Date: Sun, 14 Oct 2012 22:26:34 +1000
From: Da Rock freebsd-questi...@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
libraries.
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,
http://www.acsu.buffalo.edu/~wie/applet/spice_pndiode/spice_diode_table.html
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:
http://www.electro-tech-online.com/general-electronics-chat/5806-spice-555-timer.html
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:
Xname [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
above.
Note
