PSpice Notes

By Judith Sullivan,2014-05-27 13:40
6 views 0
PSpice Notes

    Notes for ORCAD PSpice

    ECE 65, Spring 2006

    Kristi Tsukida

    Starting a Project:

    1. Open OrCAD Capture

    2. Go to File => New => Project…

    3. Enter a name (ie Ece65_Kristi_Lab1)

    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. If you're in the PSpice lab, you may use

    the Z drive to save your files).

    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”)

    General Notes:


    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.

    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).

2) Mega- (ie megaohm, megahertz)

    When you need to enter a "Mega-" (10^6) 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"

3) 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.

4) 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:

    Part Notes

PSpice Parts summary

    Ground 0/SOURCE

    741 Opamp uA741/EVAL

    Diode D1N4148/EVAL

    Zener Diode D1N5232 *Need to add additional libraries to use this! NPN BJT Q2N3904/BIPOLAR

1) Part Libraries:

    You will need at least the ANALOG, BIPOLAR, EVAL, SOURCE, and SPECIAL libraries. If you don't see these libraries already listed, you will need to add them:

    a. Click Add Library…

    b. Navigate to C:\Program Files\OrCad_Demo\Capture\Library\Pspice (This is the location

    in the PSpice lab computers. The location may be different if you install PSpice on your

    own computer, but find the ...\Capture\Library\Pspice folder)

    c. Highlight all the *.olb files in this folder. You can hold Ctrl and click on the files, or

    drag the mouse to select multiple files.

    d. Click Open. You should now see a list of libraries in the "Libraries:" section.

2) Using the Zener Diode

    1. You need 2 files (posted on the Web site):

    a. D1N5232.lib (PSpice library file)

    b. D1N5232.olb (Orcad Capture library file)

    2. PSpice Instructions:

    a. Go to the menu: 'PSpice => Edit Simulation Settings'

    b. Go to the 'Libraries' tab. Click the 'Browse...' button. Open the D1N5323.lib file

    c. Click 'Add as Global'

    d. Press 'OK' to exit the simulation settings.

    e. Now go to the menu: 'Place => Part...'

    f. Click 'Add Library'

    g. Open the D1N5232.olb file

    h. You should now see a part named D1N5232. Select it and press OK to use the


    Simulation Notes

1) DC Bias:

The response of the circuit to DC sources are 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 this:

k. Go to PSpice=>Edit Simulation Profile

    l. Change the following settings

    i. Analysis type: DC Sweep

    ii. Options: Primary Sweep

    iii. Sweep variable: Global parameter

    iv. Parameter name: RL

    v. Setup the sweep type how you want. (Note that if you are sweeping resistance, you can't

    start at 0.)

    m. Click OK, and go to PSpice => Run to run the simulation.

3) Frequency Domain Simulations

a. Set up your circuit with VAC voltage sources.

    b. Go to PSpice => Edit Simulation Profile

    c. Select the "Frequency Domain" Analysis type

    d. Select the frequency range of interest. Don't start Frequency sweeps at 0! e. 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.

    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.

    ; Unclick the Toggle Cursor button to disable the cursor so you can move the label.

    ; 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 (Set delay time, TD = 0, for simulations in


    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.

    General Lab notes

Before coming to the lab

    1) Don't forget that you also need to do a hand analysis of the circuit for your prelabs. Meaning

    that you calculate the voltages or currents or whatever the experiment asks for. Box your

    answers (or better yet, put them in a table).

    2) Remember each person needs to do their own prelab!

    3) TAs will be signing prelabs at the beginning of lab, and anyone with incomplete prelabs will

    not be allowed to do the lab that day.

    4) Use your prelab to check your lab data as you collect it

    5) I recommend you print out and bring Prof. Najmabadi's notes to lab. The labs follow the

    notes pretty closely, and they should help with the prelab too.

Lab Report:

    1) Print out a copy of the circuit which you used along with any plots that you created using that


    2) Label the cutoff points of your bode plots (on BOTH the magnitude and phase graphs)

Report this document

For any questions or suggestions please email