This reference details the simulation models and circuit simulation analyses and describes some simulation troubleshooting techniques.

Simulation Models

The Altium Designer-based Circuit Simulator is a true mixed-signal simulator, meaning that it can analyze circuits that include both analog and digital devices.
The Simulator uses an enhanced version of the event-driven XSpice, developed by the Georgia Tech Research Institute (GTRI), which itself is based on Berkeley's SPICE3 code. It is fully SPICE3f5 compatible, as well as providing support for a range of PSpice® device models.

Model Types

The models supported by the Simulator can be effectively grouped into the following categories:

SPICE3f5 analog models

These are predefined analog device models that are built-in to SPICE. They cover the various common analog component types, such as resistors, capacitors and inductors, as well as voltage and current sources, transmission lines and switches. The five most common semiconductor devices are also modeled - diodes, BJTs, JFETs, MESFETs and MOSFETs.
A large number of model files (*.mdl) are also included, that define the behavior of specific instances of these devices.

PSpice analog models

These are predefined analog device models that are built-in to PSpice. To support these models, changes have been made to the general form for the corresponding SPICE3f5 device and/or additional parameter support has been added for use in a linked model file.
Note: These models are not listed separately in this reference. PSpice support information is included as part of the information for the relevant SPICE3f5 device model.

XSpice analog models

These are predefined analog device code models that are built-in to XSpice. Code models allow the specification of complex, non-ideal device characteristics, without the need to develop long-winded sub-circuit definitions that can adversely affect Simulator speed performance. The supplied models cover special functions such as gain, hysteresis, voltage and current limiting and definitions of s-domain transfer functions.
The SPICE prefix for these models is A.

Sub-Circuit models

These are models for more complex devices, such as operational amplifiers, timers, crystals, etc, that have been described using the hierarchical sub-circuit syntax.
A sub-circuit consists of SPICE elements that are defined and referenced in a fashion similar to device models. There is no limit on the size or complexity of sub-circuits and sub-circuits can call other sub-circuits. Each sub-circuit is defined in a sub-circuit file (*.ckt).
The SPICE prefix for theses models is X.

Digital models

These are digital device models that have been created using the Digital SimCode™ language. This is a special descriptive language that allows digital devices to be simulated using an extended version of the event-driven XSpice. It is a form of the standard XSpice code model.
Source SimCode model definitions are stored in an ASCII text file (*.txt). Compiled SimCode models are stored in a compiled model file (*.scb). Multiple device models can be placed in the same file, with each reference by means of a special "func=" parameter.
The SPICE prefix for theses models is A.
Digital SimCode is a proprietary language - devices created with it are not compatible with other simulators, nor are digital components created for other simulators compatible with the Altium Designer-based mixed-signal Simulator.

Notes

For more detailed information concerning SPICE, PSpice and XSpice, consult the respective user manuals for each. The XSpice manual is particularly useful for learning about the syntax required for the Code Models added to XSpice by GTRI and extensions that have been made to SPICE3.
Many of the component libraries (*.IntLib) that come with the installation, feature simulation-ready devices. These devices have the necessary model or sub-circuit file included and linked to the schematic component. These are pure SPICE models for maximum compatibility with analog simulators.
There were no syntax changes made between SPICE3f3 and SPICE3f5. The manual for SPICE3f3 therefore describes the correct syntax for the netlist and models supported by the Altium Designer-based mixed-signal Simulator.

Component and Simulation Multipliers

When entering a value for a component or other simulation-related parameter, the value can be entered in one of the following formats:

• As an integer value (e.g. 10)
• As a floating point value (e.g. 3.142)
• As an integer or floating point value followed by an integer exponent (e.g. 10E-2, 3.14E2)
• As an integer or floating point value followed by a valid scale factor
  With respect to the last format, the following is a list of valid scale factors (multipliers) that can be used:

Notes

Letters immediately following a value that are not valid scale factors will be ignored.
Letters immediately following a valid scale factor are also ignored. They can be beneficial as a reference to measurement units used, when viewing the component on the schematic and the relevant parameter is made visible.
The scale factor must immediately follow the value - spaces are not permitted.
The scale factors may be entered in either lower or upper case, or a mixture thereof.

Examples

10, 10V 10Volts and 10Hz all represent the same number, 10. The letters are ignored in all cases as none of them are valid scale factors.
M, m, MA, MSec and MMhos all represent the same scale factor, 10-3. In each case, the letters after the first "m" are ignored.
1000, 1000.0, 1000Hz, 1e3, 1.0e3, 1KHz and 1K all represent the same number, 1000.

Simulation-ready Components - Quick Reference

Within the vast array of integrated libraries supplied as part of the Altium Designer installation, a great number of schematic components are simulation-ready. This means they have a linked simulation model and are ready (with default parameters) to be placed on a schematic sheet, with a view to circuit simulation using the Altium Designer-based Mixed-Signal Simulator.
Simulation-ready schematic components fall into two categories - those supplied specifically for simulation or as part of a generic default set of such components and those that are part of integrated libraries supplied by a specific manufacturer.
The following sections provide a full listing of the non-manufacturer-specific, simulation-ready schematic components that are supplied as part of the installation.

Simulation Sources

The following schematic components can be found in the Simulation Sources integrated library (Library\Simulation\Simulation Sources.IntLib).

Simulation Transmission Lines

The following schematic components can be found in the Simulation Transmission Line integrated library (\Library\Simulation\Simulation Transmission Line.IntLib).

Simulation Math Functions

The following schematic components can be found in the Simulation Math Function integrated library (\Library\Simulation\Simulation Math Function.IntLib).

Simulation Special Functions

The following schematic components can be found in the Simulation Special Function integrated library (\Library\Simulation\Simulation Special Function.IntLib).

Miscellaneous Devices

The following schematic components can be found in the Miscellaneous Devices integrated library (\Library\Miscellaneous Devices.IntLib).

Simulation-Ready Components by Manufacturer

The following sections provide a listing of various manufacturer-specific integrated libraries that are supplied as part of the installation and which contain simulation-ready schematic components. The sub-folders containing the integrated libraries (arranged by Manufacturer) can be found along the following path:
\Library\ - on the drive to which you installed the software.
Note that not all schematic components in a listed library may have a linked simulation model.

Agilent Technologies

Agilent LED Display 7-Segment, 1-Digit.IntLib
Agilent LED Display 7-Segment, 2-Digit.IntLib
Agilent LED Display 7-Segment, 3-Digit.IntLib
Agilent LED Display 7-Segment, 4-Digit.IntLib
Agilent LED Display Alphanumeric.IntLib
Agilent LED Display Digit & Word Icon.IntLib
Agilent LED Display Overflow.IntLib
Agilent Optoelectronic LED.IntLib

Analog Devices

• AD Amplifier Buffer.IntLib
• AD Analog Multiplier Divider.IntLib
• AD Audio Pre-Amplifier.IntLib
• AD Differential Amplifier.IntLib
• AD Instrumentation Amplifier.IntLib
• AD Operational Amplifier.IntLib
• AD Power Mgt Voltage Reference.IntLib
• AD RF and IF Modulator Demodulator.IntLib
• AD Variable Gain Amplifier.IntLib
• AD Video Amplifier.IntLib

Burr-Brown

• BB Amplifier Buffer.IntLib
• BB Analog Integrator.IntLib
• BB Differential Amplifier.IntLib
• BB Instrumentation Amplifier.IntLib
• BB Isolation Amplifier.IntLib
• BB Logarithmic Amplifier.IntLib
• BB Operational Amplifier.IntLib
• BB Transconductance Amplifier.IntLib
• BB Universal Active Filter.IntLib
• BB Voltage Controlled Amplifier.IntLib

ECS

• ECS Crystal Oscillator.IntLib

Elantec

• Elantec Amplifier Buffer.IntLib
• Elantec Analog Comparator.IntLib
• Elantec Analog Multiplier Divider.IntLib
• Elantec Interface Line Transceiver.IntLib
• Elantec Operational Amplifier.IntLib
• Elantec Video Amplifier.IntLib
• Elantec Video Gain Control Circuit.IntLib

Fairchild Semiconductor

• FSC Discrete BJT.IntLib
• FSC Discrete Diode.IntLib
• FSC Discrete Rectifier.IntLib
• FSC Interface Display Driver.IntLib
• FSC Interface Line Transceiver.IntLib
• FSC Logic Buffer Line Driver.IntLib
• FSC Logic Counter.IntLib
• FSC Logic Decoder Demux.IntLib
• FSC Logic Flip-Flop.IntLib
• FSC Logic Gate.IntLib
• FSC Logic Latch.IntLib
• FSC Logic Multiplexer.IntLib
• FSC Logic Parity Gen Check Detect.IntLib
• FSC Logic Register.IntLib

Infineon

• Infineon Discrete BJT.IntLib
• Infineon Discrete Diode.IntLib

International Rectifier

• IR Discrete IGBT.IntLib
• IR Discrete MOSFET - Half Bridge.IntLib
• IR Discrete MOSFET - Low Power.IntLib
• IR Discrete MOSFET - Power.IntLib
• IR Discrete SCR.IntLib
• IR Rectifier - Schottky.IntLib
• IR Rectifier - Standard Recovery.IntLib
• IR Rectifier - Ultrafast Recovery.IntLib

Intersil

• Intersil Discrete BJT.IntLib
• Intersil Discrete MOSFET.IntLib
• Intersil Operational Amplifier.IntLib

KEMET Electronics

• KEMET Chip Capacitor.IntLib

Linear Technology

• LT Amplifier Buffer.IntLib
• LT Operational Amplifier.IntLib
• LT Video Amplifier.IntLib

Maxim

• Maxim Amplifier Buffer.IntLib
• Maxim Analog Comparator.IntLib
• Maxim Communication Receiver.IntLib
• Maxim Current-Feedback Amplifier.IntLib
• Maxim Multiplexed Video Amplifier.IntLib
• Maxim Operational Amplifier.IntLib
• Maxim Video Amplifier.IntLib
• Maxim Wideband Amplifier.IntLib

Motorola

• Motorola Amplifier Operational Amplifier.IntLib
• Motorola Discrete BJT.IntLib
• Motorola Discrete Diode.IntLib
• Motorola Discrete IGBT.IntLib
• Motorola Discrete JFET.IntLib
• Motorola Discrete MOSFET.IntLib
• Motorola Discrete SCR.IntLib
• Motorola Discrete TRIAC.IntLib

National Semiconductor

• NSC Amplifier Buffer.IntLib
• NSC Analog Comparator.IntLib
• NSC Converter Analog to Digital.IntLib
• NSC Discrete BJT.IntLib
• NSC Discrete Diode.IntLib
• NSC Discrete JFET.IntLib
• NSC Discrete Rectifier.IntLib
• NSC Interface Display Driver.IntLib
• NSC Interface Line Transceiver.IntLib
• NSC Logic Arithmetic.IntLib
• NSC Logic Buffer Line Driver.IntLib
• NSC Logic Comparator.IntLib
• NSC Logic Counter.IntLib
• NSC Logic Decoder Demux.IntLib
• NSC Logic Flip-Flop.IntLib
• NSC Logic Gate.IntLib
• NSC Logic Latch.IntLib
• NSC Logic Multiplexer.IntLib
• NSC Logic Parity Gen Check Detect.IntLib
• NSC Logic Register.IntLib
• NSC Operational Amplifier.IntLib
• NSC Power Mgt Voltage Regulator.IntLib

Panasonic

• Panasonic Resistor.IntLib

Philips

• Philips Discrete BJT - Darlington.IntLib
• Philips Discrete BJT - Lower Power.IntLib
• Philips Discrete BJT - Medium Power.IntLib
• Philips Discrete BJT - RF Transistor.IntLib
• Philips Discrete Diode - Schottky.IntLib
• Philips Discrete Diode - Switching.IntLib
• Philips Discrete JFET.IntLib
• Philips Discrete MOSFET - Lower Power.IntLib
• Philips Discrete MOSFET - Power.IntLib

Raltron Electronics

• Raltron Crystal Oscillator.IntLib

ST Microelectronics

• ST Discrete BJT.IntLib
• ST Interface Display Driver.IntLib
• ST Logic Arithmetic.IntLib
• ST Logic Buffer Line Driver.IntLib
• ST Logic Comparator.IntLib
• ST Logic Counter.IntLib
• ST Logic Decoder.IntLib
• ST Logic Flip-Flop.IntLib
• ST Logic Gate.IntLib
• ST Logic Latch.IntLib
• ST Logic Multiplexer.IntLib
• ST Logic Register.IntLib
• ST Operational Amplifier.IntLib

Teccor Electronics

• Teccor Discrete SCR.IntLib
• Teccor Discrete TRIAC.IntLib

Texas Instruments

• TI Analog Comparator.IntLib
• TI Interface 8-bit Line Transceiver.IntLib
• TI Interface Display Driver.IntLib
• TI Interface Line Transceiver.IntLib
• TI Logic Arithmetic.IntLib
• TI Logic Buffer Line Driver.IntLib
• TI Logic Comparator.IntLib
• TI Logic Counter.IntLib
• TI Logic Decoder Demux.IntLib
• TI Logic Flip-Flop.IntLib
• TI Logic Gate 1.IntLib
• TI Logic Gate 2.IntLib
• TI Logic Latch.IntLib
• TI Logic Multiplexer.IntLib
• TI Logic Parity Gen Check Detect.IntLib
• TI Logic Register.IntLib
• TI Operational Amplifier.IntLib
• TI Power Mgt Voltage Regulator.IntLib

Toshiba

• Toshiba Discrete IGBT.IntLib

Vishay

• Vishay Cera-Mite Ceramic Axial-Lead Capacitor.IntLib
• Vishay Draloric Ceramic Disc Capacitor.IntLib
• Vishay Draloric Ceramic Tubular Capacitor.IntLib
• Vishay Electrolytic Radial-Lead Capacitor.IntLib
• Vishay Lite-On Discrete Diode.IntLib
• Vishay Roederstein Electrolytic Axial-Lead Capacitor.IntLib
• Vishay Roederstein Electrolytic Radial-Lead Capacitor.IntLib
• Vishay Roederstein Electrolytic Snap-In Pins Capacitor.IntLib
• Vishay Roederstein Electrolytic Solder Ring Capacitor.IntLib
• Vishay Roederstein Tantalum Radial-Lead Capacitor.IntLib
• Vishay Siliconix Discrete JFET.IntLib
• Vishay Siliconix Discrete MOSFET.IntLib
• Vishay Sprague Tantalum Axial-Lead Capacitor.IntLib
• Vishay Sprague Tantalum Chip Capacitor.IntLib
• Vishay Sprague Tantalum Radial-Lead Capacitor.IntLib
• Vishay Tansitor Tantalum Axial-Lead Capacitor.IntLib
• Vishay Tansitor Tantalum Radial-Lead Capacitor.IntLib
• Vishay Telefunken Discrete Diode.IntLib
• Vishay Vitramon Ceramic Dipped Capacitor.IntLib

Zetex

• Zetex Discrete BJT.IntLib
• Zetex Discrete Diode.IntLib
• Zetex Discrete MOSFET.IntLib

Searching for Simulation-Ready Components

With such a vast collection of simulation-ready components - both generic and manufacturer-specific - scattered across a multitude of integrated libraries, you may think that finding the component you need is like searching for that proverbial 'needle in a haystack'. To simplify this process, search features are available that allow you to:

• Search for a simulation-ready component across libraries local to your installation of Altium Designer
• Search for a simulation-ready component within the available up-to-date libraries supplied by the Altium Library Development Center (ALDC) - available from the Altium Website.

Searching Installation Libraries

By using Altium Designer's Libraries Search feature, you can quickly search for simulation-ready components:

• across all available libraries for the active project
• in libraries along a specified search path.
  Search criteria is specified within the Libraries Search dialog. Access this dialog from within a schematic document (Tools » Find Component) or by clicking the Search button on the Libraries panel.
  By defining suitable queries, you can quickly find the simulation-ready components that you require. The more specific the query, the narrower the search and the greater the probability of returning favorable results.
  The coarsest search you could do is to search for all components that have a linked simulation model. To do this, you would simply enter the following query into the top section of the Libraries Search dialog (often referred to as the Query Editor section):

This expression returns all components that have a linked simulation model. The '*' entry is used as a wildcard for the model name. The 'FALSE' entry specifies that the model need not be the current model for the component (if multiple simulation models have been defined and linked to the component).

The results of the search will be listed in the Libraries panel, under a new entry to the libraries drop-down list - Query Results.
The library search facility also offers the ability to refine the last search made. This enables you to apply further, perhaps more specific search criteria, to the list of Query Results obtained by the previous search. For example, you might set up a search targeting the entire \Library directory for all components that have a linked simulation model and a description containing the word Diode, using the following query expression:

Such a search might well yield in excess of 1500 components fitting that criteria! You might then decide that out of these returned results, you wish to further search and return only Zener diodes. Simply enable the Refine last search option in the Scope region of the Libraries Search dialog, enter the following new query expression and click Search.
Description Like 'Zener'
The subset of the previous query results falling under the scope of the new, refining query, will be displayed as the new Query Results list in the Libraries panel.
Let us now consider a more complex search. You might know a partial name for the component you need for a design and have preferred manufacturers that you like to use. Again, searching is simplified through the power of the Query language. Consider a design where you need to use a particular diode, whose name is of the form 1N4*. You need to search for all components with a name based on this root, which are simulation ready, and which are manufactured by either National Semiconductor or Motorola. This search can be specified by entering the following query:

Out of a possible 18000+ simulation-ready components that come installed with Altium Designer, the preceding query returns a manageable 57 components, as illustrated by the following image.

Searching via the Altium Website

Simply click on the available link for the Altium Designer board-level design integrated libraries and then access the Search for a component facility. Use this facility to quickly search for simulation-ready components.

Use the fields provided to make your search criteria as broad or specific as required. If, for example, you wanted to quickly find all simulation-ready components of a particular type - across all manufacturer integrated libraries - simply set the Class and Sub-Class fields as required and ensure that the Show only simulation-ready components option is enabled. Such a search could be narrowed further by entering a specific package type for the component, and so on.
After running the search, the results will be listed, alphabetically, and by manufacturer. The following information is provided:

• Component Name
• Manufacturer of the component
• Description of the component
• Package Type
• Name of the integrated library into which the component has been compiled
• Downloadable zip file - containing all integrated libraries for that manufacturer
• Date Component was last updated.

From the list of results, you can access further information about a component, simply by clicking on the entry for its name. From a simulation perspective, this gives you information about any model or sub-circuit file linked as a model to the component.

The Netlist Template - Explained

The Netlist Template allows access to the information that is entered into the XSpice netlist for a given component. It is accessed by clicking on the Netlist Template tab, at the bottom of the Sim Model dialog.
For all of the predefined model kinds and sub-kinds, the Netlist Template is read-only. If, however, one of these predefined entries does not allow enough control over the information placed in the netlist, you can define your own template.
To edit the Netlist Template, you need to select Generic Editor in the Model Sub-Kind region of the Sim Model dialog - ensuring that the Model Kind field is first set to General. This will be the default model kind/sub-kind setting when adding a new simulation model to a schematic component. For all other General model sub-kinds, you can effectively change to Generic Editor and edit the predefined template - massaging it to your own requirements.
When defining the Netlist Template, the information entered should be in accordance with the requirements of SPICE3f5/XSpice and the syntax rules described below.

Netlist Template Syntax

Characters that are entered into the template are written to the XSpice netlist verbatim, except for the following special characters:

These characters are translated when creating the netlist, as shown in the following table:

In the above table,

• s represents a separator character (, . ; / |).
• <param> refers to the name of a parameter.
  If the parameter name contains any non-alphanumeric characters, it should be enclosed in double quotes. For example:
  @"DC Magnitude" - double quotes used here because the name contains a space.
  &"Init_Cond" - double quotes used here because the name contains an underscore.
  Double quotes should also be used when you wish to add an alphanumeric prefix to a parameter name. For example:
  @"DESIGNATOR"A - the use of the double quotes ensures that A is appended to the component designator.

Syntax Examples

The following are examples of the special character syntax entries in the previous table. Information is given in each case, about how the syntax entry is translated by the Netlister.
@"AC Phase"
The parameter name AC Phase is enclosed in braces because of the space. This will be replaced in the netlist with the value of the AC Phase parameter. If there is no parameter of this name, or its value is blank then an error will be given.
&Area
If a parameter named Area exists and has a value, then it's value will be entered into the netlist. If the parameter is undefined (i.e. either it does not exist or has no value assigned) then nothing will be written to the netlist, but no error will be raised. This can be used for optional parameters.
?IC|IC=@IC|
If the parameter named IC is defined then the text within the || separators will be inserted into the netlist. For example if the parameter IC had value 0.5 then IC=0.5 would be inserted into the netlist in place of this entry. If the parameter is undefined then nothing will be inserted into the netlist.
?IC/IC=@IC//IC=0/
This is the same as the previous example, except that if the parameter IC is undefined then IC=0 will be inserted into the netlist. Note also that a different separator character has been used.
~VALUE/1k/
If a parameter named VALUE is NOT defined then the text 1k will be inserted into the netlist.
~VALUE/1k//@VALUE/
This is the same as the previous example, except that if the parameter VALUE is defined then its text value will be inserted into the netlist.
#"AC Magnitude"|AC@"AC Magnitude"|@"AC Phase"
This example can be seen in the predefined netlist template for the sinusoidal voltage source.
If the AC Magnitude parameter has been defined then the contents of the separators is evaluated and inserted into the netlist. All following entries in the netlist are also evaluated and entered into the netlist (in this case @"AC Phase").
If for example AC Magnitude=1 and AC Phase=0 then AC 1 0 will be inserted into the netlist. If, however, AC Phase was undefined, an error would be raised.
If the parameter AC Magnitude is undefined then nothing following the #"AC Magnitude" entry in the netlist template will be entered into the netlist.
#|PARAMS:|?Resistance|Resistance=Resistance|?Current|Current=@Current|
This example can be seen in the predefined netlist template for a parameterized subcircuit (see F1 in Fuse.PrjPcb).
If the Resistance and Current parameters are both undefined then there will be no text to be inserted into the netlist following the #|PARAMS:| entry, so the text in the separators will be omitted also.
If for example the parameters have values Resistance=1k and Current=5mA then this will result in text following the #|PARAMS:| entry and PARAMS: Resistance=1k Current=5mA will be the entry made in the netlist.
@DESIGNATOR%1%2@VALUE
This example is to demonstrate the use of the % character.
If for example the parameters have values DESIGNATOR=R1 and VALUE=1k, and the pins are mapped on the Port Map tab of the Sim Model dialog according to the following table:

Then the text R1 GND OUT 1k will be placed into the XSpice netlist for this component.

Checking the Netlist Template

To check the Netlist Template, simply click on the Netlist Preview tab at the bottom of the Sim Model dialog. The text displayed in this tab is exactly as it will be written to the XSpice netlist file when a netlist is generated or a simulation is run. The following exception applies:

• If you are in the Schematic Library Editor, or the document/project has not been compiled, the net names that the model pins map to will not be available. In this case, the schematic pin designators are inserted, enclosed in <> braces.
  Any errors that occur while parsing user-defined entries in the Netlist Template will also be displayed, so that any errors can be resolved prior to exiting the dialog.

PSpice Support

To facilitate compatibility with PSpice, support for various additional PSpice-based functions and operators is provided, as well as the use of global parameters - to represent values in a PSpice-modeled circuit.

Additional Function Support

The following additional functions are supported:

Additional Operator Support

The following additional operators are supported:
** * (exponentiation)

• == (equality test)
• != (non-equality test)
• & (Boolean AND)
• | (Boolean OR)

.PARAM Support

The PSpice .PARAM statement is supported. This statement defines the value of a parameter, allowing you to use a parameter name in place of numeric values for a circuit description. Parameters can be constants, expressions or a combination of the two. A single parameter statement can include reference to one or more additional parameter statements.
In addition, the following three internal variables (predefined parameters) are available for use in expressions:

Global Parameters

Altium Designer's Circuit Simulator supports the use of global parameters and equations. Use a global parameter in an equation and then use that equation in a component value on your schematic. Alternatively, define the equation as a global parameter and then reference the global parameter from a component value.
Simply include the expression or parameter name within curly braces {} - when the Simulator detects this it will attempt to evaluate it, checking the Global Parameters page of the Simulator's Analyses Setup dialog for the definition of any part of the expression that cannot be immediately resolved.

SPICE3f5 models

These are predefined analog device models that are built-in to SPICE. They cover the following, common analog component types.
General
Capacitor
Capacitor (Semiconductor)
Coupled Inductors
Diode
Inductor
Potentiometer
Resistor
Resistor (Semiconductor)
Resistor (Variable)
Transistors
Bipolar Junction Transistor (BJT)
Junction Field-Effect Transistor (JFET)
Metal Semiconductor Field-Effect Transistor (MESFET)
Metal Oxide Semiconductor Field-Effect Transistor (MOSFET)
Switches
Current Controlled Switch
Voltage Controlled Switch
Transmission Lines
Lossless Transmission Line
Lossy Transmission Line
Uniform Distributed RC (lossy) Transmission Line
Current Sources
Current-Controlled Current Source
DC Current Source
Exponential Current Source
Frequency Modulated Sinusoidal Current Source
Non-Linear Dependent Current Source
Piecewise Linear Current Source
Pulse Current Source
Sinusoidal Current Source
Voltage-Controlled Current Source
Voltage Sources
Current-Controlled Voltage Source
DC Voltage Source
Exponential Voltage Source
Frequency Modulated Sinusoidal Voltage Source
Non-Linear Dependent Voltage Source
Piecewise Linear Voltage Source
Pulse Voltage Source
Sinusoidal Voltage Source
Voltage-Controlled Voltage Source
Initial Conditions
Initial Condition
Nodeset
Notes

Many of the models have associated model files (*.mdl). A model file is used to allow specification of specific device parameters (e.g. on and off resistances for a switch).
Many of the above models have been modified to make them compatible with PSpice. In such cases, PSpice support information is included as part of that model's information, later in this reference.
Many of the component libraries (*.IntLib) that come with the installation, feature simulation-ready devices. These devices have the necessary model or sub-circuit file included and linked to the schematic component. These are pure SPICE models for maximum compatibility with analog simulators.

General

Capacitor

Model Kind

General

Model Sub-Kind

Capacitor

SPICE Prefix

C

SPICE Netlist Template Format

@DESIGNATOR %1 %2 @VALUE ?"INITIAL VOLTAGE"|IC=@"INITIAL VOLTAGE"|

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Notes

The value for the Initial Voltage only applies if the Use Initial Conditions option is enabled on the Transient/Fourier Analysis Setup page of the Analyses Setup dialog.

Examples

Consider the capacitor in the above image, with the following characteristics:

• Pin1 (positive) is connected to net N1
• Pin2 (negative) is connected to net VN
• Designator is C1
• Value = 0.02uF.
  The entry in the SPICE netlist would be:
  *Schematic Netlist:
  C1 N1 VN 0.02uF
  

Capacitor (Semiconductor)

Model Kind

General

Model Sub-Kind

Capacitor(Semiconductor)

SPICE Prefix

C

SPICE Netlist Template Format

@DESIGNATOR %1 %2 &VALUE &MODEL ?LENGTH|L=@LENGTH| ?WIDTH|W=@WIDTH| ?"INITIAL VOLTAGE"|IC=@"INITIAL VOLTAGE"|

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Parameters (definable within model file)

The following is a list of process-related parameters that can be stored in the associated model file:

Notes

The value for the Initial Voltage only applies if the Use Initial Conditions option is enabled on the Transient/Fourier Analysis Setup page of the Analyses Setup dialog.
You can specify either a direct value for the capacitance OR enter values for the capacitors' length and width. In the case of the latter, a value for the capacitance will be calculated, in conjunction with parameter information stored in the model.
The equation used to calculate the capacitance from geometric data is:
CAP = CJ(LENGTH
- NARROW)(WIDTH
- NARROW)
+ 2CJSW(LENGTH
+ WIDTH
- 2 NARROW)
If a direct value for capacitance is not specified, the model name and length must be supplied in order for the geometric-based capacitance value to be calculated.
The link to the required model file (*.mdl) is specified on the Model Kind tab of the Sim Model dialog. The Model Name is used in the netlist to reference this file.
Either the direct capacitance value OR the geometric data used to calculate it can be entered, but not both.
Where a parameter has an indicated default (as part of the SPICE model definition), that default will be used if no value is specifically entered. The default should be applicable to most simulations. Generally you do not need to change this value.

Examples

Consider the semiconductor capacitor in the above image, with the following characteristics:

• Pin1 is connected to net N1
• Pin2 is connected to net VN
• Designator is C1
• The linked simulation model file is CAP.mdl
  If a value for the capacitance was entered directly, say 100 pF, and no other parameters were specified on the Parameters tab of the Sim Model dialog, then the entry in the SPICE netlist would be:
  *Schematic Netlist:
  C1 N1 VN 100pF CAP
  Consider now, instead of entering a direct value for the capacitance, the following parameters were defined in the Sim Model dialog:
• Length = 10u
• Width = 1u
  the entry in the netlist would be:
  C1 N1 VN CAP L=10u W=1u
  The value for the capacitance will be calculated accurately using the geometric data specified and any further parameter definitions in the model file (CAP.mdl).

PSpice Support

To make this device model compatible with PSpice, the following additional model parameters are supported and can be entered into a linked model file (*.mdl) for the device:

Where a parameter has an indicated default, that default will be used if no value is specifically entered.
The format for the PSpice model file is:

.MODEL ModelName CAP(Model Parameters),
where

• ModelName is the name of the model, the link to which is specified on the Model Kind tab of the Sim Model dialog. This name is used in the netlist (&MODEL) to reference the required model in the linked model file.
• Model Parameters are a list of supported parameters for the model, entered with values as required.

Coupled Inductors

Model Kind

General

Model Sub-Kind

Coupled Inductors

SPICE Prefix

K

SPICE Netlist Template Format

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Examples

Consider the transformer in the above image, which uses a coupled inductor model and has the following characteristics:

• The positive pin of the Primary is connected to net Vin2
• The negative pin of the Primary is connected to net GND
• The positive pin of the secondary is connected to net Vout2
• The negative pin of the secondary is connected to net GND
• Designator is T1
• Inductance A = 1mH
• Inductance B = 1mH
• Coupling Factor = 0.5.
  The entry in the SPICE netlist would be:
  *Schematic Netlist:
  LA_KT1 VIN2 0 1mH
  LB_KT1 VOUT2 0 1mH
  KT1 LA_KT1 LB_KT1 0.5
  Placing a transformer with a coupled inductor model is probably the simplest and quickest way of adding a coupled inductor to your source schematic. However, should you wish to place individual inductors in the schematic design and couple them, the required information for the SPICE netlist can be readily supplied through the use of a Text Frame.
  Simply place a text frame in the schematic document and ensure that the first line is:
  .NSX
  Then type the information required
  - each line will be included in the netlist, exactly as it is written, appearing between the following comment entries:
  *Begin NSX text frames
  *End of NSX text frames
  The following example illustrates the use of two inductors and a text frame to provide a coupled inductor for simulation purposes.
  Consider the circuit in the adjacent image, which contains two discrete inductors with the following characteristics:
• Designator (Primary inductor) = L1
• Designator (Secondary inductor) = L2
• The positive pin of L1 is connected to net Vin1
• The negative pin of L1 is connected to net GND
• The positive pin of L2 is connected to net Vout1
• The negative pin of L2 is connected to net GND

• Value for inductance (L1) = 10mH
• Value for inductance (L2) = 10mH
  The entries in the text frame are dissected as follows:
• .NSX
  - the mandatory first line that tells the netlister that the following lines are extra information to be added when generating the SPICE netlist.
• K1
  - the designator for the 'coupled inductor', where K is the required SPICE prefix.
• L1, L2
  - the designators of the two individual inductors
• 0.5
  - the value for the Coupling Factor
  The entry in the SPICE netlist would be:
  *Begin NSX text frames
  K1 L1 L2 0.5
  *End of NSX text frames
  .
  .
  *Schematic Netlist:
  L1 VIN1 0 10mH
  L2 VOUT1 0 10mH

Diode

Model Kind

General

Model Sub-Kind

Diode

SPICE Prefix

D

SPICE Netlist Template Format

@DESIGNATOR %1 %2 @MODEL &"AREA FACTOR" &"STARTING CONDITION" ?"INITIAL VOLTAGE"|IC=@"INITIAL VOLTAGE"| ?TEMPERATURE|TEMP=@TEMPERATURE|

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Parameters (definable within model file)

The following is a list of parameters that can be stored in the associated model file:

Notes

The value for the Initial Voltage only applies if the Use Initial Conditions option is enabled on the Transient/Fourier Analysis Setup page of the Analyses Setup dialog.
The Area Factor affects the following three model parameters:

• saturation current (IS)
• ohmic resistance (RS)
• zero-bias junction capacitance (CJO)
  If the Area Factor is omitted, a value of 1.0 is assumed.
  The link to the required model file (*.mdl) is specified on the Model Kind tab of the Sim Model dialog. The Model Name is used in the netlist to reference this file.
  Where a parameter has an indicated default (as part of the SPICE model definition), that default will be used if no value is specifically entered. The default should be applicable to most simulations. Generally you do not need to change this value.

Examples

Consider the diode in the above image, with the following characteristics:

• Pin1 (anode) is connected to net VIN
• Pin2 (cathode) is connected to net Vhw
• Designator is D1
• The linked simulation model file is 1N4002.mdl.
  If no values are entered for the parameters in the Sim Model dialog, the entries in the SPICE netlist would be:
  *Schematic Netlist:
  D1 VIN VHW 1N4002
  .
  .
  *Models and Subcircuit:
  .MODEL 1N4002 D(IS=2.55E-9 RS=0.042 N=1.75 TT=5.76E-6 CJO=1.85E-11 VJ=0.75
  + M=0.333 BV=100 IBV=1E-5 )
  and the SPICE engine would use the indicated parameter information defined in the model file, along with default parameter values inherent to the model for those parameters not specified in the file.
  If the following parameter values were specified on the Parameters tab of the Sim Model dialog:
• Area Factor = 3
• Initial Voltage = 2
• Temperature = 22
  then the entries in the SPICE netlist would be:
  *Schematic Netlist:
  D1 VIN VHW 1N4002 3 IC=2 TEMP=22
  .
  .
  *Models and Subcircuit:
  .MODEL 1N4002 D(IS=2.55E-9 RS=0.042 N=1.75 TT=5.76E-6 CJO=1.85E-11 VJ=0.75
  + M=0.333 BV=100 IBV=1E-5 )
  In this case, the SPICE engine would use this information, in conjunction with the indicated parameters defined in the model file (and any defaults for parameters not specified).

PSpice Support

To make this device model compatible with PSpice, the following additional model parameters are supported and can be entered into a linked model file (*.mdl) for the device:

Where a parameter has an indicated default, that default will be used if no value is specifically entered.
The format for the PSpice model file is:

.MODEL ModelName D(Model Parameters),
where

• ModelName is the name of the model, the link to which is specified on the Model Kind tab of the Sim Model dialog. This name is used in the netlist (@MODEL) to reference the required model in the linked model file.

• Model Parameters are a list of supported parameters for the model, entered with values as required.

  For an example of using a PSpice-compatible diode model in a simulation, refer to the example project Diode.PrjPCB, which can be found in the \Examples\Circuit Simulation\PSpice Examples\Diode folder of the installation.

Inductor

Model Kind

General

Model Sub-Kind

Inductor

SPICE Prefix

L

SPICE Netlist Template Format

@DESIGNATOR %1 %2 @VALUE ?"INITIAL CURRENT"|IC=@"INITIAL CURRENT"|

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Notes

The value for the Initial Current only applies if the Use Initial Conditions option is enabled on the Transient/Fourier Analysis Setup page of the Analyses Setup dialog.

Examples

Consider the inductor in the above image, with the following characteristics:

• Pin1 (positive) is connected to net Vin
• Pin2 (negative) is connected to net Vfw
• Designator is L1
• Value = 10mH.
  The entry in the SPICE netlist would be:
  *Schematic Netlist:
  L1 Vin Vfw 10mH
  PSpice Support
  The existing Spice3f5 model for the Inductor device has been enhanced to support the general PSpice model form:

L<name> <(+) node> <(-) node> [model name] <value> [IC = <initial value>]
A PSpice model of this type should be linked to a schematic component using a model file. Simply specify the model in a model file (*.mdl) then, in the Sim Model dialog, set the Model Kind to General and the Model Sub-Kind to Generic Editor. The Netlist Template Format should then be entered as follows:
@DESIGNATOR %1 %2 @VALUE @MODEL ?"INITIAL CURRENT"|IC=@"INITIAL CURRENT"|
The value for the INITIAL CURRENT parameter is entered on the Parameters tab of the Sim Model dialog.
The netlist format for a PSpice Inductor model is specified using the Generic Editor due to the fact that the Spice3f5 Inductor model does not support use of a linked model file.
For the circuit to be parsed correctly, ensure that the Spice Prefix field is set to L.
In the Model Name field, enter the name specified for the model in the model file. Use the options in the Model Location region of the dialog to point to the required file. Click on the Model File tab to view the content of the model file.
The following additional model parameters are supported and can be entered into a linked model file (*.mdl) for the device:

Where a parameter has an indicated default, that default will be used if no value is specifically entered.
The format for the PSpice model file is:

.MODEL ModelName IND(Model Parameters),
where

• ModelName is the name of the model, the link to which is specified on the Model Kind tab of the Sim Model dialog. This name is used in the netlist (@MODEL) to reference the required model in the linked model file.
• Model Parameters are a list of supported parameters for the model, entered with values as required.

Potentiometer

Model Kind

General

Model Sub-Kind

Potentiometer

SPICE Prefix

R

SPICE Netlist Template Format

@"DESIGNATOR"A %1 %2 {@VALUE * @"SET POSITION"}
@"DESIGNATOR"B %2 %3 {@VALUE
- (@VALUE * @"SET POSITION")}

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Examples

Consider the potentiometer in the image above, with the following characteristics:

• Pin1 (Top) is connected to net OUT
• Pin2 (Bot) is connected to net IN
• Pin3 (Tap or wiper) is connected to net IN
• Designator is RIn
• Value = 1K
• Set Position = 0.5.
  The entry in the SPICE netlist would be:
  *Schematic Netlist:
  RInA OUT IN {1K * 0.5}
  RInB IN IN {1K - (1K * 0.5)}

Resistor

Model Kind

General

Model Sub-Kind

Resistor

SPICE Prefix

R

SPICE Netlist Template Format

@DESIGNATOR %1 %2 @VALUE

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Examples

Consider the resistor in the above image, with the following characteristics:

• Pin1 (Top) is connected to net Output
• Pin2 (Bot) is connected to net GND
• Designator is RLoad
• Value = 25k.
  The entry in the SPICE netlist would be:
  *Schematic Netlist:
  RLoad OUTPUT 0 25k - the ground net is always defined as 0 in the netlist.

Resistor (Semiconductor)

Model Kind

General

Model Sub-Kind

Resistor(Semiconductor)

SPICE Prefix

R

SPICE Netlist Template Format

@DESIGNATOR %1 %2 &VALUE &MODEL ?LENGTH|L=@LENGTH| ?WIDTH|W=@WIDTH| ?TEMPERATURE|TEMP=@TEMPERATURE|

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Parameters (definable within model file)

The following is a list of process-related parameters that can be stored in the associated model file:

Notes

You can specify either a direct value for the resistance OR enter values for the resistors' length and width. In the case of the latter, a value for the resistance will be calculated, in conjunction with parameter information stored in the model.
The equation used to calculate the resistance from geometric data is:
R = RSH * ((L
- NARROW) / (W
- NARROW))
If a direct value for resistance is not specified, the model name and length must be supplied in order for the geometric-based resistance value to be calculated. If either the length or sheet resistance (RSH) is not specified, the default resistance value of 1K will be used and a warning will be generated.
The link to the required model file (*.mdl) is specified on the Model Kind tab of the Sim Model dialog. The Model Name is used in the netlist to reference this file.
Entering a direct value for the resistance will override the geometric definition.
Where a parameter has an indicated default (as part of the SPICE model definition), that default will be used if no value is specifically entered. The default should be applicable to most simulations. Generally you do not need to change this value.

Examples

Consider the semiconductor resistor in the above image, with the following characteristics:

• Pin1 is connected to net Input
• Pin2 is connected to net Inv
• Designator is RIn
• The linked simulation model file is RES.mdl.
  If a value for the resistance was entered directly, say 10K, and no other parameters were specified on the Parameters tab of the Sim Model dialog, then the entry in the SPICE netlist would be:
  *Schematic Netlist:
  RIn Input Inv RES 10K
  Consider now, instead of entering a direct value for the resistance, the following parameters were defined in the Sim Model dialog:
• Length = 10e-3
• Width = 4e-3
• Temperature = 24.
  The entry in the netlist would be:
  *Schematic Netlist:
  RIn INPUT INV RES L=10e-3 W=4e-3 TEMP=24
  As long as a value for the sheet resistance (RSH) has been defined in the model file (RES.mdl), the value for the resistance will be calculated accurately from the geometric data given.

PSpice Support

The existing Spice3f5 model for the Resistor (Semiconductor) device has been enhanced to support the general PSpice model form:
R<name> <(+) node> <(-) node> [model name] <value> [TC = <TC1> [,<TC2>]]
A PSpice model of this type should be linked to a schematic component using a model file. Simply specify the model in a model file (*.mdl) then, in the Sim Model dialog, set the Model Kind to General and the Model Sub-Kind to Generic Editor. The Netlist Template Format should then be entered as follows:
@DESIGNATOR %1 %2 &MODEL &VALUE ?TC1/TC=@TC1?TC2|, @TC2| /

Although you could use the Spice3f5 Resistor (Semiconductor) model - as this model type allows use of a linked model file - specification of the netlist format for a PSpice Resistor model using the Generic Editor allows you to make use of the additional PSpice parameters ([TC = <TC1> [,<TC2>]]).
For the circuit to be parsed correctly, ensure that the Spice Prefix field is set to R.
In the Model Name field, enter the name specified for the model in the model file. Use the options in the Model Location region of the dialog to point to the required file. Click on the Model File tab to view the content of the model file.

The following additional model parameters are supported and can be entered into a linked model file (*.mdl) for the device:

Values for TC1 and TC2 can be entered on the Parameters tab of the Sim Model dialog. Where a parameter has an indicated default, that default will be used if no value is specifically entered - either on the Parameters tab or in the linked model file.

The format for the PSpice model file is:
.MODEL ModelName RES(Model Parameters),
where

• ModelName is the name of the model, the link to which is specified on the Model Kind tab of the Sim Model dialog. This name is used in the netlist (&MODEL) to reference the required model in the linked model file.
• Model Parameters are a list of supported parameters for the model, entered with values as required.

Resistor (Variable)

Model Kind

General

Model Sub-Kind

Resistor(Variable)

SPICE Prefix

R

SPICE Netlist Template Format

@DESIGNATOR %1 %2 {@VALUE * @"SET POSITION"}

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Examples

Consider the variable resistor in the image above, with the following characteristics:

• Pin1 is connected to net Input
• Pin2 is connected to net Inv
• Designator is R1
• Value = 1K
• Set Position = 0.5.
  The entry in the SPICE netlist would be:
  *Schematic Netlist:
  R1 INPUT INV 5E+2

Transistors

Bipolar Junction Transistor (BJT)

Model Kind

Transistor

Model Sub-Kind

BJT

SPICE Prefix

Q

SPICE Netlist Template Format

@DESIGNATOR %1 %2 %3 @MODEL &"AREA FACTOR" &"STARTING CONDITION" ?"INITIAL B-E VOLTAGE"|IC=@"INITIAL B-E VOLTAGE", @"INITIAL C-E VOLTAGE"| ?TEMPERATURE|TEMP=@TEMPERATURE|

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Parameters (definable within model file)

The following is a list of parameters that can be stored in the associated model file:

Notes

The model for the BJT is an adaptation of the integral charge control model of Gummel and Poon. This enhanced version of the original Gummel-Poon model includes several effects at high bias levels. When certain parameters are not specified, the model automatically defaults to that of the simpler Ebers-Moll model.
Ground is used as the substrate node.
The values for Initial B-E Voltage and Initial C-E Voltage only apply if the Use Initial Conditions option is enabled on the Transient/Fourier Analysis Setup page of the Analyses Setup dialog.
The Area Factor affects the following model parameters:

• transport saturation current (IS)
• corner for forward beta high current roll-off (IKF)
• B-E leakage saturation current (ISE)
• corner for reverse beta high current roll-off (IKR)
• B-C leakage saturation current (ISC)
• zero bias base resistance (RB)
• current where base resistance falls halfway to its minimum value (IRB)
• minimum base resistance at high currents (RBM)
• emitter resistance (RE)
• collector resistance (RC)
• B-E zero-bias depletion capacitance (CJE)
• high-current parameter for effect on TF (ITF)
• B-C zero-bias depletion capacitance (CJC)
• zero-bias collector-substrate capacitance (CJS)
  If the Area Factor is omitted, a value of 1.0 is assumed.
  The link to the required model file (*.mdl) is specified on the Model Kind tab of the Sim Model dialog. The Model Name is used in the netlist to reference this file.
  Where a parameter has an indicated default (as part of the SPICE model definition), that default will be used if no value is specifically entered. The default should be applicable to most simulations. Generally you do not need to change this value.

Examples

Consider the BJT in the above image, with the following characteristics:

• Pin1 (collector) is connected to net C
• Pin2 (base) is connected to net GND
• Pin3 (emitter) is connected to net E
• Designator is Q1
• The linked simulation model file is 2N3904.mdl.
  If no values are entered for the parameters in the Sim Model dialog, the entries in the SPICE netlist would be:
  *Schematic Netlist:
  Q1 C 0 E 2N3904
  .
  .
  *Models and Subcircuit:
  .MODEL 2N3904 NPN(IS=1.4E-14 BF=300 VAF=100 IKF=0.025 ISE=3E-13 BR=7.5 RC=2.4
  + CJE=4.5E-12 TF=4E-10 CJC=3.5E-12 TR=2.1E-8 XTB=1.5 KF=9E-16 )
  and the SPICE engine would use the indicated parameter information defined in the model file, along with default parameter values inherent to the model for those parameters not specified in the file.
  If the following parameter values were specified on the Parameters tab of the Sim Model dialog:
• Area Factor = 3
• Starting Condition = OFF
• Temperature = 24
  then the entries in the SPICE netlist would be:
  *Schematic Netlist:
  Q1 C 0 E 2N3904 3 OFF  TEMP=24
  .
  .
  *Models and Subcircuit:
  .MODEL 2N3904 NPN(IS=1.4E-14 BF=300 VAF=100 IKF=0.025 ISE=3E-13 BR=7.5 RC=2.4
  + CJE=4.5E-12 TF=4E-10 CJC=3.5E-12 TR=2.1E-8 XTB=1.5 KF=9E-16 )
  In this case, the SPICE engine would use this information, in conjunction with the indicated parameters defined in the model file (and any defaults for parameters not specified).

PSpice Support

Many of the parameters that can be included in a linked model file for this type of device are common to both Spice3f5 and PSpice. Those that are supported can be found in the previous section - Parameters (definable within model file). The following PSpice-based parameters are not supported for this device type:

Junction Field-Effect Transistor (JFET)

Model Kind

Transistor

Model Sub-Kind

JFET

SPICE Prefix

J

SPICE Netlist Template Format

@DESIGNATOR %1 %2 %3 @MODEL &"AREA FACTOR" &"STARTING CONDITION" ?"INITIAL D-S VOLTAGE"|IC=@"INITIAL D-S VOLTAGE", @"INITIAL G-S VOLTAGE"| ?TEMPERATURE|TEMP=@TEMPERATURE|

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Parameters (definable within model file)

The following is a list of parameters that can be stored in the associated model file:

Notes

The model for the JFET is based on the FET model of Shichman and Hodges.
The values for the Initial D-S Voltage and Initial G-S Voltage only apply if the Use Initial Conditions option is enabled on the Transient/Fourier Analysis Setup page of the Analyses Setup dialog.
The Area Factor affects the following model parameters:

• transconductance parameter (BETA)
• drain ohmic resistance (RD)
• source ohmic resistance (RS)
• zero-bias G-S junction capacitance (CGS)
• zero-bias G-D junction capacitance (CGD)
• gate junction saturation current (IS).
  If the Area Factor is omitted, a value of 1.0 is assumed.
  The link to the required model file (*.mdl) is specified on the Model Kind tab of the Sim Model dialog. The Model Name is used in the netlist to reference this file.
  Where a parameter has an indicated default (as part of the SPICE model definition), that default will be used if no value is specifically entered. The default should be applicable to most simulations. Generally you do not need to change this value.

Examples

Consider the JFET in the above image, with the following characteristics:

• Pin1 (Drain) is connected to net D
• Pin2 (Gate) is connected to net G
• Pin3 (Source) is connected to net S
• Designator is J1
• The linked simulation model file is 2N4393.mdl.
  If no values are entered for the parameters in the Sim Model dialog, the entries in the SPICE netlist would be:
  *Schematic Netlist:
  J1 D G S 2N4393
  .
  .
  *Models and Subcircuit:
  .MODEL 2N4393 NJF(VTO=-1.422 BETA=0.009109 LAMBDA=0.006 RD=1 RS=1 CGS=4.06E-12
  + CGD=4.57E-12 IS=2.052E-13 KF=1.23E-16 )
  and the SPICE engine would use the indicated parameter information defined in the model file, along with default parameter values inherent to the model for those parameters not specified in the file.
  If the following parameter values were specified on the Parameters tab of the Sim Model dialog:
• Area Factor = 4
• Temperature = 29
  then the entries in the SPICE netlist would be:
  *Schematic Netlist:
  J1 D G S 2N4393 4  TEMP=29
  .
  .
  *Models and Subcircuit:
  .MODEL 2N4393 NJF(VTO=-1.422 BETA=0.009109 LAMBDA=0.006 RD=1 RS=1 CGS=4.06E-12
  + CGD=4.57E-12 IS=2.052E-13 KF=1.23E-16 )
  In this case, the SPICE engine would use this information, in conjunction with the indicated parameters defined in the model file (and any defaults for parameters not specified).

PSpice Support

To make this device model compatible with PSpice, the following additional model parameters are supported and can be entered into a linked model file (*.mdl) for the device:

Where a parameter has an indicated default, that default will be used if no value is specifically entered.

The format for the PSpice model file is:
.MODEL ModelName NJF(Model Parameters) - N-channel JFET
.MODEL ModelName PJF(Model Parameters) - P-channel JFET
where

• ModelName is the name of the model, the link to which is specified on the Model Kind tab of the Sim Model dialog. This name is used in the netlist (@MODEL) to reference the required model in the linked model file.

• Model Parameters are a list of supported parameters for the model, entered with values as required.

  For an example of using a PSpice-compatible diode model in a simulation, refer to the example project JFET.PrjPCB, which can be found in the \Examples\Circuit Simulation\PSpice Examples\Jfet folder of the installation.

Metal Semiconductor Field-Effect Transistor (MESFET)

Model Kind

Transistor

Model Sub-Kind

MESFET

SPICE Prefix

Z

SPICE Netlist Template Format

@DESIGNATOR %1 %2 %3 @MODEL &"AREA FACTOR" &"STARTING CONDITION" ?"INITIAL D-S VOLTAGE"|IC=@"INITIAL D-S VOLTAGE", @"INITIAL G-S VOLTAGE"|

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Parameters (definable within model file)

The following is a list of parameters that can be stored in the associated model file:

Notes

The model for the MESFET is based on the GaAs FET model of Statz et-al.
The values for the Initial D-S Voltage and Initial G-S Voltage only apply if the Use Initial Conditions option is enabled on the Transient/Fourier Analysis Setup page of the Analyses Setup dialog.
The Area Factor affects the following model parameters:

• transconductance parameter (BETA)
• doping tail extending parameter (B)
• saturation voltage parameter (ALPHA)
• drain ohmic resistance (RD)
• source ohmic resistance (RS)
• zero-bias G-S junction capacitance (CGS)
• zero-bias G-D junction capacitance (CGD).
  If the Area Factor is omitted, a value of 1.0 is assumed.
  The link to the required model file (*.mdl) is specified on the Model Kind tab of the Sim Model dialog. The Model Name is used in the netlist to reference this file.
  Where a parameter has an indicated default (as part of the SPICE model definition), that default will be used if no value is specifically entered. The default should be applicable to most simulations. Generally you do not need to change this value.

Examples

Consider the MESFET in the above image, with the following characteristics:

• Pin1 (Drain) is connected to net D
• Pin2 (Gate) is connected to net G
• Pin3 (Source) is connected to net S
• Designator is Q1
• The linked simulation model file is NMESFET.mdl.
  If no values are entered for the parameters in the Sim Model dialog, the entries in the SPICE netlist would be:
  *Schematic Netlist:
  ZQ1 D G S NMESFET
  .
  .
  *Models and Subcircuit:
  .MODEL NMESFET NMF(LEVEL=6, )
  In this case, there are no parameter values specified in both the Sim Model dialog and the model file. The SPICE engine would therefore use the parameter default values inherent to the model.
  

Metal Oxide Semiconductor Field-Effect Transistor (MOSFET)

Model Kind

Transistor

Model Sub-Kind

MOSFET

SPICE Prefix

M

SPICE Netlist Template Format

@DESIGNATOR %1 %2 %3 %3 @MODEL ?LENGTH|L=@LENGTH| ?WIDTH|W=@WIDTH| ?"DRAIN AREA"|AD=@"DRAIN AREA"| ?"SOURCE AREA"|AS=@"SOURCE AREA"| ?"DRAIN PERIMETER"|PD=@"DRAIN PERIMETER"| ?"SOURCE PERIMETER"|PS=@"SOURCE PERIMETER"| ?NRD|NRD=@NRD| ?NRS|NRS=@NRS| &"STARTING CONDITION" ?"INITIAL D-S VOLTAGE"|IC=@"INITIAL D-S VOLTAGE", @"INITIAL G-S VOLTAGE", @"INITIAL B-S VOLTAGE"| ?TEMPERATURE|TEMP=@TEMPERATURE|

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Parameters (definable within model file)

The following is a list of parameters that can be stored in the associated model file, when using the Shichman-Hodges, MOS2, MOS3 or MOS6 models:

The following is a list of parameters that can be stored in the associated model file, when using the BSIM or BSIM2 models:

The following is a list of parameters that can be stored in the associated model file, when using the BSIM3 model:

The following is a list of parameters that can be stored in the associated model file, when using the EKV model:

Notes

General
The Simulator supports the following MOSFET device models, which differ only in their formulation of the I-V characteristic:

• Shichman-Hodges (LEVEL=1)
• MOS2 (LEVEL=2)
• MOS3 (LEVEL=3)
• BSIM (LEVEL=4)
• BSIM2 (LEVEL=5)
• MOS6 (LEVEL=6)
• BSIM3 (LEVEL=7)
• EKV (LEVEL=8).
  The LEVEL parameter is used to specify which model to use. It is declared at the start of the parameter values list, entered in the associated model file. If no LEVEL parameter is declared, the default Schichman-Hodges model will be used.
  The Bulk (substrate) node is connected, by default, to the Source node.
  If any of the component-level Length, Width, Drain Area or Source Area parameters are not specified, default values will be used.
  The values for the component-level NRD and NRS parameters are used to multiply the sheet resistance (RSH), in order to obtain an accurate representation of the parasitic series drain and source resistance of each transistor.
  The values for the component-level parameters Initial D-S Voltage, Initial G-S Voltage and Initial B-S Voltage only apply if the Use Initial Conditions option is enabled on the Transient/Fourier Analysis Setup page of the Analyses Setup dialog.
  The component-level Temperature parameter applies to LEVEL 1,2,3,6 & 8 MOSFET models (not BSIM type models).
  The link to the required model file (*.mdl) is specified on the Model Kind tab of the Sim Model dialog. The Model Name is used in the netlist to reference this file.
  Where a parameter has an indicated default (as part of the SPICE model definition), that default will be used if no value is specifically entered. The default should be applicable to most simulations. Generally you do not need to change this value.
  BSIM/BSIM2-Related
  The BSIM and BSIM2 models are designed to be used with a process characterization system. This system is responsible for providing all parameter information (values) automatically through the use of a process file and therefore no default parameter values are specified. As a consequence, all parameters are required to be specified and the absence of any will result in an error.
  If the XPART parameter is set to 0, a 40/60 drain/source charge partition in saturation is selected. If this parameter is set to 1, a 0/100 drain/source charge partition is selected.
  Certain model parameters (those marked with an asterisk in the BSIM/BSIM2 list of parameters) also have corresponding parameters dependent on length and width. For more information on these and other aspects of the MOSFET models, consult the SPICE reference manual.
  BSIM3-Related
  The following charge partition schemes are supported, selectable based on the value entered for the XPART parameter:
• XPART = 0 - a 0/100 drain/source charge partition os selected
• XPART = 0.5 - a 50/50 drain/source charge partition os selected
• XPART = 1 - a 40/60 drain/source charge partition os selected.
  If no value is specified for one of the following parameters, it will be calculated:
• VTH0
• K1
• K2
• CGSO
• CGDO
• CF
• GAMMA1
• GAMMA2
• NCH
• VBX
  For details of the calculations involved, refer to the BSIM3v3 User Manual.
  The following BSIM3 model parameters are not supported in Altium Designer:

EKV-Related
The EKV MOSFET model was developed by the Electronics Laboratory (LEG) of the Swiss Federal Institute of Technology (EPFL). The model used in Altium Designer is version 2.6.
The following EKV model parameters are not supported in Altium Designer:

For more detailed information on model equations associated with the EKV MOSFET, refer to the document "The EPFL-EKV MOSFET Model Equations for Simulation", available from the following website
- http://legwww.epfl.ch/ekv/model.html.

Examples

Consider the MOSFET in the above image, with the following characteristics:

• Pin1 (Drain) is connected to net D
• Pin2 (Gate) is connected to net G
• Pin3 (Source) is connected to net S
• The substrate node (Bulk) is connected to Pin3 (the Source node).
• Designator is Q1
• The linked simulation model file is NMOS3.mdl.
  If no values are entered for the parameters in the Sim Model dialog, the entries in the SPICE netlist would be:
  *Schematic Netlist:
  MQ1 D G S S NMOS3
  .
  .
  *Models and Subcircuit:
  .MODEL NMOS3 NMOS(LEVEL=3)
  In this case, there are no parameter values specified in the Sim Model dialog. In the model file, there is only the LEVEL parameter specified
  - corresponding to the use of the MOS3 model. The default values for all other parameters
  - inherent to the model
  - will be used.

PSpice Support

Of the existing MOSFET device models, the following are not supported with respect to PSpice compatibility:

• BSIM3 model version 2.0
  For the other supported MOSFET device models, many of the parameters that can be included in a linked model file are common to both Spice3f5 and PSpice. Those that are supported can be found in the previous section - Parameters (definable within model file). The following PSpice-based parameters are not supported for this device type.