Re: [ng-spice] OP-AMP linux


To ng-spice@ieee.ing.uniroma1.it
From Routoure JM <routoure@greyc.ismra.fr>
Date Thu, 25 Oct 2001 09:48:32 +0200
Delivered-To mailing list ng-spice@ieee.ing.uniroma1.it
In-Reply-To <Pine.GSO.4.21.0110241349420.12169-100000@aludra.usc.edu >; from rapela@usc.edu on Wed, Oct 24, 2001 at 23:44:07 +0200
Mailing-List contact ng-spice-help@ieee.ing.uniroma1.it; run by ezmlm
References <PBEHIGMLDPFPLAANAKMPOECACCAA.jon@beigebag.com > <Pine.GSO.4.21.0110241349420.12169-100000@aludra.usc.edu >
Reply-To ng-spice@ieee.ing.uniroma1.it

Please follow this link :

http://www.sigda.org/Archives/CollectedInformation/NewsgroupHighlights/feb95/Spice_2_to_Spice_3_Conversion_Utility.txt

It's a awk script which makes the conversion from spice2 to spice3 for the
poly source. I did not test it !





Le 2001.10.24 23:44, rapela a écrit :
> 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
> > > ----------------------------------
> > >
> > 
> 
> 
> 
-- 
Routoure Jean-Marc
GREYC Ismra

Partial thread listing: