[Top][All Lists]
[Date Prev][Date Next][Thread Prev][Thread Next][Date Index][Thread Index]
Re: [Help-gnucap] spice models
From: |
al davis |
Subject: |
Re: [Help-gnucap] spice models |
Date: |
Wed, 7 Jul 2010 00:25:29 -0400 |
User-agent: |
KMail/1.13.3 (Linux/2.6.32-trunk-amd64; KDE/4.4.4; x86_64; ; ) |
Sorry about the delay .. At first I was travelling, then had a
pile of stuff waiting .. and the answer to this one isn't
simple. I will try to address the issues one at a time,
hopefully in a manner that is useful.
1. Geda / gschem / gnetlist.
This combo really doesn't work as well as it should. gschem is
a nice program, but you need to enter your schematic in a
certain way for it to generate a reasonable netlist.
The problem is gnetlist .. In my experience, the netlists
generated usually require some kind of editing to work for
simulation. Since all "spice" are a little different, it hits
some kind of middle ground that isn't really a perfect match for
any of them.
I have asked for help in solving this problem, but never got
any.
In this case, I see a few things ..
> U1 3 2 1 LM317
> ^ ? need more nodes
> U1 3 2 1 LM317
> ^ ? need and,nand,or,nor,xor,xnor,inv
"U" indicates a logic device. The error messages make it look
like you improperly specified a logic device. You can get all
kinds of strange messages in situations like this.
LM317 is a SUBCKT, so the instances should start with X , not U.
> J1 1 3 4 JN
> ^ ? illegal type
> .MODEL JN NJF(BETA=1E-4 VTO=-7)
> ^ ? not implemented
JFET is not implemented in 0.35.
In the snapshot, things like this are plugins. You would need
to load the plugin.
> I found this very helpful page:
> http://www.brorson.com/gEDA/SPICE/t1.html
Actually, I find that page to be rather confusing. I understand
why you are confused.
2. gspiceui ...
I don't use it. It works, sort of, but doesn't do what I need.
I use the schematic to generate a netlist, then load it and run
commands interactively, like some of the examples here:
http://gnucap.org/dokuwiki/doku.php?id=gnucap:manual:examples
> Now my questions:
> 1) Do I have to rewrite the spice model to work with
> gnucap?
To answer in general .... Most "spice" models are written for
a particular version of spice. It is common for them to need
changes to run on even other versions of spice. Sometimes, even
different releases of the same brand have compatibility issues.
You might run into ..
a. syntax differences ... In this case, a simple edit may fix
it. But as a beginner, how do you know? For Gnucap, recent
snapshots have improved this a lot, but it still isn't perfect.
I don't think that is the problem here.
One example of this is the use of parameters .. Hspice requires
quotes around parameters, Pspice requires curly braces. Gnucap
accepts either, but I think NGspice only accepts the Pspice way.
b. missing features ... There are some features that are
simulator specific, for example parameter passing to
subcircuits.
c. missing models .. Often models are built on top of other
models, and the model being built on isn't included. If this is
the problem, you need to find the missing piece. NGspice has
more models compiled in. Gnucap has more available as plugins
but fewer compiled in.
> 2) gEDA includes the LM317 as symbol, but apparently
> no spice model? Is this correct?
As far as I know, no gEDA symbols include simulation models.
If you look at the low-end commercial simulators (Pspice, multi-
sim) and the cover-crop simulators (LTspice), they come with
huge libraries. The free/open-source ones typically don't. You
need to "google for it" or make one yourself. It would be nice
if we could provide that too, but it's a lot of work, and we
lack the manpower to do it.
The high-end commercial simulators (Spectre, Eldo) usually don't
come with these libraries. Their users don't trust them anyway.
Parts vendors often supply models.
- [Help-gnucap] spice models, Mogliii, 2010/07/02
- Message not available
- Message not available
- Message not available
- Re: [Help-gnucap] spice models, Mogliii, 2010/07/05
- Re: [Help-gnucap] spice models, Mogliii, 2010/07/05
- Re: [Help-gnucap] spice models, Mogliii, 2010/07/06
- Re: [Help-gnucap] spice models, asomers, 2010/07/06
- Re: [Help-gnucap] spice models, Mogliii, 2010/07/06
- Re: [Help-gnucap] spice models, asomers, 2010/07/06
- Re: [Help-gnucap] spice models, al davis, 2010/07/07
- Re: [Help-gnucap] spice models, Mogliii, 2010/07/07
- Re: [Help-gnucap] spice models,
al davis <=
- Re: [Help-gnucap] spice models, Werner Hoch, 2010/07/05