I am porting a model from LT-Spice into Kicad. It works well when I take small steps and make sure each small change runs as intended. I now have a working model but my losses are too large and I can see this is related to my rectification diodes.
In the LT-Spice model I have an ideal diode as: .model Didl D(Ron=0.002 Roff=100G Vfwd=0) to have a simple and rough representation of a rectifier.
I could set up the ngspice model the same way and link the file but I am curious to use the built in diode model instead. I can imagine that setting just a few parameters in the preconfigured DC block should do the same, but which ones? Ron or Roff are not represented at all. I tried changing the junction potential but saw no major difference.
The current of the simple diode model ist described by 3 linear regions: forward conducting, reverse blocking, and reverse breakdown. So in each region the current is linear with the diode voltage. The model is available in ngspice as well.
The standard diode model is an extension of the famous exponential diode equation, with several extra parameters describing detailed behavior, but there is no linear region at all! So I don’t think it is a good idea to try to mimic the simple model by the standard diode model.
The ohmic resistance parameter rs may resemble RON, ROFF may be replaced by suitable saturation current is, but it never will be possible to achieve a knee at 0 V in the characteristics as obtained in the simple model by Vfwd=0.
For a low on-voltage you may look for a Schottky diode parameter set.
