# The Arbitrary Inductor model

LTspice allows specifying a behavioral inductance with an expression for the flux. The inductor's current *may* be referred to by the keyword "x" in the expression, but otherwise is completely arbitrary (i.e., may be any valid function of time and/or node voltages and/or branch currents within the simulation).

Below is a netlist example of an inductor with simple saturation.

L1 1 0 flux=0.33*2*tanh(x/2) ; 330mH inductor "saturates" at 2A (0.66 volt-seconds) I1 0 1 PWL(0 0 1 1) ; supplies unity di/dt so inductance corresponds to voltage .tran 0 5 1u 10m ; 5s transient run starting after 1us with 10ms maximum step size .end

LTspice's behavioral inductor may be parametrized, but the parser requires that all parameters or strictly parametric expressions must be enclosed within **curly braces**. Strictly parametric expressions may not include "x" (inductor current) or other dynamic variables. Below is a flux expression example of this technique.

flux={L*Is}*tanh(x/{Is}) ; L= inductance and Is= "saturation" current

Here further extended to add exponential control of saturation "sharpness".

flux={L*Is}*tanh((x/{Is})**{a})**{1/a} ; a= saturation "sharpness" exponent (1=normal, >1=sharper)

Note that the parameters for the above expressions must be defined elsewhere upon the schematic, usually as a parameter statement within a SPICE directive (SPICE text placed anywhere within the schematic).

.param L=330mH Is=2A a=3 ; fairly sharp saturation at 2A (the "a" saturation factor is exponential)

Unlike the standard inductor, which defaults to a series resistance of 1mOhm, the arbitrary inductor has no series resistance unless explicitly specified (ctrl-right mouse button click on the inductor). Also note that the numerical dynamic range of the arbitrary inductor seems to be about only 15 decades or so.