Diode attribute of n=10 is not 10 diodes in series (as in LTspice)

A diode second attribute of n=10 does not result in the electrical equivalent of 10 series diodes (as it does in LTspice)

Is this handy LTspice feature planned for QSPICE?


It’s not there now, but I’ll might add it at some point.

I have an LTspice solar panel model that is using the n= feature as part of the definition of the diode model in a subcircuit.
.model PVDiode2 D(Is=io_t N=a_n Tnom=temp)
.param a_n 1.3*voc/0.7

I’d like to use this in a QSPICE simulation. Do you know of alternate representations of the diode parameters that can mimic the n= scaling factor?


It should be possible to rewrite a .model to match one with N. Curve trace them side by side:

This looks like it is working. Is implementing the n= function as easy as this? How does it work? I don’t understand what we did!

In a diode model, N is the ideality factor. Ideal is 1. For there are more diodes in series, it’s less ideal. So one diode has N=1.4, then four diodes in series gives N=4*1.4.

The Is parameter stays the same.

Rs and Cjo would be Rs*N. Cjo would be Cjo/4. I think the diode parameter m would also change.


Did the LTspice implementation of the n= multiplier make adjustments for the other terms, or just mess with the voltage drop?

In your example, does the N=4 overwrite the diodes n (maybe was 1.4) or multiply the original n by 4?


Look at the temperature dependence of the voltage drop across the diode. This is the error I have seen in high-voltage diode models. I had to correct the EG value in them.

Alexander Bordodynov