ECEN 2612PSpice AC Analysis(10.0 points)Lab #3
Name:
Partner:
Objectives: To be able to use: (a)OrCAD PSpice to determine voltage and current amplitudes and phase angles in an AC circuit, and (b) to use the AC sweep capability of PSpice to compute and plot the frequency response of a circuit.
- Single-Frequency Analysis (3.0 points)
This circuit has L = 100 mH, R = 1 kΩ, C = 0.05 μF, and the sinusoidal source isdescribed by:
vg = 10 cos(2πf t + 90°) V
where f = 3kHz.
In this step for single-frequency analysis, perform an analytical solution using phasor analysisto find the magnitudes and phases of VL, VR, VC, and the current in the series circuit. Then, you are to use PSpice to find these same magnitudes and phases. Finally, compare your calculated values with your PSpice solutions.
A PSpice schematic representation of this circuit is shown below. Note the use of printer-device parts. Construct this circuit in PSpice, using the VAC part for Vg. Use OrCAD to print your schematic.
(a)These PSpice current and voltage “printers” cause the result of the analysis to be printed in the .OUT output file. In order to get the desired output data, we must edit the property spreadsheets for each of these “printer” parts. The spreadsheet can be accessed by double clicking on each part. You must specify the output to be from AC analysis by placing a “Y” (for yes) in the column labeled AC. Also place a Y in the columns labeled MAG and PHASE to have output values in polar form.
Question: How can you get the outputs in rectangular form, i.e., placing a Y in what columns?
(b)Select AC Sweep as the type of analysis. Since we only need a single frequency, set the Start and End “sweep” frequencies to the same value and the Number of Total Points to1. Note that we must specify the source file frequency value in hertz. Try doing this by omitting the End frequency; describe what happens.
(c)Run the analysis and examine the output file (PSpice → View → Output File in the PSpice window, or find it another way). Describe what happens, and what you do to find it.
Find the amplitudes and phase angles for each of the two voltages (VL and VC), and do the same for the one current. Tabulate the results in your report and mark them in your printed .Out file. The results will be found under the heading AC Analysis toward the end of the .OUT file. You could save the .OUT file as a text (*.txt) file for future reference. Always put handwritten notes on your .OUT files, too.
- Swept Frequency Analysis (3.0 points)
Usually AC Sweep is used to vary the frequency of the sinusoidal source, plotting results using Probe. (Did you see “Probe” in (1c) above? Explain.) This type of analysis is called a "frequency response." To run a frequency response, enable AC Sweep using the decade sweep type with 60 points per decade, a start frequency of 150Hz, and an end frequency of 50kHz. Note that PSpice uses Hz and not radians/sec!
Run the analysis and plot ‘IM(R)’. Run it again and plot ‘IP(R)’. Describe briefly on each plot what you have plotted. Now, create one plot with two separate vertical axes to show both of these values together. (Consult the instructor if you can’t figure this out.)
Using the cursor on the IM(R) plot, determine the resonantfrequency (which means what?) and both of the two frequencies at which the current is reduced to 70.7% of itspeak value.
Figure out how to do another plot which gives the “voltage gain” of this circuit. That is, plot M(V(C)/V(Vg)). Note: this formula may need revision to reflect the nomenclature used in your circuit. Consult with the instructor if you have any issues.
- ParametricAnalysis(3.0 points)
Now, change the schematic by replacing the value of R with a "global parameter" named “r_value” contained in curly brackets like this: {r_value}. The curly brackets are used to indicate a global parameter. Thedefault value of such a parameter is specified using the part named PARAM. Double click the PARAM part to specify a default value of r_value; do not use the curly brackets there. Set the default value ofr_value to 1 kΩ, which was your original value of R.
During a swept-frequency analysis, a global parameter can also be swept using a "parametric sweep." Examine the Parametric option under Options and notice the type of information required to specify the Sweep Variable Type and Sweep Type. List the possible Sweep Variable Types and the possible Sweep Types.
Use what you have just learned about AC Sweep analysis and about parametric sweeps to examine the effect of the resistor value on the magnitude response of I(R). Use thislist of values for R: 500 Ω, 1kΩ, and 5kΩ. Print and carefully label the Probe results in your report.
Report: Include all data, results, observations, and answers to questions, written neatly and legibly on the unlined side of standard engineering paper. Use this lab sheet attached as a cover. (1.0 points)
Normally with PSpice work like this, at least one example schematic, one printed .OUT file (for Part 1 ONLY), and several Probe outputs must be included. Write some NOTES and other careful labeling on your PSpice printouts. Set the PSpice “print area” appropriately for your circuit schematic to allow for maximum clarity of your work. Print PSpice work using the PSpice print capabilities. Donot copy/paste unless you can do that with good resolution.
Don’t be afraid to experiment (carefully) with PSpice to help you learn how to do the things you want to do. And use the PSpice helps, too.
This is due at the beginning of the next lab session.
P.Munro 26-May-2017 03:02 PM (save date)Page 1of2