- By
**boyd** - Follow User

- 445 Views
- Uploaded on

Download Presentation
## PSPICE Lecture – Transient Analysis

**An Image/Link below is provided (as is) to download presentation**

Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author.While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server.

- - - - - - - - - - - - - - - - - - - - - - - - - - E N D - - - - - - - - - - - - - - - - - - - - - - - - - -

Presentation Transcript

PSPICE Lecture – Transient Analysis

1

PSPICE – Transient Analysis

- Topics to be presented:
- Transient Analysis
- Analysis of 1st-order circuits
- Analysis of 2nd-order circuits
- Transient and Parametric Analysis

Reference: Additional examples available at: http://faculty.tcc.edu/PGordy/Orcad/index.htm

PSPICE Lecture – Transient Analysis

2

Transient Analysis in PSPICE

Simulation Settings window shows 4 analysis types

- Recall that there are 4 types of analysis in PSPICE.

- Bias Point (DC analysis where you place voltages, currents, and power on the schematic)
- DC Sweep (vary a source or component)
- AC Sweep (vary frequency)
- Transient (vary time)

PSPICE Lecture - Transient Analysis

3

Transient Analysis – A transient analysis is used to graph various quantities versus time. Recall that whatever is varied in PSPICE will be placed on the x-axis when graphs are created. So graphs created using a transient analysis will always have time, t, on the x-axis.

t = 0

+ VR -

Example: Use a transient analysis to graph the source voltage, resistor voltage, and capacitor voltage in the circuit below until they reach steady-state.

1 k

+

VC

_

+

_

100 V

1 F

PSPICE Lecture - Transient Analysis

4

Create the Project and draw the circuit: Create a project and draw the circuit shown below. Refer to earlier PSPICE lectures if you need help creating a project.

- Notes:
- Switch: Use part Sw_tClose from EVAL library for the switch
- Nodes: Label the nodes so that they can be referred to when graphing.
- Ground: Recall that all analog circuits require the 0 ground.

PSPICE Lecture - Transient Analysis

5

- Initial Capacitor Voltage: You must add the initial capacitor voltage, even if it is 0V. To do this:
- Double-click on the capacitor to open the Property Editor (shown on the left below)
- Select the part (column) named IC and select the Display tab
- Change the Display Format to Name and Value and select OK
- IC = should now appear on the schematic. Double-click on it and enter the value (20V in this example)

PSPICE Lecture - Transient Analysis

6

- Capacitor polarity: Capacitors has fixed + and - terminals in PSPICE. This is important when initial conditions are added. The 20V initial condition just added might act like -20V if the capacitor is upside down. To check the polarity:
- Select PSPICE – Create Netlist
- Select PSPICE – View Netlist
- The Netlist shown below indicates that capacitor C1 is connected from node 0 (+) to node C (-), so it is upside down! (The positive node is listed first.)

- Right-click on the capacitor and select Mirror Vertically

- Check the Netlist to see that the capacitor now has the correct polarity.

PSPICE Lecture - Transient Analysis

7

Create the Simulation Profile: Recall that exponential functions take 5Tau to decay, so we often want to perform a transient analysis for 5Tau. For this example:

Length of transient analysis = 5Tau = 5RC = 5(1k)(1uF) = 5ms

- Select PSPICE – New Simulation Profile
- Give the Simulation Profile a Name (any name is OK but using the schematic name is a good idea)
- Under Analysis Type select Time Domain (Transient)
- Under Run To Time: Enter 5ms (no spaces!)
- Select OK.

Fine point: By default approximately 100 points will be used to create each graph, so Maximum step size = (Run to time)/100.

In this example the blank box indicates that the Maximum step size is 5ms/100 = 50us. If you wished to use twice as many points you could enter 25us into the Maximum step size box.

PSPICE Lecture - Transient Analysis

8

- Analyze the circuit and graph the results
- Select PSPICE – Runto analyze the circuit. The graphing window should appear. Since we did a transient analysis from 0 to 5ms, time should vary from 0 to 5ms on the x-axis.

PSPICE Lecture - Transient Analysis

9

- Add waveforms
- Select Trace – Add trace and the Add Traces window will appear.
- Select or type the names of one or more waveforms to view

- Voltages in the list are all node voltages, so to find the resistor voltage V(B,C) was entered (positive terminal is listed first).

PSPICE Lecture - Transient Analysis

Add text

Toggle Cursor On/Off

Mark Point

10

Add text and mark points

Cursor

Cursor value – currently for V(B,C)

Select Waveform for Cursor

PSPICE Lecture - Transient Analysis

11

- Comments on the graph
- Capacitor voltage – Charges from the initial value (20V) to 100V as expected
- Resistor voltage – Decays from its initial voltage (100 – 20 = 80V) to zero
- Source voltage – Constant 100V

PSPICE Lecture - Transient Analysis

12

- Other graphing features
- There are many other graphing features which may be demonstrated in class or you may try on your own. Features include:
- Two cursors: PSPICE has two cursors that can be added to determine values of waveforms at different points.
- Controlling two cursors: The left-mouse button controls Cursor 1 and the right-mouse button controls Cursor2 (coarse adjustments). The cursors can be moved for fine adjustments with the arrow keys (Cursor1) or Shift + arrow keys (Cursor2).
- Marking Points: Use Plot - Label – Markor the toolbar.
- Saving graphs: Use Window – Display Control. Last graph is saved here automatically.
- Printing graphs: Use Window – Copy to Clipboard. This was used to create the graph on the previous slide. Note that the black background is changed to white.
- Graphing expressions: Note the functions in the Add Trace window, such as *, /, abs(), sin(), exp(), etc. You could, for example, graph V(C)*I(C1) or abs(I(C1)).
- Trace Properties: Right-click on a trace to change its color, line width, etc.
- Other: You can zoom in and out, use linear or log scales, turn off minor gridlines, etc.

PSPICE Lecture - Transient Analysis

13

Charging and discharging a capacitor using VPULSE

Suppose that the switch in the circuit below moves back and forth between A and B (for at least 5Tau in each position). The result is that the capacitor will charge and discharge repeatedly.

A

1 k

+

VC

_

B

+

_

VC

100 V

1 F

100 V

0 V

Switch moves to A

Switch moves to B

Switch moves to A

Switch moves to B

Switch moves to A

t

20Tau

5Tau

10Tau

15Tau

PSPICE Lecture - Transient Analysis

14

How is a switch moved back and forth in PSPICE?

This is simulated by using a pulse waveform.

VPulse

Connect

100 V

to the

RC circuit

Connect

0 V

to the

RC circuit

100 V

0 V

t

A

20Tau

5Tau

10Tau

15Tau

+

VC

_

+

VC

_

1 k

1 k

B

0 to100V

Pulse

Waveform

+

_

Equivalent

circuits

100 V

1 F

1 F

PSPICE Lecture - Transient Analysis

15

Part VPULSE in PSPICE

VPULSE is a part in the Source Library. It has various properties as defined below:

V1 = First voltage

V2 = Second voltage

TD = Time Delay (time before pulse starts). It is OK to use TD = 0.

TR = Rise Time (time to go from V1 to V2). TR cannot be 0.

TF = Fall Time (time to go from V2 to V1). TF cannot be 0.

PW = Pulse Width (time when output = V2)

PER = Period

Illustration:

VPulse

TF

TR

V2

PW

V1

TD

PER

t

PSPICE Lecture - Transient Analysis

17

Example: Use a transient analysis to graph the capacitor voltage in the circuit below. Assume that the switch moves to position A at t = 0 and then moves back and forth between A and B every 5Tau to repeatedly charge and discharge the capacitor. Graph VC as it charges and discharges 3 times.

A

+

VC

_

1 k

B

+

_

100 V

1 F

PSPICE Lecture - Transient Analysis

18

Solution:

Create the Project and draw the circuit: Create a project and draw the circuit shown below.

- Notes:
- Use part VPULSE from the Source Library
- 5Tau = 5RC = 5ms, so use PW = 5ms (the capacitor charges here)
- 5RC is also needed for the capacitor to discharge, so use PER = 10ms (time to charge and discharge)
- TR and TF cannot be 0, so make them very small compared to PER. Note that 1ns is only one ten-millionth of PER.
- The initial condition for the capacitor must be set to 0V.

PSPICE Lecture - Transient Analysis

19

Create a new Simulation Profile and determine the length of the analysis:

In order to charge and discharge the capacitor 3 times, the analysis should last for 30Tau (or 30ms) as illustrated below.

VC

100 V

0 V

t

30Tau

20Tau

25Tau

5Tau

10Tau

15Tau

PSPICE Lecture - Transient Analysis

21

- Parametric Analysis in PSPICE
- A parametric analysis is used to vary a second parameter to generate a series of curves. Many types of parametric analysis are possible in PSPICE.
- Examples:
- Top Example: Vary voltage and current
- Bottom Example: Vary time and resistance

Vary current (parametric analysis

Vary voltage (DC Sweep)

Vary R (parametric analysis

Vary time (Transient analysis

PSPICE Lecture - Transient Analysis

22

Example:

Graph VC versus time as the capacitor charges for R = 10k, 20k, 30k, 40k and 50k.

t = 0

R

+

VC

_

+

_

100 V

1 F

- Solution:
- A transient analysis can be used to vary time from 0 to 5Tau.
- Use the largest value of Tau, so 5Tau = 5(50k)(1F) = 250 ms
- A parametric analysis can be used to vary R from 10k to 50k

PSPICE Lecture - Transient Analysis

23

Create the Project and draw the circuit: Create a project and draw the circuit shown below.

Use the following steps to vary a resistor:

Use a variable resistor part, R_var

Change the value of R_var to a name in braces, such as {Rvalue}

Change the property SET to 1 for R_var (be sure to display it also)

Add a part named PARAM from the Special Library

Add a property (column) to PARAM with the same name as the resistor value in braces – Rvalue in this cases

PSPICE Lecture - Transient Analysis

24

- Create a new Simulation Profile
- Select Time Domain (Transient) for the Analysis type.
- Enter 250 ms for the value for Run to time:

PSPICE Lecture - Transient Analysis

25

- Check the box labeled Parametric Sweep. (Note that the window is the same one used with a DC Sweep analysis.)
- Select Global parameter
- Enter Rvalue for the Parameter name
- Enter the Start value, End value, and Increment.
- Select OK.

PSPICE Lecture - Transient Analysis

Simulate the circuit and graph the results:

(Select OK when the Available Sections window appears to select data for all 5 curves.)

PSPICE Lecture - Transient Analysis

27

- Analyzing 2nd-order circuits in PSPICE
- There is not much difference betweenanalyzing 2nd-order circuits and analyzing 1st-order circuits. A transient analysis is still used. One difference is in determining the length of the analysis.
- 1st-order circuit:
- Length of transient analysis = 5Tau
- Find Tau = ReqC or L/Req
- Or find Tau from the expression x(t) = B + Ae-t/Tau
- Example: If v(t) = 10 – 10e-500t, then Tau = 1/500 = 2ms, so 5Tau = 10ms
- 2nd-order circuit:
- Recall that the natural response has three forms: overdamped, critically-damped, and underdamped. Since an overdamped response has two exponential terms, use the one with the largest Tau (the dominant root).
- In each case assume that the exponential terms have the form e-t/Tau and again use: Length of transient analysis = 5Tau
- Example: If v(t) = e-500t[20cos(50t) + 30sin(50t)] (underdamped), then Tau = 1/500 = 2ms, so 5Tau = 10ms

PSPICE Lecture - Transient Analysis

28

Example: Graph VC versus time until the capacitor reaches steady state.

t = 0

1 mH

12.62

+

VC

_

+

_

20 V

1.57 F

Solution:First determine the length of the analysis.

This is a series RLC circuit so:

PSPICE Lecture - Transient Analysis

29

Create the Project and draw the circuit: Create a project and draw the circuit shown below.

- Notes:
- Set the initial condition to 0 for the capacitor and the inductor (IC = 0).
- Label the nodes. The node voltage V(C) is the capacitor voltage.

- Create the simulation profile
- Perform a transient analysis from 0 to 0.8 ms
- 3. Analyze the circuit and graph the capacitor voltage
- See the following slide

PSPICE Lecture - Transient Analysis

30

Note that the capacitor voltage is as expected: It has an initial voltage of 0V, a final voltage of 20V, and it is underdamped.

Two other quantities are useful to show on this graph: rise time and % overshoot. They are defined on the following slides.

PSPICE Lecture - Transient Analysis

31

Rise Time(tr) – the time for a waveform to go from 10% of its final value to 90% of its final value. Rise time can be used with any order circuit and any type of response.

Example:

10V

9V

1V

tr

t

0V

PSPICE Lecture - Transient Analysis

32

% Overshoot – This term is only used with underdampedcircuits. It is a measure of how far the waveform shoots past its final value before settling on the final value. It is defined (for a voltage) as:

Example:

v(t)

13V

10V

0V

t

PSPICE Lecture - Transient Analysis

33

Add rise time and % overshoot to the previous graph:

- A cursor was used to mark 3 points at:
- 2V (10% of the 20V final value)
- 18V (90% of the 20V final value)
- The max value (use the cursor peak tool)

Download Presentation

Connecting to Server..