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

PSpice Examples for EE-202
Hadi Saadat

bullet1 Download PSPICE Schematic Files for EE-202



Example 1


The switch in the circuit below has been closed for a long time.  Switch is opened at time t = 0.  Use PSPICE and PROBE to obtain the natural response vc(t) and ic(t).  From vc(t) obtain the circuit time constant. By inspection the initial voltage across the capacitor is given by v(0 ) = 8 volts, and the time constant of the circuit t = RC = 1 sec.  For a complete display of the waveform choose the final time of the transient analysis to be five time constants.



Schematics Netlist


V_V1         1   0  DC 18 

R_R4         1   $N_0001  10k

R_R1         2   0  30k

X_U1         $N_0001   2  Sw_tOpen PARAMS: tOpen=0 ttran=1u Rclosed=0.1m +  Ropen=100G

R_R2         2   3  20k

C_C1         3   0  45U IC=8

R_R3         3   0  40K


In PROBE, select plot control and add plot to create two graphs on the screen. Use select graph, up and down key to obtain a plot of voltage V(3) and current I(C1).  On the voltage graph draw a line at  .3678*8 and use the cursor command to locate the time constant. 

Top of Page

Example 2

Consider the network below in which the voltage input is a square pulse as shown.  Use the VPWL function to generate this square pulse.  Use PSPICE and PROBE to obtain the transient response of the capacitor voltage and capacitor current separately on one page.  In the Transient Analysis use a final value of 6 second.  On the voltage graph add a trace at 63.2% of capacitor final voltage and use the cursor command to locate the circuit time constant.




Schematics Netlist


V_V1         1   0 

+PWL 0 0 0.000001 9 3 9 3.000001 0

R_R1         1   2  6K

R_R2         2   3  4K

C_C1         2   0  100U IC=0

R_R3         3   0  8K


Top of Page


Example 3


In the series RLC circuit shown the switch is closed at t = 0. The initial voltage across the capacitor is 3 volts.  The resistance in the circuit is variable.  Obtain the transient response for the voltage across the capacitor for R = 10W, 50W, and 100W.  In the Transient Analysis use a final value of 50 ms.


The Parametric Sweep can be used to change the value of the resistor R1.  to do this get a part called PARAM from Special.slb and place it in your circuit. Double click on the text PARAMETERS.  The attributes allows you to define up to three different variable parameters.  For NAME1= define a parameter say R_x, and for VALUE1= set an initial value of 10. Click the OK button to accept the attribute.  We must now change the value of R1 to the name of the parameter.  Double click on the value of R1 and in place of its value type in the text {R_x}.  Next select the Analysis and then Setup and click the Parametric button. Mark Global Parameter, set Name to R_x. Under Sweep Type, mark Value List and set the Values: to 10 50 100. Perform the simulation.


In the Probe, from Tools pull-down menu select Cursor and check the Display and use Peak to find the peak value of the response and the time to reach this peak for the underdamped response. From the Tools pull-down menu use Label and Mark to mark the values for the peak point.


Schematics Netlist


V_Vs         1    0    DC 12 

L_L1          2    3    0mH IC=0

C_C1         3    0    80U IC=3

R_R1         1    2    {R_x}



Top of Page

Example 4

In the circuit shown the uncharged capacitor is charged for a duration of 50 seconds, it is then discharged immediately.  Use Spice and Probe to obtain the capacitor voltage during charging and discharging process.


  We can use a SW_tOpen and a SW_tClose switch  to simulate the charging and discharging process. Since the switch is opened after 50 seconds we set tOpen = 50, and tClose = 50.  The resistance Rclosed is set to a very low value (0.01m), and the resistance Ropen to a very high value 1000G.


Schematics Netlist


V_Vs        1    0   DC 5 

R_R          $N_0001   2   100k

C_C          2    0   100U IC=0

X_U5        1   $N_0001 Sw_tOpen PARAMS: tOpen=50 ttran=50 Rclosed=.1m

+  Ropen=1000G

X_U13      $N_0001 0 Sw_tClose PARAMS: tClose=50 ttran=1u Rclosed=.01m

+  Ropen=1000G

Top of Page

Example 5

The capacitor in the RC circuit of Example 4 is being charged for 10 seconds and then discharged for the next 10 seconds repeatedly. Use Spice and Probe to obtain the capacitor voltage for this cyclic charging and discharging process up to 100 seconds.



We can use a VPULSE source to simulate the on off switching action.  The pulse has an initial value of 0 V, a final value of 5 V, a pulse width of 10 seconds and a period of 20 seconds.



Schematics Netlist


R_R         1    2  100k

C_C         2    0  100U IC=0

V_Vs       1    0 

+PULSE 0  5  0  0  0  1 0  20

Top of Page


Example 6

The voltage pulse shown is applied to the series RLC circuit as shown. Obtain the response for the voltage across the capacitor.  Assume the initial charge on the capacitor is -5 V.



We can use the Piecewise Linear Voltage source VPWL to represent the above pulse. The VPWL by a series of points.  Each pair of values

(T1, V1) specifies the time and the value.   Specified times T1, T2, T3, ... must be continuously increasing.


Schematics Netlist


V_V1         1    0 

+PWL 0 ‑5 0.00001m 5 25m 5 25.00001m ‑5 50m ‑5 50.00001m 0

R_R1         1    2    50

L_L1          2    3    0.125

C_C1         3    0    1U IC=‑5




Top of Page

Site maintained by Hadi Saadat