Wireless Power Wiki

The relationship between the voltage $v_L$ over and the current $i_L$ through an inductor is determined by its inductance $L$:

$$ v_L(t)=L\frac{di_L(t)}{dt}$$

However, this current-voltage relationship is not valid when the inductor is varying in time. For a time variant inductor, the equation modifies to:

$$ v_L(t)=\frac{d}{dt}[L(t).i_L(t)]=L(t)\frac{di_L(t)}{dt}+i_L(t)\frac{dL(t)}{dt}$$

Rearranging this equation gives an expression for the current through the inductor:

$$ i_L(t)=\frac{1}{L(t)}[L(0)i_L(0)+\int_0^t v_L(t) dt] $$

valid if $L(t)\neq 0$ at any time.

We will use this expression to simulate a time-varying inductance in LT Spice. Notice the limitation that $L(t)\neq 0$ at any time.

Suppose we want we simulate a sinusoidal value in function of time with a certain offset: $L(t)$= 5 mH + 3 mH.sin(2π.100 kHz.t). In order to realize this, we have to introduce a custom component in SPICE with the following subcircuit:

.subckt inductor + - params: IL0=0
.func L(time) {5m+3m*sin(2*pi*100k*time)}
gcurr + - value={(sdt(V(+,-))+IL0*L(0))/L(time)}
.ends

The current through the inductor (see equation above) is modeled via a G-type current source gcurr. The integral is realized via the sdt function in SPICE. The initial value at time t=0 of the inductor must be given as parameter.

First, we save the code for this subcircuit into a .txt-file and, for example, place this file in the same folder as your SPICE circuit file.

Next, open the text file in LT Spice, right click on the first word “.subckt”, and select “Create symbol”.

The program asks you if you wish to automatically create a symbol. Click “yes”. A .asy file is created which contains your custom time-varying inductor, typically in the folder 'C:Users\YourUserName\AppData\Local\LTspice\lib\sym\AutoGenerated'

Let us test the time-varying inductor.

First, click “component” (F2) and insert the custom inductor by searching “inductor” in the window.

References

• Biolek, D., Kolka, Z., & Biolkova, V. (2007). Modeling time-varying storage components in PSpice. In Proc. Electronic Devices and Systems IMAPS CS International Conference EDS (Vol. 2007, pp. 39-44).