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

"Mike Engelhardt" <nospam@xxxxxxxx> wrote in message
news:Z4gZe.1791$Ur.4@xxxxxxxxxxxxxxxxxxxxxxxxxxxxx
> 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.

This is quite a valid point. Its nice to have the actual data clearly on
the spice netline so one knows exactly what the simulator is seeing. SS
actually does this by the GUI. I only very recently added hdif to the
engine itself. It then actually introduced a minor bug that I have yet
not gotten around to fix. I have check boxes on the mos set-ups to
selectively enable Ad/As to account for butting devices. Now they don't
work as the get overridden in the engine...ahmmm...

>
> 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.

I did notice that it handled single quotes as an alternative to {}. I
had to disable this in SS recently as I had a clash with xspice model
data having single quotes for state machine file names. I need to fix
that as well...

>
>> 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.

Never noticed that. I'll see about changing SS then I would rather use a
standard syntax.


Hey, you also don't document that LTSpice supports

..dc temp 0 100 1

to sweep temperature.

It should be easy for you to add

..dc r1 10k 50k 1k

Saves me a bit more bother when I get a circuit XSpice don't converge
on.

Kevin Aylward
informationEXTRACT@xxxxxxxxxxxxx
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.


.

Quantcast