Appendix: ngspice Cheatsheet

Analog (Integrated) Circuit Design

21 Appendix: ngspice Cheatsheet

ac dec|lin points fstart fstop performs a small-signal ac analysis with either linear or decade sweep
dc sourcename vstart vstop vincr [src2 start2 stop2 incr2] runs a dc-sweep, optionally across two variables
display shows the available data vectors in the current plot
echo can be used to display text, $variable or $&vector, can be useful for debugging
let name = expr to create a new vector; unlet vector deletes a specified vector; access vector data with $&vec
linearize vec linearizes a vector on an equidistant time scale, do this before an FFT; with set specwindow=windowtype a proper windowing function can be set

meas can be used for various evaluations of measurement results (see ngspice manual for details)
noise v(output <ref>) src (dec|lin) pts fstart fstop runs a small-signal noise analysis
op calculates the operating point, useful for checking bias points and device parameters
plot expr vs scale to plot something
print expr to print it, use print all to print everything
remzerovec can be useful to remove vectors with zero length, which otherwise cause issues when saving or plotting data
rusage plot information about resource usage like memory

save all or save signal specifies which data is saved during simulation; this lowers RAM usage during simulation and size of RAW file; do save before the actual simulation statement
setplot show a list of available plots
set var = value to set the value of a variable; use variable with $var; unset var removes a variable
set enable_noisy_r to enable noise of behavioral resistors; usually, this is a good idea
shell cmd to run a shell command
show : param, like show : gm shows the $g_\mathrm{m}$ of all devices after running an operating point with op

spec plots a spectrum (i.e. frequency domain plot)
status shows the saved parameters and nodes
tf runs a transfer function analysis, returning transfer function, input and output resistance
tran tstep tstop <tstart <tmax>> runs a transient analysis until tstop, reporting results with tstep step size, starting to plot at tstart and performs time steps not larger then tmax
wrdata writes data into a file in a tabular ASCII format; easy to further process

write writes simulation data (the saved nodes) into a RAW file; default is binary, can be changed to ASCII with set filetype=ascii; with set appendwrite data is added to an existing file

abstol sets the absolute current error tolerance (default is 1pA)
gmin is the conductance applied at every node for convergence improvement (default is 1e-12); this can be critical for very high impedance circuits
klu sets the KLU matrix solver
list print the summary listing of the input data
maxord sets the numerical order of the integration method (default is 2 for Gear)
method set the numerical integration method to gear or trap (default is trap)
node prints the node table

noinit suppresses printing of the initial transient solution (to quiet the output)
nomod suppresses printing of the model table (to quiet the output)
opts prints the option values
temp sets the simulation temperature
reltol set the relative error tolerance (default is 0.001 = 0.1%)
savecurrents saves the terminal currents of all devices
sparse sets the sparse matrix solver, which can run noise analysis, but is slower than klu
vntol sets the absolute voltage error tolerance (default is 1µV)
warn enables the printing of the SOA warning messages

To set the fontsize of plots, use xfont_size
To append data to an existing RAW file, use appendwrite=1
Get the name of the current plot with curplot
The filetype of the RAW file can be set with filetype, either binary (default) or ascii
The number of threads can be set with num_threads
The noise PSDs will be given in V^2/Hz or A^2/Hz when setting sqrnoise=1 (otherwise V/rtHz or A/rtHz)