Re: Wanted: LM-709 (Spice model) National Op-Amp

Kevin,

>>> And I was once told that LTSPICE does not allow import
>>> of models from other vendors like ADI and National.
>>
>> More non-sense. Users can import models and since
>> LTspice knows most Pspice and hspice syntax,
>
> It don't know HSpice's "hdif" which is used to automa-
> tically calculate AD, AS, PS, and PD. These are
> absolutely crucial for high speed work.

The lack of hdif is deliberate. LTspice insists that
every dimension, area, and perimeter be explicitly stated
for every transistor. It's done because layout
verification tools and simulators can get confused about
this so I require that the schematic tools compute and
this for each instance so that no other tools can get
confused. When one designs against one's own fab, and
one has a schematic capture tool that can do all that
for oneself(which LTspice's schematic capture will do
but it will remain an undocumented feature), one gets to
do that: Simply once and for all resolve all the
transistor dimensions.

But if the every dimension, area, and perimeter is
instanced out for each transistor, LTspice will run most
hspice models with binning, single quote parameter
substitution and usually inline comments starting the a
'$' when it doesn't conflict this PSpice syntax.

> Tell, you what though, its rather irritating that
> LTSpice stops dead in its tracks when it gets a
> .option it don't know.

Part of having a polyglot simulator is the need to be
more error verbose/intolerant of incorrect SPICE syntax.
Correct hspice syntax is .options numdgt=N If N is
greater than 6, the waveform data or compression
coefficients are stored as double precision, otherwise
LTspice uses single precision. See the help file
(F1 key)=>LTspice=>Dot Commands=>.OPTIONS=>numdgt.

--Mike


.