PSpice Examples for EE-230
Part 1 AC Power and Three-phase Circuits For the
circuit shown, use PSpice and Probe to graph the instantaneous voltage, current
and power over one cycle.
The initial
current in the inductor is given to be -10.1826 A. The reactor inductance is
.
Select Transient
analysis, set the final time to 16.6667 ms, and the Step Ceiling to 0.01
ms. In Probe plot the instantaneous voltage V(1), and from Plot add Y-axis and
the trace for current I(R1). Repeat to add the Y-axis and the trace for the
instantaneous power p (t), (in probe for trace expression type V(1)*I(R1)).
The real
power can be expressed as
Select the
power axis and add the traces with Trace Expressions as
8*MAX(I(R1))*MAX(I(R1))/2, and 6*MAX(I(R1))*MAX(I(R1))/2 to display P and Q.
* Schematics Netlist *
L_L1 2 0 15.91549mH IC=-10.1826A
R_R1 1 2 8
V_V1 1 0 +SIN 0 169.71V 60Hz 0 0 0
The result
is shown in the next page.
For the
circuit shown, use PSpice and Probe to graph the real and reactive powers
delivered to the circuit as a function of frequency. Use the AC analysis to
sweep the source frequency from 300 Hz to 500 Hz in steps of 1 Hz and Probe to
obtain one graph showing real and reactive power supplied by the source and
another graph showing power factor as a function of frequency. Determine the source frequency for unity
power factor.
* Schematics Netlist *
R_R1 1 2 50
V_Vs 1 0 AC 20V
L_L1 2 3 795.8mH IC=0
C_C1 3 0 198.94nF IC=0
The circuit
impedance is
The real power
is
and the
reactive power is
The power factor is
In probe,
select Plot control and Add Plot to create two graphs on the
screen. Select X-axis and set the range
to change the frequency axis scale to 350 450 Hz. Using Add Trace plot P and Q with the trace expressions
given by (2) and (3).
Use Plot
Control, select plot and down key to switch to the lower graph and using Add
Trace add the power factor with the Trace Expression as given by (4). Using the cursor command you can move along
the plot with the right or left arrows. The co-ordinates at which the cursor is
located are displayed on the lower right hand of the screen. You can select
between different plots by holding down the control key while pressing the
right or left arrow keys. Using the Label command you can add text, lines and arrows to the plot. The plot produced on
the probe is shown below. From the
plots we see that the circuit changes from capacitive to inductive at the
series resonance frequency where reactive power is zero.
At unity
power factor frequency, f = 400 Hz, P = 4 W
A 3-phase
line has an impedance of 3 + j4 W. The line feeds two balanced three-phase loads that are connected in
parallel. The first load is Y-connected
and has an impedance of 30 + j40 W/phase. The second load is delta connected
and has an impedance of 60 - j45 W/phase. The line is
energized at the sending-end from a 3-phase balanced supply of line to neutral
voltage
(a)
Current in
the line for each phase.
(b)
Current in
each phase of the Y-connected loads.
(c)
Current in
each phase of the delta connected loads.
The line inductance per phase is
The Y-connected load inductance per phase is
The D-connected load capacitance
per phase is
The Schematic and the Netlist are shown in
the following pages. The output files contain the following values for the
magnitude and phase angle of currents.
FREQ IM(V_PRINT1) IP(V_PRINT1)
6.000E+01 8.000E+00 -6.388E-05
FREQ IM(V_PRINT2) IP(V_PRINT2)
6.000E+01 8.000E+00 -1.200E+02
FREQ IM(V_PRINT3) IP(V_PRINT3)
6.000E+01 8.000E+00 1.200E+02
FREQ IM(V_PRINT7) IP(V_PRINT7)
6.000E+01 3.578E+00 -6.343E+01
FREQ IM(V_PRINT8) IP(V_PRINT8)
6.000E+01 3.578E+00 1.766E+02
FREQ IM(V_PRINT9) IP(V_PRINT9)
6.000E+01 3.578E+00 5.657E+01
FREQ IM(V_PRINT10) IP(V_PRINT10)
6.000E+01 4.131E+00 1.766E+02
FREQ IM(V_PRINT11) IP(V_PRINT11)
6.000E+01 4.131E+00 5.657E+01
FREQ IM(V_PRINT12) IP(V_PRINT12)
6.000E+01 4.131E+00 -6.343E+01
From
the above results the currents are:
(a) The line currents
,
(b) Currents in the Y-connected loads are:
,
(c) Currents in the D-connected loads are
,
* Schematics Netlist *
R_R1a 1a 2a 3
R_R1b 1b 2b 3
L_L1a 2a 5a 10.61mH
L_L1b 2b 5b 10.61mH
L_La4 4a 0 106.1MH
L_Lb4 4b 0 106.1mH
L_Lca 4c 0 106.1mH
R_Ra4 6a 4a 30
R_Rb4 6b 4b 30
R_Rc4 6c 4c 30
C_C5 8ca 3c 58.9463UF
R_R7 3c 7bc 60
L_L1c 2c 5c 10.61mH
R_R1c 1c 2c 3
V_Vc 1c 0 AC 200 -240
V_Va 1a 0 AC 200 0
V_Vb 1b 0 AC 200 -120
C_C6 8ab 3a 58.9463UF
R_R5 3a 7ca 60
C_C7 8bc 3b 58.9463UF
R_R6 3b 7ab 60
V_PRINT9 3c 6c 0V
.PRINT AC
+ IM(V_PRINT9)
+ IP(V_PRINT9)
V_PRINT1 5a 3a 0V
.PRINT AC
+ IM(V_PRINT1)
+ IP(V_PRINT1)
V_PRINT2 5b 3b 0V
.PRINT AC
+ IM(V_PRINT2)
+ IP(V_PRINT2)
V_PRINT3 5c 3c 0V
.PRINT AC
+ IM(V_PRINT3)
+ IP(V_PRINT3)
V_PRINT7 3a 6a 0V
.PRINT AC IM(V_PRINT7)
V_PRINT8 3b 6b 0V
.PRINT AC
+ IM(V_PRINT8)
V_PRINT10 8ca 7ca 0V
.PRINT AC
+ IM(V_PRINT10)
+ IP(V_PRINT10)
V_PRINT11 8ab 7ab 0V
.PRINT AC
+ IM(V_PRINT11)
+ IP(V_PRINT11)
V_PRINT12 8bc 7bc 0V
.PRINT AC
+ IM(V_PRINT12)
+
IP(V_PRINT12)
Mutually Coupled Circuits Determine the magnitudes and phase angles of mesh currents in
the coupled circuit shown.
PSpice uses the coupling coefficient to describe the coupled
coils, thus we find K from
The
“dot” convention for the coupling is related to the direction in which the
inductors are connected. The dot is always next to the first pin to be
netlisted. When the inductor symbol, L, is taken from the part library and is
placed without rotation, the “dotted” pin is the left one. Edit/Rotate
(<Ctrl R>) rotates the inductor +90deg, which makes this pin the one at
the bottom. The dotted terminal is always referred to the first node of the inductor
in the Netlist. So always examine the
net list and if the left node is not the dotted side, rotate the inductor in
the schematic until the desired dotted node is the first entry in the Netlist. The part K_linear can be
used to specify the mutual coupling between two or more inductors. The
parameters to be specified are L1, L2, … up to L6, whose values must be set to
the inductors symbols. The coupling value is the coefficient of mutual coupling, which must be specified between
zero and 1. The PSpice schematics
is as shown.
Three IPRINT symbols are inserted
in series in each loop to write the currents in the output file. In the text
box for each IPRINT set AC, MAG and PHASE to YES. From the analysis menu select
the Probe Setup, and disable the Probe. Enable the AC Analysis, select Linear, and set the Total pts to 1, Start
and End Frequencies to 60. Run PSpice
(Analysis, Simulate). The Schematics Netlist is as follows
L_L1 1 2 2.5mH
L_L2 2 3 10mH
C_C1 5 3 500UF
R_R1 2 0 10
V_PRINT3 3 6 0V
.PRINT AC
+ IM(V_PRINT3)
+
IP(V_PRINT3)
V_V1 4 0 DC
0V AC 120V 0
R_R2 6 0 20
Kn_K1 L_L1 L_L2 0.6
V_PRINT2 1 5 0V
.PRINT AC
+ IM(V_PRINT2)
+
IP(V_PRINT2)
V_PRINT1 4 1 0V
.PRINT AC
+ IM(V_PRINT1)
+ IP(V_PRINT1)
The output file contains the following values for the magnitude
and angles of the currents
FREQ IM(V_PRINT1) IP(V_PRINT1)
6.000E+01 1.164E+01 3.133E+01
FREQ IM(V_PRINT2) IP(V_PRINT2)
6.000E+01 2.438E+01 5.200E+01
FREQ IM(V_PRINT3) IP(V_PRINT3)
6.000E+01 4.083E+00 7.719E+01
From the above results, the mesh currents are:
For the circuit shown, use PSpice and Probe to graph the magnitude and phase angle of the output voltage Vo, i.e., V(4) as a function of frequency. Use the AC analysis to sweep the source frequency linearly from 20 HZ to 280HZ in steps of 1HZ. Determine the frequency at which the amplitude of the output voltage Vo is a maximum; find the phase angle at this frequency. Also, find the frequency at which the impedance seen by the source is purely resistive.
First we calculate the coefficient of coupling
The PSpice Schematic is as shown.
The
Schematics Netlist is as follows:
Kn_K1 L_L1 L_L2 0.6
R_R1 1 2 50
R_R2 4 0 40
V_V1 1 0 DC 0V AC
18V 0
C_C1 3 4 11.7UF
L_L1 2 0 200mH
L_L2 3 0 800mH
Since the dotted terminal is always the first pin in the Netlist, L1 and L2 are rotated three
times such that their corresponding nodes are entered as 2 0, and 3 0 respectively.
In probe, Add Plot from the Plot menu to create two graphs on
the screen. Using Add from the Trace
menu plot V(4). From Plot use Add Y axis to create a new Y-axis, and add the
trace for voltage phase angle VP(4). Select Cursor from the Tools menu, select the Display and use Peak to
find the peak voltage. Use Label from the Tools menu and Mark the values at the
peak position. Switch the Cursor to
phase angle plot and Mark the values at the frequency corresponding to the peak
value. Switch to the lower graph and
use Trace to add the input voltage and the input current phase angles VP(1) and
IP(R1). Use Cursor and Mark to get the
frequencies at 0. The Probe result is as shown. From the graph the maximum
output voltage is V =
For the circuit shown, L1 and L2 are mutually coupled with a coupling coefficient of K = 0.5. Also, L1 and L3 are mutually coupled with a coupling coefficient of K = 0.9. Use PSpice and Probe to graph the magnitude of the output voltage Vo as a function of frequency. Use the AC analysis to sweep the source frequency
linearly from 450HZ to 500HZ in steps of 0.1HZ. Determine the frequency at which the amplitude of the output
voltage Vo is a maximum. If bandwidth is the frequency range within 0.707 of the peak value, find
the bandwidth.
Two K_linear parts are used to specify the mutual
coupling between L1, L2, and L1, L3. Since the dotted terminal is always
the first pin in the Netlist, L3 is
rotated once such that the corresponding nodes for L1 and L3 are entered as
2 3, and 0 3 respectively.
The PSpice Schematic is as shown.
The
Schematics Netlist is
L_L2 3 4 1mH
V_V1 1 0 DC 0V AC 1V 0
L_L1 2 3 4mH
R_R1 1 2 1270
C_C1 2 0 50UF
Kn_K1 L_L1 L_L2 0.5
R_R2 4 0 10K
Kn_K2 L_L1 L_L3 0.9
|
Download 
The PSpice Schematic is as shown.
, and the reactive power as
(rms), 60 Hz.
, 
and
, 
and
at 60 Hz.
