Simulating Analog Audio Cicuits

This article describes an extension to ngspice that provides a libsndfile voltage source and the possibility to write ngspice's output in audio-file format.

Ngspice is a mixed-level/mixed-signal circuit simulator, based on Berkeley Spice3F5 and developed openly as ngspice sourceforge project. (see SPICE)

Libsndfile is a C library for reading and writing files containing sampled sound; released in source code format under the GNU Lesser General Public License.

Spicy Sound

The idea is simple: use a schematic as audio-effect.

When compared to traditional digital audio effects, performing a full analog circuit simulation breaks a fly on the wheel. However todays computing power allows to do so almost in real-time! But don't get your hopes up too soon.. even if passing 10 seconds 48kHz audio though a simulated RC bandpass takes 11.2 seconds on a 1.6Ghz pentium, it's far far away..

Nevertheless being able to process arbitrary audio-samples with SPICE provides off-line sound processing and (re-)engineering features for analog audio circuits.

In this exercise the audio-input represents a linear sound-controlled voltage-source in the schematic and the audio-sink can be any node in the schematic's netlist.

Preparation / Source Code

Though spice is rather flexibly importing/exporting data, adding native sound I/O functionality greatly improves performance, simplifies prototyping and shortens turnaround time at the cost of (re-)compiling ngspice 1).

The patch applies to the ngspice-rework17 source code release and does not modify exiting functionality of ngspice . It just adds new features, and also works with the current CVS version of ngspice.

Apart from ngspice' build-dependencies, you need the libsndfile-dev package to compile it:

cd /tmp
tar xzf ng-spice-rework-17.tar.gz
cd ng-spice-rework-17
patch -p1 < ../ng-spice-rework-17-snd-v3.2.diff
mkdir build && cd build
../configure && make
sudo make install

UPDATE: Hannu Vuolasaho rebased the patch to spice-0.23. The patch and information is available on


See the chapter Voltage and Current Sources in the spice3 user manual for general information.

Audio Source

The snd patched spice knows a new type of Independent voltage source extending the syntax of


with the time-dependent value:




V_V2 10 0 dc 0.0 file /tmp/stay.wav snd 0 0 0.2 0 0 1
VLEFT 2 0 file(/TmP/tEst.wAv) snd 1 0 0.2 5.0 0 64
VRIGHT 13 2 snd(1 0.0 1.0 5.0 1 64)


N+ and N- are the positive and negative nodes, and the new parameters are

  • <id> an integer identifier 0 to 5
  • <v_offset> offset added in Volts
  • <v_mult> the multiplier when converting sndfile-float [0..1] to Volts
  • <t_off> offset in seconds added when seeking the sound-file
  • <channel> the sound channel to use. 0: first channel in file.
  • <oversampling> new in v3 allows to upsample the audio-file. - see synchronization below
  • The optional <file> parameter must precede the <snd> argument to take affect.
  • Note: spice syntax treats all filenames as lowercase. Spaces and special characters are not allowed in the filename either.
  • if no filename is specified the previous filename for the given <id> is used. Default files are id=0:/tmp/test.wav id=1:/tmp/test1.wav id=2..N:NULL

If unspecified spice uses default TSTEP and TSTOP for transient analysis, which should match the sampling rate of the audio file times the oversampling factor. - unless you know what you're doing: choose the same oversampling-factor for input and output. Read more about synchronization in the next section.


Converting spice's output into a sound file is done with a standard print command. sndprint behaves just like print with the difference that it does not write text to screen but the same values into a audio file instead. each sndprint argument gets written as a channel in the file. The global parameters (filename, samplerate) can be changed for each sndprintf.




.sndparam /tmp/spice-1.wav 48000 wav16 3.0 0.0 64
.sndprint tran v(10) v(9)
.sndparam /tmp/spice-2.wav 48000 wav24
.sndprint tran v(10)


sndparam affects all following .sndprint lines. If not specified the defaults values are used: .sndparam spice.wav 48000 -1 0.0 1.0 64.

  • <filename> of the output file - it will be converted to lower case and must not contain spaces or special characters.
  • <samplerate> is the number of audio-samples to write in 1/s
  • <format> - numeric or text-shortcut.
    • -1:default (wav 24 bit/sample little endian)
    • 0: aliki .ald data file
    • >0 : libsndfile numeric format SF_FORMAT_XXX - example: (SF_FORMAT_WAV | SF_FORMAT_PCM_24) = 0x010000 | 0x003 = 65539
    • currently the following txt shortcuts are defined: wav16, wav24, wav32, aiff and aliki.
  • <v_off> is an offset voltage added after multiplication
  • <v_mult> specifies a multiplier to extend the dynamic range or normalize the value.
  • <oversamling> new in v3 allows to downsample/interpolate when writing the file.

The output range of sndprint is [-1..1] - values are clipped. Each printed parameter will be written to a separate audio-channel; fi. sndprint v(2) writes a mono file from the voltage of net 2; sndprint v(2) v(4) produces a stereo file. - The sndparam conversion parameters are set per file and apply for all channels to be written.

Further Information


Spice allows to specify a maximum time-step, which should be set to the audio-sample rate. The step-size is not guaranteed and sometimes smaller than the specified value, which makes synchronization a non trivial problem.

Unlike the txt2snd tool, the internal sndprint does not add missing samples. sndprint only drops excess samples and does not perform any resampling or interpolation; thus sndprint should only be used when simulating at audio-samplerate or even shorter interval which should best be at an integer multiple of the samplerate.

simulating 5 seconds at 1/48000Hz:

.tran 2.0833333333333e-05 5.0 0 2.0833333333333e-05

when using oversampling, the time step needs to be adjusted accordingly!

.tran 3.25520833e-07 3.0 0 3.25520833e-07

Note: the simulation time-step must be smaller than the 1sec/(sndprint_samplerate*sndprint_oversampling).


simple audio test

V_V2 1 0 file /tmp/test.wav snd 0 0 1.0 0 0
R_R1 1 0 1M

.sndparam /tmp/test-spice.wav 48000 wav24 1.0 0.0
.sndprint tran  v(1)
.tran 2.08333e-05 2.0 0 2.08333e-05

Save this file as sndtst.cir copy any audio-file (longer than 2 seconds) to /tmp/test.wav. Launch the simulation: spice -b sndtst.cir will generate /tmp/test-spice.wav - this example simply copies the first two secods of audio from the channel of the audio-file into a 24bit 48kHz mono wav file.

more examples.

Developer Notes

This patch is rather a quick experiment; already very useful though. There are some open-ends, that will be fixed after testing and receiving feedback on the patch: Most notably are verifying the command arguments; checking for libsndfile in; and printing nice warnings/statistics for missing/skipped audio-samples.

Other addons that could come in handy, would be implementing different algorithms of converting the sound into a spice-value and back (eg. logarithmic scale, linear resampling, current source) though I dare say that can be done with ngSPICE functions already. - Before settling on the sndprint command I considered using a resistor or inductance based model for a “speaker” that could be wired into the schematic and write the sound to file during the simulation. sndprint is more flexible.


1) earlier versions of the patch include a simple tool to convert spice .print text to sound. - see txt2snd
oss/spicesound/start.txt · Last modified: 07.12.2012 21:43 by root