Inductor Model

Old Content - visit altium.com/documentation

Modified by Admin on Sep 13, 2017

Model Kind

General

Model Sub-Kind

Inductor

SPICE Prefix

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.

Value	value for the inductance (in Henrys).
Initial Current	time-zero current flowing through inductor (in Amps).

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 image above, 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:

L	inductance multiplier. (Default = 1).
IL1	linear current coefficient (in Amp-1). (Default = 0).
IL2	quadratic current coefficient (in Amp-2). (Default = 0).
TC1	linear temperature coefficient (in ˚C-1). (Default = 0).
TC2	quadratic temperature coefficient (in ˚C-2). (Default = 0).

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.

The following parameters - common to most devices in PSpice - are not supported:
T_ABS
T_MEASURED
T_REL_GLOBAL
T_REL_LOCAL.

For an example of using a PSpice-compatible inductor model in a simulation, refer to the example project Inductor.PrjPCB.