Re: gEDA-user: NG-SPICE: TL071 model error

[sdb@xxxxxxxxxx (Stuart Brorson)]

Hi Wojciech --

> Spice 3 does not support nonlinear poly sources. You should try spice 2 but it 
> is much harder to build (Fortran). Or try to find or create a model that does 
> not contain poly sources.

What you say is true.  However, there is an XSpice extension to SPICE
3 which allows you to simulate netlists with SPICE 2 POLY sources.
The POLY is handled using a codemodel.  As long as you compile SPICE 3
with XSpice enabled, you should be able to use PLOY sources.

> I don't know if ngspice support poly sources, probably not since it is based 
> on spice 3.

Ngspice is based upon SPICE 3.  If you configure it with the
"--enable-xspice" flag set, then you will compile in the XSpice stuff
and you can use POLY sources.  I know this 'cause I'm the guy who
integrated the XSpice code into ngspice!  :-)   (Or at least made the
stuff which had already been integrated work properly. . . .)

Note to the original poster:  Once you get the latest ngspice from
CVS and build it using the XSpice extensions, make sure you uncomment
the stuff which loads the codemodels from the spinit file.  Spinit is
installed in the share/ng-spice-rework/scrips directory of your
install directory.  

Stuart