RE: [ng-spice] OP-AMP linux


To Jon Engelbert <jon@beigebag.com>
From rapela <rapela@usc.edu>
Date Wed, 24 Oct 2001 14:44:07 -0700 (PDT)
cc ng-spice@ieee.ing.uniroma1.it
Delivered-To mailing list ng-spice@ieee.ing.uniroma1.it
In-Reply-To <PBEHIGMLDPFPLAANAKMPOECACCAA.jon@beigebag.com >
Mailing-List contact ng-spice-help@ieee.ing.uniroma1.it; run by ezmlm
Reply-To ng-spice@ieee.ing.uniroma1.it

Hello Jon,

So it seems that using an opamp in spice for linux is not a trivial task.
Could you please email me if you find any way of using an opamp in linux.
I was not subscribed to the mailing list but now I am.

Thanks in advance, Joaquin

On Wed, 24 Oct 2001, Jon
Engelbert wrote:

> XSpice actually added backward compatibility for polynomial controlled
> sources, but I'm not sure if it ever worked correctly when the polynomial
> sources were within subcircuits.  At least when I ported their code into my
> spice 3f5 engine, it didn't work correctly within subcircuits, but it was
> close... I think that I had a problem with the ordering within the naming
> convention, i.e. there is an internal spice naming convention with the
> subcircuit's name, then the part name's first letter, then something else...
> probably for the referred variables within the polynomial controlled source.
> Anyway, if I seem confused on the details, it's probably because I am.
> If you want to "automatically" convert the subcircuits, you can do so with
> B2 spice a/d 2000... using the device editor, you can load the subcircuit as
> a new part, then look at the converted subcircuit text.  However, it's not a
> linux program, so that defeats the purpose.
> Also, I think that Tuinenga's pspice book has the formula for converting the
> terms into a polynomial.
> I don't have the formula offhand... but it might be in the b2 spice a/d user
> manual/ help file.
> 
> Here's a little blurb from the b2 spice a/d 2000 help file.
> 
> E1 1 2 poly(3)  (3,0) 1 0 0 3
> the corresponding spice3 (and B2 Spice) implementation is:
> BE1 1 2 V= 1 + 3 * V(3)^3
> B2 Spice has the capability to convert from spice2 polynomial controlled
> syntax to spice3 arbitrary source syntax when they are embedded in
> subcircuit models.
> Using the Database Editor, create the simulation model from the text file
> containing the subcircuit model.  Depending on how you do this, the Database
> Editor may automatically convert the polynomials for you.  If not, choose
> the button named Fix Controlled sources and the database editor will perform
> the conversion.
> 
> E.g. (the first line is commented out- it's the old polynomial controlled
> source.)
> * egnd 99  0 poly(2) (3,0) (4,0) 0 .5 .5
> begnd 99 0 v =0 + .5 * v(3,0) + .5 * v(4,0)
> Good luck,
> -Jon
> 
> -----Original Message-----
> From: Gillespie, Alan [mailto:Alan.Gillespie@analog.com]
> Sent: Wednesday, October 24, 2001 12:02 PM
> To: 'ng-spice@ieee.ing.uniroma1.it'
> Subject: RE: [ng-spice] OP-AMP linux
> 
> 
> 
> I think polynomial sources were dropped in spice3. They
> were replaced with the arbitrary source (B) device. If
> you can get hold of manuals for both spice2 and spice3,
> you should be able to convert the two lines with poly()
> in them to B devices. I'm afraid I can't remember the
> old syntax, off-hand,
> 
> Cheers,
> 
> Alan
> 
> > -----Original Message-----
> > From: rapela [mailto:rapela@usc.edu]
> > Sent: 24 October 2001 16:58
> > To: ng-spice@ieee.ing.uniroma1.it
> > Subject: [ng-spice] OP-AMP linux
> >
> >
> > Hello,
> >
> > First, I am a linux fun. Second, I am taking a course in
> > linear circuits
> > and I need to use an opamp in spice. I have installed spice3f4 and
> > realized that there was not a card for an opamp. I asked my
> > TA about how
> > to use opamp with my linux version of spice and he told me
> > that I should
> > go to Win because spice under linux does not have opapms. It would be
> > something really sad to go to windows so I am trying to get an opamp
> > model.
> >
> > I found a macromodel for the ua741 (attached file ua741.inc) and when
> > I tried to use it (comparator.cir) I got the following errors:
> >
> > ********************
> > Error on line 30 : e:test:gnd test:99 0 test:poly(2)
> > test:(3,0) (4,0) 0 .5
> > .5
> >      unknown parameter (test:)
> > Error on line 31 : f:test:b test:7 test:99 p:test:oly(5) vb
> > vc ve vlp vln
> > 0 10.61e6 -10e6 10e6 10e6 -10e6
> >      unknown parameter (vb)
> > Fatal error: f:test:b: unknown controlling source p:test:oly
> > doAnalyses: No such parameter on this device
> >
> > run simulation(s) aborted
> > ********************
> >
> > I am new to spice and if something could point me to a model
> > for any opamp
> > or tell me what am I doing wrong with ua741.ing. I will
> > really appreciate
> > it.
> >
> > Thanks in advance, Joaquin
> >
> > ----------------------------------
> > Joaquin Rapela
> > PhD Student, Signal and Image Processing Institute
> > University of Southern California
> > 3740 McClintock Ave, EEB 424
> > Los Angeles, CA 90089-2564
> > tel: (213) 740-6430
> > fax: (213) 740-4651
> > ----------------------------------
> >
> 



Partial thread listing: