Linking a Simulation Model to a Schematic Component

Legacy Material See the Latest Version

Altium Designer provides a powerful mixed-signal circuit simulator, enabling you to thoroughly analyze a circuit - not only observing its behavior, but also ensuring that it operates within specific design constraints. To simulate a design successfully, all components in the circuit must be simulation-ready, that is, they must each have a linked simulation model defined for them.

Altium Designer comes with a host of components stored within manufacturer-specific integrated libraries. Many of these components have linked simulation models, making creation of a simulation-ready circuit quick and efficient - a case of Place 'n Simulate if you will.

With such a vast pool of components available to designers in the real world, there will often be times where the component(s) required for use in a circuit will need to be created in libraries added by the user. As well as defining the component's symbol, a simulation model for that component needs to be acquired and then linked, in order to make that component simulation-ready.

Acquiring the Model

A simulation model can be obtained from many and varied sources. The following is a non-exhaustive list of possible places or methods to get the model you require for a target device you wish to use in your design:

  • Manufacturer - a popular place to look for a model is on the website for the manufacturer that makes the device you want to use. Typically, there will be a link to any available model from the page dealing with the specific device. Models are commonly supplied in SPICE or PSpice ® format.
  • Altium Designer's SPICE Model Wizard - use this wizard to create and automatically link a SPICE3f5 device model to an existing or new library component. If linking to a new component, that component will be created automatically by the wizard. The following device model types are supported: Semiconductor Capacitor, Semiconductor Resistor, Current-Controlled Switch, Voltage-Controlled Switch, JFET, Lossy Transmission Line, Uniform Distributed RC Transmission Line, Diode and BJT.
  • Third-Party Modeling Tools - various simulation software packages contain features for modeling a device. This typically takes the form of a model wizard.
  • Dedicated Modeling Companies - you may be able to source the required model from a third-party company which creates simulation models based on a given specification.
  • By Hand - the required model can be created yourself, from scratch. This will typically require good knowledge of the language in which the model definition is being written, for example when creating a subcircuit, or a digital device definition using Digital SimCode™. When creating a simple MDL file for a built-in SPICE3f5 or supported PSpice model, you will need good knowledge of the parameters available for, and supported by, that device.

Readying the Model for the Altium Designer Arena

Once you have the required simulation model, you need to ensure that it is in a form compatible with Altium Designer. To begin with, it must be in one of the supported model formats:

  • SPICE3f5
  • XSpice
  • PSpice

For a simple model, the definition must be saved with an mdl extension (e.g. MyBJT.mdl). For a more complex SPICE subcircuit, the definition must be saved with a ckt extension (e.g. MyOpAmp.ckt).

With Altium Designer's support for PSpice models, very little will need to be done to the majority of models acquired in PSpice format, other than to paste the required model into a file with the MDL extension.

Model Conversion

There are many variants of SPICE out in the design world today - SPICE3f5, PSpice ® , HSPICE ® , NSPICE ® and Eldo ® to name but a few. Discussion of these various formats and the models they support is beyond the scope of this document.

The majority of manufacturers will provide pure SPICE (SPICE3f5) or PSpice formats. If your model is in a format other than those supported by Altium Designer, or it is a PSpice model type that is currently not supported, you will need to convert it into the required format. This is a manual process, requiring the user manuals for both source (e.g. PSpice) and target (e.g. SPICE3f5) SPICE formats and, preferably, a detailed knowledge of the two. Compare the syntaxes of the two formats and convert to something compatible.

Some commercial versions (or variants) of SPICE have proprietary extensions that limit the portability of model descriptions between different vendor SPICE formats.
If a PSpice model type is supported but a particular parameter is not, that parameter, in many cases, can be ignored with only minor impact on the simulation results. However, the true impact on the results will depend on which parameter it is and the nature of the circuit/simulation.

Linking the Model to a Schematic Component

Once you have the required simulation model file, you will need to link it to the schematic component that you wish to place and use in your design.

To illustrate by example the steps that need to be taken to link a model to a schematic component, we shall use a simple (and fictitious) diode model - JAS33 - obtained from a manufacturer and pasted into the file JAS33.mdl.

Creating the Schematic Component

The first step (typically) when creating a new simulation-ready device is to create a schematic library component for that device and define the symbol graphics. This is done using Altium Designer's Schematic Library Editor.

The image below shows the symbol graphics for our simple diode component DIODE JAS33.

Defining the component in the Schematic Library Editor.

Often, you'll find it easier to copy an existing component and then modify it as required, rather than create the component and related graphics from scratch.

Adding the Link

Whether you have created a new schematic component, or are using an existing one, it is now time to create a link to the simulation model file. The first step in this process is to add a simulation model link to the component, carried out in the Schematic Library Editor in one of the following ways:

  • In the Models region of the Editor's main design window, click on the drop-down arrow associated with the lower-left button and choose Simulation from the list of available model types.

Adding models from the main editing window.

  • In the Models region of the SCH Library panel, click on the associated Add button and choose Simulation as the model type in the Add New Model dialog that appears.

Adding models from the SCH Library panel.

  • Use the Model Manager dialog ( Tools » Model Manager ). Simply select the entry for the component, click on the drop-down arrow associated with the Add button, and choose Simulation from the list of available model types.

Adding models using the Model Manager.

Configuring the Link

Whichever method you use to add a simulation model link to a component, you will be taken to the Sim Model dialog (shown below) - command central for configuring the link to the required simulation model.

Configuring the model link in the Sim Model dialog.

Specifying Model Type

The Model Kind and Model Sub-Kind fields need to be set according to the particular model type you are linking. The Model Kind drop-down gives access to a number of model categories containing the range of analog device models built-in to SPICE. The Model Sub-Kind region lists all model types in a chosen category.

Linking to a SPICE 3f5 Model

Many of the built-in SPICE models require no model file. Definition is made by setting the required values for model parameters at the component-level. The following is a list of the device models that support the use of an associated model file, which can contain a variety of parameters used to model advanced characteristics of the device. (Entries in the list are in the format Model Kind \ Model Sub-Kind ).

  • Current Source\Piecewise Linear
  • General\Capacitor(Semiconductor)
  • General\Diode
  • General\Resistor(Semiconductor)
  • Switch\Current-Controlled
  • Switch\Voltage-Controlled
  • Transistor\BJT
  • Transistor\JFET
  • Transistor\MESFET
  • Transistor\MOSFET
  • Transmission Line\Lossy
  • Transmission Line\Uniform Distributed RC
  • Voltage Source\Piecewise Linear.

If you are linking a SPICE 3f5 model for any of these inherent SPICE devices, simply select the Model Kind and Sub-Kind, as per the above list. The required Spice Prefix field will be set automatically.
Considering our JAS33 example diode model, the entries in the dialog at this point would be:
Model Kind : General
Model Sub-Kind : Diode
Spice Prefix : D.

The Netlist Template

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.

Example netlist template entry for a coupled inductor model.

It is read-only for the predefined SPICE3f5 model types. 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.

Linking to an XSpice Code Model

When linking an XSpice code model to the component, use of a model file is not applicable. The model itself is defined using the Netlist Template tab of the Sim Model dialog, with the parameters specified in the template declared and defined on the Parameters tab of the dialog.

Ensure that the Model Kind is set to General and that the Model Sub-Kind is set to Generic Editor. The Spice Prefix for this type of model must be set to A.

Parameter declarations for an XSpice model.

Linking to a Subcircuit Model

If the model you wish to link has been described using the hierarchical sub-circuit syntax (for an operational amplifier or crystal oscillator for example), the model definition will have been saved to file with a ckt extension.

Ensure that the Mode l Kind field is set to General and that the Model Sub-Kind is set to Spice Subcircuit. The required Spice Prefix field will be set automatically to X. The image below shows an example simulation link to a crystal subcircuit.

Example of a linked SPICE subcircuit model.

For greater control over the netlist template, you can set the Model Sub-Kind to Generic Editor.

Linking to a PSpice Model

Example of a linked PSpice Inductor model.

Altium Designer offers strong support for PSpice models. The following is a list of the PSpice device models supported:

  • Capacitor
  • Resistor
  • Diode
  • Inductor
  • Current-Controlled Switch
  • Voltage-Controlled Switch
  • Voltage-Controlled Voltage Source
  • Voltage-Controlled Current Source
  • Current-Controlled Voltage Source
  • Current-Controlled Current Source
  • Bipolar Junction Transistor (BJT)
  • Junction Field Effect Transistor (JFET)
  • Metal Oxide Semiconductor Field Effect Transistor (MOSFET)

With the exception of Resistor, Inductor and the voltage and current sources, simply select the Model Kind and Sub-Kind, as per the list for SPICE3f5 models (see Linking to a SPICE3f5 Model). The required Spice Prefix field will be set automatically. For the exceptions, you will need to set the Model Kind to General, the Model Sub-Kind to Generic Editor and enter the applicable netlist template format. You will also need to set the Spice Prefix accordingly.

Linking to a Digital SimCode Model

Digital device models are 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.

For a digital device, the schematic component is linked to the SimCode model by using an intermediate model file (*.mdl) - effectively calling the SimCode description from within its .MODEL line.

In the Sim Model dialog, ensure that the Model Kind is set to General, the Model Sub-Kind is set to Generic Editor and the Spice Prefix is set to A. You will need to enter the netlist template specific to the digital device being modeled, on the Netlist Template tab of the dialog.

Example of a linked Digital SimCode model.

Specifying Model Name

Use the Model Name field in the Sim Model dialog to specify the name of the model to which you are linking. This must be the name, as it appears in the model file.

For an MDL file, the name must be that appearing in the .MODEL line of the model's definition. Consider a model for a diode with the following definition:

.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 )

The model name here is 1N4002. This is the name that must be entered into the Model Name field.
For a CKT file, the name must be that appearing in the .SUBCKT line of the model's definition. Consider a model for a fuse with the following definition:

.SUBCKT FUSE 1 2 PARAMS: CURRENT=1 RESISTANCE=1m SW1 1 2 3 0 SMOD OFF BNLV 3 0 V=(abs(v(1,2))) .MODEL SMOD SW (VT=\{(CURRENT*RESISTANCE)\} RON=1g ROFF=\{RESISTANCE\}) .ENDS FUSE

The model name here is FUSE. This is the name that must be entered into the Model Name field.

Use the optional Description field to enter a brief description of the model - for example its purpose - should you wish.

Specifying Model Location

Use the Model Location region of the Sim Model dialog to control where the model is searched for:

  • Any - searches all valid model locations for a matching model.
  • In File - only searches for a matching model in the specified file (*.mdl, *.ckt), along all valid model locations.
  • Full Path - only searches for a matching model in the specified file (*.mdl, *.ckt) along the specified path.
  • In Integrated Library - draws the model directly from the integrated library used to place the component instance. The integrated library must be available in a valid location.

Valid model locations consist of:

  • Project Models - .mdl or .ckt files added to the project
  • Installed Models - .mdl or .ckt files added to the Installed Libraries list
  • Project Search Paths - .mdl or .ckt files made available to a project by defining one or more search paths in the Options for Project dialog.

Once successfully linked, an entry for where the corresponding model file (*.mdl, *.ckt) has been found will be displayed. The image below shows the Model Kind tab of the Sim Model dialog with the Model Location information for our JAS33 example.

Model location information for the JAS33 diode example.

Notice in the image above that the model has been located by using the Full Path option.

When the search is across all valid model locations, the order of the search is Project Models - Installed Models - Project Search Paths. The search ceases as soon as a match is found - i.e. the Model Name entry in the .MODEL line of a .mdl file (or the .SUBCKT line of a .ckt file) matches the Model Name entry in the Sim Model dialog for that component. Typically the model file is named the same as the model itself, e.g. the .MODEL line contains 74LS74 and the .mdl file has been saved with the name 74LS74.mdl.

This is not a constraint however. For example, the .MODEL line could contain the model name 74LS74 and then the .mdl file saved with the name DFlipFlop.mdl. This file would be yielded as a match, provided that the Model Name entry in the Sim Model dialog is 74LS74.

Mapping the Ports

Once the simulation model file has been linked to the schematic component, you need to ensure that the pins of the schematic component are correctly mapped to the pins of the model. This is carried out on the Port Map tab of the Sim Model dialog.

Ensuring correct component pin-to-model port mapping.

For the built-in SPICE3f5 and supported PSpice models, the function of each of the pins in a model can be found in the general form section for that model, in the SPICE 3f5 user manual.

For subcircuit models, the manufacturer will typically insert comments for each pin of the model, describing that pin's function. If no commenting is evident, then the pinout of the model will typically be that of the physical device itself. Consult the datasheet for the device in this case.

For Digital SimCode models, the mapping of the component pins to the INPUTS and OUTPUTS declared in the SimCode file will depend on the input and output node list entries in the netlist template.

For each schematic pin, simply use the available drop-down to change the associated Model Pin entry accordingly. If the device is multi-part, be sure to check the mapping for each part.

Defining Component-Level Parameters

For the built-in SPICE3f5, supported PSpice and subcircuit model kinds, the available parameters will automatically be listed. When linking models using the Generic Editor you will need to add applicable parameters manually.

For many model types it is possible to set one or more parameters at the component level. This is carried out on the Parameters tab of the Sim Model dialog.

For some of the built-in SPICE3f5 models, entering a value for a parameter at the component level will override a related parameter defined in a linked model file (*.mdl). For a semiconductor capacitor, for example, specifying a value for the component-level Width parameter will override any value specified for the DEFW parameter in the associated model file.

If a parameter is specified at the component level for a subcircuit model, that value will override the value defined for it in the linked subciruit file (*.ckt).

Many component-level parameters will have a default value assigned to them which, although not displayed, will be used if no specific value is set.

If a parameter is specified at the component level for a digital device, that value will override the value specified for that parameter in the source SimCode definition.

The image below shows the parameters available for our JAS33 diode device model. If you require any parameter values to be displayed on the schematic sheet, simply enable the corresponding Component Parameter option.

Component-level parameters for the JAS33 diode example.

 

Linking from an External Database

Component placement (with sim link) direct from a database library.

Altium Designer provides the ability to place components directly from a company database by creating and using a Database Library (*.DBLib). Placement is carried out from the Libraries panel which, after installing the database library, acts as a browser into your database (shown above).

With this method of linking the component symbol, model and parameter information for a component is stored as part of the record definition for that component in the external database. The referenced schematic component (in an underlying component library (*.SchLib)) is simply an empty shell, with a defined symbol only. There are no linked models and no defined design parameters. When the component is placed, its parameter and model information is created on-the-fly, using the corresponding fields in the matched database record and in accordance with defined mapping.

As part of the Database Library feature, you can add simulation model information to a component record in the external database. When the component is placed on the schematic, this information will be used to create the link to the referenced simulation model - filling-in the required (and corresponding) areas of the Sim Model dialog.

Adding Sim Information to an External Database Table

The following sections discuss each of the database fields that can be added to an external database table in order to define the simulation model link, which will be created upon component placement. If the field names are named exactly as indicated, the Database Field-to-Design Parameter mapping will be automatically set on the Field Mappings tab of the DBLib file. You can, of course, use your own field names in the database table, but you will then need to manually map these fields to the correct design parameters.

Note that simulation information must be entered manually into the external database. Using the Integrated Library to Database Library Translator Wizard will not extract the required simulation information and store it into the target database.

We shall use our trusty JAS33 diode model to illustrate the linking.

Only one simulation model link can be defined in an external database. Typically there will only ever be a single model linked to the component. Should you wish to set up multiple simulation model links, the other links will need to be defined and stored with the component in the source schematic library file.

Sim Model Name

Create this field in the database to specify the name of the model that you wish to use. After the component is placed, this information will appear in the Model Name field, on the Model Kind tab of the Sim Model dialog.

In the database record for our example diode, we would enter JAS33 into this field.

When mapping database fields to design parameters in the DBLib file, the Sim Model Name field is analogous to the Footprint Ref, Library Ref , etc, fields.

Sim Description

Create this field in the database if you wish to provide a description for the linked model. This information is optional and does not affect the operation of the simulation model link. After the component is placed, this information will appear in the Description field, on the Model Kind tab of the Sim Model dialog.

In the database record for our example diode, we could enter DIODE.

Sim File

Create this field in the database if you wish to specify a particular model file in which to find the simulation model specified in the Sim Model Name field. There are a number of ways in which this field can be used:

  • You can enter an absolute path to a model file (e.g. C:\DBLibs\Switching Diodes\Libraries\JAS33.mdl). The model specified in the Sim Model Name field will be searched for within this file and used if found.
  • You can enter a relative path (relative to the DBLib file) to a model file (e.g. Libraries\JAS33.mdl). The model specified in the Sim Model Name field will be searched for within this file and used if found.
  • You can enter the model filename only (e.g. JAS33.mdl). Search paths defined as part of the DBLib file will be used to locate the first model file that matches the specified name, and which contains a match for the model specified in the Sim Model Name field.
  • You can leave the field blank. Search paths defined as part of the DBLib file will be used to locate the first model file containing a match for the model specified in the Sim Model Name field.

Providing model location information.

Search paths are defined for the DBLib file from the Symbol & Model Search Paths tab of the Database Library Options dialog ( Tools » Options ).

Sim Kind

Create this field in the database to specify the parent category for the model being linked to. This information corresponds to the Model Kind field, on the Model Kind tab of the Sim Model dialog. The text entered must be as it appears in the Model Kind field.

For our example diode, we would enter General.

Sim SubKind

Create this field in the database to specify the type of model being linked to. This information corresponds to the Model Sub-Kind field, on the Model Kind tab of the Sim Model dialog. The text entered must be as it appears in the Model Sub-Kind field.
For our example diode, we would enter Diode.

Sim Netlist

Create this field in the database to enter the netlist template information, in accordance with the type of model being linked to.

For all of the predefined model kinds and sub-kinds, this information can be sourced from the Netlist Template tab of the Sim Model dialog. For example, for a standard Resistor model (Sim Kind = General, Sim SubKind = Resistor), the entry in this field will be: @DESIGNATOR %1 %2 @VALUE

This field becomes especially important if you are specifying your own netlist template and have set the Sim SubKind field to Generic Editor, giving you more control over what information is placed in the netlist.

After the component is placed, this information will appear on the Netlist Template tab of the Sim Model dialog.

This field must be defined and not left blank, otherwise no entry for the model will be made in the simulation netlist, and the part will not simulate when placed from the database library.

Example netlist specification for a linked digital device model (74LS74).

Sim Spice Prefix

Create this field in the database to specify the SPICE prefix for the model type you are linking to. This information corresponds to the Spice Prefix field, on the Model Kind tab of the Sim Model dialog. For our example diode, we would enter D.

Sim Port Map

Create this field in the database to specify the mapping of pins from the schematic component to the pins of the linked model. After the component is placed, this information will appear on the Port Map tab of the Sim Model dialog.

Specifying component-to-model pin mapping.

Each pin pairing must be entered in the following format:
(SchematicPinNumber:ModelPinNumber),
with each mapped pairing separated by a comma.
For our diode example, schematic pin 1(anode) must be mapped to model pin 1(anode), and schematic pin 3 (cathode) must be mapped to model pin 2 (cathode). This would be entered into the database field as:
(1:1),(3:2)

Sim Excluded Parts

Create this field in the database if you wish to exclude certain parts of a multi-part component from being simulated. This information corresponds to the Exclude part from simulation option on the Port Map tab of the Sim Model dialog.

By default, all parts of a multi-part component are included in a simulation, so you only need to specify the parts you wish to exclude, by number. Separate multiple parts in the exclusion list using commas. For example if a component has four parts and you do not want parts 2 and 4 to be included in any simulation, then you would enter the following into the database field:
2,4

Sim Parameters

Create this field in the database if you wish to assign values to simulation parameters for the model. These are parameters that can be defined at the component-level, as opposed to the more advanced parameters that can be included in a model file.

A parameter must be entered in the following format:

ParameterName=Value,

Multiple parameters must be separated by the pipe character (|).

You may remember that a component-level simulation parameter can also be set as a component parameter - appearing in the Parameters region of the associated Component Properties dialog, with the ability to then be displayed on the schematic sheet. By default, a parameter entry in the Sim Parameters field will be automatically added as a component parameter. If you do not want a simulation parameter to be added as a component parameter, simply add an exclamation mark prefix to the parameter name (e.g. !Initial Voltage=100mV).

Consider our diode model, which has the following four component-level parameters:

Specifying values for associated model parameters (component-level).

  • Area Factor
  • Starting Condition
  • Initial Voltage
  • Temperature.

Now consider adding values in the database for the Area Factor (say 2) and Temperature (say 22°C). Also, both of these should not be added as component parameters. The entry in the Sim Parameters field would be:

!Area Factor=2|!Temperature=22

Checking the Link

Once you have placed the component from the Database Library, it is not a bad idea to check the simulation link, and to verify that the information defined for the link is indeed as required. Simply double-click on the placed component to access its associated Component Properties dialog. In the Models region of the dialog, simply double-click on the simulation model entry to access the Sim Model dialog, from where you can check that:

  • Any linked model file has been located as expected. When found, the Model File tab of the dialog will display the content of the file.
  • The remaining simulation information from the database has been added to the dialog as expected.

The image below illustrates the information added to the Sim Model dialog for the JAS33 diode example, upon placement of the component on the schematic sheet.

Sim Model dialog entries for the JAS33 diode example.

Maintaining the Link

After placement, the chosen key parameter in the DBLib file is used to ensure that the placed component on the schematic retains its link to the corresponding record for that component in the external database. This means that at any stage in the future, changes to parameter and model information in the database can be easily passed back to the placed component, synchronizing the two.

Whereas component design parameters can be updated using either the Update Parameters From Database or Update From Libraries commands - both available from the Schematic Editor's main Tools menu - update of simulation link information must be carried out using the latter.

The update process considers the information for the link only - i.e. the fields stored in the external database. When the model link involves an associated model file (*.mdl, *.ckt), any changes (e.g. .MODEL or .SUBCKT definitions, parameter values, expressions, etc) required must be made within the file. These changes will be 'seen' by a placed component directly, and can be checked from the Model File tab of the Sim Model dialog.

Although simulation parameters can be added as component parameters, they are not recognized as design parameters for the purpose of updating.

Request Free Trial

Complete this form to request a free 15 day trial of Altium Designer: