Objective:
The experiment is designed to enable you to study ac circuit analysis in considerably more detail than would be possible without the aid of digital computation technique. Magnetic circuits will also be discussed in this experiment. It is assumed that you are already familiar with the PSPICE and have used PSPICE to analyse DC circuits and transients.
Introduction:
In addition to DC circuit analysis and transient analysis, PSpice can be used to analyse steady-state phasor problems. The syntax for an AC sources are very similar to DC sources. Sources in AC circuits are time-variant. They are alternating current and have both magnitude and phase displacement. Practical sources are generally sinusoidal or near sinusoidal. The behaviour of a circuit is normally evaluated with a sinusoidal source. The steady state voltages and currents that are normally used to evaluate the performance of a circuit can be calculated by applying the circuit laws that are applicable to dc circuits.The transient behaviour is also important under some conditions, but the analysis become more complex compared to steady–state analysis.
SPICE is an ideal software tool for simulating a circuit and for studying the behaviour of voltages,currents and power flow under steady-state and transient condition. We have discussed the SPICE representations of circuit elements and sources in previous experiments. In this Experiment we will simulate the steady-state analysis of a circuit and include mutual inductances. Students are encouraged to apply the basic circuits laws and to verify the SPICE results by hand calculation
Mutual Inductances in PSpice
Users of PSpice often need to model inductors that are magnetically coupled. This may occur in steady-state power system simulations, or in power electronic transient circuit simulations where linear or nonlinear transformer models are used. In some cases it is necessary to model weakly coupled inductors. This tutorial will address the issues of modeling magnetic coupling in these circumstances.
Basic Linear Coupled Inductors
Fig-01
In the above figure two inductors are coupled by a coefficient of coupling, k. Their nodes are designated by small integers, and polarity marks have been added. The polarity information is passed to PSpice by the order of the nodes. If the coefficient of coupling is k = 0.8, a valid PSpice coding could be:
*name node1 node2 inductance (comment line)L1 1 2 40mH
L2 3 4 10mH
*name ind1 ind2 k (comment line)
K12 L1 L2 0.8
Note that the polarity marks in the figure are beside nodes 1 and 3 of the inductors. In the listing, these are entered as the leftmost nodes. An equivalent polarity relationship could be indicated by reversing both nodes on both inductors. The coupling of the coils is entered by including a new part that must begin with the letter, K. The "K" part name is followed by a list of the coupled inductors, then by the value of the coefficient of coupling. The coefficient of coupling must occupy the range, 0 £ k £ 1.
Multiple Couplings with Different Values
Free-2
In the above figure, each inductor has mutual coupling with more than one other inductor, but with different coupling coefficient. In this case, PSpice requires a separate "K" part for each coefficient of coupling as shown in the following code:
La 1 2 15mHLb 3 4 12mH
Lc 5 6 10mH
Kab La Lb 0.08
Kbc Lb Lc 0.075
Kca Lc La 0.04
Note that the polarities of the inductors, and therefore the sense of the mutual coupling is accounted for by the order of the nodes entered for the self inductance parts. In this case, different symbols have been used in the figure to assure that it is understood which pairs are coupled and in what sense. In general, if there are n coils, there will be ½ n(n-1) "K" parts needed.
Multiple Couplings with Same Values
Free-03
In the above example, we assume that all inductors share identical coefficients of coupling. This is a reasonable assumption when coil symmetry exists and all coils are wound on a common core. Under these conditions, PSpice allows a single "K" part to describe all the coupling.
La 1 2 25uHLb 3 4 50uH
Lc 5 6 100uH
Ld 7 8 200uH
Kall La Lb Lc Ld 0.98
Again, the polarity information is entered by the order of the nodes for the self inductances. Since all the coupling coefficients were the same, only one "K" part was needed instead of six.
Circuit Example
a) Construct the circuit in Figure 5.1 for both netlist and schematic.
b) Setup your PSPICE simulation to perform a transient analysis over a suitably chosen interval of time. Take V1 to be of Magnitude 100V.Choose a suitable frequency.
c) Observe the waveshapes of currents through and voltages across through the resistor ,inductor and capacitor and mention their phase relationship.
Observe the mentioned waveshapes for the series resonance condition
No comments:
Post a Comment