On Thursday 29 May 2008, JERRY DUNMIRE wrote: > I played with the model a bit to see if I identify the > problem. I thought that gnucap was accepting POLY(1) and not > POLY(n), but based on your comments I'll guess that gnucap > was treating POLY(1) as a symbolic node. There are also > TABLE sources in the file and I don't think gnucap likes > those either. > > Interestingly the spice models from Linear Technologies, for > similar op-amps, seem to work (at least there are no errors > reported) for gnucap. So maybe I'll select an opamp from > Linear. The Linear spice models do not seem to use POLY or > TABLE elements.
Some do. Some do not. There is a common subset that all simulators support. If you stick to that it will work everywhere. Very few models stick to that subset, because there isn't much in it. I don't expect to ever see gnucap specific models, or ngspice specific models. I don't want to see them. I really would like to see an end to all those vendor-specific models. We need standards. That is part of what Verilog-AMS and VHDL-AMS are all about. Even if you only use them as an alternative netlist format, at least there is a defined standard. After putting a lot of effort into trying to both be compatible and to provide important new functionality, I realized that these concepts are mutually exclusive. This is one of the reasons for the language plugins in gnucap. Since the language is plugable, there can be a plugin for each variant. Since they are not built in, new language compatibility can be added later, perhaps by a user, perhaps by hacking an existing plugin. Gnucap does support the equivalent to the "TABLE" element, but not in a form compatible with Pspice. It is supposed to be compatible with Hspice. It's called "PWL". Now that you mention it .. it is a trivial change to make it take "TABLE" too. It looks like it will increase the code size by 6 characters... The syntax is still not Pspice compatible. Try: G324 no1 no2 ni1 ni2 PWL (..........) The Hspice format: G321 no1 no2 PWL(1) ni1 ni2 (......) also works. Some of the regression tests use that format, but I think it is ugly. Someday, there will be a "Pspice" language plugin. There are plenty of other things on my plate, so you might need to wait a while. Since it is a plugin, anyone can do it. Or, if you send money, that will make it happen faster. Actually, I do have some funding now, but not enough..... The funders are more interested in Hspice, Verilog, and Spectre compatibility, and other things. Now about that op-amp model ..... Most users really don't need all that detail. Most users are misled by the apparent detail. You are probably better off with a simple VCVS model, or maybe a two stage model with a "dominant pole" between them. The design of such a model should be covered in an undergrad electronics or circuits course, when they start talking about non-ideal op-amps. Those fancy models that you get by downloading or from databases are usually overkill. If you don't understand them, use a simpler model. Teachers that teach you to just use the magic model, without understanding it, are doing a lot of harm. _______________________________________________ geda-user mailing list [email protected] http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
