Clic ici pour langue française Ressources
French Language Resources
Power System Analysis

PSpice Examples for EE-230
Hadi Saadat

 

bullet1 Download PSPICE Schematic files for EE-230

 

 

 

Part 1 AC Power and Three-phase Circuits

Example 1

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

. The PSpice Schematic is as shown.

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 , and the reactive power 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.

 

 

 Top of Page

Example 2

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

 

 Top of Page

Example 3

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 (rms), 60 Hz.  Determine  

(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

, , and

 

(b) Currents in the Y-connected loads are:

,  , and

 

(c) Currents in the D-connected loads are

, , and

 

* 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)   

 

 Top of Page

 

Mutually Coupled Circuits

Example 4

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:

 

 Top of Page

Example 5

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  = at 60 Hz.  From the lower graph, the input impedance is purely resistive at frequencies 54.147Hz, and 62.495 Hz.

 

 

 

 Top of Page

 

Example 6

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

L_L3         0                 3          9mH

 

Use Add from the Trace menu to plot V(4).  From plot use the X_Axis Settings and set the range from 450 Hz to 500 Hz. Select Cursor from the Tools menu, check the Display and use Peak to find the peak voltage. Use Label from the Tools menu and Mark the values at the peak position.  Add a trace at 0.707 of the peak value.  Use Cursor to Mark the corner frequencies at the intersection with the 0.707 line. Determine the bandwidth and Mark it on the graph. The probe result is shown.  From the graph the maximum output voltage is  at 479.9Hz.  The corner frequencies are f1  = 478.383Hz, f2  = 481.363Hz and the bandwidth is approximately 3.0 Hz.

 

 Top of Page

 

Example 7

A 1200/120 V single-phase transformer has the following primary and secondary winding impedances, HV winding: , LV winding: . The voltage at the primary side of the transformer is (rms), 60 HZ.  Transformer is supplying a load of  at its low voltage terminal.  Determine the load voltage and current.

 

 

From the given reactances at 60 HZ, the inductances are given by

.

 

We can use K3019PL non-linear core to model the transformer, to model the ideal transformer the coupling coefficient is set to 1.  The L1_Turns and L2_Turns values are set to 1200 and 120 respectively. The PSpice Schematic is as shown.

 

The Schematics Netlist is

 

R_R2         4      5        0.03 

L_L2         5       6        0.2122mH 

R_R1         1      2        2 

R_RL         6      7        0.96 

L1_TX1     3     0         1200

L2_TX1      4    0         120

K_TX1      L1_TX1     L2_TX1 1 K3019PL_3C8

L_L1         2      3         18.568mH 

L_LL         8     0         1.90985mH 

V_V1         1     0         DC 0V AC 1335 3.85

 .PRINT         AC

+ VM([6])

+ VP([6])   

V_PRINT2         7 8 0V

 .PRINT        AC

+ IM(V_PRINT2)

+ IP(V_PRINT2)   

 

Double-click on the VPRINT1 symbol. Select 'SIMULATIONONLY=' and for value type V(6) VP(6).  In the text box for VPRINT1 set AC, MAG and PHASE to YES.  Also in the text box for 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 output file contains the following values for the magnitude and phase angle of currents.

 

FREQ              VM(6)                         VP(6)      

6.000E+01       1.200E+02                   3.730E-04

FREQ              IM(V_PRINT2)           IP(V_PRINT2)

6.000E+01       1.000E+02                   -3.687E+01

 

That is,

 

Example 8

A 300/120V ideal autotransformer is supplying a load  from a 300 V source.  Find the secondary load current.

 

We can use K3019PL non-linear core to model the transformer, to model the ideal transformer the coupling coefficient is set to 1.  For L1_Turns, we use , and L2_Turns 120. PSpice will not allow a loop of all inductor and voltage source.  To avoid this in the primary loop a negligible resistance ( ) is added. The PSpice Schematic is as shown.

The Schematics Netlist is

 

L1_TX1         1            4          180

L2_TX1         2            0          120

K_TX1          L1_TX1 L2_TX1 1 K3019PL_3C8

V_V1            1                         0          DC 0V AC 300 0

R_RL            3            0          0.96 

.PRINT         AC

+ VM([2])    

V_PRINT2   2             3          0V

 .PRINT        AC

+ IM(V_PRINT2)    

R_Rx          4               2          1U 

Double-click on the VPRINT1 symbol. Select 'SIMULATIONONLY=' and for value type V(2). In the text box for VPRINT1 set AC and MAG to YES.  Also in the text box for IPRINT set AC and MAG 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 output file contains the following values:

 

FREQ              VM(2)      

6.000E+01       1.200E+02

FREQ              IM(V_PRINT2)

6.000E+01       1.250E+02

That is, VL  = 120 V, and  IL   = 125 A.

 

 

Operational Amplifiers

                         

The operational amplifier (called op amp) is an electronic device that has become a versatile network element. The main characteristics of an op amp are very high input resistance, very low output resistance, and very high gain (to the order of 105). By focusing on the terminal behavior of an op amp, one can appreciate its use as a network element without knowledge of its internal behavior.  The PSpice evaluation version has only one op amp (UA741), and only two of these can be used before reaching the component limits.  If you have a circuit with a large number of op amps, you will be forced to use ideal op amps in the evaluation version. The op amp may be modeled as a linear amplifier to simplify the design and analysis of op amp circuits.   A voltage-controlled voltage source can be used to model an op amp in the linear range with reasonable accuracy as shown in the Figure below.

 

 

 

  is a very high value and has a very small value.  For the UA741 op amp, the typical value for A, Ri, and Ro are 105, 2 MEGW, and 75W, respectively.    For ideal op amp Ri = ¥, and Ro = 0 and A must be given a very high number.  A gain of A=1E10 works well and gives ideal op amp answers.   PSpice can represent the infinite input resistance by an open-circuit and zero output resistance by a short circuit, and a very large number can approximate the infinite gain. A gain of 1010 works well, and gives ideal op amp answers.

 

 

 

Top of Pag

 

Example 9 (EE230.Ex9.sch)

 

For the circuit shown below assume an ideal op amp and use Spice to calculate the voltage gain

 

 

A voltage-controlled voltage source (Part E) is used. The voltage gain is set to 1E10.  The input and output node voltages are viewed using the VIEWPOINT part.  The PSpice schematic containing the simulation result is as shown below. 

 

 

Schematics Netlist is

 

V_V1         Vi              0            DC 1V 

E_E            Vo   0        0   Vn    1E10

R_R2         Vn Vo         9K 

R_RL         Vo             0            6K 

R_R1         Vi               Vn          2K 

 

Thus the voltage gain is -4.5.

 

Top of Pag

Example 10 (EE230Ex10.sch)

For Example 9 use a more realistic model with the following parameters

                                   

The PSpice schematic containing the simulation result is as shown below.

 

Schematics Netlist is

R_RL         Vo 0  6K 

V_V1         Vi 0 DC 1V 

R_R1         Vi Vn  2K 

R_Ri         Vn 0  2MEG 

E_E         $N_0001 0 0 Vn 1E5

R_R2         Vn Vo  9K 

R_Ro         $N_0001 Vo  25 

                                                                

Thus the voltage gain is  = -4.5 V approximately the same as the ideal op amp model.

 

Top of Page

 

Example 11 (EE230Ex11.sch)

 

For Example 10 use a  UA741 op amp.  The op amp positive power supply Vcc = 10 V, and the negative power supply is Vee = 10 V. Two parts named BUBBLE are connected to the supply nodes. Click on each BUBBLE to name these terminals Vcc and Vee.  Two DC supply of 10 V with BUBBLES named Vcc, and Vee are made as shown to provide the necessary voltages for terminal 7 and 4 of the op amp.  The PSpice schematic containing the simulation result is as shown below.

 

Schematics Netlist  is

 

R_R1         Vi               Vn                    2K 

R_R2         Vn Vo                   9K 

V_V3         0                Vee                  10V

V_V2         Vcc           0                      10V

X_U1         0   Vn        Vcc   Vee         Vo uA741

V_V1         Vi              0                      DC 1 

R_RL         Vo             0                      6K 

 

Thus the voltage gain is  = -4.499 compared to -4.5 obtained with the ideal op amp model.

 

Top of Pag

 

Example 12 (EE230Es12.sch)

 

Determine the voltage gain in the noninverting amplifier circuit shown. The amplifier parameters are

                                   

 

The PSpice schematic containing the simulation result is as shown below.

 

 

The Schematics Netlist  is

 

V_Vi         Vp 0 DC 1V 

R_Ri         Vb Vp  2MEG 

R_R1         0 Vb  2K 

E_E         $N_0001 0 Vp Vb 1E5

R_R2         Vb Vo  8K 

R_Ro         $N_0001 Vo  25 

R_RL         Vo 0  6K 

 

Thus, the voltage gain is , the same as the ideal op amp voltage gain which is

 

Top of Page

 

Example 13 (EE230Ex13.sch, EE230Ex13b.sch)

In the circuit shown below, determine

 

(a) Use two UA741 op amps.  The op amp positive power supply Vcc = 10 V, and the negative power supply is Vee = 10 V.

 

The PSpice schematic containing the simulation result is as shown below.

 

(b) Use to voltage-controlled voltage source to model the op amps. The parameters of each op amp are

The PSpice schematic containing the simulation result is as shown below. (EE230Ex13b.sch)

 

 

 

Top of Page

 

Example 14

 

The source voltage in the circuit shown uses the PSpice VPWL function to generate a waveform that is zero from 0 to 1 second, jumps to +5 at t = 1 second, jump down to -5 at t = 2 second, jumps back to zero at t = 3 seconds and remains at zero.  The first op amp is an inverting integrator.  The second op amp is a unity gain inverter.  The overall circuit is a noninverting integrator with a gain of .  

 

The output is the integral of the input as shown below. Appling KCL at the inverting node, we get

                                         

For an ideal op amp , and , thus we have

                               

Since the second op amp is a unity gain inverter, we have

Substituting for   and , , and the output is the integral of the input,

Two voltage-controlled voltage sources with gains of 1010 are used to represent the ideal op amps.  The PSpice schematic is as shown.

The Transient analysis is used to simulate the circuit over a period of 4 seconds.  The Probe is used and the graph containing  and  plots is shown in the next page.

 

 

 

Top of Page


Site maintained by Hadi Saadat