Re: gEDA-user: Model problem?

[John Coppens <john@xxxxxxxxxxxx>]

On Fri, 22 Jul 2005 13:19:50 -0400 (EDT)
sdb@xxxxxxxxxx (Stuart Brorson) wrote:

> > For some reason, the libraries that came with gEDA didn't include
> > njfet symbols (nor nfet, pjfet, pfet etc). (looked in several of the
> > libraries- analog, etc) 
> 
> One commonly needs to create symbols for gschem.  Perhaps you could
> upload your JFET symbol to teh gEDA project symbol upload site once
> everything is working?

No problem, done that (njfet-1.sym and pjfet-1.sym). I just wondered - I'm
almost certain the jfet was in one of the earlier versions.

> Run gnetlist like this:
> 
> gnetlist -v -g spice-sdb -o circuit.cir circuit.sch
> 
> The -v flag will give you debug spew to help you figure out which
> component is the problem.

Great... The error was that two C's existed with the same component
number. Not quite an indicative error message for such an evident error
though:

Invalid wanted_pin passed to get-nets [unknown]
For C1, found pin with no pinseq attribute.  Ignoring. . . .
Invalid wanted_pin passed to get-nets [unknown]
For C1, found pin with no pinseq attribute.  Ignoring. . . .

> I don't know why that happened.  Make sure that you set the hidden,
> symbol-level attribute "DEVICE" to exactly the name of the JFETs
> specified in the spice-sdb documentation.  I believe the DEVICE name
> you need is  NFET_TRANSISTOR

That was it... It was still set to NPN_TRANSISTOR.
.
> > 
> > Warning -- Level not specified on line "(beta=1.4m betatce=-.5 rd=1
> > rs=1 lambda=4.6m vto=-3.1            vtotc=-2.5m is=33.57f isr=322.4f
> > n=1 nr=2 xti=3 alpha=311.7u             vk=243.6 cgd=2.132p m=.3622
> > pb=1 fc=.5 cgs=2.104p kf=23.06e-18  af=1)" Using level 1.
> 
> This is OK; it just says you are using the simplest JFET model by
> default.  
> 
> > 
> > Error on line 19 : 
> > .model bf256c        njf(beta=1.4m betatce=-.5 rd=1
> > rs=1 lambda=4.6m vto=-3.1 vtotc=-2.5m is=33.57f
> > isr=322.4f n=1 nr=2 xti=3 alpha=311.7u  vk=243.6 cgd=2.132p
> > m=.3622 pb=1 fc=.5 cgs=2.104p kf=23.06e-18 af=1) 
> > 
> >         unrecognized parameter (betatce) - ignored
> >         unrecognized parameter (-.5) - ignored 
> >         unrecognized parameter (vtotc) - ignored 
> >         unrecognized parameter (-2.5m) - ignored 
> >         unrecognized parameter (vtotc) - ignored 
> >         unrecognized parameter (-2.5m) - ignored 
> >         unrecognized parameter (isr) - ignored
> > 
> > etc...
> > 
> > The model doesn't seem to work at all. All nodes show 0V ('xcept for
> > the power supply)
> 
> It is possible that you need to use a higher-level model to use these
> parameters.  Try this (for example):
> 
> .model bf256c        njf(level=3 beta=1.4m betatce=-.5 rd=1
> 
> Google around a little to see which level model for the njf is
> required to get the above parameters.

Level 3 doesn't work, with this message:

 "Only JFET device levels 1-2 are supported in this binary"

> > +               Vk=243.6 Cgd=2.132p M=.3622 Pb=1 Fc=.5 Cgs=2.104p
> > Kf=23.06E-18^M
> > +               Af=1)^M
> > 
> 
> 
> The included model is messed up.  The last lines should read:
> .model BF256C   NJF(Beta=1.4m Betatce=-.5 Rd=1 Rs=1 . . . .

> ALso, if you run dos2unix on your .mod file, the ^M cruft will go
> away.

Removed the ^m's with 'fromdos' - but no difference in the execution. I
see on the 'net that some of the params are level 3. Which isn't
available in ngspice? I found a simpler model for the BF256 (level 1) and
it runs with that one.

Thanks again, Stuart.

John