PSpice Tutorial This is a tutorial designed to guide you through the simulation assignment included in the first homework set. You may either use the program as installed in the lab, or you may install it on your own computer. Installation Go to the web page http://www.electronics-lab.com/downloads/schematic/013/. Scroll to the bottom and click on Download PSPICE 9.1 student version, and when a dialog box comes up click on Run. It will then download a zip file to your computer, after which a dialog box will pop up asking you whether you want to unzip the file. Select a location where you want the files to go and then click the button to unzip the files. On the same web page you may also want to download the PSpice user guide by clicking on PSPICE.PDF and/or the Capture user guide by clicking on CAPUG.PDF (note that the web page has this last one mislabeled as digital parts ). Disable your virus protection software and then go to the area where you unzipped the installation files and double click on Setup.exe. After it starts, do the following: Click OK or YES one or two times until you get to a dialog box called Select Schematic Editor. Only Capture should be checked. (You can try the other editor if you like, but I ve never messed with it myself.) Then click on Next. It will ask you to Select Installation Directory. Click Next to accept the default. It will ask you to Select Program Folder. Click Next to accept the default. Click Next to Start copying files. You may have to click OK a couple of times in response to complaints about file types already being registered. Finally, in the last dialog box click Finish and then take a look at the release files. Making a New Project and Schematic First, make a new empty folder on your computer where you want all the files for this project to be stored. Then, start up the program Capture Student. On the File menu, select New Project. In the New Project dialog box, give the project a name, such as hw1, and use the Browse button to find your folder. Then, be sure to click Analog or Mixed A/D under Create a new project using. Finally click OK and then you ll get a box labeled Create Pspice Project with two choices. Select Create a blank project and then click OK. The new project will be opened with two windows, one labeled hw1.opj, which shows all the files in the project, and another labeled 1
Schematic 1 : Page 1. We are going to work here with the schematic window, so go ahead and maximize it. Go to the Place menu and select Part. In the Place Part dialog box click on Add Library. A Browse File dialog box will pop up. Open the folder named Pspice in this dialog box and then double click on analog.olb. Click Add Library again and this time double click on source.olb. This will give you enough parts to work with for this project, at least. Now, still in the Place Part dialog box, click on SOURCE in the Libraries list (it probably already is selected) and then scroll down through the Part List and click on AC and then click OK. The dialog box will go away and you will see that the cursor has a part attached to it. Move the cursor to where you want the part to be and then single click. Finally, hit the Esc key on your keyboard to get back the normal cursor. Next, do Place Part again and click on ANALOG in the Libraries list of the Place Part dialog box. Scroll down through the Part List and click on R followed by OK. This time, place two resistors before hitting Esc. Note that you can rotate the part before placing it by hitting ctrl-r, or you can rotate it afterwards by clicking it to highlight it and then selecting Rotate on the Edit menu. Similarly, place a capacitor ( C ) and an inductor ( L ) on your schematic. Arrange the parts neatly by clicking and dragging, more-or-less as shown on the schematic in the homework assignment. Now wire the parts together as follows. In the Place menu, select Wire. You will see the cursor change to a +. Put the cursor on a node of one part and then move it to the node of another part and click to wire them together. You can also click in-between parts to nail down the wire at a corner, for example, and you can click on top of another wire to connect two wires together. Hit the Esc key to stop making wires and get back the arrow cursor. It can be tricky to be sure that all the wires are connected. If one is not connected, drag it a little bit to a connect point, and with some luck it will connect. To see whether a part is really connected, you can click on it and drag it a little bit. If the wires are connected, then they will follow with the part. Connections between wires should be marked with a heavy dot. If two wires cross, they are not connected unless there is such a dot at the intersection. It is a good practice in drawing schematics never to make a connection where two wires cross. Instead, only connect wires at T intersections and there will be less likelihood of confusion. Now, give each part its correct value, according to the homework assignment. For example, for the capacitor, click on the value ( 1n ) and enter 20uF (the F is not required, as Spice always works in Farads for capacitance, and the u is the Spice symbol for micro ). Leave the source as 1 ac, but for illustration, also give it 0.1 dc. Now, PSpice is very particular about there being a node defined as Ground, and it must be named 0. If you don t do this, then it will give you many error messages about floating nodes. So, go to the Place menu and select Ground. In the dialog box that pops up, choose GND/CAPSYM and then click OK. Place the symbol somewhere below the circuit and then connect it with a wire to the bottom wire of the circuit. Double 2
R1 R2 I 1ac 0.1dc 1 C1 20uF L1 2mH 0 Figure 1. The schematic, as drawn using Capture Student. click on the ground symbol, and the Property Editor will appear. In the column labeled Name replace GND with 0 (that s a zero, not the letter O). After entering the 0, click on the Name column to select it and then click the Display button. In the Display Properties dialog box under Display Format click alue Only and OK. Then click the Apply button and exit the Property Editor. All the display-property business does here is make the zero appear on the schematic, but it illustrates in general how to go about making properties visible on the schematic. Now we ll add a couple of widgets that will tell PSpice what we want to look at in the circuit. Suppose we want to see the current going through the -ohm resistor (which is the same as the current through the source, of course). In the lower tool bar, click on the icon that looks like an I connected to a handle. It will appear on the cursor, so move it and attach it to one end of the resistor. Next, suppose we want to see the voltage on the node connecting the -ohm resistor to the inductor. Click on the icon that looks like a connected to a handle and attach that thing to the wire. Your completed schematic should look something like what you see in Figure 1. Simulating Your Schematic Now you have to tell PSpice what kind of simulation you want done on your circuit. Go to the PSpice menu and select New Simulation Profile. In the resulting dialog box give it a name, such as ACanalysis. In the resulting Simulation Settings dialog box select the Analysis tab, and under Analysis type select AC Sweep/Noise. Under AC Sweep Type select Logarithmic, and then enter the Start Frequency as 1, the End * source HW1 _1 N00013 0 DC 0.1dc AC 1ac R_R1 N00013 N00019 R_R2 N00019 N00022 L_L1 0 N00022 2mH C_C1 0 N00019 20uF Figure 2. The netlist generated from the schematic. 3
Figure 3. The PSpice output for the AC analysis. Frequency as 1E and the Points/Decade as 100. Then click OK. Now, go back to the PSpice menu and select Create Netlist. Then from the same menu select iew Netlist. You don t have to do this in order to simulate, but I want you to see what the netlist is. What you should see is something looking nearly identical to Figure 2. This is a text representation of your circuit. It has one line for each part in your circuit, and each line tells what nodes the part is connected to. The nodes all have names starting with N, except for the one we purposely named 0. Each line also gives the characteristics of the part. Understand that this netlist is what PSpice ingests. The PSpice program does not look at your schematic. You could have skipped the whole schematic exercise and entered the netlist by hand with a text editor. In fact, that is how people used to simulate circuits (and how a few stubborn old-fashioned engineers still do). You ll probably see lots of advantages of the graphical representation afforded by the schematic editor as you go along. Now, close the netlist, go to the PSpice menu, and select Run. A PSpice window will pop open, and you will also see the schematic updated with DC voltage readings, as shown in Figure. The PSpice window will show a plot of the circuit response versus frequency, as illustrated in Figure 3 (except that it will appear in color), where you see the current through R1 and the voltage on the right-hand-side node of R2. The current and voltage widgets that we placed on the schematic caused those two items to be plotted. Now, you can see that the PSpice window has lots of menus, and you can make use of them to plot anything else you may want to see, rerun the simulation, and so forth. To do those things, you can either interact directly with PSpice or else go back to the schematic, modify it, and then rerun PSpice.
R1 R2 100.0m I 0.00m 0 1ac 0.1dc 1 C1 20uF L1 2mH 0 0 Figure. The schematic after running the simulation. Note how the DC voltages have been marked on each of the nodes. These result from the 0.1dc setting of the source. Transient Simulation Now that you have completed a simulation in the frequency domain (AC), try a simulation in the time domain (Tran). Modify your schematic as follows. Delete the AC voltage source by selecting it and hitting the Delete key. Then place a part from the Source library called Pulse where the AC source used to be. Fill in all of the values as shown in Figure 5. The meaning of the values is, respectively, the low voltage, the high voltage, the time delay before the pulses turn on, the rise time, the fall time, the width of each pulse, and the period of the repetition. We ve set it up to produce something like a clock signal with a period of 1 ms and rise and fall times of 0.05 ms. Then, attach voltage monitor widgets as shown in the figure. Now, to go to the PSpice menu and select New Simulation Profile. Give the new profile a name something like HW1Tran and set the analysis type to Time Domain (transient), and set the Run to time to 3m. Click OK and then run the simulation. You should see a PSpice display very close to what is shown in Figure, where you see plotted both the input clock-like pulses, exactly as we defined it, and the corresponding butchered output pulses (the R1 R2 1 = 0 2 = 0.5 TD = 1m TR = 50u TF = 50u PW = 0.5m PER = 1m 2 C1 20uF L1 2mH 0 Figure 5. The schematic as modified for doing a transient analysis. 5
Figure. Result of the transient simulation. voltage across the inductor). So, by now you ve essentially completed the simulation in the first homework assignment. There will be more to come, however, especially including transistors, so I encourage you to play around with this software and get familiar with it. You should have some fun with it. Change the component values around and see if you can understand what it does to the frequency response. What happens if you feed it an input clock-like square wave with a period equal to the resonance frequency versus far above or below resonance? What if you input a step function with zero rise time? What if you input a sharp spike? Make up your own circuits and try them out. With the simulation there is no danger of blowing a fuse or smoking a part, so don t be afraid to be creative.