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

QSPICE
1

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?

Thanks,
Carl

2

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

3

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?

Thanks,
Carl

4

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

image
image945×333 17.6 KB

5

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!

6

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.

–Mike

7

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?

Thanks,
Carl

8

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.

Ndiode
Ndiode1316×729 57.8 KB

Alexander Bordodynov