Re: gEDA-user: (no subject)

[al davis <ad151@xxxxxxxxxxxxxxxx>]

On Saturday 22 November 2008, Sean Carter wrote:
> Hi, I have what I hope is a really simple question, which I
> have been unable to find by rtfm. 
>>>  (summary: it doesn't work)



> * Spice netlister for gnetlist
> R5 1 +9V 1M

1M = 1 milliohm.
Do you want "1Meg"??

Some variants of Spice don't like "+" in names.

> V1 n0 0 AC

Zero volts?
You need a value.
> V1 (n0 0)  AC 1
.. or something like that

> R4 0 4 100K
> R3 0 3 470

> Q1 1 3 2 2N5245
Q = BJT
 ... and it is interpreting "2N5245" as the substrate node.
strange ...
You need "J" for a JFET.
Check the connections ..
The BJT connections are (C B E).
JFET connections are (D G S)
I think you have the order wrong.

> R2 2 +9V 1K
> R1 0 1 1M

1 milliohm again

> C3 2 4 4.7uf
> C2 3 0 .052uf
> C1 n0 1 4.7uf
> .END

No power supply.
Just calling a node "+9V" doesn't do it.  It's just a string 
that has no meaning.

You need a DC voltage source as the power supply.
Vpower (+9V 0)  DC 9

You didn't say what a "2N5245" is ..  
You need a statement something like:
.model 2N5245 njf .......

You can probably find it on the web.  Google for "2N5245 spice 
model".  If you can't find one, but can find a data sheet, you 
should be able to fill in the important parameters from the 
data sheet.

Most spice models don't show the range of parameters you get 
with real devices.  Ideally, there would be several for each 
device, but they rarely do that.  Some of them are really 
funny ..  like specifying threshold voltage (vto) as something 
like "-2.3243242" when the real value is somewhere between -0.5 
and -8.

I didn't address the simulator commands here.  There are lots of 
ways to do it.



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