no Ngspice circuit simulator - Recipes

Interfacing ngspice with GNU Octave

Original contribution by Werner Hoch

Octave Spice

GNU Octave is a high-level language, primarily intended for numerical computations. It provides a convenient command line interface for solving linear and nonlinear problems numerically, and for performing other numerical experiments using a language that is mostly compatible with Matlab. It may also be used as a batch-oriented language.

GNU Octave can be used as a powerful post processor for the analysis of ngspice output vectors, but interfacing them is not straightforward. An import filter to read ngspice plots is needed.

Octave Spice

Octave Spice is a filter, written in Octave language, to import ngspice and spice plot. Octave spice can be downloaded from a ngspice download site.


We want simulate the transient response of the RC2 circuit and analyze the results with Octave. RC2 is the rc network depicted in the picture below.

The corresponding netlist is:

* simulation de RC2 .control tran 10n 10000n write .endc * Spice netlister for gnetlist R5 n4 n5 1k V1 n0 0 dc 1 ac 2 pulse 0 1 10n 10n 100n 1u 2u R4 n3 n4 1k R3 n2 n3 5k C5 n5 0 1n R2 n1 n2 1K C4 n4 0 1n R1 n0 n1 1k C3 n3 0 1n C2 n2 0 1n C1 n1 0 1n I1 n5 0 DC 0.01mA R6 0 n5 10k .END

To simulate the netlist we will run:

user@host:~$ ngspice -b rc2.cir

Now we can import the file ngspice produced ( named rawspice.raw) into octave with the following command:

user@host:~$ octave GNU Octave, version 2.1.69 (i386-pc-linux-gnu). Copyright (C) 2005 John W. Eaton. This is free software; see the source code for copying conditions. There is ABSOLUTELY NO WARRANTY; not even for MERCHANTIBILITY or FITNESS FOR A PARTICULAR PURPOSE. For details, type `warranty'. Additional information about Octave is available at Please contribute if you find this software useful. For more information, visit Report bugs to <> (but first, please read to learn how to write a helpful report). octave:1> k=spice_readfile("rawspice.raw");

The plot contained in file "rawspice.raw" is put into the k vector and the following output is generated:

s = { commands = {} date = Mon Sep 12 14:32:22 2005 dimensions = 0 no_points = 0 no_variables = 0 options = {} plotname = Transient Analysis title = * simulation de RC2 } octave:2>

Now we can plot the results (as in nutmeg, but we are using Octave):

octane:2>plot (k)

... and the results is shown below

Octave output

Once imported into GNU Octave you can manipulate vectors using its powerful language and produce better (than nutmeg) plots with GNUplot.