Re: SD21x spice model?

"Jim Thompson" <To-Email-Use-The-Envelope-Icon@xxxxxxxxxxxxxxx> schrieb im Newsbeitrag
news:u3laa2diol0q7d4h6t2c099rie0pscdrn2@xxxxxxxxxx
On 30 Jun 2006 08:48:25 -0700, Winfield Hill
<Winfield_member@xxxxxxxxxxx> wrote:

Klaus Bahner wrote...

Does anyone have spice models for the SD210/SD214 DMOS Fets?
I've found the models from Linear Systems, but they produce clearly
wrong results at least when used in OrCAD PSPICE. There doesn't seem
to be anything wrong with the syntax, hence I tend to believe there
is something wrong with the model parameters. I've contacted Linear
Systems a while ago, but of course no answer ...

You should be checking with Vishay (was Siliconix).

My Intusoft spice has models for sd210 through sd215.
Without looking at them all, I see the capacitance varies
between types, which is not support by the datasheets.

.MODEL SD210DE NMOS Level=1 CBD=4.65P CBS=5.58P CGBO=20.6N
+ CGDO=2N CGSO=2.4N GAMMA=.992 IS=3.25E-13 KP=7.15M
+ LAMBDA=22.5M MJ=.46 PB=.8 PHI=.75 RD=12 RS=15 VTO=1.15

.MODEL SD215DE NMOS Level=1 CBD=8.08P CBS=9.7P CGBO=20.6N
+ CGDO=2N CGSO=2.4N GAMMA=.992 IS=3.25E-13 KP=7.2M
+ LAMBDA=22.5M MJ=.46 PB=.8 PHI=.75 RD=11 RS=13 VTO=1.1

I have not evaluated these models. In my experience,
if you want to use a MOSFET model for linear work,
you have to first vet it against bench measurements,
and be prepared to make substantial changes.

Those models are Level = 1, which suck the big lemon.

Fortunately Klaus cites models that use PSpice Level = 7, same as
HSpice Level = 49, and don't require the "Win-fix" ;-)

Hello Jim,

The model given by Win has given a "correct" Rds_on of about
40 Ohms for Vgs=10V. So this model is much better suited for
switched applications than the model from Linear Systems.

Best regards,
Helmut




.