THEORY
Energy delivered by a source can be stored in an inductor or capacitor.
Once initial conditions are known, a voltage in an capacitor (V0) and current in an inductor (I0), the application of Kirchhoff laws results in the circuit equations that will yield the voltage and current relationships with time. The definitions of the current/voltage relationships are applied for the storage elements and for resistors (Ohm’s Law) and again, first order ordinary differential equations result.
The solution leads to equations that define an exponential build up with time of any energy that is stored.
Fig-01
In both instances, the growth in current and voltage is exponential with time to a final value determined by the circuit.
The time constant τ is defined as shown to characterize the exponential growth in
current/voltage in the inductor/capacitor. It does this through the factor e-t/τ. After a time
interval of 5 time constants, the factor is within 1% of its final value.
Inductors in PSpice
This part name begins with the letter, L, in column 1 of the source listing
The figure shown above shows the circuit symbol for an inductor with node designations of "1" and "2," an initial current of 2.5 A, and a value of 50 mH. An appropriate code listing for entering this element into a PSpice circuit file is:
*name nodelist L_val
Lag 1 2 50m IC=2.5
Note that the initial current is assumed to flow from the first node in the node list through the inductor towards the second node in the node list. If there is a need to change the direction of this initial current, either reverse the order of the nodes in the node list or place a minus sign in front of the value of the initial current. For better readability, the above line could be written as:
Lag 1 2 50mH IC=2.5A
The "H" for henrys and the "A" for amps will be ignored by PSpice.
Capacitors in PSpice
The part name for a capacitor must start with the letter, C.
An appropriate code listing to represent this capacitor in a PSpice listing is:
*name nodelist C_val
Cfb 4 5 50u IC=20
The capacitance of the above element is 50mF. This can be represented as "50u" in PSpice. Note that the polarity of the initial voltage (as shown) is such that the positive side is the first node in the list with the negative side on the second node in the list. To reverse the polarity of the initial voltage for the simulation, either reverse the order of the nodes in the node list or place a minus sign in front of the value in the "IC=" phrase. For better clarity, the above capacitor could be coded as:
Cfb 4 5 50uF IC=20V
PSpice would ignore the "F" for farads and the "V" for volts.
Using a subcircuit for a switch
The element statement for a subcircuit is similar to any other element. The format is as follows:
Xname N1 N2 N3 ... SUBNAME
in which Xname refers to the element (subcircuit) being used; N1, N2, N3 are the nodes to which the external nodes of the subcircuit are being connected, and SUBNAME is the name of the subcircuit being used.
An example, using the subcircuit of the switch for transient analysis is given below.
The subcircuit is called by X_U13. The name of it is Sw_tClose. The switch is normally open and tClose defined the time to close the switch. The resistance Rclosed is set to a very low value (0.01m), and the resistance Ropen to a very high value 1000G.
X_U13 $N_0001 0 Sw_tClose PARAMS: tClose=50 ttran=1u Rclosed=.01m
+ Ropen=1000G
Use of the .TRAN command
This is the command that passes the user's parameters for performing the transient analysis on a circuit to the PSpice program. There are four time parameters and an instruction to use the initial condition rather than calculated bias point values for starting conditions. First, we show a sample .TRAN statement and then we will describe its parameters.* prt_stp t_max prt_dly max_stp
.TRAN 20us 20ms 8ms 10us UIC
In the above statement, the "20us" value labeled "prt_stp" (print step) is the frequency with which data is saved. In this case, the system variables are stored each 20ms of simulation time. The actual time steps used by PSpice may be different from this. The second parameter, "20ms," labeled as "t_max" (final time) is the value of time at which the simulation will be ended. Since PSpice starts at t = 0, there will be a total of 20ms time span of simulation for the circuit. The third parameter, "8ms," labeled as "prt_dly" (print delay) is the print delay time. In some cases, we do not want to store the data for the entire time span of the simulation. In our sample statement shown above, we ignore the data from the first 8ms of simulation and then store the data for the last 12ms. Most of the time, this parameter is set to zero or not used. The fourth parameter, "10us," labeled as "max_stp" (max step) is the maximum time step size PSpice is allowed to take during the simulation. Since PSpice automatically adjusts its time step size during the simulation, it may increase the step size to a value greater than desirable for displaying the data. When the variables are changing rapidly, PSpice shortens the step size, and when the variables change more slowly, it increases the step size. Use of this parameter is optional. The last parameter in our list is "UIC." It is an acronym for "Use Initial Conditions." Unless you include this parameter, PSpice will ignore the initial conditions you set for your inductors and capacitors and will use its own calculated bias point information instead.
PROCEDURE
1.1.1. Construct the circuit shown in Figure 4.1 for both netlist and schematic. Set the initial current in the inductor to zero.
1.1.2. Setup your PSPICE simulation to perform a transient analysis over a suitably
chosen interval of time, 5τ the time constant.
1.1.3. Calculate the value of the time constant. Make sure you insert units!
τ = _________________
1.1.4. Estimate τ from the plot of the inductor current and compare with the calculated value.
1.1.5.Show graphs of voltage,current, power and energy against time for the inductor L1. Print your results and attach them to your report.
1.1.6. Change L1 to 1mH and repeat above procedure.
Fig-4
1.1.7. Set the initial current in the inductor to 5mA. Run your PSPICE simulation. Print
the trace for the current in the inductor. What is the final value of the inductor
current?
Final Inductor Current = ___________________
1.1.8. Measure how long it takes for the current to rise to 90% of its final value.
Calculate this time with the equation provided. Compare the two results and
calculate the % difference. Show your work.
2.1.1. Construct the circuit shown in Figure 4.2 for both netlist and schematic. Set the initial voltage across the capacitor to zero.
2.1.2. Setup your PSPICE simulation to perform a transient analysis over a suitably
chosen interval of time, 5τ the time constant.
2.1.3. Calculate the value of the time constant. Make sure you insert units!
τ = _________________
Fig-5
2.1.4. Estimate τ from the plot of the capacitor voltage and compare with the calculated value.
2.1.5. Show graphs of voltage, current, power and energy against time for the capacitor, C1. Print your results and attach them to your report.
2.1.6. Change C1 to 10μF and repeat above procedure.
2.1.7. Set the initial voltage on the capacitor to 5Volts. Run your PSPICE simulation.
Print the trace for the voltage in the capacitor. What is the final value of the
capacitor voltage?
Final capacitor voltage = ___________________
2.1.8. Measure how long it takes for the voltage to rise to 90% of its final value.
Calculate this time with the equation provided. Compare the two results and
calculate the % difference. Show your work.
No comments:
Post a Comment