LTspice diode model parallel capacitance

Question

Some datasheets define parasitic/parallel capacitance for a diode. MA4E2532 datasheet even list SPICE Cjpar parameter.

But the LTspice D model lacks this parameter. An inductor L model has Cpar parameter but diodes don't. Am I missing something? Is this parameter has a different name or is it inherently useless to define and model it? When I manually add parallel capacitor to a diode it drastically change the results on high frequency.

Answer 1

The capacitance of a diode is a function of the bias. The D model has zero-bias capacitance as a parameter. For example, the OnSemi 1N5819 model has Cjo of 110pF.

Edit:

Schottky junction capacitance is:

Cj = \$\frac{\text{Cjo}}{(1-\text {Vf}/ \text{Vj})^{M}}\$

For the 1N5819 mentioned above, Cjo = 110pF, M = 0.35 and Vj = 1.0 (default).

Modelling the capacitance as a fixed parallel capacitor would be very inaccurate.

For very high frequencies, this is an interesting paper showing modeling of the package parasitics as well.

Answer 2

It's not very clear in the datasheet (and the extra j typo doesn't help much), but they want you to model the Cpar as an additional fixed capacitor across the diode. My guess is that it's meant to represent the package parasitics. Since this is marketed as a very low capacitance diode, the package has significant effects beyond the Cjo of the metal-semiconductor junction. Anyway, you can either do this manually by explicitly putting an extra 0.09pF capacitor across each instance of the diode...or it might be better to just create the entire model as a subcircuit, like so:

.subckt MA4E2532L-1113 A K
D1 A K diode_base
C1 A K 0.09p
.model diode_base D(Is=26n Rs=12.8 N=1.2 Cjo=0.01p M=0.5 Ikf=14m Vj=80m FC=0.5 BV=5 IBV=10u)
.ends

If you use the subcircuit along with one of the standard LTspice diode symbols, don't forget to ctrl-rightclick and change the "Prefix" attribute from D to X, as shown below.