OT: gEDA, SPICE, electronic cad/simulation
russo at bogodyn.org
Sun Oct 28 17:55:18 UTC 2012
Date: Sun, 14 Oct 2012 22:26:34 +1000
From: Da Rock <freebsd-questions at herveybayaustralia.com.au>
Subject: OT: gEDA, SPICE, electronic cad/simulation
> I'm struggling with this damn gEDA/SPICE thing - I think I have gEDA
> schem figured, but I can't be sure because I can't test it. For the life
> of me I can't seem to get my head around it, but then I might just be
> too tired.
> Can anyone point out what I'm missing? I open geda, create a sch file
> (circuit), and then run gnetlist -g spice-sdb <sch-file>. I then run
> ngspice (or gspiceui) but it comes up with errors over the 555 (U1) and
> diodes (d?) I'm running like this:
> Error on line 9 : d1 2 0 unknown
> unable to find definition of model unknown - default assumed
> Error on line 13 : u1 0 4 3 +9v 1 4 5 +9v unknown
> unable to find definition of model +9v - default assumed
> unknown parameter (4)
I see some folks have tried to answer you, but it seems that it's expected
that these models somehow already exist on your system and you're just not
finding them. That's not the case.
Without seeing the entire netlist, I can't be precise, but there are several
important things to know about SPICE and device models:
1) SPICE provides only the infrastructure for simulating diodes, i.e. a module
that lets you specify all the parameters of a diode and which will then
simulate the circuit using the parameters you provide. A "model" in this
case means a set of parameters, which is specified in a .model "card".
Basically, your schematic has defined a diode without telling the simulator
the name of a model card to look for, so gnetlist has inserted "unknown" as
the model name. You then did not provide a ".model unknown d" card to define
"unknown" as a diode model.
No open-source SPICE-like simulator provides model "cards" for common
devices. You either have to find one from a manufacturer's web site,
find one someone has posted on a web site somewhere, or extract the
relevant parameters yourself (this list sorted in order of increasing
complexity). Commercial spice packages do come with enormous model,
libraries, but you pay big, big bucks for those versions.
Werner Hoch wrote a system called "spicelib" for gEDA that attempts to
download a large number of spice-compatible models from vendor web sites
and massage them to work with ng-spice. I have run it once, and found that
it needed a little patching up to make it work on FreeBSD instead of Linux
(for example, the "md5sum" program is used througout, and this doesn't
exist on BSD --- I had to hand-edit scripts all over the place to make it
use md5 instead). Even so, there are few basic parts in these model
Once in a while I have found cool web sites with hundreds of spice models
for common discrete parts. They disappear after a year or five.
You *COULD* try adding ".model unknown d" to your netlist to let ng-spice
use all the default parameters for the diode. It might not work well, but
it *will* shut up the error. It's what SPICE wound up doing itself when
it couldn't find the model named "unknown."
For details about spice diode models, see, for example,
2) There is no 555 model in SPICE, ng-spice, or any other spice. Such devices
are always simulated by creating a subcircuit model (.subckt). gschem will
gleefully create a line in your netlist for such a device, but unless you
also provide a subcircuit model for it, you won't be able to simulate it,
no way, no how. ng-spice does NOT come with a 555 subcircuit model, nor
does geda/gschem. gschem merely provides a symbol for such a device.
Try googling for "spice 555 model subcircuit" and go from there. One post
in the thread on this site:
has a UA555 subcircuit model that you may be able to use, if you make sure
that the subcircuit "pins" match the pins gschem/gnetlist are assigning.
3) SPICE (and ng-spice) always uses the first character of a device line to
determine the type of the device. While most designers will draw a
circuit with an IC in it and give the IC a name like "U1", the character
"u" in the first position on a device line means "lossy transmission line"
in spice, not "IC." Thus, in your netlist you're simply telling the
simulator to create a lossy transmission line using nodes "0", "4", "3"
and "+9v" as its four ports, and it's getting confused by all the extra
parameters on the line.
To create a subcircuit instance (which is what you want), you need to use
the "X" device. The format of the X device is:
X<name> [nodes] <subcircuit definition name>
so, in your case, you would want something like:
XU1 0 4 3 +9v 1 4 5 +9v UA555
and a .subckt UA555 card like the one in the post I mentioned in point 2
Note that I can't be absolutely certain that gschem's 555 symbol has
its pins defined so that it maps exactly onto the input nodes of the UA555
subcircuit model in the forums post I pointed you at. You will have to
check for yourself.
4) Your circuit as is is having a really hard time in the solvers (not
surprising, given all the errors), so SPICE is using its "gmin stepping"
process trying to force a solution.
5) You are attempting to use expressions somewhere (on a print line?) and this
is not a supported feature in most free versions of spice.
6) gnetlist will dutifully produce a netlist from the schematic you give it, but
unless you've prepared the netlist with an understanding of how gnetlist
is going to process it, you can get garbage.
While gEDA/gschem/gnetlist/ng-spice are cool tools, they are not easy to dive
into without a previous knowledge of spice.
You can try looking at the internal help in ngspice. Just fire up ngspice
and type help, then explore. This will not teach you the answers to your
specific issue, but *will* let you know what the format of various netlist
For more detail, you're better off with a textbook on SPICE simulation, and
probably need to ask more detailed questions on a gEDA mailing list.
Tom Russo KM5VY SAR502 DM64ux http://www.swcp.com/~russo/
Tijeras, NM QRPL#1592 K2#398 SOC#236 http://kevan.org/brain.cgi?DDTNM
"And, isn't sanity really just a one-trick pony anyway? I mean all you get is
one trick, rational thinking, but when you're good and crazy, oooh, oooh,
oooh, the sky is the limit!" --- The Tick
More information about the freebsd-questions