University of Pennsylvania Department of Electrical and Systems Engineering

PSPICE

A brief primer

Contents

1. Introduction 2. Use of PSpice with OrCAD Capture 2.1 Step 1: Creating the circuit in Capture 2.2 Step 2: Specifying the type of analysis and simulation BIAS or DC analysis DC Sweep simulation 2.3 Step 3: Displaying the simulation Results 2.4 Other types of Analysis: 2.4.1 Transient Analysis 2.4.2 AC Sweep Analysis 3. Additional Circuit Examples with PSpice 3.1 Transformer circuit 3.2 AC Sweep of Filter with Ideal Op-amp (Filter circuit) 3.3 AC Sweep of Filter with Real Op-amp (Filter Circuit) 3.4 Rectifier Circuit (peak detector) and the use of a parametric sweep. Peak Detector simulation Parametric Sweep 3.5 AM Modulated Signal 3.6 Center Tap Transformer 4. Adding and Creating Libraries: Model and Part Symbol files 4.1 Using and Adding Vendor Libraries 4.2 Creating PSpice Symbols from an existing PSpice Model file 4.3 Creating your own PSpice Model file and Symbol Parts References

1. INTRODUCTION

SPICE is a powerful general purpose analog and mixed-mode circuit simulator that is used to verify circuit designs and to predict the circuit behavior. This is of particular importance for integrated circuits. It was for this reason that SPICE was originally developed at the Electronics Research Laboratory of the University of California, Berkeley (1975), as its name implies:

JVdS 2006

Simulation Program for Integrated Circuits Emphasis. PSpice is a PC version of SPICE (which is currently available from OrCAD Corp. of Cadence Design Systems, Inc.). A student version (with limited capabilities) comes with various textbooks. The OrCAD student edition is called PSpice AD Lite. Information about Pspice AD is available from the OrCAD website: http://www.orcad.com/pspicead.aspx The PSpice Light version has the following limitations: circuits have a maximum of 64 nodes, 10 transistors and 2 operational amplifiers. SPICE can do several types of circuit analyses. Here are the most important ones:
Non-linear DC analysis: calculates the DC transfer curve. Non-linear transient and Fourier analysis: calculates the voltage and current as a function of time when a large signal is applied; Fourier analysis gives the frequency spectrum. Linear AC Analysis: calculates the output as a function of frequency. A bode plot is generated. Noise analysis Parametric analysis Monte Carlo Analysis
In addition, PSpice has analog and digital libraries of standard components (such as NAND, NOR, flip-flops, MUXes, FPGA, PLDs and many more digital components, ). This makes it a useful tool for a wide range of analog and digital applications. All analyses can be done at different temperatures. The default temperature is 300K. The circuit can contain the following components:

Independent and dependent voltage and current sources Resistors Capacitors Inductors Mutual inductors Transmission lines Operational amplifiers Switches Diodes Bipolar transistors MOS transistors JFET MESFET Digital gates and other components (see users manual).
2. PSpice with OrCAD Capture (release 9.2 Lite edition)
Before one can simulate a circuit one needs to specify the circuit configuration. This can be done in a variety of ways. One way is to enter the circuit description as a text file in terms of the elements, connections, the models of the elements and the type of analysis. This file is called the SPICE input file or source file and has been described somewhere else (see http://www.seas.upenn.edu/%7Ejan/spice/spice.overview.html). An alternative way is to use a schematic entry program such as OrCAD CAPTURE. OrCAD Capture is bundled with PSpice Lite AD on the same CD that is supplied with the textbook. Capture is a user-friendly program that allows you to capture the schematic of the circuits and to specify the type of simulation. Capture is non only intended to generate the input for PSpice but also for PCD layout design programs.

Figure 4: Place Part window 3. Select the library that contains the required components. Type the beginning of the name in the Part box. The part list will scroll to the components whose name contains the same letters. If the library is not available, you need to add the library, by clicking on the Add Library button. This will bring up the Add Library window. Select the desired library. For Spice you should select the libraries from the Capture/Library/PSpice folder. Analog: contains the passive components (R,L,C), mutual inductane, transmission line, and voltage and current dependent sources (voltage dependent voltage source E, currentdependent current source F, voltage-dependent current source G and current-dependent voltage source H). Source: give the different type of independent voltage and current sources, such as Vdc, Idc, Vac, Iac, Vsin, Vexp, pulse, piecewise linear, etc. Browse the library to see what is available. Eval: provides diodes (D), bipolar transistors (Q), MOS transistors, JFETs (J), real opamp such as the u741, switches (SW_tClose, SW_tOpen), various digital gates and components. Abm: contains a selection of interesting mathematical operators that can be applied to signals, such as multiplication (MULT), summation (SUM), Square Root (SWRT), Laplace (LAPLACE), arctan (ARCTAN), and many more. Special: contains a variety of other components, such as PARAM, NODESET, etc.
4. Place the resistors, capacitor (from the Analog library), and the DC voltage and current source. You can place the part by the left mouse click. You can rotate the components by clicking on the R key. To place another instance of the same part, click the left mouse button again. Hit the ESC key when done with a particular element. You can add initial conditions to the capacitor. Double-click on the part; this will open the Property window that looks like a spreadsheet. Under the column, labeled IC, enter the value of the initial condition, e.g. 2V. For our example we assume that IC was 0V (this is the default value). 5. After placing all part, you need to place the Ground terminal by clicking on the GND icon (on the right side toolbar see Fig. 3). When the Place Ground window opens, select GND/CAPSYM and give it the name 0 (i.e. zero). Do not forget to change the name to 0, otherwise PSpice will give an error or "Floating Node". The reason is that SPICE needs a ground terminal as the reference node that has the node number or name 0 (zero).

Figure 5: Place the ground terminal box; the ground terminal should have the name 0 6. Now connect the elements using the Place Wire command from the menu (PLACE/WIRE) or by clicking on the Place Wire icon. 7. You can assign names to nets or nodes using the Place Net Alias command (PLACE/NET ALIAS menu). We will do this for the output node and input node. Name these Out and In, as shown in Figure 2.
2.1.3. Assign Values and Names to the parts 1. Change the values of the resistors by double-clicking on the number next to the resistor. You can also change the name of the resistor. Do the same for the capacitor and voltage and current source. 2. If you haven't done so yet, you can assign names to nodes (e.g. Out and In nodes). 3. Save the project
2.1.4. Netlist The netlist gives the list of all elements using the simple format: R_name node1 node2 value C_name nodex nodey value, etc. 1. You can generate the netlist by going to the PSPICE/CREATE NETLIST menu. 2. Look at the netlist by double clicking on the Output/name.net file in the Project Manager Window (in the left side File window). Note on Current Directions in elements: The positive current direction in an element such as a resistor is from node 1 to node 2. Node 1 is either the left pin or the top pin for an horizontal or vertical positioned element (.e.g a resistor). By rotating the element 180 degrees one can switch the pin numbers. To verify the node numbers you can look at the netlist: e.g. e.g. R_R2 R_R2 node1 node2 10k 0 OUT 10k
Since we are interested in the current direction from the OUT node to the ground, we need to rotate the resistor R2 twice so that the node numbers are interchanged: R_R2 OUT 0 10k
2.2 Step 2: Specifying the type of analysis and simulation As mentioned in the introduction, Spice allows you do to a DC bias, DC Sweep, Transient with Fourier analysis, AC analysis, Montecarlo/worst case sweep, Parameter sweep and Temperature sweep. We will first explain how to do the Bias and DC Sweep on the circuit of Figure 2.
2.2.1 BIAS or DC analysis 1. With the schematic open, go to the PSPICE menu and choose NEW SIMULATION PROFILE. 2. In the Name text box, type a descriptive name, e.g. Bias 3. From the Inherit From List: select none and click Create. 4. When the Simulation Setting window opens, for the Analyis Type, choose Bias Point and click OK. 5. Now you are ready to run the simulation: PSPICE/RUN 6. A window will open, letting you know if the simulation was successful. If there are errors, consult the Simulation Output file. 7. To see the result of the DC bias point simulation, you can open the Simulation Output file or go back to the schematic and click on the V icon (Enable Bias Voltage Display) and I icon (current display) to show the voltage and currents (see Figure 6).

JVdS 2006 7

The check the direction of the current, you need to look at the netlist: the current is positive flowing from node1 to node1 (see note on Current Direction above).
Figure 6: Results of the Bias simulation displayed on the schematic.
2.2.2 DC Sweep simulation
We will be using the same circuit but will evaluate the effect of sweeping the voltage source between 0 and 20V. We'll keep the current source constant at 1mA. 1. Create a new New Simulation Profile (from the PSpice Menu); We'll call it DC Sweep 2. For analysis select DC Sweep; enter the name of the voltage source to be swept: V1. The start and end values and the step need to be specified: 0, 20 and 0.1V, respectively (see Fig. below).
Figure 7: Setting for the DC Sweep simulation. 3. Run the simulation. PSpice will generate an output file that contains the values of all voltages and currents in the circuit.
2.3 Step 3: Displaying the simulation Results PSpice has a user-friendly interface to show the results of the simulations. Once the simulation is finished a Probe window will open.
Figure 8: Probe window 1. From the TRACE menu select ADD TRACE and select the voltages and current you like to display. In our case we'll add V(out) and V(in). Click OK.
Figure 9: Add Traces window

JVdS 2006 9

2. You can also add traces using the "Voltage Markers" in the schematic. From the PSPICE menu select MARKERS/VOLTAGE LEVELS. Place the makers on the Out and In node. When done, right click and select End Mode.
Figure 10: Using Voltage Markers to show the simulation result of V(out) and V(in) 3. Go to back to PSpice. You will notice that the waveforms will appear. 4. You can add a second Y Axis and use this to display e.g. the current in Resistor R2, as shown below. Go to PLOT/Add Y Axis. Next, add the trace for I(R2). 5. You can also use the cursors on the graphs for Vout and Vin to display the actual values at certain points. Go to TRACE/CURSORS/DISPLAY 6. The cursors will be associated with the first trace, as indicated by the small small rectangle around the legend for V(out) at the bottom of the window. Left click on the first trace. The value of the x and y axes are displayed in the Probe window. When you right click on V(out) the value of the second cursor will be given together with the difference between the first and second cursor. 7. To place the second cursor on the second trace (for V(in)), right click the legend for V(in). You'll notice the outline around V(in) at the bottom of the window. When you right click the second trace the cursor will snap to it. The values of the first and second cursor will be shown in Probe window. 8. You can chance the X and Y axes by double clicking on them. 9. When adding traces you can perform mathematical calculations on the traces, as indicated in the Add Trace Window to the right of Figure 9.

Figure 16: Transient simulation with a sinusoidal input.
2.4.2 AC Sweep Analysis The AC analysis will apply a sinusoidal voltage whose frequency is swept over a specified range. The simulation calculates the corresponding voltage and current amplitude and phases for each frequency. When the input amplitude is set to 1V, then the output voltage is basically the transfer function. In contrast to a sinusoidal transient analysis, the AC analysis is not a time domain simulation but rather a simulation of the sinusoidal steady state of the circuit. When the circuit contains non-linear element such as diodes and transistors, the elements will be replaced their small-signal models with the parameter values calculated according to the corresponding biasing point. In the first example, we'll show a simple RC filter corresponding to the circuit of Figure 17.
Figure 17: Circuit for the AC sweep simulation. 1. 2. 3. 4. 5. 6. 7. Create a new project and build the circuit For the voltage source use VAC from the Sources library. Make the amplitude of the input source 1V. Create a Simulation Profile. In the Simulation Settings window, select AC Sweep/Noise. Enter the start and end frequencies and the number of points per decade. For our example we use 0.1Hz, 10 kHz and 11, respectively. Run the simulation In the Probe window, add the traces for the input voltage. We added a second window to display the phase in addition to the magnitude of the output voltage. The voltage can be displayed in dB by specifying Vdb(out) in the Add Trace window (type Vdb(out) in the Trace Expression box. For the phase, type VP(out). An alternative to show the voltage in dB and phase is to use markers on the schematics: PSPICE/MARKERS/ADVANCED/dBMagnitude or Phase of Voltage, or current. Place the markers on the node of interest. We used the cursors in Figure 18 to find the 3dB point. The value is 6.49 Hz corresponding to a time constant of 25 ms (R1||R2.C). At 10 Hz the attenuation of Vout is 11.4db or a factor of 3.72. This corresponds to the value of the amplitude of the output voltage obtained during the transient analysis of Figure 16 above.

3. Additional Circuit Examples with PSpice
3.1 Transformer circuit SPICE has no model for an ideal transformer. An ideal transformer is simulated using mutual inductances such that the transformer ratio N1/N2 = sqrt(L1/L2). The part in PSpice is called TFRM_LINEAR (in the Analog Library). Make the coupling factor K close to or equal to one (ex. K=1) and choose L such that wL >> the resistance seen be the inductor. The secondary circuit needs a DC connection to ground. This can be accomplished by adding a large resistor to ground or giving the primary and secondary circuits a common node. The following example illustrates how to simulate a transformer.
Figure 3.1.1: Circuit with ideal transformer For the above example, lets make wL2 >> 500 Ohm or L2> 500/(60*2pi) ; lets make L2 at least 10 times larger, ex. L2=20H. L1 can than be found from the turn ratio: L1/L2 = (N1/N2)^2. For a turn ratio of 10 this makes L1=L2x100=2000H. The circuit as entered in PSpice Capture is shown in Figure 3.1.2 and the result in Figure 3.1.3
Figure 3.1.2: Circuit with ideal transformer as entered in PSpice Capture (the transformer TX is modeled by the part XFRM_LINEAR of the Analog Library).
Figure 3.1.3: Results of the transient simulation of the above circuit.
3.2 AC Sweep of Filter with Ideal Op-amp (Filter circuit) The following circuit will be simulated with PSpice.
Figure 3.2.1: Active Filter Circuit with ideal op-amp.
We have used off-page connectors (OFFPAGELEFT-R from the CAPSYM library; or by clicking on the off-page icon) for the input and outputs. The name of the connectors can be changed by double-clicking on the name of the off-page connector. By giving the same name to two connectors (or nodes), the two nodes will be connected (no wires are needed). For te voltage source we used the VAC from the SOURCE Library. We gave it an amplitude of 1V so that the output voltage will correspond to the amplification (or transfer function) of the filter. In the Simulation Analysis, select AC Sweep, and enter the starting, ending frequency and the number of points per decade. The result is given in the figure below. The magnitude is given on the left Y axis while the phase is given by the right Y axis. The cursors have been used to find the 3db points of the bandpass filters, corresponding to 0.63 Hz and 32 Hz for the low and high breakpoints, respectively. These numbers correspond to the values of the time constants given in Fig. 3.2.1. The phase at these points is -135 and -224 degrees.

Figure 3.2.2: Results of the AC sweep of the Active Filter Circuit of the figure above. 3.3 AC Sweep of Filter with Real Op-amp (Filter circuit) The circuit with a real op-amp is shown below. We selected the U741 op-amp to build the filter. The simulation results are shown in Figure 3.3.2. As one would expect the differences between the filter with the real and ideal op-amps are minimal in this frequency range.
Figure 3.3.1: Active Filter Circuit with the U741 Op-amp.
Figure 3.3.2: Results of the AC sweep of the Active Filter Circuit with real Op-amp (U741) of the figure above. 3.4 Rectifier Circuit (peak detector) and the use of a parametric sweep. 3.4.1: Peak Detector simulation
Figure 3.4.1: Rectifier circuit with the D1N4148 diode and a load resistor of 500 Ohm. The results of the simulation are given in Fig. 3.4.2. The ripple has a peak-to-peak value of 777mV as indicated by the cursors. The maximum output voltage is 13.997V which is one volt below the input of 15V.
Figure 3.4.2: Simulation results of the rectifier circuit. 3.4.2 Parametric Sweep It is interesting to see the effect of the load resistance on the output voltage and its ripple voltage. This can be done using the PARAM part.
Figure 3.4.3: Circuit used for the parametric sweep of the load resistor. a. Adding the Parameter Part a. Double click on the value (500 Ohms) of the load resistor R1 to {Rval}. Use curly brackets. PSpice interprets the text between curly brackets as an expression that it evaluate to a numerical expression. Click OK when done. b. Add the PARAM part to the circuit. You'll find this part in the SPECIAL library. c. Double click on the PARAM part. This will open a spreadsheet like window showing the PARAM definition. You will need to add a new column to this spread sheet. Click on NEW COLUMN and enter for Property Name, Rlval (without the curly brackets). d. You will notice that the new column Rlval has been created. Below the Rlval enter the initial value for the resistor: lets make it 500, as shown in Figure 3.4.4 below.
Figure 3.4.4: Property Editor window for the PARAM part, showing the newly created Rlval column. e. While the cell in which you entered the value 500 still selected click the DISPLAY button. You can now specify what to display: select Name and Value. Click OK. f. Click the APPLY button before closing the Property editor. g. Save the design. b. Create the Simulation Profile for the Parametric Analysis a. Select PSPICE/NEW_SIMULATION_PROFILE b. Type in the name of the profile, e.g. Parametric c. In the Simulation Setting window, select Analysis Tab if the window does not open. d. For the Analysis type select Transient (or the type of analysis you intend to perform; in this example we'll do a transient analysis) e. Under Option, slect Parametric sweep as shown in Figure 3.4.5. f. For the Sweep Variable, select Global Parameter and enter the Parameter name: Rlval. Under sweep type give the start, end and increment for the parameter. We'll used 250, 1kOhm and 250, respectively (see Figure 3.4.5). g. Click OK

Figure 3.4.5: Window for the Simulation Settings of the Parametric Sweep. c. Run Spice and Display the waveforms. a. Run PSpice b. When the simulation is finished the Probe window will open and display a pop up box with the Available Selection. Select ALL and OK. c. The multiple traces will show, as given in Figure 3.4.6. d. You can use the cursors to determined specific valueson the traces; you can also adjust the axis by double-clicking on the Y and X axes.
Figure 3.4.6: Results of the parametric sweep of the load resistor, varying from 250 to 1000 Ohm in steps of 250 Ohm.
3.5 AM Modulated Signal (AM Modulation) An Amplitude modulated (AM) signal has the expression, vam(t) = [(A + Vm cos(2fmt)] cos(2fct) = A[1 + m cos(2fmt)] cos(2fct) in which a sinusoidal high frequency carrier waveform cos(2fct) is modulated by a sinusoidal modulating of frequency fm. The modulating frequency can be any signal. For this example well assume it is a sinusoid. The modulation index is called m. To generate a AM signal in PSpice we can make use of the Multiplication function MULT that can be found in the ABM library. Figure 3.51 shows the schematic that generates the AM signal over the resistor R1.
Figure 3.5.1: Schematic for the generation of an AM signal
The result of a transient simulation is shown in the figure below. One can also look at the Fourier of the simulated output signal. In the Probe window click on the FFT icon, located on the top toolbar, or go to the PSPICE/FOURIER menu. The Fourier spectrum of the displayed trace will be shown. You can change the X axis by double-clicking on it. Figure 3.5.3 gives the Fourier spectrum with the main peak corresponding to the carrier frequency of 5kHz and two side peaks at 4.5 and 5.5 kHz, indicating that the modulating frequency is 500Hz. You can use the cursors to get accurate readings.
Figure 3.5.2: Simulated waveform (transient analysis) of the circuit above, with (A=1V, fm=500 Hz, fc=5kHz and m=0.5)
Figure 3.5.3: Fourier spectrum of the waveform of Figure 3.5.2.
3.6. Center Tap Transformer There is no direct model in PSpice for a center tap transformer. However, one can use mutually coupled inductors to simulate a center tap transformer. Figure 3.6.1 shows the schematic of the circuit. We used one primary inductor L1 and two secondary inductors L1 and L2 put in series. In addition we added a K-Linear element.

Figure 3.6.1: Circuit with Center Tap Transformer with a ratio of 10:1. After placing the element on the schematic give each element its value. Use for the input voltage a sinusoid with amplitude of 100 V and frequency 60 Hz. Notice that we added a small resistor R1 in series with the voltage source and the inductor. This was needed to prevent a short circuit in DC (Spice would give en error without this resistor). We have kept it small equal to 1 Ohm. Assume that we want to have a step-down transformer with a ratio of 10:1 to each secondary output. The ratios of the inductors L2/L1 and L3/L1 must then be equal to 1/102 (or =sqrt(L2/L1)=0.1). We made L1=1000 and L2-L3=10H. Double-click on the K-Linear element and type under the column headings for L1, L2, L3, the values LP, Ls1, Ls2. When done, click the APPLY button and close the properties window. Go to PSpice/CREATE_NETLIST to generate the netlist. To see the list, go to the Project Manager and double-click on OUTPUTs: name.net file. The netlist looks as follows:
* source CENTERTAPTRANSFOR2 Kn_K1 L_Lp L_Ls1 L_Ls2 L_Lp 0 NL_LsVOL_Ls2 VO10 V_V1 N+SIN 0V 100V R_R1 N00203 N00241 1k R_RVO1 1k R_R3 VO1k 1
Create a new Simulation Profile (Transient) with " Time to run = 50ms". The result is shown in Figure 3.6.2. Notice that the max output is 10V as one would expect from a transformer ratio of 10:1 with an input voltage of 100Vmax. The two outputs are 180 degrees out of phase.

JVdS 2006 24

Figure 3.6.2: Output of the circuit of Fig. 3.6.1.
4. Adding and Creating Libraries: Model and Parts files
4.1 Using and Adding Vendor Libraries We assume that the model (.lib) as well as the Part Symbols files (.olb) is available from the vendor. In case only the model file is available see the next section on how to create a Part Symbol. In some cases you may want to add model libraries and symbols from vendors that contain the devices you want to use in your design. The ORCAD PSpice website list many vendercontributed models. You can download these files. You will need both the model definition file (with extension.lib) and the symbol file (extension.olb). When entering the symbols in the schematic you will need to "add the library". You need also to tell the simulator that the file exists. You do this in the Schematics when defining the Simulation Profile: In the Simulation Setting window, select the Libraries tab. In the Filename box, enter the name of the new library (the full path name or the library name if it is located in the same folder as the standard libraries). You can make the library modesl global so that it will be available for every schematic or you can keep it local (for the current schematic only). Figure 4.1 shows who we added the library nat_semi-.lib as a global library (click on the Add as Global).

Figure 4.1: Adding a library
4.2 Creating Symbol Parts file from a Model file In many cases you may have the models of devices available but not the Part Symbol that is used in PSpice Capture. In this case you need to create the symbol file (.olb). In many cases you will have a model file that contains models of many devices including subcircuits. This section describes how to use the model file to create a Part Symbol for the corresponding devices in the model file [9]. The model file is a text file that can be read using a text editor (.e.g Notepad). In many cases existing vendor Spice files will have the extension.cir or.mod. We assume that you have such a file available but not the Part Symbol. 4.2.1 Open the PSpice Model Editor (this program came with the PSpice package). a. Under the FILE Menu, select NEW b. Next, under the MODEL menu, select IMPORT and find the model file for which you need to create the Part Symbol file. This will open the model file. c. Save this file with the extension.lib and put it in a directory where you store the library files (you can put it in any directory; the default libraries are stored in Program Files/OrCadLite/Capture/Library/PSpice/). d. The next step is to create the Parts for Capture. While the model file (.lib) is still open, go to FILE/CREATE_CAPTURE_FILE menu. A window (Create parts for Library) will pop us as shown below. Click on the top Browse Button and find the location of the model library is stored (.lib). This will automatically fill the Output Part Library entry with the same file name as the model library but with the.olb extension.
Figure 4.2.1 Create Parts for Library window. In this example we created a Model Library called ESE216LIB.lib and Parts ESE216LIB.olb e. Click the OK button. A window will open, giving the status of the library creation. This should give you no errors. f. Click OK in the Status window. The next step is to edit the Part Symbols that you just created. 4.4.2. Editing the Part Symbol a. Open OrCad Capture. b. Go to the FILE/OPEN/LIBRARY menu. Browse for the location of the newly created file (e.g. ESE216LIB.OLB). Click OK. This will open the PCB window fpr the library, as shown below. In our example, our library contains two devices (NMOS and PMOS devices). In practical cases the library can contain many different devices and subcircuits. An example is the sedra_lib.lib and sedra_lib.olb that comes with the textbook [10], shown in Figure 4.2.3.

Figure 4.2.2 Library Editor Window in OrCad Capture
Figure 4.2.3 Library sedra_lib.lib showing the various devices in the library file. The left window pane list all the devices and subcircuits. The right pane shows the model of the NMOS5PO (highlighted on the left). c. To edit the symbol of any of the devices double click on it in the Library Editor window. Lets select e.g. the NMOS5PO device. This will open the Part Symbol window, as shown in Figure 4.2.4. OrCad Capture is smart enough to know when a model corresponds to a transistor and will create a transistor model, as shown in Figure 4.2.4. However for subcircuits is will usually give you a generic box. You can than modify this box using the editing tools of Capture.
Figure 4.2.4 Part Symbol Window allowing you to edit the part. The example shown here is a NMOS symbol without a separate bulk contact. In that case the source and bulk are automatically shorted together.

JVdS 2006 28

d. The red line on the Parts symbol correspond to pins. These can be added by clicking on the "Place Pin" icon on the right side menu bar (or PLACE/PIN menu). This will open the Place Pin window shown below. e. You can edit the pins by first selecting it and then right clicking and selecting Edit Properties. The pin name and type are important. In general you should not change the pin names since these relate back to the Spice model. The pin type is usually "Input" or "Output." If you make a pin a "Power" type, it will be invisible in the part symbol. For shape you can select "Line" or "Short" which corresponds to a short line. Check out the other options. In case you create a symbol for a subcircuit you can give the pin numbers that correspond to those of the datasheet. f. When the part symbol is finished, save the library. You are now ready to use your newly created library and symbols. Before doing a simulation you need to add the library to the library path, in both the schematic and the simulator setting. See section on "Adding Vendor Libraries" above.
Figure 4.2.5: Place Pin window.

References

1. OrCAD website for PSpice (http://www.orcad.com/pspicead.aspx), has application notes, download, examples and interesting links. 2. OrCAD website for CAPTURE. (http://www.orcad.com/orcadcapture.aspx) 3. PSpice Users manual, OrCAD Corp. (Cadence Design Systems, Inc.) 4. PSpice Reference Guide, OrCAD Corp. (Cadence Design Systems, Inc.) 5. PSpice Library Guide, OrCAD Capture User's Guide, (Cadence Design Systems, Inc.) 6. OrCAD Capture Users Guide, OrCAD Corp., (Cadence Design Systems, Inc.) 7. SPICE Tutorial, http://www.seas.upenn.edu/~jan/spice/ 8. A. Vladimirescu, The Spice Book, J. Wiley & Sons, New York, 1994. 9. B. Carter, "Using Texas Instruments Spice Models in PSpice, Application Report, SLOA070, Texas Instruments, Dallas, TX, September 2001.

10. A. Sedra and K. C. Smith, "Microelectronic Circuits," Oxford University Press, 2004, with accompanying Rom CD containing Spice Circuit Examples.
Jan Van der Spiegel, 2006 jan_at_seas.upenn.edu Updated March 19, 2006

You can get context-sensitive help for a error message by placing your cursor in the error message line in the session log and pressing 1. Online interactive tutorial A series of self-paced interactive lessons. You can practice what youve learned by going through the tutorials specially designed exercises that interact directly with Insert Product Name. You can start the tutorial by choosing Learning Insert Product Name from the Help menu. An online, searchable version of this guide, available when choosing Online Manuals from the Orcad family program group (on the Start menu). Concise descriptions of the commands, shortcuts, and tools available in Insert Product Name, available when choosing Online Manuals from the Orcad family program group (on the Start menu).
Online Orcad Capture Users Guide
Online Insert Product Name quick reference
capug.book Page xxi Tuesday, May 23, 2000 12:08 PM
How to use this guide This documentation component.
Orcad family customer support at www.orcad.com/technical/technical.asp
An Internet-based support service available to customers with current support options. A few of the technical solutions within the customer support area are:
The Knowledge Base, which is a searchable database
containing thousands of articles on topics ranging from schematic design entry and VHDL-based PLD design to PCB layout methodologies. It also contains answers to frequently asked questions.
The Knowledge Exchange, which enables you to share
information and ideas with other users and with our technical experts in a real-time online forum. You can submit issues or questions for open discussion, search the Knowledge Exchange for information, or send email to another participant for one-on-one communication. A list of new postings will appear each time you visit the Knowledge Exchange, providing you with a quick update of whats been discussed since your last visit.
The Technical Library, which contains online customer
support information that you can search through by category or product. You can find product manuals, product literature, technical notes, articles, samples, books, and other technical information. Additionally, technical information can be obtained through SourceLink, which is an online customer support information service for users of Cadence software other than Capture, Component Information System (CIS), Express, Layout, or PSpice.
The Support Connection, which allows you to choose to
either view and update existing incidents, or create new incidents. The information is delivered directly to us via our internal database. This service is only available to customers with current maintenance or Extended Support Options (ESOs) in the United States and Canada.
The Live Connection, which enables you to open access
to your computer to a Customer Support person, who can then view your actions on your computer monitor as you demonstrate the problem youre having. Live Connections two-way transmission can also let you view the actions on the Customer Support persons computer monitor, as he or she demonstrates a method or procedure to help you solve your problem. To participate in Live Connection, you need to contact a Customer Support person, in order to obtain a support number to grant you access to the Live Connection site, and to set up a time to meet online using Live Connection.

Figure 8 Session log Tip You can clear the session log by choosing the Clear Session Log command, or by pressing C+ X. You can search for information in the session log using the Find command on the Edit menu. You can also save the contents of the session log to a file, which is useful when working with Orcads customer support staff to solve technical problems. The default filename is SESSION.TXT.
capug.book Page 15 Tuesday, May 23, 2000 12:08 PM
To display the session log
1 Click on the session logs maximize button, or choose Session Log from the Window menu.
To minimize the session log
1 Click the minimize button on the title bar.
To copy session log text to the Clipboard
Select the session log window to make it active. Select the text and choose Copy from the Edit menu.

To print the session log

Select the session log window to make it active. From the File menu, choose the Print command.
To use Find in the session log
Select the session log window to make it active. From the Edit menu, choose the Find command. The Find dialog box appears. Enter the word or words that you want to find. Click Find Next.
To save the session log to a text file
3 Select the session log window to make it active. From the File menu, choose the Save As command. The Save As dialog box appears. Enter a file name in the File name text box. By default, the session log is saved to SESSION.TXT in the current directory. If necessary, specify a new location for the file. Click Save. The session log text is saved to the file.
capug.book Page 16 Tuesday, May 23, 2000 12:08 PM

The toolbar

Note The toolbar is always docked on the top edge of the session frame the first time you open a project in a new session frame of Capture. The position of the tool palette is not saved. Captures toolbar is dockable (that is, you can select an area between buttons and drag the toolbar to a new location) and resizable. By choosing a tool button, you can quickly perform a task. If a tool button is dimmed, you cant perform that task in the current situation.
Figure 9 Captures toolbar Some of the tools operate only on what you have selected, while others give you a choice of either operating on what is selected or expanding the scope to the entire project. Table 1 summarizes the tools on the toolbar. The tasks that these tools perform are described throughout this manual. Table 1

capug.book Page 20 Tuesday, May 23, 2000 12:08 PM

Table 2

Tools on the schematic page editor tool palette
Name Select Part Description Select objects. This is the normal mode. Select parts from a library for placement. Equivalent to the Part command on the Place menu. For more information, see Placing parts on page 7-118. Draw wires. Press and hold S to draw non-orthogonal (not a multiple of 90) wires. Equivalent to the Wire command on the Place menu. For more information, see Placing wires on page 7-149. Place aliases on wires and buses. Equivalent to the Net Alias command on the Place menu. For more information, see Placing buses on page 7-152. Draw buses. Press S to draw non-orthogonal segments. Equivalent to the Bus command on the Place menu. For more information, see Placing buses on page 7-152. Place junctions. Equivalent to the Junction command on the Place menu. Draw bus entries. Equivalent to the Bus Entry command on the Place menu. For more information, see Placing bus entries on page 7-153. Place power symbols. Equivalent to the Power command on the Place menu. For more information, see Placing power and ground symbols on page 7-128. Place ground symbols. Equivalent to the Ground command on the Place menu. For more information, see Placing power and ground symbols on page 7-128.

Net Alias

Junction Bus Entry

Ground

capug.book Page 21 Tuesday, May 23, 2000 12:08 PM
Tools on the schematic page editor tool palette (continued)
Hierarchical Block Place hierarchical blocks. Equivalent to the Hierarchical Block command on the Place menu. For more information, see Placing hierarchical blocks on page 7-134. Place hierarchical ports on schematic pages. Equivalent to the Hierarchical Port command on the Place menu. For more information, see Placing hierarchical ports on page 7-139. Place hierarchical pins in hierarchical blocks. Equivalent to the Hierarchical Pin command on the Place menu. For more information, see Placing hierarchical pins on page 7-141. Place off-page connectors. Equivalent to the Off-Page Connector command on the Place menu. For more information, see Placing off-page connectors on page 7-144. Place no-connect symbols on pins. Equivalent to the No Connect command on the Place menu. See

Hierarchical Port

Hierarchical Pin

Off-Page Connector

No Connect
Placing and editing no-connect symbols on page 7-132.
Line Draw lines. Equivalent to the Line command on the Place menu. For more information, see Drawing lines on page 8-159. Draw polylines. Press and hold S to draw non-orthogonal polylines. Equivalent to the Polyline command on the Place menu. For more information, see Drawing polylines and polygons on page 8-163. Draw rectangles. Holding S constrains to a square. Equivalent to the Rectangle command on the Place menu. For more information, see Drawing rectangles and squares on page 8-160. Draw ellipses. Holding S constrains shape to a circle. Equivalent to the Ellipse command on the Place menu. For more information, see Drawing circles and ellipses on page 8-161.

capug.book Page 57 Tuesday, May 23, 2000 12:08 PM
Working with files in a project
Using the project manager, you can add or delete project files. You can add any file to your project, including libraries and VHDL files. Files not in ASCII format, or a Capture generated format, may not appear as expected when opened in Capture.
To add a file to your project
3 Or 1 Drag the file from the Windows Explorer into the folder in the project manager. In the project manager, select the folder to which you want to add a file. From the Edit menu, choose Project. The Add File to Project Folder dialog box displays. Select the file you want to add and choose the Open button. The file is added to the project. Note You can also add files to your project interactively. When you create a design using the New command on the File menu, it is placed in the project managers Design Resources folder.
To delete a file from a project
In the project manager, select the file you want to delete. Press the D key. The file is removed from the project. Caution You will not be given a chance to cancel this process after you press the D key. If you delete a file by mistake, you will have to add it back to the project.
capug.book Page 58 Tuesday, May 23, 2000 12:08 PM
Saving projects, designs, and libraries
When the project manager window is active, you can save a new or existing project, design, or library. The Save command saves all open documents referenced by the project, as well as the project itself. Note To avoid overwriting a design file with a misnamed project file, type in the filename without a file extension. Capture automatically saves the file with the correct file extension. A Capture design file (.DSN) is associated with a project file (.OPJ). Each time you use the Save As command from the File menu to save a design file to another name or directory, you should also use Save As for the project file. The Save As command saves files depending on what you have selected in the project manager.
If one or more designs or libraries are selected, Capture prompts you to save each file in turn. If no top-level folders (Design Resources or Outputs) are selected, and items other than designs or libraries are selected, the Save As command is unavailable. If no designs or libraries are selected in the project manager, Capture prompts you to save the project.
Tip To protect your work in the event of a system crash or power outage you can enable Auto Recovery, and set the interval at which your design, library, or VHDL file is saved. For information about the Auto Recovery option, see Setting miscellaneous options on page 4-73. Note If you choose Save when a schematic page window is active, only that pages design is saved, not the entire project. However, when you attempt to close the project, a dialog box asks if you want to save any project files that have been edited but not yet saved.

capug.book Page 104 Tuesday, May 23, 2000 12:08 PM
capug.book Page 105 Tuesday, May 23, 2000 12:08 PM

Design structure

Many schematic designs can fit on one schematic page. Some designs, however, are too large for even the biggest page, and even if a complex design could fit on one page, there are good reasons for dividing it:
To fit at full scale on your printers page. To partition a design so that several people can work on it at once. To develop the design using a top-down approach. That is, you may want to begin with a block diagram in which each block represents a major function and then construct more detailed diagrams for each block. To organize your design by functional parts. To meet department specifications.
Capture offers two ways of handling multiple-page designs: a flat design structure and a hierarchical design structure.
capug.book Page 106 Tuesday, May 23, 2000 12:08 PM
Chapter 6 Design structure

Flat designs

Flat designs are practical for small designs with few schematic pages. A flat design is a structure in which the output nets of one schematic page connect laterally to the input nets of another schematic page in the same schematic folder through objects called off-page connectors. A flat design has no hierarchy (no hierarchical blocks, hierarchical ports, hierarchical pins, or parts with attached schematic folders). The structure of a flat design is shown to the left. All schematic pages in a flat design are contained within a single schematic folder, and are on a single level, as shown at left. In the figure, SCHEMATIC1 is a schematic folder. It contains schematic pages named PAGE1 and PAGE2. Since you must manage all of the interconnections between the pages of a flat design using names assigned to off-page connectors, it is best to keep a flat design relatively small.
capug.book Page 107 Tuesday, May 23, 2000 12:08 PM

Hierarchical designs

You can create symbols on schematic pages that represent other schematic folders. These symbols are called hierarchical blocks. The layered arrangement created by placing schematic folders inside schematic pages is called a hierarchy. Any schematic page can contain hierarchical blocks (or parts with attached schematic folders) that refer to other schematic folders; a designs structure can be many levels deep. The schematic folder at the top of a hierarchy, which directly or indirectly refers to all other schematic folders in the project, is called the root module. In the project manager, the root module has a backslash in its folder icon. The root module, as well as any other schematic folder, can contain as many schematic pages as you need. Tip If you intend to take your design into a digital simulator like PSpice, it is best to place only one schematic page in each lower level schematic folder. This may reduce problems you encounter while troubleshooting your designs.

Use the mouse. Expand the MRU drop-down list by clicking on the arrow at the right of the list, then click on a part or symbol to select it. Type the part or symbol name. Click in the MRU list box and begin typing the name of the part or symbol. Capture automatically completes the name if the item is in the list. When the name is highlighted in the MRU list box, press R.
If the part or symbol is not in the MRU list, but is a part in the set of configured libraries, an image of the part attaches to your pointer when you press R.
Use the shortcut. Press C+M to highlight a part in the MRU list. Press t and b to select a part or symbol in the list. When the correct part or symbol is highlighted in the list box, press R.
capug.book Page 125 Tuesday, May 23, 2000 12:08 PM

Searching for parts

Capture can search for a particular part inside all the libraries it finds in the specified directory.

To find a part

5 In the schematic page editor, choose Part from the Place menu. Click the Part Search button. The Part Search dialog box appears. Enter the part name you want to locate. Click Browse to locate the directory where your libraries are located. Click Begin Search. Capture returns the names of all the libraries in the specified directory, that contain your part.
Note Using the Find command on the schematic page editors Edit menu, you can specify a search and replace for parts, nets, title blocks, off-page connectors, flat nets, power or ground symbols, bookmarks, hierarchical ports, text, or DRC markers.

Editing parts

You can move a part on a schematic page by selecting it and dragging it to a new location. You can use the Rotate or the Mirror command from the Edit menu. You can use the part editor to change the parts physical appearance, and you can edit the parts properties. When you edit a part on a schematic page, your edited part differs from the part in the library and exists only in your design; you can place another copy of the part you edited by using the Copy command from the Edit menu, and by dragging the part from the design cache. Note For more information about editing parts, see Chapter 12, Creating and editing parts.

Implementation Name

Specifies the name of the attached schematic folder, VHDL entity, netlist, or project for the hierarchical block. Schematic folder names are case sensitive.
Path and filename Specifies the path and filename of
the attached schematic folder, VHDL entity, netlist, or project for the hierarchical block.
Caution An attached schematic folder or other file external to the project or library is not stored with the project or library. If you copy or move your project or library to a new location, you must also move or copy the attached file, to keep them together. In addition, you may need to edit the path to the attached schematic folder or file if you move your project to a new location with a different directory structure. 137
capug.book Page 138 Tuesday, May 23, 2000 12:08 PM
Editing hierarchical blocks
You can edit a hierarchical block after it is placed. Select the hierarchical block and do one of the following:
Double-click it. Choose Properties from the Edit menu. Choose Edit Properties from the pop-up menu.
Each of these methods displays the property editor, in which you can change the blocks reference, choose among the options in the Primitive group box, or modify the attached schematic folders name or path. You can also add and modify user properties in the property editor. You can also edit the display properties of the text associated with the hierarchical block. Select the text of the hierarchical block and do one of the following:
Each of these methods displays the Display Properties dialog box, in which you can edit the visibility, color, font, or rotation of the text of the hierarchical block. You can click a hierarchical block and move it to another location, or you can drag its selection handles to resize it. You can also use the Mirror or Rotate commands to change the appearance of the block.
capug.book Page 139 Tuesday, May 23, 2000 12:08 PM
Placing and editing hierarchical ports and hierarchical pins

To place an off-page connector
1 Figure 54 Off-page connectors in CAPSYM.OLB Tip You can add more libraries to the Libraries list box by clicking Add Library. Capture displays a standard Open dialog box that you can use to locate a library to add to the list. You can remove a library from the Libraries list box by selecting it and clicking Remove Library. You can assign a name by typing it in the Name text box. The name is used to connect to other off-page connectors in the same schematic folder. You can also assign a name after the symbol is placed. All of the options on the Place Off-Page Connector dialog box are described later in this section. 144 From the schematic page editors Place menu, choose Off-Page Connector. or Choose the off-page connector tool on the schematic page editors tool palette. The Place Off-Page Connector dialog box appears. 2 In the Symbol text box, type the name of the symbol to place. If you arent sure of the exact name of the symbol, you can enter wildcard characters to constrain the list of symbols, then click OK. Valid wildcard characters are an asterisk (*) to match multiple characters and a question mark (?) to match a single character. After you type the name of the symbol to place, click OK. All symbols in the libraries listed in the Libraries list box that match the symbol name are listed in the box below the Symbol text box. When you select a symbol from this box, its graphic image displays.
capug.book Page 145 Tuesday, May 23, 2000 12:08 PM
When you have located the symbol you want to place, click OK. An image of the symbol is attached to your pointer. You can press the right mouse button to display a pop-up menu with commands that you can use to change the appearance of the symbol before you place it. You can mirror the symbol horizontally or vertically, rotate the symbol, or edit its properties.
Move the pointer to the location on your schematic page where you want the symbol and click the left mouse button. This places the symbol on your schematic page. You can place multiple instances of the symbol by clicking the left mouse button each place you want an instance of the symbol.

To move a wire, select it and drag it to a new location; the wire stretches to maintain its connectivity. To break the wires connectivity, press A while you move it. To move a vertex, select a wire segment next to the vertex and drag the vertex to the new location. Capture warns you of connectivity changes as you drag an object by placing markers at the connectivity change points visible on the schematic page. At the same time, the cursor changes to an exclamation point as shown below, and the status line warns of net connectivity changes. Tip Before you edit a design created in an earlier version of Capture in Capture Release 9.1 or later, run a Design Rules Check to show where Capture will place junctions in your design. If you do not want electrical connections at "T" intersections and on pins where wires cross, you can adjust the design as necessary using Capture Release 9 or earlier.
Figure 56 Connectivity change warning Because some connectivity changes may not be visible on screen, most connectivity changes for which you see an alert are documented in the session log. For more information about connectivity and orthogonal drag, see Captures online help.
capug.book Page 152 Tuesday, May 23, 2000 12:08 PM

Placing buses

A bus is a group of scalar signals (wires). Once the bus acquires a valid name or alias, then that name or alias defines the signals carried by the bus and connects those signals to the corresponding nets. For example, the alias A[0:3] defines a four-signal bus that connects the four bus signals to the individual wires named A0, A1, A2, and A3. Net aliases on wires do not use brackets.

To place a bus

1 From the schematic page editors Place menu, choose Bus. or Choose the bus tool on the schematic page editors tool palette. Click the left mouse button to start the bus. Move the mouse to draw the bus. Click the left mouse button if you want to place a vertex and change directions, or to connect to another bus as you pass over it. The bus is constrained to multiples of 90 unless you hold down the S key while you draw the bus. Double-click to end the bus, then click the Select button on the schematic page editors tool palette. Highlight the bus and choose Net Alias from the Place menu. Enter an alias for the bus in the Place Net Alias dialog box that appears, then click OK. When you are done placing buses, choose the selection tool or press E to dismiss the bus tool.

capug.book Page 177 Tuesday, May 23, 2000 12:08 PM

Recording a macro

A location recorded within a macro is relative to the previous action, not relative to where you began recording the macro. For example, you can record a macro to place a wire, move the cursor down one grid space, then place another wire. When you run the macro at a different location on your schematic page, the macro places a wire, moves down one grid space, then places another wire below the original wire.

To record a macro

Click the left mouse button on the schematic page to set a location to begin recording the macro. From the schematic page editors Macro menu, choose Record. The macro recorder tool palette containing three buttons displays, as shown. Perform the series of edits that you want to record as a macro, using the three macro record buttons as necessary.
Use the left button to stop recording the macro. Use the center button to pause recording. The pause mode is in effect until you click the center button again. Use the right button to cause a command to begin recording in a with dialog mode. If a command is recorded in this mode, the value you enter while recording the macro is not saved. Instead, when the macro is run, the command displays a dialog box so that you can fill in a value. When recording, the with dialog mode is in effect until you click the right button again. Use this button again to stop recording in with dialog mode.
Choose the left macro record button to stop recording the macro.
capug.book Page 178 Tuesday, May 23, 2000 12:08 PM

Playing a macro

Choose Play from the Macro menu to play back the most recently recorded macro or any macro you choose in the Configure Macro dialog box.

To play a macro

Click the left mouse button on the schematic page to set a location to begin playing the macro. From the schematic page editors Macro menu, choose Play. or From the Configure Macro dialog box, choose Play.
capug.book Page 179 Tuesday, May 23, 2000 12:08 PM

Configuring a macro

After you record a macro, you give it a name, and you can also assign it a menu entry, a shortcut key definition, and a description. Once you give a macro a name and save it, it automatically displays in the Macro name list box in the Configure Macro dialog box the next time you run Capture. The text you enter as the menu entry displays on the Macro menu, along with the macros shortcut key definition, if you specified one. The text you enter as the description displays in the Description text box in the Configure Macro dialog box when you highlight the macro name.

Editing a part in a library
Once you edit a part in a library, you can update existing projects with the new part using the Update Cache or Replace Cache commands on the project managers Design menu.
To edit a part in a library
From the File menu, choose Open. A standard Open dialog box appears. Choose the library containing the part you want to edit. The library opens, showing all its parts. Double-click on the part you want to edit. The selected part appears in the part editor. Edit the part. You can resize it, add or delete graphics or symbols, and add or delete pins. These processes are all described in Creating a new part earlier in this chapter. You can also edit the parts properties. Editing properties is described in Chapter 2, The Capture work environment. 5 When you are done editing the part, you must save it. From the File menu, choose Save. The part is saved in the library.
Tip If you need to know a parts library of origin, you can select the part in the project manager, then select Replace Cache from the Design menu. The part name and the library and path are listed in the dialog box that appears. Click Cancel to return to the project manager. Tip You can discover the library of origin for multiple parts by creating a cross reference report.
capug.book Page 230 Tuesday, May 23, 2000 12:08 PM
Editing a part on a schematic page
Once you edit a part on a schematic page, you can apply the edits to all instances of the same part in the project, or you can apply the edits only to the particular part instance you edit.
Caution Once you edit a part instance on a schematic page, it is no longer linked to its corresponding library part. In addition, a new part (with _n appended to the original part name) appears in the design cache. This means that you cant perform an Update Cache on an edited part, since there is no link to the original library. To edit a part instance on a schematic page
Select a part instance on a schematic page. From the Edit menu, choose Part. The library part that was used to define the part instance appears in the part editor. 3 Edit the part. You can resize it, add graphics or symbols, and add or delete pins. These processes are all described in Creating a new part earlier in this chapter. You can also edit the parts properties. Editing properties is described in Chapter 2, The Capture work environment. 4 When you are done editing the part, you must close it and save the changes on the schematic page. From the File menu, choose Close. A dialog box appears asking if you would like to:

mirror named net net
capug.book Page 331 Tuesday, May 23, 2000 12:08 PM

net alias

A name used to specify signal connections between unconnected wires or buses. For example, if you have wires in two remote locations in a schematic folder, you can assign each wire an alias (such as ABC) to connect the signals without physically drawing a wire between them. A file that lists the interconnections of the project components by the names of the connected signals, parts, and pins. A part with an underlying hierarchy, such as an attached schematic folder. An instance placed on a schematic page with one or more sets of unique property values that may differ from other occurrences of the same instance. An occurrence typically appears in a complex hierarchy where a schematic is reused. Each use of the schematic is an occurrence, while the schematic itself is the instance. See also instance, occurrence property. A property attached to an occurrence, as opposed to a property attached to an instance or added to a part in a library. Occurrence properties override instance properties, but are not reflected on the instance. See also instance, occurrence. An object that conducts signals between schematic pages within the same schematic folder. See also flat design. A physical part that contains more than one logical part. For example, a 2N3905 transistor, a fuse, and a 74LS00 are packages. Each part in a package has a unique part reference comprised of an alphanumeric prefix common to all the parts in the package, and a letter unique to each part. For example, a 74LS00 with a part reference prefix of U15 would have four parts with part references of U15A, U15B, U15C, and U15D. See also homogeneous part, heterogeneous part. To change the portion of the schematic page or part being viewed by dragging objects from one location to another. As you drag an object, the schematic page or part pans across the active window.

netlist

nonprimitive occurrence

occurrence property

off-page connector package
capug.book Page 332 Tuesday, May 23, 2000 12:08 PM

parent

A schematic page containing a hierarchical block that references another schematic folder (called a child). See also child, hierarchical block. A part is a basic building block of a project that may represent one or more physical elements, or a function, a simulation model, or a text description for use by another application. A parts behavior is described by a SPICE model, an attached schematic folder, HDL statements, or other means. Parts usually correspond to physical objects (gates, connectors, and so on) that come in packages of one or more parts. You can think of these packages as physical parts and the parts you place on a schematic page as logical parts. Physical parts with more than one logical part are sometimes referred to as multiple-part packages. For simplicity, Capture usually refers to both as parts. See also package. A duplicate copy of a part that uses a different name. A part alias uses the same graphics, attached schematic folders, and properties as the original, with the exception of the part value. The editor used to create and edit parts and symbols. An instance of a part. See also instance. See primitive. Acronym for printed circuit board. A pin acts as a point of connectivity for the part it is attached to. In addition to input and output pins, there are also 3-state, bidirectional, open collector, open emitter, passive, and power pins. If a pin connects to a wire, it is a scalar pin; if it connects to a bus, it is a bus pin. See also hierarchical pin. The exchange of identical pins in order to decrease route lengths. The physical spacing between pins on a device. A graphic object made up of polylines (multiple contiguous segments) whose beginning and end are attached to form a closed shape that can be filled. See also polyline.

part alias

part editor part instance part primitive PCB pin
pin swap pin-to-pin spacing polygon
capug.book Page 333 Tuesday, May 23, 2000 12:08 PM

polyline port

A line with multiple contiguous segments. You place a polyline using the Polyline command on the Place menu. A VHDL term for an interface element of a VHDL entity. Serves as a communication channel between VHDL design units. Capture part pins and hierarchical ports will produce a VHDL port. See also hierarchical port. A part or hierarchical block with no underlying hierarchy. A single file that includes all of the schematic folders, schematic pages, parts, and symbols that make up a project. You can view these project elements in the project manager. A basic project contains one schematic folder and one schematic page, while a complicated project may contain an unlimited number of schematic folders, each with many schematic pages. The Capture window used to perform project-wide tasks, such as locating objects, creating a netlist, or generating reports. This window displays the structure of the schematic folders and schematic pages contained in a design. See also hierarchical design, simple hierarchy. A characteristic of an object that can be edited. A property consists of a name and a value. Examples of property names are part value and color. Their respective property values can be something such as capacitor and red. The schematic folder at the top of a hierarchical design. The root schematic folder contains a backslash in its folder icon in the project manager. A project has only one root schematic folder. A pin width that carries only one signal, as opposed to a bus pin that can carry multiple signals. A graphical representation of a circuit using a set of electronic symbols, hierarchical blocks, and connections. Typically used by system and programmable logic designers to express a structural design description. A collection of all schematic pages at the same level of hierarchy in a design. In the project manager, a schematic folder behaves like a container. See also flat design, hierarchical design, schematic page, root schematic folder.