Lab 1: Analysis of DC and AC circuits using PSPICE

Transcription

1 Lab 1: Analysis of DC and AC circuits using PSPICE 1. Objectives. 1) Familiarize yourself with PSPICE simulation software environment. 2) Obtain confidence in performing DC and AC circuit simulation. 2. Introduction. The Simulation Program with Integrated Circuit Emphasis (SPICE) became an industry standard for circuit simulation. In this course we will use the PC-compatible version (PSPICE). You can perform the assignments either on your own PC or in the CADLAB (Room 281 Light Eng. Bldg). It is beneficial to start working in CADLAB since you can get some help there to speed up the learning process. Demo version of the PSPICE (enough for our purposes) can be downloaded from Cadence website. 3. OrCAD Pspice installation. If you would like to use OrCAD Pspice software with your own computer, you can install it by following the steps below. 1) Follow the link: 2) Click on: Download FREE - OrCAD 16.5 demo software (851MB) includes OrCAD Flow Tutorial with the example design files. 3) You will be prompted to enter and submit your information. Provide necessary information and wait for an from Cadence. 4) Follow the link provided in the from Cadence 5) Check OrCAD 16.5 Demo Software (All Products) and click on submit 6) Follow the link to start downloading the software 7) Unzip the downloaded folder and install the software 4. OrCAD Pspice preparation. 1) Start OrCAD Capture 2) Create a new project: Click the Create document icon on the toolbar or follow [File] [New] [Project]. Create document Create document 1

2 3) Enter a project name and a folder location to save your work and choose Analog or Mixed A/D. Then click OK. Enter project name Choose Analog or Mixed A/D Select folder location for this project 4) Select Create a blank project and click OK. 5) You will see two main windows at this point: Project Manager window and Schematic wondow. You will draw the circuit in Schematic window. First you are going to make sure that all the libraries are added to your system. Click on Schematic window to activate it. Project Manager window Schematic window 2

3 6) Select Place Part... or click on Place part icon in Draw toolbar or ribbon. 7) Place Part window will pop up somewhere in the main window. Make sure you see ANALOG and SOURCE in Libraries window. If not click on Add library icon, find analog.olb and source.olb under../orcad_16.5_xxx/tools/capture/library/pspice/ and open the files to add them to the libraries to your system. If you cannot find any of those files, consult with your teaching assistant. Make sure you have ANALOG and SOURCE here Add library icon 8) Select Place Ground... or click on Place ground icon in Draw toolbar or ribbon. 3

4 9) Place Ground window will pop up somewhere in the main window. Make sure you see SOURCE in Libraries window. If not, find source.olb in the same location shown in 3). Now we are ready to draw circuits for simulations. Make sure you have SOURCE here 5. Examples. You can learn step by step how to draw and simulate basic DC and AC circuit using simple examples here. 5.1 DC Analysis We are going to simulate the circuit shown below. Let s simulate the voltage at node 1 and current through R2 as we change the voltage V1 from -10V to +10V and obtain IV characteristics of R1. We will add two resistors, one DC voltage source, a ground and wires connecting components. node 1 1) Place DC voltage source: Open Place Part again. Click on SOURCE in Libraries window, find and double click on VDC in Part List. Then you will see a floating VDC icon on Schematic window. Click once somewhere in the window and then the part will be placed. Then right click somewhere in the window then select End Mode or simply use ESC to terminate the mode. Double click on VDC The icon moves with your mouse pointer Select SOURCE 4

5 2) Place a ground: Open Place Ground window (see 4-(8)). Click on SOURCE in Libraries window, find and double click on 0 in Part List. Place it in Schematic window in the same manner as you did for VDC. 3) Place resistors: Open Place Part again. Simple resistor R is in the library ANALOG Place the part in the same manner as you did for VDC. After placing the resistors, hover the mouse pointer on the left and right end of the resistors. You will see one end [/R1/1 Number:1] and the other end [/R1/2 Number:2]. Pspice recognizes the current through R1, I(R1) as shown below. I(R1) is the current entering R1 at node R1:1 (or R1/1) and leaving its node R1:2 (or R1/2). You will see the importance of the polarity of elements in Pspice simulations. [/R1/1 Number:1] [/R1/2 Number:2] + - I(R1) 4) Place wires: Select Place Wire... or click on Place wire icon in Draw toolbar or ribbon. Then connect the circuits components 5

6 5) Using the wires connect the circuit components like shown below. Make sure the polarity of elements is in the same manner. Click on R1, R2 or V1 It turns magenta Right click on it Bring up the menu besides your mouse pointer and you can modify the component. For now you are going to use Mirror Horizontally, Mirror Vertically, Mirror Both and Rotate to change it to the required direction in the circuit. Make sure the polarity of elements by repeating 3). [/R1/1 Number:1] [/R1/2 Number:2] [/R2/1 Number:1] [/R2/2 Number:2] 6) Now we are ready to run the simulation: Select Pspice New Simulation Profile. New Simulation window will pop up 7) New Simulation window will pop up. Give a name for the simulation and click on Create 6

7 8) Select Pspice Edit Simulation Profile. 9) You will see the new window Simulation Settings - your simulation name. Under Analysis tab, change Analysis type to DC sweep and make sure Primary Sweep is checked in Options. Select Voltage source in Sweep variable and give the exact name of your voltage source under Name:. In our case V1. Select Linear for Sweep type and make Start value -10, End value 10 and Increment 0.1. Then click OK to exit the window. The setting you made here means that simulator changes the voltage of V1 from -10V to 10V with the increment of 0.1V (-10V, -9.9V, -9.8V,..., 10V) and simulate the voltages and currents of the circuit each time. Select DC Sweep Check Primary Sweep Give the name of your voltage source 10) Now you can run the simulation: Pspice Run 7

8 11) SCHEMATIC1-your simulation name will pop up as a whole new window. X-axis is for voltage V1 (labeled as V_V1) from -10V to 10V and y-axis is not defined yet. 12) Add voltage at node 1 as y-axis: Trace Add Trace... 13) Add Traces will pop up. Node 1 (in the schematic at page 4) is identical to the node R2:1. Click once on V(R2:1) and it should appears on Trace Expression window. Then click OK. Click on V(R2:1) 8

9 14) Then you will see the result shown below. 15) If you want to see the voltage across R1, then repeat 13) but with V(R1:1)-V(R1:2). 16) If you want to delete the traces, Trace Delete All Traces. Then you will see the original window shown in 11). 9

10 17) IV characteristics of R1: x-axis has to be replaced with the voltage across R1 (V(R1:1)-V(R1:2)) and y-axis should be set I(R1). First let us replace x-axis variable with V(R1:1)-V(R1:2). Plot Axis Settings ) Axis Settings will pop up. Click on Axis Variable under X Axis tab. 19) X Axis Variable window appears and make changes on Trace Expression to V(R1:1)-V(R1:2). 10

11 20) Delete the traces by following 16) and add I(R1) on y-axis by following 12) and 13). Then you will see the IV characteristics of R1 as shown below. 21) Output File: To see the simulation output file (including netlists), View Output File. 22) Bias Point solution: If you simply want to see the voltages, currents and powers dissipated and delivered in a given steady state condition, you can use Bias Point instead of DC Sweep in 9). 23) Set the value of V1 to whatever value you want: Click on 0Vdc in the schematic and Display Properties will pop up. Change the value to 5Vdc and click OK to close the window. Then run the simulation in the same manner like in 10). 11

12 24) Schematic1 - your simulation name will be generated again like in 11) but we do not use this output window, so close it. In the OrCAD Capture window while your schematic being active, follow Pspice Bias Points and click on whichever you need. Make sure it is checked 25) Then you will see the corresponding values besides the schematic you drew. The currents are shown in absolute values (shown in positive values). To see the direction of the currents, see the node where the dashed lines are leaving. The dashed line always leaves at one end of an element and it is the node where the current entering into the element. The example below is for V(V1)=-5Vdc. Direction of the current 12

13 5.2 AC Analysis Consider the simple RC circuit shown below. We are going to perform a circuit analysis in frequency domain. - Obtain magnitude and phase response of voltages across the resistor and capacitor. - Draw vector diagram of voltage phasors. 1) If you like to use the same project, then make a new page. Under Project manager window, right click on SCHEMATIC1 and select New Page 2) Draw the circuit in the same manner. You will use VAC instead of VDC for the voltage source. [/R3/1 Number:1] [/R3/2 Number:2] [/C1/1 Number:1] [/C1/2 Number:2] 13

14 3) Once the circuit is ready, create the new simulation profile as shown in 5-1-6) and 7) and select Edit Simulation Profile. Simulation Settings - your simulation profile name will appear. Under Analysis tab, change the analysis type to AC Sweep/Noise and corresponding modifications shown below. Points/Decade means the number of simulation points in a decade (for example from 10kHz to 100kHz) in frequency domain. 4) After leaving the window, run the simulation. Then Schematic1 - your simulation profile name will appear in the same way, but x-axis is for frequency domain from 10 to 100 MHz. Y-axis is not defined yet. 5) Magnitude response: Open Add Traces window and set Trace Expression to be (V(R3:1)-V(R3:2))/V(V2:+). This is the expression for magnitude response. Do the same thing for C1 and you will see the simulation result as shown below. Remember that magnitude response should not have any unit. 14

15 6) Phase response: First we need to add plot. Plot Add Plot to Window. 7) Then you will see a new plot with SEL>> on the bottom left corner. It means that the upper graph is now activated and you can add traces on it. 15

16 8) Open Add Traces. Functions and Macros on the right pane of this window shows the available functions you can use to trace the simulation results. To trace a phase, you will use P() from the choices and insert your variable in the parenthesis or you can simply type in P(V(R3:1)-V(R3:2)) in Trace Expression for phase response of the voltage across R3. 9) Do the same for C1 and you will see the phase response of the voltages of R3 and C1. 16

17 10) Remember that the phase responses you obtained here are with respect to the phase of the voltage supplied by V2, since V(V2) has the phase of zero degree in your simulations. The vector diagrams of the voltage phasor at 1kHz, resonance and 1MHz are shown below. Remember the diagrams take V(V2) as reference. 1kHz resonance 1MHz P(V R3 ) 90 P(V C1 ) 0 P(V V2 ) = 0 P(V R3 ) = 45 P(V C1 ) = -45 P(V V2 ) = 0 V R3 P(V R3 ) 10 P(V C1 ) -80 P(V V2 ) = 0 V R3 V R3 V C1 V R3 0 V C1 1 V V2 = 1 V V2 V R3 0.7 V C1 0.7 V V2 = 1 V C1 V V2 V R3 1 V C V V2 = 1 V C1 V V2 If you take current phasor I=I V2 =I R3 =I C1 as reference, then P(V C1 ) is always -90 and P(V R3 ) is always 0. For detail, check our lecture notes and textbook Basic Electronic Circuit Analysis by D. Johnson et al. 6. Netlist. We will be using graphical interface but it is recommended that you learn how to use the netlist circuit descriptions approach as well. To perform the circuit analysis using file based simulations: Type and save the netlist file with the extension *.cir in any text editor. Then open the file and run the simulation with PSpice. The results of the analysis (nodal DC voltages, currents in voltage sources, voltages across current sources) can be found in the output file, created by PSpice. 7. Simulation Exercises. 7.1 DC Analysis Consider the circuit below. 1) Find the voltage at nodes N1 and N2 using bias point analysis. 2) Obtain the plots of the currents through resistors R1, R2, R3 and R4 as a function of voltage V1 using DC sweep with the voltage source value in the range form 10V to +10V with 0.1V increment. 3) Obtain the plot of the current through resistor R2 as a function of voltage across it. N1 N2 17

18 7.2 AC Analysis Consider the series LCR circuit shown below. 1) Obtain the frequency dependences of the (magnitude and phase of) voltages across resistor R1, capacitor C1 and inductor L1. 2) Obtain frequency dependences of the magnitude and phase of the current supplied by source V1. Find the resonant frequency and indicate it on the plots. 3) Repeat 1) for: (a) L1 = 1 H, C1 =1 µf but R1 changed to 10 kω; and (b) L1 = 1H, R1 = 1kΩ but C1 changed to 10 µf. Comment on observed changes. 4) Using the simulation results, draw the voltage phasors on vector diagrams for L1 = 1 H, C1 =1 µf, R1 = 1 kω at frequencies 10 Hz, 100 Hz, 1 khz, and at the resonance. For reference use the current phasor I. 8. Report. The report is due at the beginning of Lab 3. It should include the goal, a short description of the work, the results and conclusions of part 7.1 and 7.2. Please comment as much as you can on the results you have obtained. For instance, explain why the currents through R1 and R2 are different while the currents through R3 and R4 are the same (for 7.1). Be creative in your analysis. Look for interesting things to comment on. 18