Re: gEDA-user: Spice Example RF_Amp

[Dan McMahill <dan@xxxxxxxxxxxx>]

Thomas D. Dean wrote:
> I downloaded geda-examples-1.4.3.tar.gz, containing the RF_Amp example.
> 
> I built ngspice 19 from sources without error.
> 
> I get a max data size warning on any simulation, but, see no strange
> actions when simulating other circuits.  I tried a dozen emitter
> followers with different models and the results were about what I
> expected.
> 
> I wanted to use gEDA to generate models using hierarchy.  The RF_Amp
> example is exactly what I want to do.
> 
> I get a 'singular matrix' error when doing an op in ngspice 19 with the
> MSA-2643.cir file from the tarball.
> 
> I think I missed something.
> 
> tomdean
> 
> # ngspice MSA-2643.cir 
> Warning -approaching max data size: current size=5.488 kB, limit=0 bytes

I suspect the code for checking memory usage and limits is broken.  Are 
you on somthing other than 32-bit i386?  Actually it works on an old 
(ngspice-17) for me on an alpha but there could easy be machine and os 
dep. code in the mix.

> ngspice 7 -> op
> Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
> 
> Warning: singular matrix:  check nodes l6#branch and l6#branch
> 

take a look at the schematic and look for L6.  What you will see is 
there is a loop containing only inductors.

ground -[L4]---[L6]--- ground.

So what is the dc operating point of this part of the circuit?  Answer 
is it is undefined because you can have any arbitrary circulating 
current in this loop.  This is why spice is unhappy.  Try removing L6 
and lumping it in with L4 or put a small resistor, say 0.001 Ohm, in 
series with L6 and your problem will likely go away.

-Dan


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user