Coupled Inductors Model

Old Content - visit altium.com/documentation

Modified by Phil Loughhead on Mar 4, 2014

Model Kind

General

Model Sub-Kind

Coupled Inductors

SPICE Prefix

SPICE Netlist Template Format

LA_@DESIGNATOR %1 %2 @"INDUCTANCE A" LB_@DESIGNATOR %3 %4 @"INDUCTANCE B" @DESIGNATOR LA_@DESIGNATOR LB_@DESIGNATOR @"COUPLING FACTOR"

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.

Inductance A	value for the inductance of discrete inductor A (in Henrys).
Inductance B	value for the inductance of discrete inductor B (in Henrys).
Coupling Factor	the coupling coefficient, representing the flux linkage between the windings of the two individual inductors. Permissible values lie in the range 0<CF≤1, where 1 (the ideal) means all flux linking inductor A also links inductor B.

Examples

Consider the transformer in the image above, 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:

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 image above, 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