1 / 33

PSPICE Lecture – Transient Analysis

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

boyd
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. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. 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

  2. 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)

  3. 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

  4. 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.

  5. 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)

  6. 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.

  7. 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.

  8. 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.

  9. 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).

  10. 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

  11. 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

  12. 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.

  13. 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

  14. 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

  15. 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

  16. PSPICE Lecture - Transient Analysis 16 PSPICE Example using part VPULSE

  17. 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

  18. 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.

  19. 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

  20. PSPICE Lecture - Transient Analysis 20 Simulate the circuit and graph the results:

  21. 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

  22. 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)(1F) = 250 ms • A parametric analysis can be used to vary R from 10k  to 50k 

  23. 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

  24. 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:

  25. 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.

  26. 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.)

  27. 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

  28. 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:

  29. 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

  30. 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.

  31. 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

  32. 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

  33. 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)

More Related