Re: gEDA-user: Multivibrator Simulation

[al davis <ad252@xxxxxxxxxxxxxxxx>]

On Tuesday 23 June 2009, Michael B Allen wrote:

> *==============  Begin SPICE netlist of main design
> ============ 
> Q2 output 2 0 2N3904
> .MODEL 2N3904 NPN (Is=6.734f Xti=3 Eg=1.11 Vaf=74.03 Bf=416.4
> Ne=1.259 Ise=6.734 Ikf=66.78m Xtb=1.5 Br=.7371 Nc=2 Isc=0
> Ikr=0 Rc=1 Cjc=3.638p Mjc=.3085 Vjc=.75 Fc=.5 Cje=4.493p
> Mje=.2593 Vje=.75 Tr=239.5n Tf=301.2p Itf=.4 Vtf=4 Xtf=2 Rb)

This syntax is incorrect .. Rb) ???


> V1 4 0 DC 9V
> R4 output 4 0.999K
> Q1 1 3 0 2N3904
> .MODEL 2N3904 NPN (Is=6.734f Xti=3 Eg=1.11 Vaf=74.03 Bf=416.4
> Ne=1.259 Ise=6.734 Ikf=66.78m Xtb=1.5 Br=.7371 Nc=2 Isc=0
> Ikr=0 Rc=1 Cjc=3.638p Mjc=.3085 Vjc=.75 Fc=.5 Cje=4.493p
> Mje=.2593 Vje=.75 Tr=239.5n Tf=301.2p Itf=.4 Vtf=4 Xtf=2
> Rb=10)

syntax correct this time, but there should be only one .model statement.

> R3 1 4 1.001K
> R2 3 4 15K
> R1 2 4 15K
> C2 output 3 10uF
> C1 1 2 10uF
> .end
>
> > You need to explicitly start the oscillator.
>
> I'm not having any luck with this. It seems the syntax of
> netlist vs. interpreter mode commands vs. gspiceui fields is
> different enough that it's totally unclear as to how to
> achieve non-trival things.

Why I don't like the GUI ..  There are hundreds of things you can do.
The GUI gives you about three of them.

> First, do I want to use GNU-Cap or NG-Spice?

Gnucap, if you want my help.  If you are really into it, try both
and you will see that some things work better in one, some
in the other.

> Also, what timing do I want? I was thinking something like
> 50ms - 100ms in 1ms increments reasoning that it will take
> time for the oscillation to start.

It depends on your circuit.  What frequency did you design it for.

You need to run it a while to start up.  See the example I referenced
in the other mail.

> Regarding simulating power on, I don't recognize the format
> on the page cited:
>
>   Vcc (vcc 0) pulse(iv=0 pv=12 rise=.01)
>
> My netlist above does not have parenthesis.

Parenthesis are optional, but make it easier to read.

> And it seems
> gspiceui overrules the voltage source properties anyway?

I think you put the whole string pulse ( ...) as the "value" in the schematic.

With Spice, you list a bunch of numbers in a particular order.
Gnucap accepts that too, but I can never remember what
order they go in, so the labels are a better way to do it.

That statement says the initial value (iv) is 0, pulsed (final)
value (pv) is 12, and the rise time is .01 seconds.  Look 
up the "pulse" 

http://gnucap.org/gnucap-man-html/gnucap-man094.html

> Similarly I'm not sure where the "OFF" property would go. I
> tried sticking it in the parameters of the .MODEL description
> but gspiceui choked on it.

"OFF" may not do what you want.  You really need to ramp
up the power supply to start the oscillator.

> What is the definitive guide for interactive mode?

The old manual: (for version 0.35)
http://gnucap.org/gnucap-man-html
http://gnucap.org/gnucap-man.pdf

The new (unfinished) manual, for the development version:
http://wiki.gnucap.org/dokuwiki/doku.php?id=gnucap:manual



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