Sorry about the delay .. At first I was travelling, then had a pile of stuff waiting .. and the answer to this one isn't simple. I will try to address the issues one at a time, hopefully in a manner that is useful.
1. Geda / gschem / gnetlist. This combo really doesn't work as well as it should. gschem is a nice program, but you need to enter your schematic in a certain way for it to generate a reasonable netlist. The problem is gnetlist .. In my experience, the netlists generated usually require some kind of editing to work for simulation. Since all "spice" are a little different, it hits some kind of middle ground that isn't really a perfect match for any of them. I have asked for help in solving this problem, but never got any. In this case, I see a few things .. > U1 3 2 1 LM317 > ^ ? need more nodes > U1 3 2 1 LM317 > ^ ? need and,nand,or,nor,xor,xnor,inv "U" indicates a logic device. The error messages make it look like you improperly specified a logic device. You can get all kinds of strange messages in situations like this. LM317 is a SUBCKT, so the instances should start with X , not U. > J1 1 3 4 JN > ^ ? illegal type > .MODEL JN NJF(BETA=1E-4 VTO=-7) > ^ ? not implemented JFET is not implemented in 0.35. In the snapshot, things like this are plugins. You would need to load the plugin. > I found this very helpful page: > http://www.brorson.com/gEDA/SPICE/t1.html Actually, I find that page to be rather confusing. I understand why you are confused. 2. gspiceui ... I don't use it. It works, sort of, but doesn't do what I need. I use the schematic to generate a netlist, then load it and run commands interactively, like some of the examples here: http://gnucap.org/dokuwiki/doku.php?id=gnucap:manual:examples > Now my questions: > 1) Do I have to rewrite the spice model to work with > gnucap? To answer in general .... Most "spice" models are written for a particular version of spice. It is common for them to need changes to run on even other versions of spice. Sometimes, even different releases of the same brand have compatibility issues. You might run into .. a. syntax differences ... In this case, a simple edit may fix it. But as a beginner, how do you know? For Gnucap, recent snapshots have improved this a lot, but it still isn't perfect. I don't think that is the problem here. One example of this is the use of parameters .. Hspice requires quotes around parameters, Pspice requires curly braces. Gnucap accepts either, but I think NGspice only accepts the Pspice way. b. missing features ... There are some features that are simulator specific, for example parameter passing to subcircuits. c. missing models .. Often models are built on top of other models, and the model being built on isn't included. If this is the problem, you need to find the missing piece. NGspice has more models compiled in. Gnucap has more available as plugins but fewer compiled in. > 2) gEDA includes the LM317 as symbol, but apparently > no spice model? Is this correct? As far as I know, no gEDA symbols include simulation models. If you look at the low-end commercial simulators (Pspice, multi- sim) and the cover-crop simulators (LTspice), they come with huge libraries. The free/open-source ones typically don't. You need to "google for it" or make one yourself. It would be nice if we could provide that too, but it's a lot of work, and we lack the manpower to do it. The high-end commercial simulators (Spectre, Eldo) usually don't come with these libraries. Their users don't trust them anyway. Parts vendors often supply models. _______________________________________________ Help-gnucap mailing list [email protected] http://lists.gnu.org/mailman/listinfo/help-gnucap
