SlideShare a Scribd company logo
1 of 67
Download to read offline
UNIVERSITY OF ENGINEERING & TECHNOLOGY
2017
Power Electronics
ORCAD Simulation
AC/DC Converters
Dr. Sajid Iqbal
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Table of Contents
1. General Notes Page 3
2. Simulation Notes Page 6
3. Single phase full converter Page 10
4. Three phase semi converter Page 23
5. Three phase full converter Page 36
6. Single phase square wave inverter Page 49
7. Three phase square wave inverter Page 53
Lab Instructor: Dr. Sajid Iqbal 2
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
General Notes
1. How to make a project
1. Open OrCAD Capture
2. Go to File => New => Project.
3. Enter a name
4. Choose "Analog or Mixed A/D"
5. Set the location. (You should create a new directory for your project since PSpice will generate a
bunch of project files in this folder.
6. Click OK
7. Choose "Create blank project" and click OK
8. You should see a window where you can draw the schematic (i.e., your circuit diagram).
9. To add parts for your circuit (i.e., resistors, etc.)
a. Go to Place => Parts
b. Click on the library you want to use, or select multiple libraries by holding Ctrl or dragging
the mouse. In the part window you should see at least the ANALOG, BIPOLAR, EVAL,
SOURCE, and SPECIAL libraries (see below for more information on “Parts Notes”)
c. Find the part you want to add and press OK
d. Click where you want to place the part on your schematic. (Press R to rotate the part by 90
degrees)
e. Use wires to connect part to complete your circuit
10. Run simulation by choosing simulation type (see below for more information under “Simulation
Notes”)
11. Plot your output (see below for more information under “Simulation Notes”)
2. Ground
There are many types of grounds (common points in the circuit, noise reduction, etc.) PSpice uses
node-voltage method for circuit simulation and, therefore, needs a reference node with “zero
voltage”. This is the 0/SOURCE ground. You need to have it in your circuits! (It looks like a ground
symbol with a zero) If you don't, PSpice may complain of "floating nodes" even if you have a
ground.
Lab Instructor: Dr. Sajid Iqbal 3
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
To place the ground on the circuit Go to Place => Ground and choose 0/source (If you don't see the
"source" in the Libraries section, you will need to add the source library. See Part Notes below).
3. Mega- (i.e. mega-ohm, mega-hertz)
When you need to enter a "Mega-" (106
) unit use "MEG". (Case doesn't matter). "M" is NOT mega,
it is milli (10^-3). Example: for 6.5 megahertz, enter "6.5 Meg", for 3 milli-amps, enter "3 m"
4. All parts must have unique names.
You can't have two parts named "R1" in your circuit. If you are copying and pasting parts or circuits,
you will need to rename your parts because PSpice doesn't do this automatically.
5. Labeling Nodes:
I recommend you use aliases to label your input and output nodes. This makes your node easier to
find. V(Vout) is simpler than finding V(R1:1)
a. Go to Place => Net Alias
b. Enter a name, i.e., Vout or Vin
c. Place the label close to a node
d. Example below shows a simple circuit with aliases:
Lab Instructor: Dr. Sajid Iqbal 4
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Lab Instructor: Dr. Sajid Iqbal 5
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Simulation Notes
1) DC Bias:
The response of the circuit to DC sources is always calculated. To display DC bias voltages and
currents on your circuit after you run the simulation, go to PSpice => Bias Points, and check Enable,
Enable Bias Current Display, and/or Enable Bias Voltage Display
2) Parametric Sweep
This simulation is used to find the response of the circuit (e.g., current in one element) if the value of
an element (R1 in the example below) is changed. To do so:
a. Change the value of the part to {RL} (use curly braces, name is arbitrary)
b. Go to Place => Part
c. Add a PARAM/SPECIAL part to your schematic
d. Double click on the PARAM part
e. Click “New Column”
f. Set the name to RL (same name as in “a” but with no curly braces)
g. Set the value to something, e.g., 1k (this is the value that is used in calculating DC bias
values, choose somewhere in the range of your sweep).
h. Click "Display"
i. Select "Name and Value" and press OK
j. Your schematic should look like as in figure below
k. Go to PSpice=>Edit Simulation Profile.
l. Change the following settings, Analysis type: DC Sweep ,Options: Primary Sweep, Sweep
variable: Global parameter, Parameter name: RL, Setup the sweep type how you want. (Note
that if you are sweeping resistance, you can't start at 0)
Lab Instructor: Dr. Sajid Iqbal 6
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
m. Click OK, and go to PSpice => Run to run the simulation.
3) Frequency Domain Simulations
1. Set up your circuit with VAC voltage sources.
2. Go to PSpice => Edit Simulation Profile
3. Select the "Frequency Domain" Analysis type
4. Select the frequency range of interest. Don't start Frequency sweeps at 0!
5. Set the points/Decade to be at least 20.
Bode Plots
1. Use a logarithmic x-axis for the frequency.
2. The magnitude should be measured in decibels. Use the PSpice DB() function to convert to
decibels. For example, DB(V(Vout)/V(Vin)), assuming you have labeled your output and
input nodes with "Vout" and "Vin" aliases. Note that DB(Vout) is NOT the transfer function
in dB.
3. Remember you also need a phase graph (unless instructed otherwise). Use the PSpice P()
function to get the phase angle. For example, P(V(Vout)/V(Vin))
4. Be sure to mark the cutoff points on your bode plots (on both magnitude AND phase graphs).
Remember cutoff is 3dB below the highest point (NOT always at -3dB)
a. Click the "Toggle Cursor" button. (Or go through the menu, Trace => Cursor =>
Display) You will now be able to move the cursor along your plot.
b. Click the "Cursor Max" button to find the highest point. (Or go through the
menu, Trace => Cursor => Max)
c. Click the "Mark Label" button to label that point. (Or go through the menu, Plot
=> Label => Mark)
d. Click the "Cursor Search" button (Or go through the menu, Trace => Cursor
=>Search Commands)
e. Select 1 for Cursor To Move to search along the y-axis
f. Enter "search forward level (max-3)" (don't enter the quotation marks) to move the
cursor to the right to the point which is 3 below the max.
Lab Instructor: Dr. Sajid Iqbal 7
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
g. Or enter "search back level (max-3)" (don't enter the quotation marks) to move the
cursor to the left
h. Click the "Mark Label" button to label that cutoff point.
a. Unclick the Toggle Cursor button to disable the cursor so you can move the label.
b. Double click on the label to edit the text (to add units, or to name the point)
5. It may help to increase the width of the lines in the plot.
• The colored symbol at the bottom of the graph, or on the graph line
• Note you can select all of the lines by going to Edit => Select All
• Right click on the line. Make sure the selection list has Information, Properties,
Cursor 1, and Cursor 2.(If it lists Settings and Properties, you clicked on the
background, not on the line).
• Select Properties
• You can change the width and other settings of that trace
4) Time Domain Simulations
a. Use VSIN for your voltage source instead of VAC (VOFF is the DC offset, VAMPL is the
amplitude, and FREQ is the frequency of the sine wave).
b. For Square and triangular wave, use VPULSE
Lab Instructor: Dr. Sajid Iqbal 8
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Square Wave is the VPLUSE function in the limit of TR = TF = 0 and PW = 0.5 * PER (PER is the
period of the wave). This limit case, however, causes numerical difficulties in calculations. In any
case, we can never make such a square function in practice. In reality, square waves have very small
TR and TF. Typically, we use a symmetric function, i.e., we set TR = TF and PW = 0.5 * PER - 2 *
TR. Thus, for a given frequency we can set up the square function if we choose TR. If we choose TR
too large, the function does not look like a square wave. If we choose TR too small, the program will
take a long time to simulate the circuit and for TR smaller than a certain value, the simulation will
not converge numerically. A good choice for TR is to set it to be 1% of the PER (a period): TR = TF
= 0.01 * PER, PW = 0.48 * PER. This usually results in a nice signal without a huge amount of
computational need. Note that TR does not have to be exactly 1% of PER. You can choose nice
round numbers for TR, TF, and PW.
Triangular Wave is the VPLUSE function in the limit of TR = TF = 0.5* PER and PW = 0
(convince yourself that this is the case). As before, the limit case of PW = 0 causes numerical
difficulties in calculations. So we have to choose PW to be a reasonably small value. A good choice
for PW is to be set at 1% of the PER (period): PW = 0.01* PER, TR = TF = 0.49 * PER (and not TR
= TF = 0.495 * PER so that we get a symmetric function). This usually results in a nice signal
without a huge amount of computational need. Again, note that PW does not have to be exactly 1%
of PER. You can choose nice round numbers for TR, TF, and PW.
Simulation settings
1. Go to PSpice => Edit Simulation Profile
2. Select the "Time Domain (Transient)" Analysis type
3. Enter a Run to time: so that a few periods will be displayed. Remember that the period
(seconds) = 1/frequency (Hz), i.e, if you are using a 1kHz sine wave, it has a 1/1kHz=1ms
period, so use a Run to time of 5ms for 5 periods
4. Set the Maximum step size to be much smaller than the period i.e. for a 1kHz sine wave: It
has a 1ms period, so set a maximum step size of approx .01ms. (This works out to 100 data
points per period).
5. If you don't set the maximum step size, PSpice may choose one which is too big, making
your sine wave look angular and ugly.
Lab Instructor: Dr. Sajid Iqbal 9
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Experiment
Single Phase Full Converter
Instructions:
 All Practice and Exercise Questions must be completed in this lab session for full credit.
 You must show the outputs to the instructor before proceeding to the next question.
 Read this lab manual completely at least once before coming to lab.
Recommended Reading:
 “Power Electronics Circuits Devices and Applications” by Muhammad H. Rashid 3rd
edition.
Objectives:
 The purpose of this experiment is to simulate Single Phase Full Converter.
Tools required:
 Software simulator ORCAD
 Calculator
LAB ACTIVITY:
1. Run the simulation software Orcad on your computer.
2. Go to file and select new project.
3. Name the project with your roll no. like 20XXEXXX and also specify the directory to save
project. Choose Analog or Mixed A/D. Click ok.
Lab Instructor: Dr. Sajid Iqbal 10
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
4. In the next window Check create a blank project and click ok.
5. In the schematic window make the following circuit.
6. Go to place, select part and add all the PSPICE libraries. Then select the following parts and
place on the schematic page.
• Resistor
• Inductor
• Vsine
• Vpulse
• Thyristor S2800N
7. Go to place, select part and place PARAM in the schematic to specify parameters.
8. Double click on PARAMETER after placing it and add variables to it one by one by clicking
on add new column button at the top of spread sheet. Specify the name and value of each
parameter. Use bracket {} as shown in schematic to specify values.
Lab Instructor: Dr. Sajid Iqbal 11
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
9. After placing the components and specifying parameters make the simulation profile. Go to
PSICE and select New Simulation Profile. A new window will appear.
10. Set the values as shown in figure below and click ok.
11. Run the simulation by pressing the play button.
Lab Instructor: Dr. Sajid Iqbal 12
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
12. A new window will appear, go to ADD TRACE and plot the required waveforms.
13. Nominal values are: Vs = 220 V L = 20 mH R = 100 ohms f = 50 Hz
PARAMETERS:
TD1 = {((0/360)*T)+((angle/360)*T)}
TD2 = {((0/360)*T)+((angle/360)*T)}
TD3 = {((180/360)*T)+((angle/360)*T)}
TD4 = {((180/360)*T)+((angle/360)*T)}
PARAMETERS:
f = 50
T = {1/f }
Vac = 220
angle = 30
PW = 350u
Rload = 100
Lload = 100m
Lab Instructor: Dr. Sajid Iqbal 13
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Practice No.1
Set the value of angle=30 and run the simulation and compare your results with figures given
below.
Figure 1: Output Voltage.
Figure 2: Output Current.
Figure 3: Input Current.
Lab Instructor: Dr. Sajid Iqbal 14
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Figure 4: Input Voltage.
Figure 5: FFT of Output Voltage.
Comments about waveforms:
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________
Lab Instructor: Dr. Sajid Iqbal 15
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Exercise No.1
Set the value of angle 60, 90 and plot output current and voltage waveforms. Also plot input
supply current and FFT of output Voltage.
1) Firing Angle = 60 degree
Plot Output Voltage
Plot current through load
Plot Voltage across the thyristor
Lab Instructor: Dr. Sajid Iqbal 16
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Plot input current
Plot FFT of output voltage
2) Set the firing angle equal to 90 degree
Plot output voltage
Lab Instructor: Dr. Sajid Iqbal 17
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Plot Output Current
Plot Input Current
Plot voltage across thyristor
Lab Instructor: Dr. Sajid Iqbal 18
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Plot FFT of output voltage
Exercise No.2
Repeat Exercise No.1 with resistive load R=10Ω
1) Set the firing angle equal to 60 degree
Plot the Output Voltage
Plot the load current
Lab Instructor: Dr. Sajid Iqbal 19
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Plot the input/supply current
Plot the FFT of Output Voltage
2) Set the firing angle equal to 90 degree
Plot output voltage
Lab Instructor: Dr. Sajid Iqbal 20
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Plot the load current
Plot the supply current
Plot the FFT of Output Voltage
Lab Instructor: Dr. Sajid Iqbal 21
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Exercise No.3
Repeat Exercise No.1 with inductive load L=20mH.
1) Set the firing angle equal to 60 degree
Plot the output voltage
Plot the load current
Plot the supply current
Lab Instructor: Dr. Sajid Iqbal 22
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Plot the FFT of output voltage
2) Set the firing angle equal to 90 degree
Plot the load voltage
Plot the load current
Lab Instructor: Dr. Sajid Iqbal 23
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Plot the supply current
Plot the load voltage spectrum
Exercise No.4
Observe and plot the FFT of the input and output voltage and current waveforms from
fundamental frequency to 1000 Hz. Use R=100Ω and L=20mH.
Plot load voltage spectrum
Lab Instructor: Dr. Sajid Iqbal 24
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Plot load current spectrum
Plot supply current spectrum
FFT of Intput Voltage
Lab Instructor: Dr. Sajid Iqbal 25
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Experiment
Three Phase Semi Converter
Instructions:
 All Practice and Exercise Questions must be completed in this lab session for full credit.
 You must show the outputs to the instructor before proceeding to the next question.
 Read this lab manual completely at least once before coming to lab.
Recommended Reading:
 “Power Electronics Circuits Devices and Applications” by Muhammad H. Rashid 3rd
edition.
Objectives:
 The purpose of this experiment is to simulate Single Phase Full Converter.
Tools required:
 Software simulator ORCAD
 Calculator
LAB ACTIVITY:
1. Run the simulation software Orcad on your computer.
2. Go to file and select new project.
3. Name the project with your roll no. like 20XXEXXX and also specify the directory to save
project. Choose Analog or Mixed A/D. Click ok.
4. In the next window Check create a blank project and click ok.
Lab Instructor: Dr. Sajid Iqbal 26
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
5. In the schematic window make the following circuit.
6. Go to place, select part and add all the PSPICE libraries. Then select the following parts and
place on the schematic page.
• Resistor
• Inductor
• Vsine
• Vpulse
• Thyristor S2800N
7. Go to place, select part and place PARAM in the schematic to specify parameters.
8. Double click on PARAMETER after placing it and add variables to it one by one by clicking
on add new column button at the top of spread sheet. Specify the name and value of each
parameter. Use bracket {} as shown in schematic to specify values.
Lab Instructor: Dr. Sajid Iqbal 27
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
9. After placing the components and specifying parameters make the simulation profile. Go to
PSICE and select New Simulation Profile. A new window will appear.
10. Set the values as shown in figure below and click ok.
11. Run the simulation by pressing the play button.
12. A new window will appear, go to ADD TRACE and plot the required waveforms.
Lab Instructor: Dr. Sajid Iqbal 28
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
13. Nominal values are: Vs = 250 V L= 6.2 mH R = 100 ohms F= 50 Hz
PARAMETERS:
f = 50
T = {1/f }
Vac = 250
angle = 30
PW = 350u
Rload = 100
Lload = 6.2m
PARAMETERS:
TD1 = {((30/360)*T)+((angle/360)*T)}
TD2 = {((150/360)*T)+((angle/360)*T)}
TD3 = {((270/360)*T)+((angle/360)*T)}
Lab Instructor: Dr. Sajid Iqbal 29
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Practice No.1
Set the value of angle=30 and run the simulation and compare your results with figures given
below.
Figure 1:Output Voltage.
Figure 2: Output Current.
Figure 3: Input Current.
Lab Instructor: Dr. Sajid Iqbal 30
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Figure 4: Input Voltage.
Figure 5: FFT of Output Voltage.
Comments about waveforms:
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________
Lab Instructor: Dr. Sajid Iqbal 31
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Exercise No.1
Set the value of angle 60,90 and plot output current and voltage waveforms. Also plot input
supply current and FFT of output Voltage.
1) Firing Angle = 60 degree
Output Voltage
Output Current
Input Current
Lab Instructor: Dr. Sajid Iqbal 32
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
FFT of Output Voltage
2) Firing Angle = 90 degree
Output Voltage
Output Current
Lab Instructor: Dr. Sajid Iqbal 33
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Input Current
FFT of Output Voltage
Exercise No.2
Repeat Exercise No.1 with resistive load R=10Ω
1) Firing Angle = 60 degree
Output Voltage
Lab Instructor: Dr. Sajid Iqbal 34
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Output Current
Input Current
FFT of Output Voltage
Lab Instructor: Dr. Sajid Iqbal 35
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
2) Firing Angle = 90 degree
Output Voltage
Output Current
Input Current
Lab Instructor: Dr. Sajid Iqbal 36
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
FFT of Output Voltage
Exercise No.3
Repeat Exercise No.1 with inductive load L=20mH.
1) Firing Angle = 60 degree
Output Voltage
Output Current
Lab Instructor: Dr. Sajid Iqbal 37
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Input Current
FFT of Output Voltage
2) Firing Angle = 90 degree
Output Voltage
Lab Instructor: Dr. Sajid Iqbal 38
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Output Current
Input Current
FFT of Output Voltage
Lab Instructor: Dr. Sajid Iqbal 39
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Exercise No.4
Observe and plot the FFT of the input and output voltage and current waveforms from
fundamental frequency to 1000 Hz. Use R=100Ω and L=20mH.
FFT of Output Voltage
FFT of Output Current
Lab Instructor: Dr. Sajid Iqbal 40
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
FFT of Intput Voltage
FFT of Intput Current
Lab Instructor: Dr. Sajid Iqbal 41
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Experiment
Three Phase Full Converter
Instructions:
 All Practice and Exercise Questions must be completed in this lab session for full credit.
 You must show the outputs to the instructor before proceeding to the next question.
 Read this lab manual completely at least once before coming to lab.
Recommended Reading:
 “Power Electronics Circuits Devices and Applications” by Muhammad H. Rashid 3rd
edition.
Objectives:
 The purpose of this experiment is to simulate Single Phase Full Converter.
Tools required:
 Software simulator ORCAD
 Calculator
LAB ACTIVITY:
1. Run the simulation software Orcad on your computer.
2. Go to file and select new project.
3. Name the project with your roll no. like 20XXEXXX and also specify the directory to
save project. Choose Analog or Mixed A/D. Click ok.
4. In the next window Check create a blank project and click ok.
Lab Instructor: Dr. Sajid Iqbal 42
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
5. In the schematic window make the following circuit.
6. Go to place, select part and add all the PSPICE libraries. Then select the following
parts and place on the schematic page.
 Resistor
 Inductor
 Vsine
 Vpulse
 Thyristor S2800N
7. Go to place, select part and place PARAM in the schematic to specify parameters.
8. Double click on PARAMETER after placing it and add variables to it one by one by
clicking on add new column button at the top of spread sheet. Specify the name and
value of each parameter. Use bracket {} as shown in schematic to specify values.
Lab Instructor: Dr. Sajid Iqbal 43
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
9. After placing the components and specifying parameters make the simulation profile. Go to
PSICE and select New Simulation Profile. A new window will appear.
10. Set the values as shown in figure below and click OK.
Lab Instructor: Dr. Sajid Iqbal 44
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
11. Run the simulation by pressing the play button.
12. A new window will appear, go to ADD TRACE and plot the required waveforms.
13. Nominal values are: Vs = 250 V L= 6.2 mH R = 100 ohms f= 50 Hz
PARAMETERS:
f = 50
T = {1/f }
Vac = 250
angle = 30
PW = 350u
Rload = 100
Lload = 6.2m
PARAMETERS:
TD1 = {((30/360)*T)+((angle/360)*T)}
TD2 = {((90/360)*T)+((angle/360)*T)}
TD3 = {((150/360)*T)+((angle/360)*T)}
TD4 = {((210/360)*T)+((angle/360)*T)}
TD5 = {((270/360)*T)+((angle/360)*T)}
TD6 = {((330/360)*T)+((angle/360)*T)}
Lab Instructor: Dr. Sajid Iqbal 45
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Practice No.1
Set the value of angle=30 and run the simulation and compare your results with figures given
below.
Figure 1: Output Voltage.
Figure 2: Output Current.
Figure 3: Input Current.
Lab Instructor: Dr. Sajid Iqbal 46
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Figure 4: Input Voltage.
Figure 5: FFT of Output Voltage.
Comments about waveforms:
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________________________________
_________________________________________________________
Lab Instructor: Dr. Sajid Iqbal 47
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Exercise No.1
Set the value of angle 60, 90 and plot output current and voltage waveforms. Also plot input
supply current and FFT of output Voltage.
1) Firing Angle = 60 degree
Output Voltage
Output Current
Lab Instructor: Dr. Sajid Iqbal 48
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Input Current
FFT of Output Voltage
3) Firing Angle = 90 degree
Output Voltage
Lab Instructor: Dr. Sajid Iqbal 49
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Output Current
Input Current
FFT of Output Voltage
Lab Instructor: Dr. Sajid Iqbal 50
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Exercise No.2
Repeat Exercise No.1 with resistive load R=10Ω
1) Firing Angle = 60 degree
Output Voltage
Output Current
Lab Instructor: Dr. Sajid Iqbal 51
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Input Current
FFT of Output Voltage
2) Firing Angle = 90 degree
Output Voltage
Lab Instructor: Dr. Sajid Iqbal 52
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Output Current
Input Current
FFT of Output Voltage
Lab Instructor: Dr. Sajid Iqbal 53
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Exercise No.3
Repeat Exercise No.1 with inductive load L=20mH.
1) Firing Angle = 60 degree
Output Voltage
Output Current
Lab Instructor: Dr. Sajid Iqbal 54
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Input Current
FFT of Output Voltage
2) Firing Angle = 90 degree
Output Voltage
Lab Instructor: Dr. Sajid Iqbal 55
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Output Current
Input Current
FFT of Output Voltage
Lab Instructor: Dr. Sajid Iqbal 56
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Exercise No.4
Observe and plot the FFT of the input and output voltage and current waveforms from
fundamental frequency to 1000 Hz. Use R=100Ω and L=20mH.
FFT of Output Voltage
FFT of Output Current
Lab Instructor: Dr. Sajid Iqbal 57
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
FFT of Intput Voltage
FFT of Intput Current
Lab Instructor: Dr. Sajid Iqbal 58
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Experiment
DC-AC Inverter: Single-phase Square Wave Inverter
Part 1: To get acquainted with the simulation environment for Single-phase Square
wave inverter
Graphically model and simulate the single-phase square wave inverter (dc-ac converter) using
ORCAD 10.5 and PSpice. Study the dc source (input) current and ac load (output) voltage and
current waveforms. Compare the same with the results obtained from the analytical expressions.
Objective:
Part 1:
Graphically model the square wave inverter shown in Fig. 1 using the graphical front end of
ORCAD. The nominal values for the inverter are as follows:
Vs = 120 V L= 20 mH R = 5 ohms F= 50 Hz
Figure 1
Part 2:
Lab Instructor: Dr. Sajid Iqbal 59
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
1. Observe and plot the load voltage and current waveforms from time 0 to 0.1sec
(Output voltage across R & L), (Current through L).
2. Observe and plot supply current and voltage for the same duration.
3. Observe and plot the FFT of the input and output voltage and current
waveforms from fundamental frequency to 1000 Hz.
Part 3:
Repeat the above for R = 10 ohms.
Part 4:
Repeat the above experiment for a purely inductive load of L = 10 mH.
Tools required:
1. Software simulator ORCAD
2. Calculator
Software modules and settings
1. Add all the available libraries to the project
2. Add MOSFETs IRF450, Resistor, Inductor, VDC, VPULSE and 0/Ground
3. Set VDC = 120V
4. Set Vpulse1: V1=0, V2=15 TR=10u, TF=10u TD=0 PW=={0.5*T} PR = {T}
5. Set Vpulse2: V1=0, V2=15 TR=10u, TF=10u TD={0.5*T} PW=={0.5*T} PR = {T}
6. Set Vpulse3: V1=0, V2=15 TR=10u, TF=10u TD={0.5*T} PW=={0.5*T} PR = {T}
7. Set Vpulse4: V1=0, V2=15 TR=10u, TF=10u TD=0 PW=={0.5*T} PR = {T}
8. Set load inductance and resistance as given above.
Procedure
1. Start ORCAD 10.5
2. Make a new project with the name ‘Single_phase_square_inverter’ and select
the option of analog and mixed A/D.
Lab Instructor: Dr. Sajid Iqbal 60
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
3. Add all the libraries to the project
4. Place components in the schematic page
5. Arrange the components as shown in the figure 1
6. Set the values of the components as required
7. Place ‘PARAM’ in the schematic page and add the variables ‘frequency’ and
‘T’ and assign values as 50 and {1/frequency}.
8. Make a new simulation profile PSpice>New Simulation Profile> Give any
name>Set the simulation time to 0.1sec and other parameters according to
requirements
9. Place the voltage and current marker across the load.
Lab Instructor: Dr. Sajid Iqbal 61
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Frequency Spectrum of load voltage and current
Lab Instructor: Dr. Sajid Iqbal 62
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Experiment
DC-AC Inverter: Three-phase Square Wave Inverter
Part 1: To get acquainted with the simulation environment for three-phase Square
wave inverter
Graphically model and simulate the three-phase square wave inverter (dc-ac converter) using
ORCAD 10.5 and PSpice. Study the dc source (input) current and ac load (output) voltage and
current waveforms. Compare the same with the results obtained from the analytical expressions.
Objective:
Part 1:
Graphically model the square wave inverter shown in Figure using the graphical front end of
ORCAD. The nominal values for the inverter are as follows:
Vs = 400 V L= 10 mH R = 2 ohms F= 50 Hz
Part 2:
1. Observe and plot the phase voltage and current waveforms from time 20ms to
100ms (Output voltage across R & L), (Current through L).
2. Observe and plot the line to line voltage waveforms from time 20ms to 100ms
3. Observe and plot supply current and voltage for the same duration.
4. Observe and plot the FFT of the input and output voltage and current
waveforms from fundamental frequency to 1000 Hz.
Part 3:
Repeat the above for R = 10 ohms.
Part 4:
Repeat the above experiment for a purely inductive load of L = 10 mH.
Lab Instructor: Dr. Sajid Iqbal 63
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
Tools required:
1. Software simulator ORCAD
2. Calculator
Software modules and settings
1. Add all the available libraries to the project
2. Add MOSFETs IRF450, Resistor, Inductor, VDC, VPULSE and 0/Ground
3. Set VDC = 120V
4. Set VG1: V1=0, V2=15 TR=10u, TF=10u TD=0 PW= {0.5*T} PR = {T}
5. Set VG2: V1=0, V2=15 TR=10u, TF=10u TD={T/6} PW= {0.5*T} PR = {T}
6. Set VG3: V1=0, V2=15 TR=10u, TF=10u TD={T/3} PW= {0.5*T} PR = {T}
7. Set VG4: V1=0, V2=15 TR=10u, TF=10u TD={T/2} PW= {0.5*T} PR = {T}
8. Set VG5: V1=0, V2=15 TR=10u, TF=10u TD={T*(2/3)} PW= {0.5*T} PR =
{T}
Lab Instructor: Dr. Sajid Iqbal 64
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
9. Set VG6: V1=0, V2=15 TR=10u, TF=10u TD={T*(5/6)} PW= {0.5*T} PR =
{T}
10.Set load inductance and resistance as given above.
Procedure
1. Start ORCAD 10.5
2. Make a new project with the name ‘three_phase_square_inverter’ and select the
option of analog and mixed A/D.
3. Add all the libraries to the project
4. Place components in the schematic page
5. Arrange the components as shown in the figure
6. Set the values of the components as required
7. Place ‘PARAM’ in the schematic page and add the variables ‘frequency’, ‘T’,
‘Rload’ and ‘Lload’ and assign values.
8. Make a new simulation profile PSpice>New Simulation Profile> Give any
name>Set the simulation time to 0.1sec and other parameters according to
requirements
9. Place the voltage and current marker across the load.
Lab Instructor: Dr. Sajid Iqbal 65
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
• Load current waveforms for R=2 ohm and L=10mH
• Phase A voltage
Lab Instructor: Dr. Sajid Iqbal 66
Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore
• Line to Line Voltage Vab
Lab Instructor: Dr. Sajid Iqbal 67

More Related Content

Similar to manual-pe-2017_compress.pdf

The Doppler EffectWhat is the Doppler effect, and why is it impo.docx
The Doppler EffectWhat is the Doppler effect, and why is it impo.docxThe Doppler EffectWhat is the Doppler effect, and why is it impo.docx
The Doppler EffectWhat is the Doppler effect, and why is it impo.docxcherry686017
 
Ecet 345 Massive Success / snaptutorial.com
Ecet 345 Massive Success / snaptutorial.comEcet 345 Massive Success / snaptutorial.com
Ecet 345 Massive Success / snaptutorial.comHarrisGeorgx
 
Ecet 345 Enthusiastic Study / snaptutorial.com
Ecet 345 Enthusiastic Study / snaptutorial.comEcet 345 Enthusiastic Study / snaptutorial.com
Ecet 345 Enthusiastic Study / snaptutorial.comStephenson34
 
Ecet 345 Success Begins / snaptutorial.com
Ecet 345  Success Begins / snaptutorial.comEcet 345  Success Begins / snaptutorial.com
Ecet 345 Success Begins / snaptutorial.comWilliamsTaylorzl
 
Halderman ch043 lecture
Halderman ch043 lectureHalderman ch043 lecture
Halderman ch043 lecturemcfalltj
 
Introduction to Oscilloscope and Function generator
Introduction to Oscilloscope and Function generatorIntroduction to Oscilloscope and Function generator
Introduction to Oscilloscope and Function generatorcyberns_
 
IEE572 Final Report
IEE572 Final ReportIEE572 Final Report
IEE572 Final Reportjgoldpac
 
Frame detection.pdf
Frame detection.pdfFrame detection.pdf
Frame detection.pdfinfomerlin
 
Assignment 1 Description Marks out of Wtg() Due date .docx
Assignment 1  Description Marks out of Wtg() Due date .docxAssignment 1  Description Marks out of Wtg() Due date .docx
Assignment 1 Description Marks out of Wtg() Due date .docxfredharris32
 
1 P a g e A semester of Experiments for ECE 225 .docx
1  P a g e  A semester of Experiments for ECE 225  .docx1  P a g e  A semester of Experiments for ECE 225  .docx
1 P a g e A semester of Experiments for ECE 225 .docxmercysuttle
 
555 timer lab projects
555 timer lab projects555 timer lab projects
555 timer lab projectsBien Morfe
 
Plc analog Tutorial
Plc analog TutorialPlc analog Tutorial
Plc analog TutorialElectro 8
 
Power System Modeling and Simulation lab manual
Power System Modeling and Simulation lab manualPower System Modeling and Simulation lab manual
Power System Modeling and Simulation lab manualDHEERAJ DHAKAR
 
WEEK 1· Op-Amp Introduction1. Read Chapters 1-2 in the text Op Amp.docx
WEEK 1· Op-Amp Introduction1. Read Chapters 1-2 in the text Op Amp.docxWEEK 1· Op-Amp Introduction1. Read Chapters 1-2 in the text Op Amp.docx
WEEK 1· Op-Amp Introduction1. Read Chapters 1-2 in the text Op Amp.docxcelenarouzie
 
Criterion Unacceptable Minimum Satisfactory Excellent Weight.docx
Criterion Unacceptable Minimum Satisfactory Excellent Weight.docxCriterion Unacceptable Minimum Satisfactory Excellent Weight.docx
Criterion Unacceptable Minimum Satisfactory Excellent Weight.docxfaithxdunce63732
 
Design & Construction of Switched Mode Power Supplies
Design & Construction of Switched Mode Power Supplies Design & Construction of Switched Mode Power Supplies
Design & Construction of Switched Mode Power Supplies Sachin Mehta
 
「SPICEの活用方法」セミナー資料(28JAN2011) PPT
「SPICEの活用方法」セミナー資料(28JAN2011) PPT「SPICEの活用方法」セミナー資料(28JAN2011) PPT
「SPICEの活用方法」セミナー資料(28JAN2011) PPTTsuyoshi Horigome
 

Similar to manual-pe-2017_compress.pdf (20)

Gene's law
Gene's lawGene's law
Gene's law
 
The Doppler EffectWhat is the Doppler effect, and why is it impo.docx
The Doppler EffectWhat is the Doppler effect, and why is it impo.docxThe Doppler EffectWhat is the Doppler effect, and why is it impo.docx
The Doppler EffectWhat is the Doppler effect, and why is it impo.docx
 
Ecet 345 Massive Success / snaptutorial.com
Ecet 345 Massive Success / snaptutorial.comEcet 345 Massive Success / snaptutorial.com
Ecet 345 Massive Success / snaptutorial.com
 
Ecet 345 Enthusiastic Study / snaptutorial.com
Ecet 345 Enthusiastic Study / snaptutorial.comEcet 345 Enthusiastic Study / snaptutorial.com
Ecet 345 Enthusiastic Study / snaptutorial.com
 
Ecet 345 Success Begins / snaptutorial.com
Ecet 345  Success Begins / snaptutorial.comEcet 345  Success Begins / snaptutorial.com
Ecet 345 Success Begins / snaptutorial.com
 
Halderman ch043 lecture
Halderman ch043 lectureHalderman ch043 lecture
Halderman ch043 lecture
 
ControlsLab1
ControlsLab1ControlsLab1
ControlsLab1
 
Introduction to Oscilloscope and Function generator
Introduction to Oscilloscope and Function generatorIntroduction to Oscilloscope and Function generator
Introduction to Oscilloscope and Function generator
 
Adc manual
Adc manualAdc manual
Adc manual
 
IEE572 Final Report
IEE572 Final ReportIEE572 Final Report
IEE572 Final Report
 
Frame detection.pdf
Frame detection.pdfFrame detection.pdf
Frame detection.pdf
 
Assignment 1 Description Marks out of Wtg() Due date .docx
Assignment 1  Description Marks out of Wtg() Due date .docxAssignment 1  Description Marks out of Wtg() Due date .docx
Assignment 1 Description Marks out of Wtg() Due date .docx
 
1 P a g e A semester of Experiments for ECE 225 .docx
1  P a g e  A semester of Experiments for ECE 225  .docx1  P a g e  A semester of Experiments for ECE 225  .docx
1 P a g e A semester of Experiments for ECE 225 .docx
 
555 timer lab projects
555 timer lab projects555 timer lab projects
555 timer lab projects
 
Plc analog Tutorial
Plc analog TutorialPlc analog Tutorial
Plc analog Tutorial
 
Power System Modeling and Simulation lab manual
Power System Modeling and Simulation lab manualPower System Modeling and Simulation lab manual
Power System Modeling and Simulation lab manual
 
WEEK 1· Op-Amp Introduction1. Read Chapters 1-2 in the text Op Amp.docx
WEEK 1· Op-Amp Introduction1. Read Chapters 1-2 in the text Op Amp.docxWEEK 1· Op-Amp Introduction1. Read Chapters 1-2 in the text Op Amp.docx
WEEK 1· Op-Amp Introduction1. Read Chapters 1-2 in the text Op Amp.docx
 
Criterion Unacceptable Minimum Satisfactory Excellent Weight.docx
Criterion Unacceptable Minimum Satisfactory Excellent Weight.docxCriterion Unacceptable Minimum Satisfactory Excellent Weight.docx
Criterion Unacceptable Minimum Satisfactory Excellent Weight.docx
 
Design & Construction of Switched Mode Power Supplies
Design & Construction of Switched Mode Power Supplies Design & Construction of Switched Mode Power Supplies
Design & Construction of Switched Mode Power Supplies
 
「SPICEの活用方法」セミナー資料(28JAN2011) PPT
「SPICEの活用方法」セミナー資料(28JAN2011) PPT「SPICEの活用方法」セミナー資料(28JAN2011) PPT
「SPICEの活用方法」セミナー資料(28JAN2011) PPT
 

More from Abdo Brahmi

Cours_P627_19_03_2024.pptfjghgfjjfjhggjb
Cours_P627_19_03_2024.pptfjghgfjjfjhggjbCours_P627_19_03_2024.pptfjghgfjjfjhggjb
Cours_P627_19_03_2024.pptfjghgfjjfjhggjbAbdo Brahmi
 
Cours_P627_09_03_2023.pptghfgggghgghhghh
Cours_P627_09_03_2023.pptghfgggghgghhghhCours_P627_09_03_2023.pptghfgggghgghhghh
Cours_P627_09_03_2023.pptghfgggghgghhghhAbdo Brahmi
 
capteurs I.pptxfgggghghghghhghhhhhhhhhhh
capteurs I.pptxfgggghghghghhghhhhhhhhhhhcapteurs I.pptxfgggghghghghhghhhhhhhhhhh
capteurs I.pptxfgggghghghghhghhhhhhhhhhhAbdo Brahmi
 
Cours_P627_11_03_2023.ppthghggggghhhjhhh
Cours_P627_11_03_2023.ppthghggggghhhjhhhCours_P627_11_03_2023.ppthghggggghhhjhhh
Cours_P627_11_03_2023.ppthghggggghhhjhhhAbdo Brahmi
 
Cours_P627_09_03_2023.pptafrsecxghgghjgj
Cours_P627_09_03_2023.pptafrsecxghgghjgjCours_P627_09_03_2023.pptafrsecxghgghjgj
Cours_P627_09_03_2023.pptafrsecxghgghjgjAbdo Brahmi
 
Cours2 Master Embarqué 2022-2023.ppt
Cours2 Master Embarqué 2022-2023.pptCours2 Master Embarqué 2022-2023.ppt
Cours2 Master Embarqué 2022-2023.pptAbdo Brahmi
 
M312_Electricité_BCG.ppt
M312_Electricité_BCG.pptM312_Electricité_BCG.ppt
M312_Electricité_BCG.pptAbdo Brahmi
 
Cours_P627_11_03_2023.ppt
Cours_P627_11_03_2023.pptCours_P627_11_03_2023.ppt
Cours_P627_11_03_2023.pptAbdo Brahmi
 
Cours_SAM(M14).ppt
Cours_SAM(M14).pptCours_SAM(M14).ppt
Cours_SAM(M14).pptAbdo Brahmi
 
Cours Master Embarqué 2019-2020.pptx
Cours Master Embarqué 2019-2020.pptxCours Master Embarqué 2019-2020.pptx
Cours Master Embarqué 2019-2020.pptxAbdo Brahmi
 
Cours_SAM(M14).ppt
Cours_SAM(M14).pptCours_SAM(M14).ppt
Cours_SAM(M14).pptAbdo Brahmi
 
capteurs II.pptx
capteurs II.pptxcapteurs II.pptx
capteurs II.pptxAbdo Brahmi
 
diaporama_1_professeurs_94e.ppt
diaporama_1_professeurs_94e.pptdiaporama_1_professeurs_94e.ppt
diaporama_1_professeurs_94e.pptAbdo Brahmi
 
pres_chapter5 (5).pptx
pres_chapter5 (5).pptxpres_chapter5 (5).pptx
pres_chapter5 (5).pptxAbdo Brahmi
 
card_sorting.ppt
card_sorting.pptcard_sorting.ppt
card_sorting.pptAbdo Brahmi
 
Initiation_a_l_informatique.pptx
Initiation_a_l_informatique.pptxInitiation_a_l_informatique.pptx
Initiation_a_l_informatique.pptxAbdo Brahmi
 
Les microcontrôleurs PIC.pptx
Les microcontrôleurs PIC.pptxLes microcontrôleurs PIC.pptx
Les microcontrôleurs PIC.pptxAbdo Brahmi
 
pic16f84-200306072553.pdf
pic16f84-200306072553.pdfpic16f84-200306072553.pdf
pic16f84-200306072553.pdfAbdo Brahmi
 
Cours_Physique_des_Composants_dElectroni.pptx
Cours_Physique_des_Composants_dElectroni.pptxCours_Physique_des_Composants_dElectroni.pptx
Cours_Physique_des_Composants_dElectroni.pptxAbdo Brahmi
 
Etude-Du-Microcontrleur-Pic16f84-160919133655
Etude-Du-Microcontrleur-Pic16f84-160919133655Etude-Du-Microcontrleur-Pic16f84-160919133655
Etude-Du-Microcontrleur-Pic16f84-160919133655Abdo Brahmi
 

More from Abdo Brahmi (20)

Cours_P627_19_03_2024.pptfjghgfjjfjhggjb
Cours_P627_19_03_2024.pptfjghgfjjfjhggjbCours_P627_19_03_2024.pptfjghgfjjfjhggjb
Cours_P627_19_03_2024.pptfjghgfjjfjhggjb
 
Cours_P627_09_03_2023.pptghfgggghgghhghh
Cours_P627_09_03_2023.pptghfgggghgghhghhCours_P627_09_03_2023.pptghfgggghgghhghh
Cours_P627_09_03_2023.pptghfgggghgghhghh
 
capteurs I.pptxfgggghghghghhghhhhhhhhhhh
capteurs I.pptxfgggghghghghhghhhhhhhhhhhcapteurs I.pptxfgggghghghghhghhhhhhhhhhh
capteurs I.pptxfgggghghghghhghhhhhhhhhhh
 
Cours_P627_11_03_2023.ppthghggggghhhjhhh
Cours_P627_11_03_2023.ppthghggggghhhjhhhCours_P627_11_03_2023.ppthghggggghhhjhhh
Cours_P627_11_03_2023.ppthghggggghhhjhhh
 
Cours_P627_09_03_2023.pptafrsecxghgghjgj
Cours_P627_09_03_2023.pptafrsecxghgghjgjCours_P627_09_03_2023.pptafrsecxghgghjgj
Cours_P627_09_03_2023.pptafrsecxghgghjgj
 
Cours2 Master Embarqué 2022-2023.ppt
Cours2 Master Embarqué 2022-2023.pptCours2 Master Embarqué 2022-2023.ppt
Cours2 Master Embarqué 2022-2023.ppt
 
M312_Electricité_BCG.ppt
M312_Electricité_BCG.pptM312_Electricité_BCG.ppt
M312_Electricité_BCG.ppt
 
Cours_P627_11_03_2023.ppt
Cours_P627_11_03_2023.pptCours_P627_11_03_2023.ppt
Cours_P627_11_03_2023.ppt
 
Cours_SAM(M14).ppt
Cours_SAM(M14).pptCours_SAM(M14).ppt
Cours_SAM(M14).ppt
 
Cours Master Embarqué 2019-2020.pptx
Cours Master Embarqué 2019-2020.pptxCours Master Embarqué 2019-2020.pptx
Cours Master Embarqué 2019-2020.pptx
 
Cours_SAM(M14).ppt
Cours_SAM(M14).pptCours_SAM(M14).ppt
Cours_SAM(M14).ppt
 
capteurs II.pptx
capteurs II.pptxcapteurs II.pptx
capteurs II.pptx
 
diaporama_1_professeurs_94e.ppt
diaporama_1_professeurs_94e.pptdiaporama_1_professeurs_94e.ppt
diaporama_1_professeurs_94e.ppt
 
pres_chapter5 (5).pptx
pres_chapter5 (5).pptxpres_chapter5 (5).pptx
pres_chapter5 (5).pptx
 
card_sorting.ppt
card_sorting.pptcard_sorting.ppt
card_sorting.ppt
 
Initiation_a_l_informatique.pptx
Initiation_a_l_informatique.pptxInitiation_a_l_informatique.pptx
Initiation_a_l_informatique.pptx
 
Les microcontrôleurs PIC.pptx
Les microcontrôleurs PIC.pptxLes microcontrôleurs PIC.pptx
Les microcontrôleurs PIC.pptx
 
pic16f84-200306072553.pdf
pic16f84-200306072553.pdfpic16f84-200306072553.pdf
pic16f84-200306072553.pdf
 
Cours_Physique_des_Composants_dElectroni.pptx
Cours_Physique_des_Composants_dElectroni.pptxCours_Physique_des_Composants_dElectroni.pptx
Cours_Physique_des_Composants_dElectroni.pptx
 
Etude-Du-Microcontrleur-Pic16f84-160919133655
Etude-Du-Microcontrleur-Pic16f84-160919133655Etude-Du-Microcontrleur-Pic16f84-160919133655
Etude-Du-Microcontrleur-Pic16f84-160919133655
 

Recently uploaded

Mine Environment II Lab_MI10448MI__________.pptx
Mine Environment II Lab_MI10448MI__________.pptxMine Environment II Lab_MI10448MI__________.pptx
Mine Environment II Lab_MI10448MI__________.pptxRomil Mishra
 
US Department of Education FAFSA Week of Action
US Department of Education FAFSA Week of ActionUS Department of Education FAFSA Week of Action
US Department of Education FAFSA Week of ActionMebane Rash
 
Secure Key Crypto - Tech Paper JET Tech Labs
Secure Key Crypto - Tech Paper JET Tech LabsSecure Key Crypto - Tech Paper JET Tech Labs
Secure Key Crypto - Tech Paper JET Tech Labsamber724300
 
Katarzyna Lipka-Sidor - BIM School Course
Katarzyna Lipka-Sidor - BIM School CourseKatarzyna Lipka-Sidor - BIM School Course
Katarzyna Lipka-Sidor - BIM School Coursebim.edu.pl
 
Robotics Group 10 (Control Schemes) cse.pdf
Robotics Group 10  (Control Schemes) cse.pdfRobotics Group 10  (Control Schemes) cse.pdf
Robotics Group 10 (Control Schemes) cse.pdfsahilsajad201
 
Curve setting (Basic Mine Surveying)_MI10412MI.pptx
Curve setting (Basic Mine Surveying)_MI10412MI.pptxCurve setting (Basic Mine Surveying)_MI10412MI.pptx
Curve setting (Basic Mine Surveying)_MI10412MI.pptxRomil Mishra
 
SOFTWARE ESTIMATION COCOMO AND FP CALCULATION
SOFTWARE ESTIMATION COCOMO AND FP CALCULATIONSOFTWARE ESTIMATION COCOMO AND FP CALCULATION
SOFTWARE ESTIMATION COCOMO AND FP CALCULATIONSneha Padhiar
 
March 2024 - Top 10 Read Articles in Artificial Intelligence and Applications...
March 2024 - Top 10 Read Articles in Artificial Intelligence and Applications...March 2024 - Top 10 Read Articles in Artificial Intelligence and Applications...
March 2024 - Top 10 Read Articles in Artificial Intelligence and Applications...gerogepatton
 
A brief look at visionOS - How to develop app on Apple's Vision Pro
A brief look at visionOS - How to develop app on Apple's Vision ProA brief look at visionOS - How to develop app on Apple's Vision Pro
A brief look at visionOS - How to develop app on Apple's Vision ProRay Yuan Liu
 
The Satellite applications in telecommunication
The Satellite applications in telecommunicationThe Satellite applications in telecommunication
The Satellite applications in telecommunicationnovrain7111
 
Gravity concentration_MI20612MI_________
Gravity concentration_MI20612MI_________Gravity concentration_MI20612MI_________
Gravity concentration_MI20612MI_________Romil Mishra
 
Computer Graphics Introduction, Open GL, Line and Circle drawing algorithm
Computer Graphics Introduction, Open GL, Line and Circle drawing algorithmComputer Graphics Introduction, Open GL, Line and Circle drawing algorithm
Computer Graphics Introduction, Open GL, Line and Circle drawing algorithmDeepika Walanjkar
 
Triangulation survey (Basic Mine Surveying)_MI10412MI.pptx
Triangulation survey (Basic Mine Surveying)_MI10412MI.pptxTriangulation survey (Basic Mine Surveying)_MI10412MI.pptx
Triangulation survey (Basic Mine Surveying)_MI10412MI.pptxRomil Mishra
 
Stork Webinar | APM Transformational planning, Tool Selection & Performance T...
Stork Webinar | APM Transformational planning, Tool Selection & Performance T...Stork Webinar | APM Transformational planning, Tool Selection & Performance T...
Stork Webinar | APM Transformational planning, Tool Selection & Performance T...Stork
 
STATE TRANSITION DIAGRAM in psoc subject
STATE TRANSITION DIAGRAM in psoc subjectSTATE TRANSITION DIAGRAM in psoc subject
STATE TRANSITION DIAGRAM in psoc subjectGayathriM270621
 
Cost estimation approach: FP to COCOMO scenario based question
Cost estimation approach: FP to COCOMO scenario based questionCost estimation approach: FP to COCOMO scenario based question
Cost estimation approach: FP to COCOMO scenario based questionSneha Padhiar
 
CS 3251 Programming in c all unit notes pdf
CS 3251 Programming in c all unit notes pdfCS 3251 Programming in c all unit notes pdf
CS 3251 Programming in c all unit notes pdfBalamuruganV28
 
AntColonyOptimizationManetNetworkAODV.pptx
AntColonyOptimizationManetNetworkAODV.pptxAntColonyOptimizationManetNetworkAODV.pptx
AntColonyOptimizationManetNetworkAODV.pptxLina Kadam
 
Novel 3D-Printed Soft Linear and Bending Actuators
Novel 3D-Printed Soft Linear and Bending ActuatorsNovel 3D-Printed Soft Linear and Bending Actuators
Novel 3D-Printed Soft Linear and Bending ActuatorsResearcher Researcher
 
Detection&Tracking - Thermal imaging object detection and tracking
Detection&Tracking - Thermal imaging object detection and trackingDetection&Tracking - Thermal imaging object detection and tracking
Detection&Tracking - Thermal imaging object detection and trackinghadarpinhas1
 

Recently uploaded (20)

Mine Environment II Lab_MI10448MI__________.pptx
Mine Environment II Lab_MI10448MI__________.pptxMine Environment II Lab_MI10448MI__________.pptx
Mine Environment II Lab_MI10448MI__________.pptx
 
US Department of Education FAFSA Week of Action
US Department of Education FAFSA Week of ActionUS Department of Education FAFSA Week of Action
US Department of Education FAFSA Week of Action
 
Secure Key Crypto - Tech Paper JET Tech Labs
Secure Key Crypto - Tech Paper JET Tech LabsSecure Key Crypto - Tech Paper JET Tech Labs
Secure Key Crypto - Tech Paper JET Tech Labs
 
Katarzyna Lipka-Sidor - BIM School Course
Katarzyna Lipka-Sidor - BIM School CourseKatarzyna Lipka-Sidor - BIM School Course
Katarzyna Lipka-Sidor - BIM School Course
 
Robotics Group 10 (Control Schemes) cse.pdf
Robotics Group 10  (Control Schemes) cse.pdfRobotics Group 10  (Control Schemes) cse.pdf
Robotics Group 10 (Control Schemes) cse.pdf
 
Curve setting (Basic Mine Surveying)_MI10412MI.pptx
Curve setting (Basic Mine Surveying)_MI10412MI.pptxCurve setting (Basic Mine Surveying)_MI10412MI.pptx
Curve setting (Basic Mine Surveying)_MI10412MI.pptx
 
SOFTWARE ESTIMATION COCOMO AND FP CALCULATION
SOFTWARE ESTIMATION COCOMO AND FP CALCULATIONSOFTWARE ESTIMATION COCOMO AND FP CALCULATION
SOFTWARE ESTIMATION COCOMO AND FP CALCULATION
 
March 2024 - Top 10 Read Articles in Artificial Intelligence and Applications...
March 2024 - Top 10 Read Articles in Artificial Intelligence and Applications...March 2024 - Top 10 Read Articles in Artificial Intelligence and Applications...
March 2024 - Top 10 Read Articles in Artificial Intelligence and Applications...
 
A brief look at visionOS - How to develop app on Apple's Vision Pro
A brief look at visionOS - How to develop app on Apple's Vision ProA brief look at visionOS - How to develop app on Apple's Vision Pro
A brief look at visionOS - How to develop app on Apple's Vision Pro
 
The Satellite applications in telecommunication
The Satellite applications in telecommunicationThe Satellite applications in telecommunication
The Satellite applications in telecommunication
 
Gravity concentration_MI20612MI_________
Gravity concentration_MI20612MI_________Gravity concentration_MI20612MI_________
Gravity concentration_MI20612MI_________
 
Computer Graphics Introduction, Open GL, Line and Circle drawing algorithm
Computer Graphics Introduction, Open GL, Line and Circle drawing algorithmComputer Graphics Introduction, Open GL, Line and Circle drawing algorithm
Computer Graphics Introduction, Open GL, Line and Circle drawing algorithm
 
Triangulation survey (Basic Mine Surveying)_MI10412MI.pptx
Triangulation survey (Basic Mine Surveying)_MI10412MI.pptxTriangulation survey (Basic Mine Surveying)_MI10412MI.pptx
Triangulation survey (Basic Mine Surveying)_MI10412MI.pptx
 
Stork Webinar | APM Transformational planning, Tool Selection & Performance T...
Stork Webinar | APM Transformational planning, Tool Selection & Performance T...Stork Webinar | APM Transformational planning, Tool Selection & Performance T...
Stork Webinar | APM Transformational planning, Tool Selection & Performance T...
 
STATE TRANSITION DIAGRAM in psoc subject
STATE TRANSITION DIAGRAM in psoc subjectSTATE TRANSITION DIAGRAM in psoc subject
STATE TRANSITION DIAGRAM in psoc subject
 
Cost estimation approach: FP to COCOMO scenario based question
Cost estimation approach: FP to COCOMO scenario based questionCost estimation approach: FP to COCOMO scenario based question
Cost estimation approach: FP to COCOMO scenario based question
 
CS 3251 Programming in c all unit notes pdf
CS 3251 Programming in c all unit notes pdfCS 3251 Programming in c all unit notes pdf
CS 3251 Programming in c all unit notes pdf
 
AntColonyOptimizationManetNetworkAODV.pptx
AntColonyOptimizationManetNetworkAODV.pptxAntColonyOptimizationManetNetworkAODV.pptx
AntColonyOptimizationManetNetworkAODV.pptx
 
Novel 3D-Printed Soft Linear and Bending Actuators
Novel 3D-Printed Soft Linear and Bending ActuatorsNovel 3D-Printed Soft Linear and Bending Actuators
Novel 3D-Printed Soft Linear and Bending Actuators
 
Detection&Tracking - Thermal imaging object detection and tracking
Detection&Tracking - Thermal imaging object detection and trackingDetection&Tracking - Thermal imaging object detection and tracking
Detection&Tracking - Thermal imaging object detection and tracking
 

manual-pe-2017_compress.pdf

  • 1. UNIVERSITY OF ENGINEERING & TECHNOLOGY 2017 Power Electronics ORCAD Simulation AC/DC Converters Dr. Sajid Iqbal
  • 2. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Table of Contents 1. General Notes Page 3 2. Simulation Notes Page 6 3. Single phase full converter Page 10 4. Three phase semi converter Page 23 5. Three phase full converter Page 36 6. Single phase square wave inverter Page 49 7. Three phase square wave inverter Page 53 Lab Instructor: Dr. Sajid Iqbal 2
  • 3. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore General Notes 1. How to make a project 1. Open OrCAD Capture 2. Go to File => New => Project. 3. Enter a name 4. Choose "Analog or Mixed A/D" 5. Set the location. (You should create a new directory for your project since PSpice will generate a bunch of project files in this folder. 6. Click OK 7. Choose "Create blank project" and click OK 8. You should see a window where you can draw the schematic (i.e., your circuit diagram). 9. To add parts for your circuit (i.e., resistors, etc.) a. Go to Place => Parts b. Click on the library you want to use, or select multiple libraries by holding Ctrl or dragging the mouse. In the part window you should see at least the ANALOG, BIPOLAR, EVAL, SOURCE, and SPECIAL libraries (see below for more information on “Parts Notes”) c. Find the part you want to add and press OK d. Click where you want to place the part on your schematic. (Press R to rotate the part by 90 degrees) e. Use wires to connect part to complete your circuit 10. Run simulation by choosing simulation type (see below for more information under “Simulation Notes”) 11. Plot your output (see below for more information under “Simulation Notes”) 2. Ground There are many types of grounds (common points in the circuit, noise reduction, etc.) PSpice uses node-voltage method for circuit simulation and, therefore, needs a reference node with “zero voltage”. This is the 0/SOURCE ground. You need to have it in your circuits! (It looks like a ground symbol with a zero) If you don't, PSpice may complain of "floating nodes" even if you have a ground. Lab Instructor: Dr. Sajid Iqbal 3
  • 4. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore To place the ground on the circuit Go to Place => Ground and choose 0/source (If you don't see the "source" in the Libraries section, you will need to add the source library. See Part Notes below). 3. Mega- (i.e. mega-ohm, mega-hertz) When you need to enter a "Mega-" (106 ) unit use "MEG". (Case doesn't matter). "M" is NOT mega, it is milli (10^-3). Example: for 6.5 megahertz, enter "6.5 Meg", for 3 milli-amps, enter "3 m" 4. All parts must have unique names. You can't have two parts named "R1" in your circuit. If you are copying and pasting parts or circuits, you will need to rename your parts because PSpice doesn't do this automatically. 5. Labeling Nodes: I recommend you use aliases to label your input and output nodes. This makes your node easier to find. V(Vout) is simpler than finding V(R1:1) a. Go to Place => Net Alias b. Enter a name, i.e., Vout or Vin c. Place the label close to a node d. Example below shows a simple circuit with aliases: Lab Instructor: Dr. Sajid Iqbal 4
  • 5. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Lab Instructor: Dr. Sajid Iqbal 5
  • 6. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Simulation Notes 1) DC Bias: The response of the circuit to DC sources is always calculated. To display DC bias voltages and currents on your circuit after you run the simulation, go to PSpice => Bias Points, and check Enable, Enable Bias Current Display, and/or Enable Bias Voltage Display 2) Parametric Sweep This simulation is used to find the response of the circuit (e.g., current in one element) if the value of an element (R1 in the example below) is changed. To do so: a. Change the value of the part to {RL} (use curly braces, name is arbitrary) b. Go to Place => Part c. Add a PARAM/SPECIAL part to your schematic d. Double click on the PARAM part e. Click “New Column” f. Set the name to RL (same name as in “a” but with no curly braces) g. Set the value to something, e.g., 1k (this is the value that is used in calculating DC bias values, choose somewhere in the range of your sweep). h. Click "Display" i. Select "Name and Value" and press OK j. Your schematic should look like as in figure below k. Go to PSpice=>Edit Simulation Profile. l. Change the following settings, Analysis type: DC Sweep ,Options: Primary Sweep, Sweep variable: Global parameter, Parameter name: RL, Setup the sweep type how you want. (Note that if you are sweeping resistance, you can't start at 0) Lab Instructor: Dr. Sajid Iqbal 6
  • 7. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore m. Click OK, and go to PSpice => Run to run the simulation. 3) Frequency Domain Simulations 1. Set up your circuit with VAC voltage sources. 2. Go to PSpice => Edit Simulation Profile 3. Select the "Frequency Domain" Analysis type 4. Select the frequency range of interest. Don't start Frequency sweeps at 0! 5. Set the points/Decade to be at least 20. Bode Plots 1. Use a logarithmic x-axis for the frequency. 2. The magnitude should be measured in decibels. Use the PSpice DB() function to convert to decibels. For example, DB(V(Vout)/V(Vin)), assuming you have labeled your output and input nodes with "Vout" and "Vin" aliases. Note that DB(Vout) is NOT the transfer function in dB. 3. Remember you also need a phase graph (unless instructed otherwise). Use the PSpice P() function to get the phase angle. For example, P(V(Vout)/V(Vin)) 4. Be sure to mark the cutoff points on your bode plots (on both magnitude AND phase graphs). Remember cutoff is 3dB below the highest point (NOT always at -3dB) a. Click the "Toggle Cursor" button. (Or go through the menu, Trace => Cursor => Display) You will now be able to move the cursor along your plot. b. Click the "Cursor Max" button to find the highest point. (Or go through the menu, Trace => Cursor => Max) c. Click the "Mark Label" button to label that point. (Or go through the menu, Plot => Label => Mark) d. Click the "Cursor Search" button (Or go through the menu, Trace => Cursor =>Search Commands) e. Select 1 for Cursor To Move to search along the y-axis f. Enter "search forward level (max-3)" (don't enter the quotation marks) to move the cursor to the right to the point which is 3 below the max. Lab Instructor: Dr. Sajid Iqbal 7
  • 8. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore g. Or enter "search back level (max-3)" (don't enter the quotation marks) to move the cursor to the left h. Click the "Mark Label" button to label that cutoff point. a. Unclick the Toggle Cursor button to disable the cursor so you can move the label. b. Double click on the label to edit the text (to add units, or to name the point) 5. It may help to increase the width of the lines in the plot. • The colored symbol at the bottom of the graph, or on the graph line • Note you can select all of the lines by going to Edit => Select All • Right click on the line. Make sure the selection list has Information, Properties, Cursor 1, and Cursor 2.(If it lists Settings and Properties, you clicked on the background, not on the line). • Select Properties • You can change the width and other settings of that trace 4) Time Domain Simulations a. Use VSIN for your voltage source instead of VAC (VOFF is the DC offset, VAMPL is the amplitude, and FREQ is the frequency of the sine wave). b. For Square and triangular wave, use VPULSE Lab Instructor: Dr. Sajid Iqbal 8
  • 9. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Square Wave is the VPLUSE function in the limit of TR = TF = 0 and PW = 0.5 * PER (PER is the period of the wave). This limit case, however, causes numerical difficulties in calculations. In any case, we can never make such a square function in practice. In reality, square waves have very small TR and TF. Typically, we use a symmetric function, i.e., we set TR = TF and PW = 0.5 * PER - 2 * TR. Thus, for a given frequency we can set up the square function if we choose TR. If we choose TR too large, the function does not look like a square wave. If we choose TR too small, the program will take a long time to simulate the circuit and for TR smaller than a certain value, the simulation will not converge numerically. A good choice for TR is to set it to be 1% of the PER (a period): TR = TF = 0.01 * PER, PW = 0.48 * PER. This usually results in a nice signal without a huge amount of computational need. Note that TR does not have to be exactly 1% of PER. You can choose nice round numbers for TR, TF, and PW. Triangular Wave is the VPLUSE function in the limit of TR = TF = 0.5* PER and PW = 0 (convince yourself that this is the case). As before, the limit case of PW = 0 causes numerical difficulties in calculations. So we have to choose PW to be a reasonably small value. A good choice for PW is to be set at 1% of the PER (period): PW = 0.01* PER, TR = TF = 0.49 * PER (and not TR = TF = 0.495 * PER so that we get a symmetric function). This usually results in a nice signal without a huge amount of computational need. Again, note that PW does not have to be exactly 1% of PER. You can choose nice round numbers for TR, TF, and PW. Simulation settings 1. Go to PSpice => Edit Simulation Profile 2. Select the "Time Domain (Transient)" Analysis type 3. Enter a Run to time: so that a few periods will be displayed. Remember that the period (seconds) = 1/frequency (Hz), i.e, if you are using a 1kHz sine wave, it has a 1/1kHz=1ms period, so use a Run to time of 5ms for 5 periods 4. Set the Maximum step size to be much smaller than the period i.e. for a 1kHz sine wave: It has a 1ms period, so set a maximum step size of approx .01ms. (This works out to 100 data points per period). 5. If you don't set the maximum step size, PSpice may choose one which is too big, making your sine wave look angular and ugly. Lab Instructor: Dr. Sajid Iqbal 9
  • 10. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Experiment Single Phase Full Converter Instructions:  All Practice and Exercise Questions must be completed in this lab session for full credit.  You must show the outputs to the instructor before proceeding to the next question.  Read this lab manual completely at least once before coming to lab. Recommended Reading:  “Power Electronics Circuits Devices and Applications” by Muhammad H. Rashid 3rd edition. Objectives:  The purpose of this experiment is to simulate Single Phase Full Converter. Tools required:  Software simulator ORCAD  Calculator LAB ACTIVITY: 1. Run the simulation software Orcad on your computer. 2. Go to file and select new project. 3. Name the project with your roll no. like 20XXEXXX and also specify the directory to save project. Choose Analog or Mixed A/D. Click ok. Lab Instructor: Dr. Sajid Iqbal 10
  • 11. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 4. In the next window Check create a blank project and click ok. 5. In the schematic window make the following circuit. 6. Go to place, select part and add all the PSPICE libraries. Then select the following parts and place on the schematic page. • Resistor • Inductor • Vsine • Vpulse • Thyristor S2800N 7. Go to place, select part and place PARAM in the schematic to specify parameters. 8. Double click on PARAMETER after placing it and add variables to it one by one by clicking on add new column button at the top of spread sheet. Specify the name and value of each parameter. Use bracket {} as shown in schematic to specify values. Lab Instructor: Dr. Sajid Iqbal 11
  • 12. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 9. After placing the components and specifying parameters make the simulation profile. Go to PSICE and select New Simulation Profile. A new window will appear. 10. Set the values as shown in figure below and click ok. 11. Run the simulation by pressing the play button. Lab Instructor: Dr. Sajid Iqbal 12
  • 13. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 12. A new window will appear, go to ADD TRACE and plot the required waveforms. 13. Nominal values are: Vs = 220 V L = 20 mH R = 100 ohms f = 50 Hz PARAMETERS: TD1 = {((0/360)*T)+((angle/360)*T)} TD2 = {((0/360)*T)+((angle/360)*T)} TD3 = {((180/360)*T)+((angle/360)*T)} TD4 = {((180/360)*T)+((angle/360)*T)} PARAMETERS: f = 50 T = {1/f } Vac = 220 angle = 30 PW = 350u Rload = 100 Lload = 100m Lab Instructor: Dr. Sajid Iqbal 13
  • 14. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Practice No.1 Set the value of angle=30 and run the simulation and compare your results with figures given below. Figure 1: Output Voltage. Figure 2: Output Current. Figure 3: Input Current. Lab Instructor: Dr. Sajid Iqbal 14
  • 15. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Figure 4: Input Voltage. Figure 5: FFT of Output Voltage. Comments about waveforms: _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________ Lab Instructor: Dr. Sajid Iqbal 15
  • 16. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Exercise No.1 Set the value of angle 60, 90 and plot output current and voltage waveforms. Also plot input supply current and FFT of output Voltage. 1) Firing Angle = 60 degree Plot Output Voltage Plot current through load Plot Voltage across the thyristor Lab Instructor: Dr. Sajid Iqbal 16
  • 17. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Plot input current Plot FFT of output voltage 2) Set the firing angle equal to 90 degree Plot output voltage Lab Instructor: Dr. Sajid Iqbal 17
  • 18. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Plot Output Current Plot Input Current Plot voltage across thyristor Lab Instructor: Dr. Sajid Iqbal 18
  • 19. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Plot FFT of output voltage Exercise No.2 Repeat Exercise No.1 with resistive load R=10Ω 1) Set the firing angle equal to 60 degree Plot the Output Voltage Plot the load current Lab Instructor: Dr. Sajid Iqbal 19
  • 20. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Plot the input/supply current Plot the FFT of Output Voltage 2) Set the firing angle equal to 90 degree Plot output voltage Lab Instructor: Dr. Sajid Iqbal 20
  • 21. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Plot the load current Plot the supply current Plot the FFT of Output Voltage Lab Instructor: Dr. Sajid Iqbal 21
  • 22. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Exercise No.3 Repeat Exercise No.1 with inductive load L=20mH. 1) Set the firing angle equal to 60 degree Plot the output voltage Plot the load current Plot the supply current Lab Instructor: Dr. Sajid Iqbal 22
  • 23. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Plot the FFT of output voltage 2) Set the firing angle equal to 90 degree Plot the load voltage Plot the load current Lab Instructor: Dr. Sajid Iqbal 23
  • 24. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Plot the supply current Plot the load voltage spectrum Exercise No.4 Observe and plot the FFT of the input and output voltage and current waveforms from fundamental frequency to 1000 Hz. Use R=100Ω and L=20mH. Plot load voltage spectrum Lab Instructor: Dr. Sajid Iqbal 24
  • 25. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Plot load current spectrum Plot supply current spectrum FFT of Intput Voltage Lab Instructor: Dr. Sajid Iqbal 25
  • 26. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Experiment Three Phase Semi Converter Instructions:  All Practice and Exercise Questions must be completed in this lab session for full credit.  You must show the outputs to the instructor before proceeding to the next question.  Read this lab manual completely at least once before coming to lab. Recommended Reading:  “Power Electronics Circuits Devices and Applications” by Muhammad H. Rashid 3rd edition. Objectives:  The purpose of this experiment is to simulate Single Phase Full Converter. Tools required:  Software simulator ORCAD  Calculator LAB ACTIVITY: 1. Run the simulation software Orcad on your computer. 2. Go to file and select new project. 3. Name the project with your roll no. like 20XXEXXX and also specify the directory to save project. Choose Analog or Mixed A/D. Click ok. 4. In the next window Check create a blank project and click ok. Lab Instructor: Dr. Sajid Iqbal 26
  • 27. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 5. In the schematic window make the following circuit. 6. Go to place, select part and add all the PSPICE libraries. Then select the following parts and place on the schematic page. • Resistor • Inductor • Vsine • Vpulse • Thyristor S2800N 7. Go to place, select part and place PARAM in the schematic to specify parameters. 8. Double click on PARAMETER after placing it and add variables to it one by one by clicking on add new column button at the top of spread sheet. Specify the name and value of each parameter. Use bracket {} as shown in schematic to specify values. Lab Instructor: Dr. Sajid Iqbal 27
  • 28. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 9. After placing the components and specifying parameters make the simulation profile. Go to PSICE and select New Simulation Profile. A new window will appear. 10. Set the values as shown in figure below and click ok. 11. Run the simulation by pressing the play button. 12. A new window will appear, go to ADD TRACE and plot the required waveforms. Lab Instructor: Dr. Sajid Iqbal 28
  • 29. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 13. Nominal values are: Vs = 250 V L= 6.2 mH R = 100 ohms F= 50 Hz PARAMETERS: f = 50 T = {1/f } Vac = 250 angle = 30 PW = 350u Rload = 100 Lload = 6.2m PARAMETERS: TD1 = {((30/360)*T)+((angle/360)*T)} TD2 = {((150/360)*T)+((angle/360)*T)} TD3 = {((270/360)*T)+((angle/360)*T)} Lab Instructor: Dr. Sajid Iqbal 29
  • 30. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Practice No.1 Set the value of angle=30 and run the simulation and compare your results with figures given below. Figure 1:Output Voltage. Figure 2: Output Current. Figure 3: Input Current. Lab Instructor: Dr. Sajid Iqbal 30
  • 31. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Figure 4: Input Voltage. Figure 5: FFT of Output Voltage. Comments about waveforms: _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________ Lab Instructor: Dr. Sajid Iqbal 31
  • 32. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Exercise No.1 Set the value of angle 60,90 and plot output current and voltage waveforms. Also plot input supply current and FFT of output Voltage. 1) Firing Angle = 60 degree Output Voltage Output Current Input Current Lab Instructor: Dr. Sajid Iqbal 32
  • 33. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore FFT of Output Voltage 2) Firing Angle = 90 degree Output Voltage Output Current Lab Instructor: Dr. Sajid Iqbal 33
  • 34. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Input Current FFT of Output Voltage Exercise No.2 Repeat Exercise No.1 with resistive load R=10Ω 1) Firing Angle = 60 degree Output Voltage Lab Instructor: Dr. Sajid Iqbal 34
  • 35. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Output Current Input Current FFT of Output Voltage Lab Instructor: Dr. Sajid Iqbal 35
  • 36. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 2) Firing Angle = 90 degree Output Voltage Output Current Input Current Lab Instructor: Dr. Sajid Iqbal 36
  • 37. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore FFT of Output Voltage Exercise No.3 Repeat Exercise No.1 with inductive load L=20mH. 1) Firing Angle = 60 degree Output Voltage Output Current Lab Instructor: Dr. Sajid Iqbal 37
  • 38. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Input Current FFT of Output Voltage 2) Firing Angle = 90 degree Output Voltage Lab Instructor: Dr. Sajid Iqbal 38
  • 39. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Output Current Input Current FFT of Output Voltage Lab Instructor: Dr. Sajid Iqbal 39
  • 40. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Exercise No.4 Observe and plot the FFT of the input and output voltage and current waveforms from fundamental frequency to 1000 Hz. Use R=100Ω and L=20mH. FFT of Output Voltage FFT of Output Current Lab Instructor: Dr. Sajid Iqbal 40
  • 41. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore FFT of Intput Voltage FFT of Intput Current Lab Instructor: Dr. Sajid Iqbal 41
  • 42. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Experiment Three Phase Full Converter Instructions:  All Practice and Exercise Questions must be completed in this lab session for full credit.  You must show the outputs to the instructor before proceeding to the next question.  Read this lab manual completely at least once before coming to lab. Recommended Reading:  “Power Electronics Circuits Devices and Applications” by Muhammad H. Rashid 3rd edition. Objectives:  The purpose of this experiment is to simulate Single Phase Full Converter. Tools required:  Software simulator ORCAD  Calculator LAB ACTIVITY: 1. Run the simulation software Orcad on your computer. 2. Go to file and select new project. 3. Name the project with your roll no. like 20XXEXXX and also specify the directory to save project. Choose Analog or Mixed A/D. Click ok. 4. In the next window Check create a blank project and click ok. Lab Instructor: Dr. Sajid Iqbal 42
  • 43. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 5. In the schematic window make the following circuit. 6. Go to place, select part and add all the PSPICE libraries. Then select the following parts and place on the schematic page.  Resistor  Inductor  Vsine  Vpulse  Thyristor S2800N 7. Go to place, select part and place PARAM in the schematic to specify parameters. 8. Double click on PARAMETER after placing it and add variables to it one by one by clicking on add new column button at the top of spread sheet. Specify the name and value of each parameter. Use bracket {} as shown in schematic to specify values. Lab Instructor: Dr. Sajid Iqbal 43
  • 44. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 9. After placing the components and specifying parameters make the simulation profile. Go to PSICE and select New Simulation Profile. A new window will appear. 10. Set the values as shown in figure below and click OK. Lab Instructor: Dr. Sajid Iqbal 44
  • 45. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 11. Run the simulation by pressing the play button. 12. A new window will appear, go to ADD TRACE and plot the required waveforms. 13. Nominal values are: Vs = 250 V L= 6.2 mH R = 100 ohms f= 50 Hz PARAMETERS: f = 50 T = {1/f } Vac = 250 angle = 30 PW = 350u Rload = 100 Lload = 6.2m PARAMETERS: TD1 = {((30/360)*T)+((angle/360)*T)} TD2 = {((90/360)*T)+((angle/360)*T)} TD3 = {((150/360)*T)+((angle/360)*T)} TD4 = {((210/360)*T)+((angle/360)*T)} TD5 = {((270/360)*T)+((angle/360)*T)} TD6 = {((330/360)*T)+((angle/360)*T)} Lab Instructor: Dr. Sajid Iqbal 45
  • 46. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Practice No.1 Set the value of angle=30 and run the simulation and compare your results with figures given below. Figure 1: Output Voltage. Figure 2: Output Current. Figure 3: Input Current. Lab Instructor: Dr. Sajid Iqbal 46
  • 47. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Figure 4: Input Voltage. Figure 5: FFT of Output Voltage. Comments about waveforms: _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________________________________ _________________________________________________________ Lab Instructor: Dr. Sajid Iqbal 47
  • 48. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Exercise No.1 Set the value of angle 60, 90 and plot output current and voltage waveforms. Also plot input supply current and FFT of output Voltage. 1) Firing Angle = 60 degree Output Voltage Output Current Lab Instructor: Dr. Sajid Iqbal 48
  • 49. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Input Current FFT of Output Voltage 3) Firing Angle = 90 degree Output Voltage Lab Instructor: Dr. Sajid Iqbal 49
  • 50. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Output Current Input Current FFT of Output Voltage Lab Instructor: Dr. Sajid Iqbal 50
  • 51. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Exercise No.2 Repeat Exercise No.1 with resistive load R=10Ω 1) Firing Angle = 60 degree Output Voltage Output Current Lab Instructor: Dr. Sajid Iqbal 51
  • 52. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Input Current FFT of Output Voltage 2) Firing Angle = 90 degree Output Voltage Lab Instructor: Dr. Sajid Iqbal 52
  • 53. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Output Current Input Current FFT of Output Voltage Lab Instructor: Dr. Sajid Iqbal 53
  • 54. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Exercise No.3 Repeat Exercise No.1 with inductive load L=20mH. 1) Firing Angle = 60 degree Output Voltage Output Current Lab Instructor: Dr. Sajid Iqbal 54
  • 55. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Input Current FFT of Output Voltage 2) Firing Angle = 90 degree Output Voltage Lab Instructor: Dr. Sajid Iqbal 55
  • 56. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Output Current Input Current FFT of Output Voltage Lab Instructor: Dr. Sajid Iqbal 56
  • 57. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Exercise No.4 Observe and plot the FFT of the input and output voltage and current waveforms from fundamental frequency to 1000 Hz. Use R=100Ω and L=20mH. FFT of Output Voltage FFT of Output Current Lab Instructor: Dr. Sajid Iqbal 57
  • 58. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore FFT of Intput Voltage FFT of Intput Current Lab Instructor: Dr. Sajid Iqbal 58
  • 59. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Experiment DC-AC Inverter: Single-phase Square Wave Inverter Part 1: To get acquainted with the simulation environment for Single-phase Square wave inverter Graphically model and simulate the single-phase square wave inverter (dc-ac converter) using ORCAD 10.5 and PSpice. Study the dc source (input) current and ac load (output) voltage and current waveforms. Compare the same with the results obtained from the analytical expressions. Objective: Part 1: Graphically model the square wave inverter shown in Fig. 1 using the graphical front end of ORCAD. The nominal values for the inverter are as follows: Vs = 120 V L= 20 mH R = 5 ohms F= 50 Hz Figure 1 Part 2: Lab Instructor: Dr. Sajid Iqbal 59
  • 60. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 1. Observe and plot the load voltage and current waveforms from time 0 to 0.1sec (Output voltage across R & L), (Current through L). 2. Observe and plot supply current and voltage for the same duration. 3. Observe and plot the FFT of the input and output voltage and current waveforms from fundamental frequency to 1000 Hz. Part 3: Repeat the above for R = 10 ohms. Part 4: Repeat the above experiment for a purely inductive load of L = 10 mH. Tools required: 1. Software simulator ORCAD 2. Calculator Software modules and settings 1. Add all the available libraries to the project 2. Add MOSFETs IRF450, Resistor, Inductor, VDC, VPULSE and 0/Ground 3. Set VDC = 120V 4. Set Vpulse1: V1=0, V2=15 TR=10u, TF=10u TD=0 PW=={0.5*T} PR = {T} 5. Set Vpulse2: V1=0, V2=15 TR=10u, TF=10u TD={0.5*T} PW=={0.5*T} PR = {T} 6. Set Vpulse3: V1=0, V2=15 TR=10u, TF=10u TD={0.5*T} PW=={0.5*T} PR = {T} 7. Set Vpulse4: V1=0, V2=15 TR=10u, TF=10u TD=0 PW=={0.5*T} PR = {T} 8. Set load inductance and resistance as given above. Procedure 1. Start ORCAD 10.5 2. Make a new project with the name ‘Single_phase_square_inverter’ and select the option of analog and mixed A/D. Lab Instructor: Dr. Sajid Iqbal 60
  • 61. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 3. Add all the libraries to the project 4. Place components in the schematic page 5. Arrange the components as shown in the figure 1 6. Set the values of the components as required 7. Place ‘PARAM’ in the schematic page and add the variables ‘frequency’ and ‘T’ and assign values as 50 and {1/frequency}. 8. Make a new simulation profile PSpice>New Simulation Profile> Give any name>Set the simulation time to 0.1sec and other parameters according to requirements 9. Place the voltage and current marker across the load. Lab Instructor: Dr. Sajid Iqbal 61
  • 62. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Frequency Spectrum of load voltage and current Lab Instructor: Dr. Sajid Iqbal 62
  • 63. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Experiment DC-AC Inverter: Three-phase Square Wave Inverter Part 1: To get acquainted with the simulation environment for three-phase Square wave inverter Graphically model and simulate the three-phase square wave inverter (dc-ac converter) using ORCAD 10.5 and PSpice. Study the dc source (input) current and ac load (output) voltage and current waveforms. Compare the same with the results obtained from the analytical expressions. Objective: Part 1: Graphically model the square wave inverter shown in Figure using the graphical front end of ORCAD. The nominal values for the inverter are as follows: Vs = 400 V L= 10 mH R = 2 ohms F= 50 Hz Part 2: 1. Observe and plot the phase voltage and current waveforms from time 20ms to 100ms (Output voltage across R & L), (Current through L). 2. Observe and plot the line to line voltage waveforms from time 20ms to 100ms 3. Observe and plot supply current and voltage for the same duration. 4. Observe and plot the FFT of the input and output voltage and current waveforms from fundamental frequency to 1000 Hz. Part 3: Repeat the above for R = 10 ohms. Part 4: Repeat the above experiment for a purely inductive load of L = 10 mH. Lab Instructor: Dr. Sajid Iqbal 63
  • 64. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore Tools required: 1. Software simulator ORCAD 2. Calculator Software modules and settings 1. Add all the available libraries to the project 2. Add MOSFETs IRF450, Resistor, Inductor, VDC, VPULSE and 0/Ground 3. Set VDC = 120V 4. Set VG1: V1=0, V2=15 TR=10u, TF=10u TD=0 PW= {0.5*T} PR = {T} 5. Set VG2: V1=0, V2=15 TR=10u, TF=10u TD={T/6} PW= {0.5*T} PR = {T} 6. Set VG3: V1=0, V2=15 TR=10u, TF=10u TD={T/3} PW= {0.5*T} PR = {T} 7. Set VG4: V1=0, V2=15 TR=10u, TF=10u TD={T/2} PW= {0.5*T} PR = {T} 8. Set VG5: V1=0, V2=15 TR=10u, TF=10u TD={T*(2/3)} PW= {0.5*T} PR = {T} Lab Instructor: Dr. Sajid Iqbal 64
  • 65. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore 9. Set VG6: V1=0, V2=15 TR=10u, TF=10u TD={T*(5/6)} PW= {0.5*T} PR = {T} 10.Set load inductance and resistance as given above. Procedure 1. Start ORCAD 10.5 2. Make a new project with the name ‘three_phase_square_inverter’ and select the option of analog and mixed A/D. 3. Add all the libraries to the project 4. Place components in the schematic page 5. Arrange the components as shown in the figure 6. Set the values of the components as required 7. Place ‘PARAM’ in the schematic page and add the variables ‘frequency’, ‘T’, ‘Rload’ and ‘Lload’ and assign values. 8. Make a new simulation profile PSpice>New Simulation Profile> Give any name>Set the simulation time to 0.1sec and other parameters according to requirements 9. Place the voltage and current marker across the load. Lab Instructor: Dr. Sajid Iqbal 65
  • 66. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore • Load current waveforms for R=2 ohm and L=10mH • Phase A voltage Lab Instructor: Dr. Sajid Iqbal 66
  • 67. Power Electronics Lab Department of Mechatronics & Control Engineering, UET Lahore • Line to Line Voltage Vab Lab Instructor: Dr. Sajid Iqbal 67