On Tue, May 17, 2005 at 12:52:57AM +0200, Davide Anastasia wrote: > Il giorno lun, 16-05-2005 alle 21:24 +0200, Leva ha scritto: > > ..of what? > > I've got only a schematic... It's possible to perform this task with > Spice?
Yes... Most certainly. The best tutorial on the topic of getting a netlist from gschem to run in SPICE is probably: http://www.brorson.com/gEDA/SPICE/t1.html Basically what you need to get out of the netlister is something like this: -------------------------------------- Test Circuit Vin in 0 DC 0 AC 1.0 L1 in out 10e-6 C1 out 0 10e-9 R1 out 0 100 .ac dec 100 1 100meg .plot ac vdb(out) xlog .end -------------------------------------- Then run this file in some kind of spice simulator. Using original Berkeley spice it goes something like this: laptop daniel/tmp> spice3 test.sp Program: Spice, version: 3f5 Date built: Fri Sep 17 21:45:05 EDT 2004 Type "help" for more information, "quit" to leave. Circuit: Test Circuit Spice 11 -> run Spice 12 -> plot vdb(out) xlog Spice 13 -> quit Warning: the following plot hasn't been saved: ac1 Test Circuit, AC Analysis Are you sure you want to quit (yes)? yes Spice-3f5 done Or, in batch mode: laptop daniel/tmp> spice3 -b -r test.raw test.sp Circuit: Test Circuit Circuit: Test Circuit Date: Mon May 16 21:04:27 2005 .plot line ignored since rawfile was produced. CPU time since last call: 0.040 seconds. Total CPU time: 0.040 seconds. Current dynamic memory usage = 135168, Dynamic memory limit = -258049. laptop daniel/tmp> nutmeg test.raw Program: nutmeg, version: 3f5 Date built: Fri Sep 17 21:45:13 EDT 2004 Type "help" for more information, "quit" to leave. Loading raw data file ("test.raw") . . . done. Title: Test Circuit Name: AC Analysis Date: Mon May 16 21:04:27 2005 nutmeg 4 -> plot vdb(out) nutmeg 5 -> quit nutmeg-3f5 done You can also use gwave instead of nutmeg to view the results, but I'm not sure how to get the dB plot in gwave. Hope that helps Daniel
