Re: Problems with SPICE models from vendors

zineddine.zidane_at_gmail.com
Date: 03/25/05 

Date: 25 Mar 2005 15:25:44 -0800

Hmm useless huh? the AD8614 has 1mV of Vos and the model has 1mV, I
just looked at it, so I don't know what you mean by not working. I
think you may be overlooking some things here. Here's the Vos in the
netlist...
EOS 7 1 POLY(2) (73,98) (81,98) 1E-3 1 1

Robert Baer wrote:
> Helmut Sennewald wrote:
> > "Robert Baer" <robertbaer@earthlink.net> schrieb im Newsbeitrag
> > news:1PQ0e.3481$gI5.1145@newsread1.news.pas.earthlink.net...
> >
> >> The LM324 model from TI works fine,but the one from National
> >>Semiconductor is junk.
> >> I tried numerous Analog Devices models for various rail-to-rail
opamps,
> >>and found that almost all i tried gave me the same kind of cryptic
square
> >>root error.
> >> Those tried: AD8605, AD531, AD541, AD8552, and the AD8571; the
only one
> >>tried that did work was for the AD8614.
> >> Now i would dearly like to have a set of models that were known
to work
> >>(and more or less correctly), but i need to get a working AD8605
model.
> >> The sets i have came from the manufacturer created in the latter
of
> >>1992, and thus are not quite up-to-date.
> >> However, the model for the AD8605 was downloaded via the web just

> >>yesterday - implying the problem is not fixed.
> >>
> >> Can anyone help?
> >
> >
> > Hello Robert,
> > I don't believe that you really can judge the quality of these
> > models as a beginner with SPICE simulations.
> > I agree with you that most models have difficulties with
convergence.
> > Many of them are really over complicated and sometimes generated
> > by stupid programs or "roboters" and not by engineers.
> >
> > I assume that the listed models will work with some tweaking
> > of the convergence parameters.
> >
> > What simulator do you use?
> > If it's LTspice then send me your files and I will make
> > you a working example with your AD8605.
> > I always want to see the schematic, because I know that
> > people sometimes have errors in their circuit.
> > One important thing is to have a DC path to ground(0).
> >
> >
> > Best Regards,
> > Helmut
> > Moderator of the LTspice user group
> >
> >
> >
> >
> Well, in a sense you are correct in labellling be as a beginner; i

> rarely use SPICE, but that useage has covered over 30 years.
> When one models a simple voltage follower, with the NI input half
way
> between the poser supplies for the op-amp, one expects it to work,
and
> not give a cryptic square root error.
> Furthermore, replacing the model used to a different one (eg
replace
> the call from the AD8605 to the AD8614 (and changing *nothing* else)
and
> have it work begs the question: what is wrong with the AD8605 model?
> The same can be said about the models for the LM324; the TI model
> works and the NatSemi does not.
>
> And speaking of bad models that DO "work", the AD8614 is rather
poor
> (from the .OUT file):
>
> .OPTIONS ACCT LIST NODE OPTS NUMDGT=6 RELTOL=0.00001 NOPAGE
> .TEMP 27
> .LIB ANLG_DEV.LIB ; most rail-to-rail opamps die with error
> .DC VBAT 4.499 4.501 0.001
> VBAT 01 00 DC 4.5
> VSET 10 00 0.209171
> VIN 05 00 0.018051
> R2 05 07 18.4K
> R3 10 08 18.4K
> R4 09 07 100K
> * NI I OUT
> XAMP2 08 07 01 00 09 AD8614/AD
> .PRINT DC V(05) V(07) V(08) V(09)
> .PLOT DC V(05) V(07) V(08) V(09)
> .SAVE
>
> V(5) V(7) V(8) V(9)
>
> 1.80510E-02 2.22746E-01 2.21746E-01 1.26487E+00
>
> Look at the poor results: large input currents, large Vos. Almost

> useless; certainly not representative of the part.