Orcad ' e yeni başlayanlar için güzel bir kaynak .

Katılım
16 Şub 2012
Mesajlar
2
Puanları
1
Yaş
33
PSPICE Seminar / DeVry KC - Spring 2002 - Page 1
© 2002 Tom A. Wheeler
Introduction to OrCAD PSPICE
OrCAD Capture 9.2 - Lite Edition - 9.2.448 - D
PSPICE Rules
1. All circuits must have a reference node. In PSPICE, this node is usually marked with the
number “0.” Note: The conventional OrCAD ground symbol is not appropriate for
PSPICE simulation.
This is a proper ground:
2. All component leads must be connected. Unconnected wires and leads will cause the
simulation to fail.
3. All components must have a value. The following suffixes are used to modify values:
k, K = 1K = 1 x 103
m,M = 1 m = 1 x 10-3
MEG,meg = 1 M = 1 x 106
u, U = 1 m = 1 x 10-6
p, P = 1 p = 1 x 10-12
f, F = 1 f = 1 x 10-15
Caution: Note that “m” and “M” mean milli to PSPICE, not meg!
4. All components must have a unique designator. For example, there can’t be two instances
of a component reference “R1” within the same circuit.
5. There must be no space between a number value and its modifying suffix. For example,
the value “1 k” for a resistor or “1 V” for a voltage source will cause an error.
The correct way of specifying these parts is “1k” and “1V” (upper and lower case make no
difference.)
PSPICE Seminar / DeVry KC - Spring 2002 - Page 2
© 2002 Tom A. Wheeler
DC Static Analysis Example
1. Start OrCAD Lite as shown below:
Note that the only program you need to start is “Capture Lite Edition.” The other
programs will run automatically as they’re needed.
2. Click the “Create Document” button on the toolbar.
Create Document
3. The following dialog will appear. Fill in the information as shown.
1. Type in the
name of the project
2. Select “Analog or
Mixed A/D” as
shown.
3. Specify where the
project will be saved
on your computer
4. Click OK
PSPICE Seminar / DeVry KC - Spring 2002 - Page 3
© 2002 Tom A. Wheeler
4. The following dialog will appear:
Choose “Create a blank project” and click OK.
5. The schematic editor will open. Enter the following schematic into the program:
0
R3
1k
0
R2
1k
V1
10V
R1
1k
Note the following:
· Parts are placed by SHIFT-P
· The voltage source is called “VDC” in the parts library
· The resistors are called “R”
· The ground is obtained by clicking the ground button
and choosing part “0/SOURCE.”
SOURCE library
should show here.
If not, press “Add
Library” button.
PSPICE Seminar / DeVry KC - Spring 2002 - Page 4
© 2002 Tom A. Wheeler
6. Create a new simulation profile for the circuit by going to the PSPICE menu and choosing
“New Simulation Profile” as shown:
1. Type a name for the
profile and click “Create.”
2. The Simulation Settings
dialog will appear, but
there’s nothing to set, so
click OK.
You can have multiple profiles for a given project. This allows you to analyze a circuit in
different ways without having to change settings back and forth.
7. Click the toolbar buttons for displaying the bias-point voltages and currents so that they
are depressed.
8. Press F11 to run the simulation. (This is the same as going to the PSPICE menu and
choosing Run). The screen will show the DC voltages and currents directly on the
schematic.
PSPICE Seminar / DeVry KC - Spring 2002 - Page 5
© 2002 Tom A. Wheeler
Debugging PSPICE Simulation Errors
Sooner or later (probably sooner), you’ll get a nasty error message from the simulator.
Because this program uses a PSPICE core to do the actual work, you need to be able to
locate and decipher the actual error within the OUTPUT file, then correct it in your circuit.
1. Let’s “break” the circuit. Delete one of the conductors and press F11 to run the simulation
again. I broke mine like this:
R2
1k
0
V1
10V
R1
1k
3.333V
R3
1k
0V
0V
0
Depending on how your version of PSPICE is configured, you’ll get either a dialog box
with an error, or a full screen dump of the output file, which shows the error.
If you don’t get the output file, select “View Output” from the PSPICE menu to see it. It
might look like this:
2. You can see the ERROR. At node N00812 there’s a problem. By looking at the netlist
portion of the listing, you can see that node N00812 is associated with R1.
** Creating circuit file "wheels-schematic1-dc simulation.sim.cir"
** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT
SIMULATIONS
*Libraries:
* Local Libraries :
* From [PSPICE NETLIST] section of C:\Program Files\OrcadLite\PSpice\PSpice.ini
file:
.lib "nom.lib"
*Analysis directives:
.PROBE V(*) I(*) W(*) D(*) NOISE(*)
.INC ".\wheels-SCHEMATIC1.net"
**** INCLUDING wheels-SCHEMATIC1.net ****
* source WHEELS
V_V1 N00893 0 10V
R_R1 N00812 N00197 1k
R_R2 0 N00197 1k
R_R3 0 N00197 1k
**** RESUMING "wheels-schematic1-dc simulation.sim.cir" ****
.END
ERROR -- Less than 2 connections at node N00812
Node N00812 belongs to R1.
PSPICE Seminar / DeVry KC - Spring 2002 - Page 6
© 2002 Tom A. Wheeler
Transient Analysis
In PSPICE, the transient analysis option is used to do both steady and transient analysis of
circuits. This can involve both AC and DC signal sources. Steady-state AC time-domain
results are obtained by the same setup as for transient analysis. Let’s try it out.
1. Start a new project called “boing” and build the following schematic into it. (Make sure to
completely close the previous project).
0
C1
25uF
V1
TD = 1
TF = 0
PW = 10
PER = 0
V1 = 0v
TR = 0
V2 = 1v
L1
1000H
1 2
V
0
0V
0V
0V
0V
R1
632
V
0V
Place the two voltage probes by clicking the probe button on the toolbar. Note the
color of each probe; it will match the color of the trace in the PROBE readout during
simulation.
The source used is called “VPULSE” and the parameters on the source have the following
meanings:
· V1 is the “off” voltage
· V2 is the “on” voltage
· The simulation begins with the source in the OFF state. TD is the time delay in
seconds before the pulse turns on.
· TR and TF are the rise and fall times of the step function.
· PW is the pulse width (how long the source stays “on” after TD has passed.)
· PER is the period. Enter 0 for a one-shot pulse, or a non-zero period for the pulse to
be periodic.
PSPICE Seminar / DeVry KC - Spring 2002 - Page 7
© 2002 Tom A. Wheeler
2. Build a new simulation profile called “transient” and make it look like this:
· “Run to time” says how long to run the simulation. 10 seconds is forever in the world
of circuits, but this one is special.
· “Start saving data after 0 seconds” means to use all simulation results starting with
time = 0. Entering a non-zero value causes initial data points to be discarded.
· “Maximum step size” is a very important setting. It specifies how often PSPICE will
recalculate the circuit parameters during simulation. If you’re expecting sinusoids to
look good, you need at least 100 or more calculations for each sine wave period.
3. Press the F11 key. (Warning: Stand several feet back from the circuit when doing this!)
You should get the following display:
PSPICE Seminar / DeVry KC - Spring 2002 - Page 8
© 2002 Tom A. Wheeler
4. Try replacing the DC pulse source in the circuit with an AC signal source and repeat the
analysis again. You might want to change the “Run to time” in the analysis profile to 20
seconds. The circuit looks like this:
R1
632
0
V
0
V1
FREQ = 1
VAMPL = 1
VOFF = 0
L1
1000H
1 2
V
0V
0V
0V
0V
C1
25uF
0V
For the VSIN signal source, the parameters have the following meanings:
· VOFF is the DC offset
· VAMPL is the peak voltage of the sine wave
· FREQ is (you guessed it), the frequency of the signal in Hz.
You can set other parameters of the VSIN source by double-clicking the body of the part.
You’ll get a complete listing of the settable parameters and their values.
PSPICE Seminar / DeVry KC - Spring 2002 - Page 9
© 2002 Tom A. Wheeler
AC Parametric Sweeps
In order to learn about the frequency response of circuits, an AC parametric sweep can be
performed. This is a different type of analysis than transient analysis as far as PSPICE is
concerned, because instead of calculating the instantaneous values for voltages and currents,
PSPICE instead calculates the steady-state effective currents and voltages.
Any source with an AC parameter can be used as a swept-frequency AC voltage source. The
object “VSRC” is a generic AC signal source. The “VSIN” device also has the capability to be
used during AC sweeps. It is usually more convenient to use “VSIN” since the same signal
source can be used for both steady state and transient analysis.
PSPICE can present the results of an AC sweep in many useful ways. We’ll first look at raw
voltage data, then have PSPICE display the data in decibel form.
1. Change the schematic diagram of the project to look like this:
V
V1
FREQ = 10.065
VAMPL = 1
VOFF = 0
L1
10H
1 2
0
V
C1
25uF
0
R1
6.32
This modification raises the resonant frequency of the circuit to 10.065 Hz, and the Q
becomes 100.
2. Change the simulation profile to look like this:
PSPICE Seminar / DeVry KC - Spring 2002 - Page 10
© 2002 Tom A. Wheeler
3. Run the simulation. Notice that the circuit takes a little while to build its voltage up due
to the high Q of the tank circuit!
4. Let’s find the frequency response of this filter circuit. First, let’s create a new simulation
profile (remember, a project can contain multiple simulation profiles.)
· At the PSPICE menu, choose “New Simulation Profile”
· Fill in the resulting dialog box as follows and click the CREATE button.
· A new simulation profile will appear. Set it up as follows:
This profile will sweep any AC sources in the circuit from 1 Hz to 100 Hz (two
decades), with 100 points for each decade.
PSPICE Seminar / DeVry KC - Spring 2002 - Page 11
© 2002 Tom A. Wheeler
5. To do an AC frequency sweep, there must be at least one signal source with an “AC”
parameter in the circuit. Double click the body of the voltage source and you’ll get a
detailed screen like this one:
Click on any field to change its value.
Change the ACfield to 1V and the DC
f ield to 0V (no DCoffset).
This screen is available for all components in a design. Not all of the parameters display
on your drawing because the display isn’t turned on for them. To fix that, highlight one of
the items, then click the “Display...” button. Choose “Name and Value” from the dialog to
make the parameter show on the drawing.
To exit the property editor, click the lower “X” button at the upper-right portion of the
display.
6. The circuit should now simulate. Press the F11 key to do so. But wait, there’s a problem --
why doesn’t the output voltage rise all the way to 1 V (Vin) at resonance? The circuit
doesn’t work! (Try more points per decade in the simulation setup -- 1000 is a good
number.)
7. You can easily switch back to the previous simulation profile. Simulation profiles are
stored with the project.
· From the Window menu of the schematic editor, choose “boing.opj”. You’ll see the
following display:
PSPICE Seminar / DeVry KC - Spring 2002 - Page 12
© 2002 Tom A. Wheeler
· By expanding the “Simulation Profiles” folder, you can see that your project has two
different profiles.
· You can enable any profile by highlighting it, then selecting “Make Active” from the
“PSPICE” menu.
· The active profile is always highlighted with a red “P!” (for Probe).
8. Let’s look at the data with a decibel display. Switch back to the schematic (making sure
the “frequency response” profile is active).
PSPICE provides special probes that read in dBV units. By definition:



=
Volt
V
dBV
1
20log
These special probes are available by following the menus as follows:
Place two of these probes onto the circuit (and delete the other voltage probes). The
circuit should look like this:
V1
FREQ = 10.065
VAMPL = 1
VOFF = 0
AC = 1
DC = 0
C1
25uF
L1
10H
1 2
0
R1
6.32
VDB
0
VDB
PSPICE Seminar / DeVry KC - Spring 2002 - Page 13
© 2002 Tom A. Wheeler
9. With these special probes in the circuit, run the analysis again. Notice that we played a
dirty little trick. By setting the input voltage to 1 V (0 dBV), we get output voltage
magnitude readings that correspond to the voltage gain.
It is possible to mathematically compute gain by adding a trace to the plot. See if you can
figure out how it works.
DC Parametric Sweeps
It is also possible to vary the parameters in a DC-swept fashion. Common examples of
parameters that can be varied include resistance, capacitance, transistor Beta, and so on.
A good example of this is to demonstrate the maximum power transfer theorem, where the
load resistance of a circuit must equal the source resistance in order to get maximum power
into the load.
1. Create a new project called “power” and add a schematic to the project as follows. Note
that the value of R2 is {RLOAD}, which will refer to a global parameter.
0 0
V1
100V
W
R2
{RLOAD}
R1
1k
2. Place a new part on the drawing called “PARAM” (from the SPECIAL library.) Place it on
the schematic, then double-click its body to open its property sheet.
Within the property sheet editor, make the following changes to the PARAM block:
· Select the “OrCAD-PSpice” Filter to make it easier to see the important fields.
· Click the “New Column” button and add a column called RLOAD. Set its value to 1k,
as shown below.
· Make sure to set RLOAD visible by highlighting it and clicking the “Display” button.
PSPICE Seminar / DeVry KC - Spring 2002 - Page 14
© 2002 Tom A. Wheeler
· Close the property sheet. Your drawing should now have a parameter block that
looks something like this:
PARAMETERS:
RLOAD = 1k
The value of 1k has no effect on a DC swept analysis, but will instead be used for
bias point (steady-state) calculation (if that is required).
3. Edit the analysis profile to look like this:
The sweep will vary the global parameter you named -- RLOAD -- in accordance with the
rules set forth under “Sweep type.”
4. Run the analysis with F11.
PSPICE Seminar / DeVry KC - Spring 2002 - Page 15
© 2002 Tom A. Wheeler
Solid State Circuit Analysis
OrCAD PSPICE can model circuits with mixed analog and digital components. Below is a
common-emitter amplifier. Using PSPICE simulation we can determine:
· What are the DC operating voltages of the amplifier?
· What is the voltage gain and compliance of the amplifier?
· What is the frequency response of the unit?
1. Start a new project called “transistor” and insert the circuit of the amplifier below.
C2
1uF
C3
220uF
R2
150
V
0
Q1
Q2N3904
V2
FREQ = 1k
VAMPL = .1
VOFF = 0
V
R1
22
R3
1k
0
V1
18v
RL
1k
C1
1uF
0
R6
33k
0 0 0
R5
4.7k
PSPICE Seminar / DeVry KC - Spring 2002 - Page 16
© 2002 Tom A. Wheeler
2. Create a new simulation profile and set it as follows:
Note that the VSIN source in the circuit is set to 1 KHz, and that the analysis steps are
1 mS -- so there will be 1000 calculations for each sine wave cycle. With the TSTOP
setting of 10 mS, we should see 10 cycles of the waveform on the display.
3. Run the simulation. To see the DC voltages and currents, click the appropriate toolbar
buttons.
Compliance Evaluation
To perform a compliance test of an amplifier, we gradually increase the input signal
amplitude until clipping is observed at the amplifier output. We can “sweep” the VSIN
amplitude in our circuit to achieve this.
1. Create a new simulation profile called “Compliance Test.” Inherit the profile from the
original profile in your project.
PSPICE Seminar / DeVry KC - Spring 2002 - Page 17
© 2002 Tom A. Wheeler
2. Modify the simulation profile to look like this:
To set this up, first click on the checkbox by “Parametric Sweep” in the Options window.
Then fill in the fields on the right as shown.
3. Add a part called “PARAM” to the schematic page. Double-click the PARAM block body
and add a field called “VIN.” Set the value of VIN to 0.1 V (for static analysis) and turn
its display on.
4. Modify the signal source VAMP parameter to be “{VIN}”, which will cause the signal
source amplitude to ramp up in step with the parametric sweep.
5. Run the simulation. You’ll now see a family of curves for Vin and Vout. You can now tell
when the amplifier will clip.
Frequency Response of the Amplifier
1. Create a new simulation profile called for the circuit called “Frequency Response.” Inherit
this profile from the base profile “steadystate.”
PSPICE Seminar / DeVry KC - Spring 2002 - Page 18
© 2002 Tom A. Wheeler
2. Do an AC sweep on this profile as follows:
3. Recall that the VSIN component is a dual-purpose signal source - it can be used for both
transient and AC sweep analysis - you just have to enable the AC parameters. Doubleclick
the body of the VSIN source and set the AC value to 0.1v (RMS), and the DC value
to 0v. Turn on the display of these items so that you can see them on the schematic.
4. Run the simulation. You may want to exchange the Vin and Vout voltage markers for
VDB markers.
 
Merhabalar arkadaşlar,

Pspice 9.1 student ile Analog ve dijital devre simulastonu yapmam lazım dönem ödevi olarak. Bu ödevde A/D sümulasyonun en azından bir yönünü tamamıyla kapsamam gerekiyor. 10 dakikalık video olarak kaydedecem. Fly back converter dizaynı mı yapsam ne yapsam bilemedim. Çokta vaktim yok 2 gün içinde vermem gerekiyor. Yardımcı olabilecek arkadaş varsa sevinirim. Communication dan pek anlamıyorum. Güç elektroniği bana yakın geliyor ama dediğim gibi pek sürem yok. Kim yardım edebilirse çok sevinirim.
Teşekkürler
 

Forum istatistikleri

Konular
127,950
Mesajlar
913,849
Kullanıcılar
449,596
Son üye
anilhikmet

Yeni konular

Geri
Üst