Re: PSpice Ideal Diode ... and Crash

"Bob Penoyer" <bob@xxxxxxxxxxxxxxxxxxxx> schrieb im Newsbeitrag
news:tilrk1d2orvu4m088eaamp87p3111nq9g4@xxxxxxxxxx
>I recently had a need for an ideal diode. When I found one and used
> it, I got results that worked great in one circuit and crashed PSpice
> in another circuit. I've had convergence problems before, but never a
> crash.
>
> I found a model for an ideal diode at this MIT site:
> http://ocw.mit.edu/NR/rdonlyres/Electrical-Engineering-and-Computer-Science/6-334Spring2003/56F6E619-0B02-424D-AC10-88D1AC4AB3E1/0/idealdiode.lib


Hello Bob,

This model uses an extreme low value of N=0.001 in the diode model.
The diode equation looks like

Id = Is*exp(V/(N*Vt))

It's obvious that this small value of N can cause very big
exponents if the equation solver in SPICE makes too big steps.
This can lead to a math overflow. Neverthess a good program
shouldn't crash in this case. You could also try with a
bigger value like N=0.005 or maybe adding a small series
resistance parameter RS=0.01 may help.

Btw, it's nonsense to make a subcircuit around a simple .model
statement.

Other SPICE programs may or may not have problems with
this extreme paramter value. It's just a question if the
programmers had such values in mind or not.
LTspice works with this diode model.

I recommend you send your test case to Cadence and ask for
"bug" fix.


Best regards,
Helmut



The model from the link above.

************************************************************************
**** diode_ideal (approximates ideal diode) ****
************************************************************************
..subckt diode_ideal 1 2
D12 1 2 diode_ideal
..model diode_ideal D (N=0.001)
..ends diode_ideal
*******************************************************






.