 15V and a gain of 500.
PWM Generator compares a tria ngular carrier with three sinusoid al reference
signals, one for each phase. The triangular carrier signal is s ymmetrical with
respect to the time axis. The va lues cover the range from –1.0 to 1.0. For linear
modulation, the amplitude range o f the reference signals is lim ited to the amplitude
of the triangular carrier, e.g. 1V. The ratio of the reference wave amplitude and the
carrier amplitude is called amplitude modulation ratio "m_a". I n the circuit shown
in Fig. 1 "m_a" has a value of 0.8. This value is defined by a parameter symbol and
represents a global parameter, which is visible throughout all levels of the
hierarchy.
In Fig. 2 the control functions for the "E_x+, E_x–" sources, w here x denotes
the phase a, b or c, are chosen such that the activation voltag e levels are ± 2 V. If
the output voltage of the soft limiter is between –2 V and +2V, no MOSFET is
activated, and shoot-through, mean ing a short-circuit between t he positive and
negative bus, is avoided.

Fig. 3 – Output waveforms of the three-phase inverter with MOS FET.

5 Simulation of power electronics circuit and motor drives 37

Figure 3 shows the simulation results for the three-phase inver ter. The time
scale is slightly stretched to show the details of the PWM sign als better. The graph
represents the line-to-line voltage VAB and load currents for all three phases. Due to
the inductors contained in the load, the current cannot instant aneously change and
follow the PWM signal. Therefore the load current is an almost pure sinusoid with
very little ripple. This is repre sentative of the line currents in induction motors.
3. SIMULATION OF INDUCTION MACHINE FED
BY THREE-PHASE INVERTER
The start-up of an induction motor, fed by the three-phase inve rter shown in
Fig. 1, is shown. For this purpose, an induction motor replaces the simple passive
load in Fig. 1. The induction motor symbol represents the elect romechanical model
of an induction motor. The model is suitable for studies of ele ctrical and
mechanical transients as well as steady state conditions. The i nduction motor
model has been derived for a two-phase equivalent motor. Attach ed to the motor is
a bidirectional two-phase to three-phase converter module. This module is voltage
and current invariant. This means that the voltage and current levels in the two-
phase and the three-phase machine are equal. Consequently, the power in the two-
phase machine is only 2/3 of the power in the three-phase circu it. In Fig. 4 the
motor is represented by a custom symbol called "Motor l". A sim ple hierarchical
block could have been used for the motor, but a custom symbol h as been created to
achieve a more realistic and pleasing graphical representation.

Fig. 4 – Induction motor start-up with three-phase inverter cir cuit.
The d-q model of induction machine is presented in Fig. 5. The upper portion
of this subcircuit represents the electrical model. The task of the electrical model is
to calculate the stator and rotor currents, where the stator vo ltages and the
mechanical speed of the machine are input parameters.

38 Adrian Șchiop, Viorel Popescu 6

Fig. 5 – Subcircuit for d- q induction motor model.
The equation system for the electrical model is given by equati on (1). The
theory for this equation system is derived in [4]. The equation system and the
model are formulated for the stationary reference frame.
;
00








+ ω− ω−ω + ω++
=




rqrdsqsd
r rot re m mere r rot me mm s statm s stat
qd
IIII
pL R L pL LL pL R L pLpL pL RpL pL R
VV
0 00 0
(1)
Ls=L m+L sl; Lr=L m+L rl; p = d/dt. (2)
The bottom of Fig. 5 represents the mechanical model. This circ uit calculates
the internally generated electromagnetic toque using the stator and rotor currents as
input values. The equation for the torque is given by (3) [4]:
Te = (3/2) p(IsqIrd – IsdIrq). (3)
Using the generated torque, the load torque and the moment of i nertia, the
angular acceleration can be calculated. Integration of the angu lar acceleration
yields the rotor speed, which is used in the electrical model. Since typical induction
machines are three-phase machines, it is often desirable to hav e a machine model
w i t h a t h r e e – p h a s e i n p u t . T h e r e f ore a bidirectional two-phase t o three-phase
converter module, which can be attached to the motor, has been developed. A
subcircuit for this module is shown in Fig. 6. This circuit is truly bidirectional,
meaning that the circuit can be fed with voltage or current sou rces from either side.
An interesting detail of the subc ircuit is the three-phase swit ch on the input. This
switch is necessary to ensure a stable initialization of the si mulator in case the
machine is fed with a controlled current source. The switch pro vides an initial

7 Simulation of power electronics circuit and motor drives 39

shunt resistor from the three-pha se input to ground. Soon after the simulation has
started, the switch opens and l eaves only a negligible shunt co nductance to ground.

Fig. 6 – Subcircuit for ABC-DQ transformation.
Fig. 7 shows the results for the start-up of the induction moto r for the circuit
of Fig. 4. The motor's parameter is presented in Fig. 4. The to p trace in Fig. 7
shows the developed electromagnetic torque. The scale for this graph is 1V =
= 1 Nm. The graph below shows the mechanical angular velocity w ith a scale of
1 V = 1 r a d / s . B e l o w t h e g r a p h f o r t h e r o t o r s p e e d , a l l t h r e e i nput currents are
shown. Input voltage is the PWM waveform shown in the bottom gr aph.

Fig. 7 – Induction machine with three-phase inverter.
4. SIMULATION OF AC INDUCTION MACHINES
USING VECTOR CONTROL
This example will demonstrate the use of PSpiceTM f o r s i m u l a t i o n s o f a c
induction machines using Field Oriented Control. The basic idea of field oriented

40 Adrian Șchiop, Viorel Popescu 8

control is to inject currents into the stator of an induction m achine such that the
magnetic flux level and the production of electromagnetic torqu e can be
independently controlled and the dynamics of the machine resemb les that of a
separately excited dc machine without armature reaction [5]. Us ing induction
motor model for the synchronous reference frame, the d input of the induction
machine would correspond to the field current that produces the flux, and q input to
the current component that produces electromagnetic torque. The frequency of ac
voltages and currents that fed induction motor are mostly deter mined by the rotor
speed to a small extent by the commanded torque. We still suppl y dc values
representing the commanded flux and torque but we transform the se dc values to
appropriate ac values. We will assume that we can measure the a ctual rotor speed
with a sensor. If we add the slip speed, that we determine math ematically from the
torque command, to the measured rotor speed, we obtain the sync hronous speed for
the given operating point. With this synchronous speed we can t ransform the dc
flux and torque command values from the synchronous reference f rame to the
stationary reference frame. We accomplish this by using a rotat ional transformation
[4] according to the matrix equation (4). θ angle can be interp reted as the
momentary rotational displacement angle between two Cartesian c oordinate
systems; one containing the input values and the other one the output values. This
angle is obtained by integration of the angular velocity which the coordinate
systems are rotating.
.) cos() sin() sin( ) cos(
__
__




θθθ−θ=

inqind
outqoutd
VV
VV
(4)
Fig. 8 shows the top level of a simulation example that impleme nts vector
control for induction machine with a stationary reference frame .

Fig. 8 – Indirect vector control.
The objective of the speed loop is to keep the speed at its ini t i a l v a l u e o f
182 rad/s, in spite of the load torque disturbance at t = 2 s. We will design the
speed loop with a bandwidth of 25 rad/s and a phase margin of 6 0 degrees [6].
Figure 9 shows the subcircuit for the vector control unit. The central part is a
vector rotator for positive direction. This element transforms the dc reference

9 Simulation of power electronics circuit and motor drives 41

values for the flux (d axis) and the torque (q axis) to the sta tionary reference frame.
The input angle for the vector rotator is the integral of the s ynchronous angular
velocity. The signal called "Wmech" is the measured rotor speed . This speed is
multiplied with the number of pole-pairs to obtain the electric al angular velocity.
Then the slip value appropriate to the torque command is added and the resulting
signal is routed through an integrator to generate the input an gle for the vector
rotator. In the d axis, a differentiator is used in a compensat ion element which
assures that the actual flux in the machine follows the command ed signal without
delay.
PSpiceTM simulation results are presented in Fig. 10 for electromagneti c
torque, load torque, and speed variation.
Fig. 9 – Sub-circuit for indirect vector control. Fig. 10 – Spi ceTM simulation results.
Unlike Matlab/SimulinkTM environment, PSpiceTM can’t accomplishes the
start of simulation from steady state because it can’t calculat es the initial values of
the currents and fluxes for this state. As a result, for visual ization the steady state in
PSpiceTM, the length of simulation will be chosen sufficiently large, s o that this
state occurring. For PSpiceTM simulation, induction motor starts with load torque
TL = 12.64 Nm, the steady state is achieved around 0.5 s and at t i m e t = 2 s TL
suddenly goes to one half of initial value. For the sake of com parison between the
PSpiceTM and other available software, we have considered Matlab/Simuli nkTM. In
Matlab/SimulinkTM it was supposing that induction motor work in steady state wit h
load torque TL = 12.64 Nm and at time t = 0.1 s TL suddenly goes to one half of
initial value. The initial values of the currents and fluxes we re calculated by using
an initializing m file.The simulation results are presented in Fig. 12. It is to b e
mentioned that there is very good agreement between the results obtained by the
PSpiceTM in Fig. 11 and Matlab/SimulinkTM in Fig. 12. The SpiceTM simulation
results from Fig. 11 are the same like in Fig. 10, but for anot her scale.

42 Adrian Șchiop, Viorel Popescu 10

Fig. 11 – SpiceTM simulation results. Fig. 12 – Matlab/SimulinkTM results.
5. CONCLUSIONS
This paper shows how power electronics circuits, electric motor s and drives,
can be simulated with PSpiceTM software. A simulation example is presented, and
the results are compared with t hose obtained with Matlab/Simuli nkTM.
Received on December 6, 2005
REFERENCES
1. H. Dommel, Electromagnetic transients program reference manual (EMTP) theo ry book , Contract
DE-AC79-81BP31364, July 1995.
2. A Vladimirescu, The SPICE BOOK , John Wiley & Sons, Inc., New York –London –Sydney, 1994.
3. Ș. Andrei, PSpice–Analiza asistată de calculator a circuitelor electronice Edit. ICPE, Bucharest,
1996.
4. B. K. Bose, Modern Power Electronics and AC Drives , Prentice Hall PTR, Upper Saddle River,
2002.
5. A. M. Trzynadlowski, The Field Orientation Principle in Control of Induction Motors , Kluwer
Academic Press, Boston, 1994.
6. A. Șchiop, Analysis and Design of Speed Controller for Vector Controlled I nduction Motor Drives ,
EMES, 2003, Oradea, pp. 122-128.