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 [email protected] http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
