. 13-7. 13-7. 13-8. 13-9. 13-9 13-10 13-12 13-15 13-15 13-16 13-16 13-17 13-18 13-19 13-22 13-22 13-23 13-25 13-28 13-28 13-28
Chapter 14 Output Options
Chapter Overview. 14-1 Viewpoints. 14-2 Printpoints. 14-3
Appendix ASetting Initial State
Appendix Overview. Save and Load Bias Point Save Bias Point. Load Bias Point. Setpoints. Setting Initial Conditions.. A-1 A-2 A-2 A-3 A-4 A-6

Figures

Figure 1-1 Figure 2-1 Figure 2-2 Figure 2-3 Figure 2-4 Figure 2-5 Figure 2-6 Figure 2-7 Figure 2-8 Figure 2-9 Figure 2-10 Figure 2-11 Figure 2-12 Figure 2-13 Figure 2-14 Figure 2-15 Figure 2-16 Figure 2-17 Figure 2-18 Figure 2-19 Figure 2-20 Figure 2-21 Figure 2-22 Figure 2-23 Figure 3-1 Figure 4-1 Figure 5-1 Figure 5-2 Figure 5-3 Figure 5-4 Figure 5-5
Circuit Analysis File Interactions. 1-2 Diode Clipper Circuit. 2-2 Connection Points. 2-4 PSpice Simulation Status Window. 2-6 Simulation Output File. 2-7 DC Sweep Dialog Box. 2-9 Probe Plot. 2-10 Voltage at In and Mid. 2-11 Trace Legend with Cursors Activated. 2-11 Trace Legend with V(Mid) Symbol Outlined. 2-12 Voltage Difference at V(In) = 4 Volts. 2-13 Diode Clipper Circuit with a Voltage Stimulus. 2-14 Stimulus Editor Window. 2-15 Transient Analysis Dialog Box. 2-16 Sinusoidal Input and Clipped Output Waveforms. 2-17 Clipper Circuit with AC Stimulus. 2-18 AC Sweep and Noise Analysis Dialog Box. 2-19 dB Magnitude Curves for Gain at Mid and Out. 2-20 Bode Plot of Clippers Frequency Response. 2-21 Clipper Circuit with Global Parameter Rval. 2-22 Parametric Dialog Box. 2-24 Small Signal Response as R1 is Varied from 100 to 10 k. 225 Comparison of Small Signal Frequency Response at 100 and 10 k Input Resistance 2-27 Performance Analysis Plots of Bandwidth and Gain vs. Rval. 2-29 Lossy Line Comprised of Lumped Line Segments. 3-6 Rules for Pin Callout in Subcircuit Templates. 4-11 Relationship of Parts Utility with Schematics and PSpice. 5-4 Process and Data Flow for the Parts Utility. 5-6 Parts Utility Window with Data for a Bipolar Transistor. 5-11 Schematic for a Half-Wave Rectifier. 5-13 Dbreak-X Instance Model. 5-14
Figure 5-6 Figure 5-7 Figure 5-8 Figure 5-9 Figure 5-10 Figure 6-1 Figure 6-2 Figure 6-3 Figure 6-4 Figure 6-5 Figure 6-6 Figure 6-7 Figure 6-8 Figure 6-9 Figure 6-10 Figure 6-11 Figure 6-12 Figure 6-13 Figure 6-14 Figure 6-15 Figure 6-16 Figure 6-17 Figure 6-18 Figure 6-19 Figure 6-20 Figure 7-1 Figure 8-1 Figure 8-2 Figure 8-3 Figure 8-4 Figure 8-5 Figure 9-1 Figure 9-2 Figure 10-1 Figure 10-2 Figure 10-3 Figure 10-4 Figure 10-5 Figure 10-6 Figure 11-1

Notation

ALL CAPS C+r monospace font

Examples

ANALOG.SLB or CLIPPER.SCH Press C+r Type VAC.

Description

Library files and file names. A specific key or key stroke on the keyboard. Commands/text entered from the keyboard.

Mouse Conventions

If you have a multiple-button mouse, the left mouse button is the primary mouse button, unless you have configured it differently. Point means to position the mouse pointer until the tip of the pointer rests on whatever you want to point to on the screen. Click means to press and then immediately release the mouse button without moving the mouse. Right-click means to press the right mouse button and then immediately release the mouse button without moving the mouse. Drag means to point and then hold down the mouse button as you move the mouse.

Related Documentation

The documentation for all MicroSim products is available in both hard-copy and on-line.

Manual Name*

MicroSim Schematics Users Guide MicroSim PCBoards Users Guide MicroSim PCBoards Autorouter Users Guide MicroSim PSpice A/D & Basics+ Users Guide
Provides information about how to use MicroSim Schematics, which is a schematic capture front-end program with a direct interface to other MicroSim programs and options. Provides information about MicroSim PCBoards, which is a PCB layout editor that allows you to specify printed circuit board structure, as well as the components, metal and graphics required for fabrication. Provides information on the integrated interface to Cooper & Chyan Technologys (CCT) SPECCTRA autorouter in MicroSim PCBoards. Describes the capabilities of PSpice A/D, Probe, Stimulus Editor, and Parts utility. It provides examples for demonstrating the process of specifying simulation parameters, analyzing simulation data results, editing device stimuli, and creating models. Provides reference material for PSpice A/D. Also included: detailed descriptions of the simulation controls and analysis specifications, start-up option definitions, and a list of device types in the analog and digital model libraries. User interface commands are provided to instruct you on each of the screen commands. Provides a variety of articles that show you how a particular task can be accomplished using MicroSims products, and examples that demonstrate a new or different approach to solving an engineering problem. Provides information for using the PSpice Optimizer for analog performance optimization. Provides information for using programmable logic synthesis. Provides information about the implementation of a PLD design targeted for using one or more of AMDs devices. Provides information about designing electronic frequency selective filters. Provides a complete list of the analog and digital parts in the model and symbol libraries.

You can visually verify the DC response of the clipper by performing a DC sweep of the input voltage source and displaying the waveform results in Probe. This example sets up DC sweep analysis parameters to sweep Vin from -10 to 15 volts in 1 volt increments.
Setting Up and Running a DC Sweep Analysis
To set up and run a DC sweep analysis
3 Select Setup from the Analysis menu. Click on the DC Sweep button in the Analysis Setup dialog box. Set up the DC Sweep dialog box as shown in Figure 2-5.

Shortcut: Click on.

The default settings for the DC Sweep dialog box are Voltage Source as the swept variable type and Linear as the sweep type. To select a different swept variable type or sweep type, click on the appropriate radio button.
Figure 2-5 DC Sweep Dialog
Click on OK to exit the DC Sweep dialog box. If needed, click on the DC Sweep check box in the Analysis Setup dialog box so that it is checked on (enabled). Click on Close to exit the Analysis Setup dialog box. Click on the Save icon. You can also save the circuit under a different name. To save the circuit as clipperd.sch, for example, select Save As from the File menu in the schematic editor and enter clipperd as the file name.

Save icon:

To run the analysis as specified, select Simulate from the Analysis menu.

Shortcut: Click on !.

or press
Displaying DC Analysis Results in Probe
To set up Probe to automatically run after simulation, select Probe Setup from the Analysis menu and click on the Automatically Run Probe After Simulation box so that it is checked on. Shortcut: Click on I. or press
If Probe is set up to automatically run upon successful completion of a simulation (the default setting), then the Probe window is displayed when the simulation is finished. The Probe window displays a plot screen like the one shown in Figure 2-6.
To plot voltages at nets 1 and 2
3 Select Add from the Trace menu. Click on V(In) and V(Mid) in the Add Traces dialog box. Click on OK.
To display traces using markers
1 Delete the two traces you plotted above: a b c Click on the text V(In) located under the X axis of the plot to select trace V(In). Press and hold the V key and click on V(Mid) to also select trace V(Mid). Press X to remove both traces.

Figure 2-6 Probe Plot

DC Sweep Analysis 2-11
In Schematics, select Mark Voltage/Level from the Markers menu. Click to place the first marker on net In. Click to place the second marker on net Mid. Right-click to end marker mode. Waveform traces are displayed as shown in Figure 2-7.

NAME1 = VSUPPLY VALUE1 = 12V The OPTPARAM pseudocomponent can also be used to define global parameters, though its primary use is to define design parameters for use with the PSpice Optimizer. If you choose to use OPTPARAM, up to eight parameters can be defined by specifying values for Name and Initial Value.
Note The system variables in Table 3-7 on page 3-13 have reserved parameter names. User-defined parameters should not use these parameter names.
By using parameters, multiple devices can respond to a change in that parameter. For instance, if a second independent source, VEE, also has its value set to {VSUPPLY} as well, then both sources can be changed to 14 volts by simply reassigning the VALUE1 attribute of the PARAM pseudocomponent to 14V.

Expressions

Additional flexibility can be provided by using parameters in expressions. See Parameters on page 3-9 for more information about parameters.
In many applications, it is helpful to have more flexibility in setting up values by using expressions in place of literal values. For example, an independent source, VEE, could have its VALUE attribute defined as:

VALUE = {-10*FACTOR}

where FACTOR is assigned the value of 1.2 using a PARAM pseudocomponent. The value for VEE resolves to (-10 * 1.2) or -12.0 volts. Expressions can contain the standard operators listed in Table 3-5, the functions in Table 3-6, and the system variables listed in Table 3-7. The simulator accepts expressions of any length, but MicroSim Schematics imposes some length limits. Part attribute definitions, for example, are limited to 1,024 characters in Schematics. In such cases, it is appropriate to define custom functions for expressions, thus decreasing length and improving readability. The simulator evaluates expressions upon reading in the entire circuit file set. Parameter values that change as an analysis proceeds (a DC sweep or parametric analysis, for example) cause the simulator to reevaluate the expression at that time. Table 3-5 Operators in Expressions
Type arithmetic Operato rs + * / ** Meaning addition (or string concatenation) subtraction multiplication division exponentiation

Table 3-5

Operators in Expressions (continued)
Operato rs == != > >= < <= Meaning equality test non-equality test greater than test greater than or equal to test less than test less than or equal to test

Linking a Symbol to a Model
For a description of the MODEL attribute, see MODEL on page 4-6.
When the electrical behavior of a part is described by a model, the associated model is identified by the MODEL attribute for the part symbol. To tell PSpice where to find the model library file containing the definition of the simulation model referenced, use Library and Include Files on the Analysis menu in the schematic editor. In the Library and Include Files dialog box, the files listed must be in a directory on the library search path or be specified with a complete path. You can display or modify the library search path using Editor Configuration on the Options menu in the schematic editor.
Relating Subcircuits to Part Symbols
When the electrical behavior of a part is described by a subcircuit, the associated subcircuit is identified by the MODEL attribute for the part symbol. In the standard symbol and model libraries, the symbol name and corresponding subcircuit name are identical. This
convention should be followed when creating user-defined parts with subcircuit definitions. If the subcircuit has variable input parameters using the PARAMS: construct, the part symbol must have corresponding attributes which can be optionally set on a part instance basis. For example, the LM7805C subcircuit definition in the model library has two variable parameters: Av_feedback and Value as defined in the following.SUBCKT statement:
.SUBCKT LM7805C Input Output Ground x1 Input Output Ground x_LM78XX PARAMS: + Av_feedback=1665, R1_Value=1020
The equivalent part symbol attributes for this subcircuit are:
MODEL = LM7805C Av_feedback=1665 R1_Value=1020
These part symbols also have a TEMPLATE attribute, which defines how Schematics should translate the attributes of a given part instance into an X (subcircuit) device declaration written to the netlist. A LM7805C TEMPLATE is defined in a single line of text as:
TEMPLATE=X^@REFDES %IN %OUT %COMMON @MODEL
For a description of the TEMPLATE attribute, see TEMPLATE on page 4-7.
X^@REFDES instructs Schematics to substitute the hierarchical (if applicable) reference designator for this part instance prefixed with the letter X, thus producing a simulatorcompatible subcircuit device. Template items preceded by a % character produce simulator compatible node names. The required connecting terminals must be listed in the order specified in the subcircuit definition. In this example, %IN, %OUT, and %COMMON reflect the exact order of the terminals in the LM7805C.SUBCKT definition. @MODEL is substituted with the subcircuit name LM7805C. When creating a subcircuit definition for a new part (rather than modifying an existing part symbol or part instance), you need to create a new part symbol (and possibly a package definition), being sure to define all of the appropriate attributes.

Figure 5-2 Parts Utility Window with Data for a Bipolar Transistor
Using the Parts Utility 5-11
Extract all model parameters for the current specification using Parameters on the Extract menu. Repeat steps 2-3 until the model meets target behaviors. Save the model by selecting Save from the Part menu. Update the model file by selecting Save Library from the File menu. End the Parts utility session by selecting Exit from the File menu.
Manual Model Configuration
Although you can configure models manually as described in this section, it is recommended to use automatic configuration as described in Automatic Model Configuration on page 5-10 instead.
If you opened an existing model file to which model definitions were appended, then this step can be skipped.
Configure Parts output files into your schematic: a b c Select Library and Include Files from the Analysis menu. Enter the file name as <model file name>.lib (mycir.lib, for example). If the model definitions are for local use in the current schematic, click on the Add Library (or Add Include) button. For global configuration, use Add Library* (or Add Include*) instead. Click on OK.
Either part instances or symbols can be modified to reference the new model. To change model references locally for a part instance: a b c Select one or more part instances. Select Model from the Edit menu. Click on Change Model Reference and type in the appropriate model name.
To change model references globally for a symbol: a
See Chapter 4,Creating Symbols, for a description of how to create and edit symbols.
Enter the symbol editor by selecting Edit Library from the File menu. Create or change a symbol definition, making sure to define the following attributes: Symbol name; it is good practice to have the symbol name match the MODEL name. Model name as defined in the Parts utility.
Creating Model and Subcircuit Definitions by Characterization
This method does not support the variable parameters construct, PARAMS:, the local.PARAM command, or the local.FUNC command. To refine the subcircuit definition for these constructs, use the model editor described in Using the Model

resulting netlist. When a match is found, the original fragment is replaced by the fully qualified name of the net or device. For example, suppose we have a hierarchical part U1. Inside the schematic representing U1 we have an ABM expression including the term V(Reference). If Reference is the name of a local net, then the fragment written to the netlist will be translated to V(U1_Reference). If Reference is the name of a global net, the corresponding netlist fragment will be V(Reference). Names of voltage sources are treated similarly. For example, an expression including the term I(Vsense) will be output as I(V_U1_Vsense) if the voltage source exists locally, and as I(V_Vsense) if the voltage source exists at the top level.
Forcing the Use of a Global Definition
If a net name exists both at the local hierarchical level and at the top level, the search mechanism used by Schematics will find the local definition. You can override this, and force Schematics to use the global definition, by prefixing the name with a single quote (') character. For example, suppose there is a net called Reference both inside hierarchical part U1 and at the top level. Then, the ABM fragment V(Reference) will result in V(U1_Reference) in the netlist, while the fragment V('Reference) will produce V(Reference).

ABM Part Templates

For most ABM symbols, a single PSpice E or G device declaration is output to the netlist per symbol instance. The TEMPLATE attribute in these cases is straightforward. For example the LOG symbol defines an expression variant of the E device with its output being the natural logarithm of the voltage between the input pin and ground:
E^@REFDES %out 0 VALUE { LOG(V(%in)) }
The fragment E^@REFDES is standard. The E specifies a PSpice controlled voltage source (E device); %in and %out are the input and output pins, respectively; VALUE is the keyword specifying the type of ABM device; and the expression inside the curly braces defines the logarithm of the input voltage. Several ABM symbols produce more than one primitive PSpice device per symbol instance. In this case, the TEMPLATE attribute may be quite complicated. An example is the DIFFER (differentiator) symbol. This is implemented as a capacitor in series with a current sensor together with an E device which outputs a voltage proportional to the current through the capacitor. The template has several unusual features: it gives rise to three primitives in the PSpice netlist, and it creates a local node for the connection of the capacitor and its current-sensing V device.

Method 2

This turns off the message that pops up each time a simulation is completed. 4 Update the command line in one of the following ways:
Include a list of circuit file names separated by spaces. Read a file of run time properties (using the @<file name> syntax) which contains a list of circuit file names.
Circuit file names may be fully qualified or contain the wild card characters * and ?.
The Simulation Status Window
As PSpice performs the circuit simulation, a status window is displayed so that you can monitor the progress of the simulation. Figure 7-1 shows an example of the PSpice status window.
Figure 7-1 PSpice Status Window The status window includes the following:
Title bar This area at the top of the window identifies the name of the circuit file currently under simulation, and the name of the simulation output file where audit trail information will be written. Menus The menus accessed from the menu bar include items to control the simulator and customize the window display characteristics. These are especially useful when invoking PSpice directly. Simulation progress display The lower portion of the window displays the progress of each simulation as it proceeds.

DC Analyses

This chapter describes how to set up DC analyses and includes the following sections: DC Sweep on page 8-2 Bias Point Detail on page 8-7 Small-Signal DC Transfer on page 8-8 DC Sensitivity on page 8-10

DC Sweep

Minimum Requirements to Run a DC Sweep Analysis
Minimum circuit design requirements
Table 8-1 DC Sweep Circuit Design Requirements
Swept Variable Type voltage source temperature current source model parameter global parameter Requirement voltage source with a DC specification (VDC, for example) none current source with a DC specification (IDC, for example) PSpice model (.MODEL) global parameter defined with a parameter block (.PARAM)
See Setting Up Analyses on page 7-3 for a description of the Analysis Setup dialog box.
Minimum software setup requirements
In the Analysis Setup dialog box, click on the DC Sweep button. Complete the DC Sweep dialog box as needed. If needed, click on the DC Sweep check box in the Analysis Setup dialog box so that it is checked on (enabled). Start the simulation as described in Starting Simulation on page 7-11.
Do not specify a DC sweep and a parametric analysis for the same variable.
Figure 8-1 DC Sweep Setup

Overview of DC Sweep

MicroSim Schematics MicroSim Stimulus Editor input waveforms MicroSim PSpice

stimulus files

Figure 10-1 Relationship of Stimulus Editor with Schematics and PSpice The stimulus specification created using the Stimulus Editor is saved to a file, automatically configured into the schematic, and associated with the corresponding VSTIM, ISTIM, or DIGSTIM part instance or symbol definition.
The Stimulus Editor Utility 10-5
The Stimulus Editor Utility
The Stimulus Editor is a utility which allows you to quickly set up and verify the input waveforms for a transient analysis. You can create and edit voltage sources and current sources for your circuit. Graphical feedback allows you to verify the waveform quickly.

Stimulus Files

The Stimulus Editor produces a file containing the stimuli with their transient specification. These stimuli are defined as simulator device declarations using the V (voltage source) and I (current source) forms. Since the Stimulus Editor produces these statements automatically, you will never have to be concerned with their syntax. However, if you are interested in a detailed description of their syntax, see the descriptions of V and I devices in the PSpice Reference Manual.
MicroSim software versions without the Stimulus Editor must use the characterized-byattribute sources listed in Table 10-1 on page 10-3.
Configuring Stimulus Files
In the schematic editor, Library and Include Files on the Analysis menu allows you to view the list of stimulus files pertaining to your current schematic, or to manually add, delete, or change the stimulus file configuration. The Stimulus Library Files list box displays all of the currently configured stimulus files. One file is specified per line. Files can be configured as either global to the Schematics environment or local to the current schematic. Global files are marked with an asterisk (*) after the file name. When starting the Stimulus Editor from Schematics, stimulus files are automatically configured (added to the list) as local to the current schematic. Otherwise, new stimulus files can be added to the list by entering the file name in the File Name text
box and then clicking on the Add Stimulus (local configuration) or Add Stimulus* (global configuration) button. All other commands work as described for model and include files in Global and local model files on page 5-36.

Running multiple analyses for different temperatures can also be achieved using parametric analysis (see Parametric Analysis on page 11-2). With parametric analysis, the temperatures can be specified either by list, or by range and increments within the range.
are recomputed based upon the CRES model which has parameters TC1 and TC2 reflecting linear and quadratic temperature dependencies. Likewise, the Q3 and Q4 device values are recomputed using the Q2N2222 model which also has temperature-dependent parameters. In the simulation output file, these recomputed device values are reported in the section labeled TEMPERATURE ADJUSTED VALUES.
Figure 11-7 Example Schematic example.sch
Monte Carlo and Sensitivity/ Worst-Case Analyses
This chapter describes how to set up Monte Carlo and sensitivity/worst-case analyses and includes the following sections: Statistical Analyses on page 12-2 Monte Carlo Analysis on page 12-7 Worst-Case Analysis on page 12-21
This entire chapter describes features which are not included in PSpice Basics.
Monte Carlo and Sensitivity/Worst-Case Analyses

Statistical Analyses

Monte Carlo and sensitivity/worst-case are statistical analyses. This section describes information common to both types of analyses. See Monte Carlo Analysis on page 12-7 for information specific to Monte Carlo analyses, and see Worst-Case Analysis on page 12-21 for information specific to sensitivity/worst-case analyses.
Overview of Statistical Analyses
Generating statistical results for Probe As the number of Monte Carlo or worst-case runs increase, simulation takes longer and the Probe data file gets larger. Large Probe data files may be slow to open and slow to draw traces. One way to avoid this problem is to set up an overnight batch job to run the simulation and execute Probe commands. You can even set up the batch job to produce a series of plots on paper which are ready for you in the morning.
The Monte Carlo and worst-case analyses vary the lot or device tolerances of devices between multiple runs of an analysis (DC, AC, or transient). Before running the analysis, you must set up the model and/or lot tolerances of the model parameter to be investigated. A Monte Carlo analysis causes a Monte Carlo (statistical) analysis of the circuit to be performed. A worst-case analysis causes a sensitivity and worst-case analysis of the circuit to be performed. Sensitivity/worst-case analyses are different from Monte Carlo analysis in that they compute the parameters using the sensitivity data rather than random numbers. You can run either a Monte Carlo or a worst-case analysis, but you cannot run both at the same time. Multiple runs of the selected analysis are done while parameters are varied. You can select only one analysis type (AC, DC, or transient) per run. The analysis selected is repeated in subsequent passes of the analysis.

Since we performed a Monte Carlo analysis, we are asked to select the runs for which we wish to display the data. Click on All and then on OK to view all sections. The steps to display a histogram are enumerated below. 1
Select X Axis Settings from the Plot menu. Check the Performance Analysis check box in the Processing Options box and click on OK.
The display changes to the histogram display where the Y axis is the percent of samples. To display a histogram of the distribution of the 1 dB bandwidth for our filter: Select Add from the Trace menu. Click on the Bandwidth(1, db_level) goal function. Click on V(OUT). In the Trace Command text box, place the cursor after the V in Bandwidth(V(OUT) , ) and type DB. The text box should now read as Bandwidth(VDB(OUT) , ). Place the cursor after the comma and type 1 for the 1 dB level. The text box should now read as

Bandwidth(VDB(OUT) , 1).

You can also display this histogram by using the performance analysis wizard to display Bandwidth (VDB(OUT) , 1).
Click on OK to view the histogram.
To change the number of histogram divisions, select Options from the Tools menu and replace 10 with 20 in the Number of Histogram Divisions text box. Click on Save and then OK. The histogram of the 1 dB bandwidth is as shown in Figure 12-12.
Figure 12-dB Bandwidth Histogram The statistics for the histogram are displayed along the bottom of the display by default. They can be turned off by selecting Options from the Tools menu, clicking on the Display Statistics check box to remove the X, and clicking on Save and OK. The statistics show the number of Monte Carlo runs, the number of divisions or vertical bars that make up the histogram, mean, sigma, minimum, maximum, 10th percentile, median, and 90th percentile. Ten percent of the goa1 function values are less than or equal to the 10th percentile number, and 90% of the goal function values are greater than or equal to that number. If there is more than one goal function value that satisfies this criteria, then the 10th percentile is the midpoint of the interval between the goal function values that satisfy the criteria. Similarly, the median and 90th percentile numbers represent goal function values such that 50% and 90% (respectively) of the goal function values are less than or equal to those numbers. Sigma is the standard deviation of the goal function values. We can also show the distribution of the center frequency of our filter. The steps to display the center frequency are enumerated below. Select Add from the Trace menu. Select the CenterFreq(1, db_level) goal function by clicking on it.

To automatically start Probe after simulation
In Schematics, select Probe Setup from the Analysis menu. In the Auto-Run Option area, click on Automatically Run Probe after Simulation. Click on any other options you want to use. Click on OK.
To start Probe and monitor results during a simulation
1 Turn on waveform monitoring: a b Select Probe Setup from the Analysis menu. Select Monitor Waveforms (Auto-update). If this entry is grayed out, then disable the Text Data File Format (CSDF) check box. Click on OK.
Once the simulation is complete (all data sections), the PSpice window reverts to manual mode. If a new Probe window is opened (using New on the Window menu) while monitoring the data, the new window also starts in monitor mode since it is associated with the same Probe data file.
Select Simulate from the Analysis menu to start the simulation. Probe starts automatically and displays one window in monitor mode. In Probe, select the waveforms to be monitored using Add on the Trace menu or by placing markers.
During a multiple run simulation (such as Monte Carlo, parametric or temperature), only the data for the first run is displayed. To view the curves for several runs: a b c Select Close from the File menu to close the data file, then select Open from the File menu to reload it. Specify the data sections (runs) to load. Select the traces to monitor. Waveforms for all loaded sections are displayed.
To start Probe from Schematics
Select Run Probe from the Analysis menu, or press @.
To start Probe in Windows
Display Program Manager. Double-click the Probe icon in the MicroSim program group.

Setup Requirements

For information about customizing Probe colors in msim.ini, see Appendix A in the Schematics Users Guide.
The configuration file msim.ini contains settings which control the way Probe is run on your system. Foreground, background, and trace colors for display and hard copy can be configured for Probe by editing the file msim.ini. files, command files, and switches can be specified in the Run Probe Command text box of the Options/Editor Configuration/App Settings dialog box. The command line entered here is saved to msim.ini. Probe recognizes these options when you start it automatically after simulation or when you start it from Schematics by selecting Run Probe from the Analysis menu or by pressing @.

Manual Startup

The command for running Probe at the Windows Properties command line is: probe <options>* <data file> where options are the command line options for running Probe with a command file (C switch), log file (L switch), etc., where switches are preceded with / or -. is the name of the Probe data file generated by the simulator.

Probe Function ABS(x) SGN(x) SQRT(x) EXP(x) LOG(x) LOG10(x) M(x) P(x) R(x) IMG(x) G(x) PWR(x,y) SIN(x) COS(x) TAN(x) ATAN(x) ARCTAN(x) d(x) s(x) AVG(x) derivative of x with respect to the X axis variable integral of x over the range of the X axis variable running average of x over the range of the X axis variable NO NO NO
Probes Arithmetic Functions
Description |x| +1 (if x>0), 0 (if x=0), -1 (if x<0) x1/2 Available in PSpice? YES YES YES YES YES YES YES YES YES YES NO YES YES YES YES YES

ln(x) log(x)

magnitude of x phase of x {in degrees} real part of x imaginary part of x group delay of x {in seconds} |x|y

sin(x) cos(x) tan(x) tan

Table 13-6 Probes Arithmetic Functions (continued)
Probe Function AVGX(x,d) RMS(x) DB(x) MIN(x) MAX(x) Description running average of x from X_axis_value(x)-d to X_axis_value(x) running RMS average of x over the range of the X axis variable magnitude in decibels of x minimum of the real part of x maximum of the real part of x Available in PSpice? NO NO NO NO NO
For AC analysis, Probe uses complex arithmetic to evaluate expressions. If the result of the expression is complex, then its magnitude is displayed.
Explicit numeric values are input in the same form as the simulator (via Schematics symbol attributes), except that the suffixes M and MEG are replaced with m (milli, 1E-3) and M (mega, 1E+6), respectively. Also, MIL and mil are not supported. With the exception of the m and M scale suffixes, Probe is not case sensitive, therefore upper/lower case characters are equivalent (V(5) and v(5), for example). Unit suffixes are only used to label the axis; they never affect the numerical results. Therefore, it is always safe to leave off a unit suffix. The quantities 2e-3, 2mV, and 0.002V all have the same numerical value. For plotting purposes, Probe notes that the second and third forms are in volts, whereas the first is dimensionless. The units which Probe recognizes are shown in Table 13-7. Table 13-7 Output Units Recognized by Probe
Symbol V A W Unit Volt Amps Watt

Table 13-7

Symbol d s H
Output Units Recognized by Probe
Unit degree (of phase) second Hertz
Probe also knows that W=VA, V=W/A, and A=W/V. So, if you add a trace which is

V(5)*ID(M13)

the axis values will be labeled with W For a demonstration of trace presentation, see Probe Example on page 13-12.

. 2-6. 2-24

. 2-36. 2-39. 2-41. 2-42. 2-44. 2-54. 2-63. 2-83. 2-99 2-103 2-108. 3-48. 3-96 3-101. 4-52. 5-10. 8-4. 8-5. 8-10. 8-11. 8-13. 8-13. 8-14

Tables

Table 0-1 Table 0-2 Table 0-3 Table 1-1 Table 1-2 Table 1-3 Table 1-4 Table 1-5 Table 1-6 Table 2-1 Table 2-2 Table 2-3 Table 2-4 Table 2-5 Table 2-6 Table 2-7 Table 2-8 Table 2-9 Table 2-11 Table 2-12 Table 2-13 Table 2-14 Table 2-15 Table 2-16 Table 2-17 Table 2-18 Table 2-19 Table 2-20 Table 2-21 Table 2-22 Table 2-23
Probe Command Line Options. Parts Command Line Options. Command Summary. Model Parameters for Device Temperature. Flag Options. Option With a Name as its Value. Options With Their Default Values. PSpice Simulation Condition Messages. Analog Device Summary. GaAsFET Model Parameters for All Levels. GaAsFET Model Parameters for Level 1. GaAsFET Model Parameters for Level 2. GaAsFET Model Parameters for Level 3. GaAsFET Model Parameters for Level 4. GaAs FET Model Parameter for Level 5. Capacitor Model Parameters. Diode Model Parameters. Independent Current Source and Stimulus Exponential Waveform Formulas Independent Current Source and Stimulus Pulse Waveform Parameters. Independent Current Source and Stimulus Pulse Waveform Formulas. Independent Voltage Source and Stimulus PWL Waveform Parameters. Independent Current Source and Stimulus Frequency-Modulated Waveform Parameters 2-41 Independent Current Source and Stimulus Sinusoidal Waveform Parameters Independent Current Source and Stimulus Sinusoidal Waveform Formulas. Junction FET Model Parameters. Inductor Coupling Model Parameters. Transmission Line Coupling Device Parameters. Inductor Model Parameters. MOSFET Levels. MOSFET Level 1, 2, and 3 Model Parameters.
xxviii. xl. xli. 1-2. 1-29. 1-36. 1-36. 1-37. 1-39. 2-3. 2-8. 2-9. 2-9. 2-10. 2-10. 2-11. 2-22. 2-25. 2-35. 2-35. 2-36. 2-38
. 2-42. 2-43. 2-45. 2-50. 2-58. 2-62. 2-64. 2-66
Table 2-24 Table 2-25 Table 2-26 Table 2-27 Table 2-28 Table 2-29 Table 2-30 Table 2-31 Table 2-32 Table 2-33 Table 2-34 Table 2-35 Table 3-1 Table 3-2 Table 3-3 Table 3-4 Table 3-5 Table 3-6 Table 3-7 Table 3-8 Table 3-9 Table 3-10 Table 3-11 Table 3-12 Table 3-13 Table 3-14 Table 3-15 Table 3-16 Table 3-17 Table 3-18 Table 3-19 Table 3-20 Table 3-21 Table 3-22 Table 3-23 Table 3-24 Table 3-25 Table 4-1 Table 4-2 Table 4-3 Table 4-4 Table 4-5 MOSFET Level 4 Model Parameters. MOSFET Level 6 Model Parameters. MOSFET Level 6 Expert Parameters. MOSFET Model Parameters for All Levels. Bipolar Transistor Model Parameters. How XCJC and XCJC2 Specify the Distribution of the CJC Capacitance Resistor Model Parameters. Voltage-Controlled Switch Model Parameters. Transmission Line Model Parameters. Current-Controlled Switch Model Parameters. IGBT Device Parameters. IGBT Model Parameters. Digital Device Summary. Digital Primitives Summary. Standard Gate Types. Standard Gate Timing Model Parameters. Tristate Gate Types. Tristate Gate Timing Model Parameters. Edge-Triggered Flip-Flop Timing Model Parameters. D-Type Flip-Flop (DFF) Truth Table. J-K Flip-Flop (JKFF) Truth Table. Dual-Edge D Flip-Flop (DFFDE) Truth Table. Dual-edge J-K Flip-Flop (JKFFDE) Truth Table. Gated Latch Timing Model Parameters. S-R Flip-Flop (SRFF) Truth Table. D-Type Latch (DLTCH) Truth Table. Delay Line Timing Model Parameters. Programmable Logic Array Types. Programmable Logic Array Timing Model Parameters. Read Only Memory Timing Model Parameters. Random Access Memory Timing Model Parameters. Multi-Bit A/D Converter Timing Model Parameters. Multi-Bit D/A Converter Timing Model Parameters. Input/Output Model Parameters. Digital Input Model Parameters. Digital Output Model Parameters. Digital Libraries. Toolbar buttons. Diode Model Default Parameters. Bipolar Transistor Model Default Parameters. IGBT Model Parameters and Default Values. Junction-Field-Effect Transistor Model Default Parameters. 2-68. 2-70. 2-73. 2-75. 2-84. 2-87. 2-95. 2-96. 2-100. 2-104. 2-109. 2-109. 3-2. 3-3. 3-13. 3-14. 3-16. 3-17. 3-23. 3-25. 3-25. 3-26. 3-27. 3-29. 3-30. 3-31. 3-33. 3-36. 3-37. 3-42. 3-44. 3-48. 3-50. 3-91. 3-95. 3-100. 3-105. 4-3. 4-19. 4-24. 4-34. 4-40

Provides information about the implementation of a PLD design targeted for using one or more of AMD devices. Provides information about designing electronic frequency selective filters. Provides a complete list of all of the analog and digital parts in the model and symbol libraries.
* On-line documentation is available only to those users who install MicroSim products by CD-ROM. ** This manual is provided in on-line format only.
Command Line Options for MicroSim Application

Command Files

A command file is an ASCII text file which contains a list of commands to be executed. A command file can be specified in multiple ways: At the command line when starting Probe, StmEd, or Parts, By selecting Run Commands from the File menu and entering a command file name (for Windows Probe and StmEd only), or At the PROBECMD or STMEDCMD command line, found in the configuration file msim.ini (for Windows Probe and StmEd only). The command file is read by the program and all of the commands contained within the file are executed. When the end of the command file is reached, commands are taken from the keyboard and the mouse. If no command file is specified, all of the commands are received from the keyboard and mouse. The ability to record a set of commands can be useful when executing Probe, Parts, and StmEd. This is especially useful in Probe, when you are repeatedly doing the same simulation and looking at the same waveform with only slight changes to the circuit before each run. It can also be used to automatically create hard copy output at the end of very long (e.g., overnight) simulation runs.
Creating and Editing Command Files
You can create your own command file using a text editor, or in Probe and StmEd, you can use the File/Log Commands menu item (see Log Files on page xxxi for an example), to record a list of transactions in a log file, then use File/Run Commands to start running the logged file. If you choose to create a command file using a text editor, note that the commands in the command file are the same as those available from the keyboard with these differences: The name of the command or its first capitalized letter can be used.
Any line that begins with an * is a comment. Blank lines are ignored, therefore, they can be added to improve the readability of the command file. The commands @CR, @UP, @DWN, @LEFT, @RIGHT, and @ESC are used to represent the <Enter>, <>, <>, <>, <>, and <Esc> keys, respectively. The command Pause causes Probe, Parts, or StmEd to wait until any key on the keyboard is pressed. In the case of Probe, this can be useful to examine a waveform before the command file draws the next one. The commands are one to a line in the file, but comment and blank lines can be used to make the file easier to read. Assuming that a Probe data file has been created by simulating the circuit example.sch, you can manually create a command file (using a text editor) called example.cmd which contains the commands listed below. This set of commands draws a waveform, allows you to look at it, and then exits Probe.

* Display trace v(out2) and wait Trace Add v(out2) Pause * Exit Probe environment File Exit
See Simulation Command Line Specification Format on page xxxiv and Simulation Command Line Options on page xxxiv for specifying command files on the simulation command line. See Probe Command Line Specification Format on page xxxviii and Probe Command Line Options on page xxxviii for details on specifying the /C or -c option for Probe.
Once you activate cursors via the Tools/Cursor command, any mouse or keyboard movements that you make for moving the cursor will not be recorded in the command file. You can use the Tools/Cursor commands (i.e., Peak, Trough, etc.), and they will be recorded in your command file, but when replaying the command file, they may not work the same since cursor movement is not recorded. For example, the direction of the cursor movement is not recorded if you use the mouse or arrow keys.
The Search Commands feature is a Cursor option that allows you to position the cursor at a particular point. You can learn more about Search Commands by consulting Probe Help.

Log Files

Instead of creating command files by hand, using a text editor, they can be automatically generated by creating a log file while running Probe, Parts, or StmEd. While executing the particular package, all of the commands given are saved in the log file. The format of the log file is correct for use as a command file. You can automatically create a.log file in Windows Probe or StmEd by selecting File/Log Commands and entering a log file name. This will turn logging on. Any action taken after starting Log Commands is logged in the named file and can be run in another session by using the File/Run Commands option. You can also create a log file for Probe, StmEd, or Parts by using the /l or -l option at the command line. For example:
PROBE /L EXAMPLE.LOG(PC) probe -l example.log(Sun or HP)
Of course, you can use a name for the log file that is more recognizable, such as acplots.cmd (to Probe, Parts, and StmEd, the file name is any valid file name for your computer).
Sun and HP users must use the dash (-) separators, and file names are case sensitive. PC users can use either separator (/) or (-), and file names can be in upper or lower case.

Editing Log Files

After Probe, Parts, or StmEd is finished, the log file is available for editing to customize it for use as a command file. You can edit the following items: Add blank lines and comments to improve readability (perhaps a title and short discussion of what the file does). Add the Pause command for viewing waveforms before proceeding.

Remove the Exit command from the end of the file, so that Probe, Parts, and StmEd do not automatically exit when the end of the command file is reached. You can add or delete other commands from the file or even change the file name to be more recognizable. It is possible to build onto log files, either by using your text editor to combine files or by running Probe, Parts, and StmEd with both a command and log file:
PROBE /C IN.CMD /L OUT.LOG(PC) probe -c in.cmd -l out.log(Sun & HP)
The file in.cmd gives the command to Probe, and Probe saves the (same) commands into the out.log file. When in.cmd runs out of commands, and Probe is taking commands from the keyboard, these commands also go into the out.log file.
Example: Log and Run Commands in Probe
Following is a simple example (using the data file example.dat), of how logging can be used in Probe to record and save user actions to a command file. Command files are useful if you need to remember the steps taken in order to display a set of waveforms for any given data file.
Start Probe. Select File/Log Commands. Enter 2traces in the Log file name field, and click OK. When a check mark is placed in the box next to File/Log Command, this indicates that logging is turned on, and stays on until the box is no longer checked. Select File/Open. Select example.dat (from the examples directory) and click OK. Select Trace/Add, click on the trace names V(OUT1) and V(OUT2), and click OK. At this point, turn logging off by selecting File/Log Commands. This removes the check mark next to the command. Now that logging is turned off, any command issued is no longer logged in the command file. Probe accepts commands from the mouse and keyboard but does not record them. You can view the command file from any text editor. Command files can be edited or appended to depending on the types of commands you want to store for future use. The file 2traces.cmd should look as shown

xxxiii

below (with the exception of a different file path).

Table 0-3

-c <file name> -d <file name>
Specifies the macro command file, which runs the session until the command file ends or Parts quits. Specifies a particular device file, which defines the display and hard copy device types for Parts. If a device file is not specified, the default is pspice.dev. Creates a log file, which saves the commands from this session in a command file for later use.

-l <file name>

The command line options can be space separated or a continuous string, so that:
parts -d ega.dev -c makeplot.cmd parts -cmakeplot.cmd-dega.dev
are equivalent. As shown in this example, the order of the options does not matter. If you do not specify a device file, Parts looks for the device file pspice.dev. So:
parts parts -d pspice.dev
are equivalent. As you finish each device, its model or subcircuit is written to a file with that devices name and with the extension.mod. For instance, if you extracted the parameters for the 1N914 diode, the 2N3306 transistor, and the OP27 opamp, at the end of the Parts session your working directory would contain the files D1N914.MOD, Q2N3306.MOD, and OP27.MOD with the corresponding models and subcircuits. Normally, you would copy the data from these result files into your library file(s), and then delete the individual model (.mod) files.
Stimulus Editor Command Line Options
StmEd command line options can be entered in the following format:
stmed [option]* [input file]

input file option

The name of a new or existing circuit file, and One or more of the options listed in the table that follows. The command line options can be separated by spaces or listed as a continuous string. This means:
stmed -dega.dev -cmakestm.cmd newstm.cir stmed -cmakestm.cmd-dega.dev newstm.cir stmed -d ega.dev -c makestm.cmd newstm.cir

are all equivalent.

-c <command file>
Specifies the name of the command file to be run. For the Sun and HP, -c specifies the macro command file which runs the session until the command file ends or StmEd quits. Specifies a particular device file, which defines the display and hard copy device types for StmEd. If a device file is not specified, the default is pspice.dev. Specifies the name of an alternate initialization file. If not specified, the simulator uses <windows directory>\msim.ini. Creates a log file, which saves the commands from this session. This log file can later be used as an input command file for StmEd.

[NOSUBCKT]

When used, the node voltages and inductor currents for subcircuits are not saved.
[TIME=<value> [REPEAT]] Used to define the transient analysis time at which the bias point is to be saved. If REPEAT is not used, then the bias at the next time point greater than or equal to TIME=<value> is saved. If REPEAT is used, then TIME=<value> is the interval at which the bias is saved. However, only the latest bias is saved; any previous times are overwritten. The [TIME=<value> [REPEAT]] can only be used with a transient analysis. [TEMP=<value>] [STEP=<value>] [MCRUN=<value>] The number of the Monte Carlo or worst-case analysis run for which the bias point is to be saved. [DC=<value>], [DC1=<value>], and [DC2=<value>] Used to specify the DC sweep value at which the bias point is to be saved. The [DC=<value>] should be used if there is only one sweep variable. If there are two sweep variables, then [DC1=<value>] should be used to specify the first sweep value and [DC2=<value>] should be used to specify the second sweep value. The saved bias point information is in the following format: one or more comment lines that list items such as: circuit name, title, date and time of run, analysis, and temperature, or a single.NODESET command containing the bias point voltage values and inductor currents. Only one bias point is saved to the file during any particular analysis. At the specified time, the bias point information and the operating point data for the active devices and controlled sources are written to the output file. When the supplied specifications on the.SAVEBIAS command line match the state of the simulator during execution, the bias point is written out. Defines the temperature at which the bias point is to be saved. The step value at which the bias point is to be saved.

Example of Usage

A.SAVEBIAS command and a.LOADBIAS command can be used to shorten the simulation time of large circuits, and also to aid in convergence. A typical application for a.SAVEBIAS and a.LOADBIAS command is for a simulation which takes a considerable amount of time to converge to a bias point. The bias point can be saved using a.SAVEBIAS command and when the simulation is run again, the previous bias point calculated is used as a starting point for the bias solution to save processing time. The following example illustrates this procedure for a transient simulation.
.SAVEBIAS "SAVEFILE.TRN" TRAN
When the simulation is run, the transient analysis bias point information is saved to the file SAVEFILE.TRN in the form of a.NODESET command. This.NODESET command provides the simulator with a starting solution for determining the bias point calculation for future simulations. To use this file, replace the.SAVEBIAS command in the circuit file using the following.LOADBIAS command.

Model parameter

The.STEP command only steps the DC component of an AC source. In order to step the AC component of an AC source, a variable parameter has to be created. For example,
Vac AC {variable}.param variable=0.step param variable 0 5.ac dec 1e6

<start value>

Can be greater or less than <end value>: that is, the sweep can go in either direction.
<increment value> and <points value> Must be greater than zero. The following examples illustrate two ways of stepping a resistor from 30 to 50 ohms in steps of 5 ohms. This example uses a global parameter:
.PARAM RVAL = 1 R2 {RVAL}.STEP PARAM RVAL 30,50,5
The parameter RVAL is global and PARAM is the keyword used by the.STEP command when using a global parameter. The following example steps the resistor model parameter R:
R2 RMOD 1.MODEL RMOD RES(R=30).STEP RES RMOD(R) 30,50,5
(Note: Do not use R={30}.)
RMOD is the model name, RES is the sweep variable name (a model type), and R is the parameter within the model to step. To step the value of the resistor, the line value of the resistor is multiplied by the R parameter value to achieve the final resistance value, that is: final resistor value = line resistor value R Therefore, if the line value of the resistor is set to one ohm, the final resistor value is 1 R or R. Stepping R from 30 to 50 ohms then steps the resistor value from ohms to ohms. In both examples, all of the ordinary analyses (e.g.,.DC,.AC, and.TRAN) are run for each step.
The.STEP command is similar to the.DC command and immediately raises the question of what happens if both.STEP and.DC try to set the same value. The same question can come up using the Monte Carlo analysis. The answer is that this is not allowed: no two analyses (.STEP,.TEMP,.MC,.WCASE, and.DC) can try to set the same value. This is flagged as an error during read-in and no analyses are performed. The.STEP command provides the capability to look at the response of a circuit as a parameter varies. For example, how does the center frequency of a filter shift as a capacitor varies? Using.STEP, that capacitor can be varied, yielding a family of AC waveforms showing the variation. Similar comments apply to looking at, for example, propagation delay in transient analysis.

Capacitance 1

Cbs = bulk-source capacitance = area cap. + sidewall cap. + transit time cap. Cbd = bulk-drain capacitance = area cap. + sidewall cap. + transit time cap. For: CBS = 0 and CBD = 0 Cbs = ASCJCbsj + PSCJSWCbss + TTGbs Cbd = ADCJCbdj + PDCJSWCbds + TTGds otherwise Cbs = CBSCbsj + PSCJSWCbss + TTGbs Cbd = CBDCbdj + PDCJSWCbds + TTGds where Gbs = DC bulk-source conductance = dIbs/dVbs Gbd = DC bulk-drain conductance = dIbd/dVbd or: Vbs < FCPB Cbsj = (1-Vbs/PB)-MJ Cbss = (1-Vbs/PBSW)-MJSW For: Vbs > FCPB Cbsj = (1-FC)-(1+MJ)(1-FC(1+MJ)+MJVbs/PB) Cbss = (1-FC)-(1+MJSW)(1-FC(1+MJSW)+MJSWVbs/PBSW) For: Vbd < FCPB Cbdj = (1-Vbd/PB)-MJ Cbds = (1-Vbd/PBSW)-MJSW For: Vbd > FCPB Cbdj = (1-FC)-(1+MJ)(1-FC(1+MJ)+MJVbd/PB) Cbds = (1-FC)-(1+MJSW)(1-FC(1+MJSW) +MJSWVbd/PBSW) Cgs = gate-source overlap capacitance = CGSOW Cgd = gate-drain overlap capacitance = CGDOW Cgb = gate-bulk overlap capacitance = CGBOL For MOSFETs the capacitance model has been changed to conserve charge. This change affects the level 1, 2, and 3 models. The level 4 (BSIM) and level 6 (BSIM3) models have their own capacitance model, which already conserves charge and remains unchanged. See reference [6] and reference [7] on page 82 for the equations describing the capacitances due to the channel charge.
1. All capacitances are between terminals of the intrinsic MOSFET. That is, to the inside of the ohmic drain and source resistances.

2-80 Analog Devices

IS(T) JS(T)
= ISe(Eg(Tnom)T/Tnom - Eg(T))/Vt = JSe(Eg(Tnom)T/Tnom - Eg(T))/Vt = JSSWe(Eg(Tnom)T/Tnom - Eg(T))/Vt

JSSW(T) PB(T)

= PBT/Tnom - 3Vtln(T/Tnom) - Eg(Tnom)T/Tnom + Eg(T) = PBSWT/Tnom - 3Vtln(T/Tnom) - Eg(Tnom)T/Tnom + Eg(T)

PBSW(T) PHI(T)

= PHIT/Tnom - 3Vtln(T/Tnom) - Eg(Tnom)T/Tnom + Eg(T) where Eg(T) = silicon bandgap energy = 1.16 -.000702T2/(T+1108) = CBD(1+MJ(.0004(T-Tnom)+(1-PB(T)/PB))) = CBS(1+MJ(.0004(T-Tnom)+(1-PB(T)/PB)))

CBD(T) CBS(T) CJ(T)

= CJ(1+MJ(.0004(T-Tnom)+(1-PB(T)/PB))) = CJSW(1+MJSW(.0004(T-Tnom)+(1-PB(T)/PB)))

CJSW(T) KP(T) UO(T)

= KP(T/Tnom)-3/2 = UO(T/Tnom)-3/2 = MUS(T/Tnom)-3/2

MUS(T) MUZ()

= MUZ(T/Tnom)-3/2 = X3MS(T/Tnom)-3/2

X3MS(T)

The ohmic (parasitic) resistances have no temperature dependence.
Noise is calculated assuming a one hertz bandwidth, using the following spectral power densities (per unit bandwidth): the parasitic resistances (Rd, Rg, Rs, and Rb) generate thermal noise. Id2 = 4kT/Rd Ig2 = 4kT/Rg Is2 = 4kT/Rs Ib2 = 4kT/Rb the intrinsic MOSFET generates shot and flicker noise. Idrain2 = 4kTgm2/3 + KFIdrainAF/(FREQUENCYKchan) where gm = dIdrain/dVgs (at the DC bias point) Kchan = (effective length)2(permittivity of SiO2)/TOX

Model parameters: KP VT MOSFET transconductance, in amps/(square volt) Internal MOSFET channel threshold voltage, in volts
This screens displays the transfer characteristics at nominal temperature as the gate-emitter voltage increases from zero volt. Data sheets usually provide the transfer characteristics curve. Points (Vge, Ic) should be sampled along the entire region of the curve. Care should be taken when sampling points near the threshold region as they will affect the accuracy of the parameter VT.
IGBT - Saturation Characteristics
Device data: Vce Ic Vge Collector-emitter voltage at the given Ic, in volts, at 25C at which the saturation characteristics is measured Collector current at the given Vge, in amps, at which the saturation characteristics is measure Gate-emitter voltage, in volts, at which the saturation characteristics is measured
Model parameters: KF MOSFET linear region transconductance, in amps/(square volt)
This screen shows the saturation characteristics at nominal temperature as the collector current increases from zero amp. Data sheets usually provide the saturation characteristics curve. Points should be sampled along the entire region of the curve.

IGBT - Gate Charge

Device data: Qge Qgc Qg Vg Vcc Ic Gate-emitter charge at turn-on at the given Vcc and Ic, in coulombs Gate-collector charge at turn-on at the given Vcc and Ic, in coulombs Total gate charge at turn-on at the given Vg, Vcc, and Ic, in coulombs Gate voltage at which Qg is measured, in volts Collector voltage at which Qge, Qgc, and Qg are measured, in volts Collector current at which Qge, Qgc, and Qg are measured, in amps
Model parameters: CGS Internal MOSFET gate-source capacitance per unit area, in farads/(square cm)
COXD Internal MOSFET gate-drain overlap oxide capacitance per unit area, in farads/(square cm) AGD Internal MOSFET gate-drain area, in square centimeters
This screen displays the gate charge characteristics at turn-on at the given Vcc and Ic. It shows the gate-emitter voltage, Vge, as a function of gate charge. Usually, the gate charge curve is divided into three distinct regions. The first region shows Vge rising at a constant rate until the collector current reaches Ic as a constant gate current is charging the constant gate-emitter capacitance CGS. The total charge supplied to the gate in this region is Qge. This parameter is obtained in data sheets either in the electrical characteristics table or from the gate-charge curve.
In the second region, Vge is nearly constant as the gate current discharges the internal MOSFET gate-drain capacitance. The charge supplied in this region is Qgc. Like Qge, it is obtained in data sheets either in the electrical characteristics table or from the gate-charge curve. Vge increases at a constant rate again in the third region as the device is now operating in the linear region. The gate current charges both CGS and the internal MOSFET gate-drain overlap oxide capacitance COXD. Qg and Vg represent a point along the curve in this region. They are obtained either in the electrical characteristics table or from the gatecharge curve. Note that Qg must be greater than the sum of Qge and Qgc. Furthermore, Vg must be greater than the gate-emitter plateau voltage Vge in the second region.

FET Input Only Device data: Cc Ib Av-dc f-0db CMRR compensation capacitor input bias current open-loop gain (DC) unity gain frequency common-mode rejection ratio
Macro model internal parameters: BETA C2 CSS GA GCM IS ISS RD RP RSS input transistor transconductance compensation capacitor slew-rate limiting capacitor interstage transconductance common-mode transconductance input leakage current input stage current input stage load resistance power dissipation input stage current source output resistance
This screen completes the input stage and inner stage. The compensation capacitor value (Cc) is sometimes available on the data sheet in the circuit diagram of the opamp. If not, 10-to-20pF is a fair value. For opamps using external compensation, use one of the values on the data sheet for the external capacitor. Then be sure to use that value for the other input data. Open-loop gain: This is a ratio of input/output signal, i.e., small-signal amplification. Being a pure number, it has no units. If the gain is specified as 20V/mV, the gain is 20,000; if the gain is specified as 90 dB, put in 90 dB (Parts converts x dB to 10x/20). Unity gain frequency: This frequency is the intersection of a straight-line extension of the of the mid-band, open-loop, gain roll-off to unity gain (zero decibel). The graph can show gain having only the low-frequency pole included. The high-frequency pole is calculated from open-loop phase margin. CMRR has no frequency dependence.
Operational Amplifier - Open Loop Phase
Device data: Phi phase margin (in degrees) @ unity gain frequency
Macro model internal parameter: C1 phase control capacitor
This screen adjusts the open-loop unity-gain phase margin, which models the high-frequency pole. Sometimes this value is not available in a table but can be found from a graph. This value is not critical for lower-frequency circuits or lower-Q filters: just use the value we provided, which is typical for normal opamps.
Operational Amplifier - Maximum Output Swing
Device data: Ro-dc DC output resistance Ro-ac AC output resistance Ios short-circuit output current limit Macro model internal parameters: RO1 RO2 GB output resistor #1 output resistor #2 output stage transconductance
This screen adjusts the output drive. The graph shows the maximum output level for a resistive load. The data sheet usually lists an output resistance Ro = Ro-dc + Ro-ac. Split this value so that Ro-dc is about two times Ro-ac.

Voltage Comparator Model

The voltage comparator is not an internal PSpice model. Instead, it is an equivalent circuit, or macro model, composed of several devices and bound together using the subcircuit feature of PSpice (see.SUBCKT in Chapter 1,Commands). The model includes the following effects: (i) input impedance and bias current, (ii) differential gain, (iii) output resistive and capacitive loading, (iv) time delay and slew-rate vs. input overdrive, and (v) DC power drain.

Device names and the associated Parts file names are case sensitive.
The screen name is also the label for the graph, which is similar to the graphs on a data sheet. Each screen name is unique to a device, and is used as a guide through this tutorial. A command menu is provided at the bottom of the screen.
To set the X axis to the range.6 to 1.6 volts
Select the command X_axis followed by Set_range, and type.6,1.6 followed by J in the range text box.
To add values for the device curve
The values in this list come from measurements reported on the data sheet. Select the command Device_curve, and immediately start entering data points as pairs of numbers. In this case, enter the forward voltage (Vfwd) first, followed by J. Then enter the forward current (Ifwd) followed by J. Use the following values:

Vfwd = 1 Ifwd = 1

After the last J, a menu appears which allows changes to the data curve. At this point, select Exit, or press E. The screen changes and is similar to that of Figure 8-5. The lower data list has model parameters using values for the PSpice model being worked on. These parameters are fitted whenever the device data is complete enough to do a fit. The model parameters are re-fitted whenever the Fit command is selected, or when a value is changed in the device data. (Parts does not keep track of the value that is changed, so entering the same value still activates a fit.) The graph shows the effect of the changed model parameter values. At this point, the example diode has been given a new value for the model parameter IS only, since there is only one data point.
To add another data point to fit values for both IS and N
Select the command Device_curve, then select Add, and use the following values:

Vfwd =.8 Ifwd =.15

Figure 8-5 Diode model screen after entering one data point in the device curve Notice that the list keeps its values in order. Select Exit or press E. The screen changes and is similar to that of Figure 8-7.
Figure 8-6 Diode model screen after entering two data points in the device curve This time, both IS and N have new values.

To change the transient waveform of VIN, select the Modify_stimulus command from the Main Menu. In the bottom portion of the display, similar to that of Figure 8-9, notice that VIN has a transient specification type of SIN (sinusoidal) and a list of values for each of the parameters that describe the waveform.
To change the peak amplitude from.1 volts to.2 volts
Figure 8-9 Modifying a sinusoidal waveform choose the Transient_parameters command. Select VAMPL from the list of parameter names. Enter.2 and press J. Select Exit. The waveform should now be redrawn using a peak amplitude of.2 volts. 5 Select Exit again to return to the Main Menu.

To create a new stimulus

3 Figure 8-10 Display of

VPULSE from EXAMPLE1

Select the New_stimulus command from the Main Menu. When asked for the name, type VPULSE and press J. Select PULSE from the Transient Parameter Menu to create a pulsed waveform.
Type -1v at the prompt to define the waveform and press J. Repeat steps 1-4 for 1v,.1u,.1u,.1u,.1u, and.4u (the initial voltage, pulsed voltage, delay, rise time, fall time, pulse width, and period, respectively).

To exit the program

Repeatedly select the Exit command until the Exit_program command appears. Exit_program writes the changes made to VIN and the new stimulus VPULSE into example1.cir. Select Abort_program if saving the changes in example1.cir is not wanted.
StmEd Tutorial for a Digital Stimulus
StmEd can be used to edit the digital stimulus in the circuit file digital.cir that is shipped with MicroSim software platforms supporting mixed analog/digital design. Start StmEd by typing:

stmed digital.cir

Figure 8-11 Analog and digital

stimuli in digital.cir

This time, plots are presented for both the analog stimulus VIN, and the digital stimulus U2 as shown in Figure 8-11.

To modify U2

Select the Modify_stimulus command from the Main Menu. Mark U2 as the current stimulus to be edited by pointing to its name (to the left of the digital area) using the mouse, and clicking the left mouse button. A < symbol appears to the right of U2 indicating that it is current. Type J to display the edit screen for U2. Notice that the U2 device is described by digital state value changes at specified time intervals. Select the Add_command item, followed by the Set selection. Type 900.00E-9 for the time value as shown in Figure 8-12. Then type 1 for the digital state value. Figure 8-12 Editing the digital

Modify_stimulus

Allows you to change an existing stimulus that is displayed on the currently selected plot. After selecting Modify_Stimulus, you will be prompted to select the stimulus to modify. Either the Analog Modify Stimulus menu or Digital Modify Stimulus menu will be displayed, depending on the type of stimulus chosen.

Delete_stimulus

Enters the Delete Stimulus menu, which allows you to delete one or all of the stimuli that are displayed in the currently selected plot. Deleting will also remove the stimuli from the circuit file.
Exits the Delete Stimulus menu and returns to the Main menu.
Removes all analog and digital stimuli from the currently selected plot.

all_Digital

Removes all of the digital stimuli from the currently selected plot.

all_aNalog

Removes all of the analog stimuli from the currently selected plot.

Select

Allows you to select one or more analog and/or digital stimuli to be removed. The stimulus selection process is accomplished by highlighting the desire stimlui and then pressing J to remove them. After selecting Select, the first analog stimulus is highlighted. If only digital stimuli are displayed, then the first digital stimulus is highlighted. If the currently highlighted stimulus is one to be removed, use the M to mark that stimulus for removal. The highlight may be moved among the analog stimuli using the l and r, and the digital stimuli using the t and b. The t and b may also be used to scroll the digital stimuli, if there are more displayed then can fit on the digital plot. If both analog and digital stimuli exist, the highlight can be moved from the analog to the digital part or from the digital to the analog part by using the T key. You can also use the left mouse button to select the name of the stimulus to be removed.

Undelete

Redisplays the last stimuli deleted since entering the Delete Stimulus menu. Undelete only appears in the menu if traces have been deleted since entering the Delete Stimulus menu.

Plot_control

Displays the Plot Control menu.

X_axis

Displays the X Axis menu. Since all plots on the display share the same X axis, these commands affect every plot.

Y_axis

Displays the Y Axis menu.

Hard_copy

Prints or plots the display onto a hard copy device. The Hard_copy command works the same as in Print in Probe; see the Print command under the File menu in the Probe chapter.