This section contains links to ngspice applications or short paragraphs describing the usage of ngspice. Its content will grow over time. You are welcome to contribute!
Google/SkyWater 130 nm CMOS PDK
ngspice supports the Open Source Google/Skywater PDK (process design kit) for the 130 nm CMOS process from Skywater. To install the PDK, a good choice is to follow the installation procedure offered by Tim Edwards (Chapter "Prerequisites", steps 1 to 12). Design support is also available by Stefan Schippers' XSCHEM. See his video for further installation instructions.
To successfully simulate with ngspice
and the SkyWater PDK, at least ngspice-34 is required, however much better results
(speed-up of at least a factor of 3, large circuits with 200k transistors have been
tested) are available with the KLU solver in ngspice, available in our
file download branch for
ngspice-43 . To enable KLU, compile ngspice with the configure flag
--enable-klu . The MS Windows build from the distribution has KLU
already enabled.
KLU is now optionally selectable ('option klu' in .spiceinit), then replacing
the venerable Sparse 1.3 matrix solver by the KLU method. It is still
under test, but so far has yielded good results. Your user feedback is welcome!
You will have to create an initialization file .spiceinit (or alternatively called spice.rc) in your HOME directory. It should contain the following lines:
* .spiceinit for use with Skywater PDK and ngspice KLU
set ngbehavior=hsa ; set compatibility for reading PDK libs
set skywaterpdk ; skip some checks for faster lib loading
set ng_nomodcheck ; don't check the model parameters
set num_threads=8 ; CPU processor cores available
option noinit ; don't print operating point data
option klu ; select KLU as matrix solver
optran 0 0 0 100p 2n 0 ; don't use dc operating point, but transient op
set num_threads=8 should be set to the number of physical cores of
the computer in use (here for example 8 cores), set ngbehavior=hsa
will ensure HSPICE compatibility
with some important and essential tweaks for the PDK,
set ng_nomodcheck will suppress some unwanted warnings,
option noinit will suppress the printing of the operating point results.
The calculation of the dc operating point,
delivering the node voltage for starting the transient simulation,
often has caused trouble (long duration, sometimes no convergence etc.).
A new feature in ngspice is the optran method, calculating the
operating point by a distinct transient simulation. The command
optran 0 0 0 100p 2n 0, to be given in .spiceinit, does take care
of this method. 0 0 0 denotes: no initial iteration, no gmin
stepping, no source stepping, 100p 2n 0 then denotes:
use an extra transient simulation with
step size 100 ps and about 20 steps until 2 ns to set up all dc voltages,
without explicitedly setting a voltage ramp. Only after a successful
operating point calculation by optran the normal transient sim is started.
For MS Windows users, a pre-compiled executable of ngspice-43 (including KLU option) is available. Linux or macOS users might apply the compile scripts ./compile_linux.sh or ./compile_macos_gcc.sh from the ngspice top directory of the ngspice-43 tarball to compile an OS specific executable.
After having installed the PDK, you may run the ISCAS85 SkyWater example. Please edit the ngspice input files for a simple inverter and the ISCAS85 C7552_ann and add the correct path to your PDK installation. Simulating the C7552_ann will take a few minutes because it contains 15000 MOS transistors (BSIM4v5 model) and 82000 passives (R and C). Overall speedup of the c7552 simulation is a factor of two, the plain transient simulation time is reduced by a factor of three, when using KLU. And it is now possible to run simulations with 200k transistors. Setup time may be reduced (for experimental purposes) by directly including the model file with .inc, instead of using .lib (see the netlist file).
Please see also SKY130 installation for a detailed description.
In an ongoing development IHP is working towards an Open Source PDK for its 130 nm SG13G2 BiCMOS process. Data are available as IHP Open Source PDK. The process offers bipolar devices with exceptional performance with fT/fmax = 350/450 GHz. ngspice has been selected as the preferred analog simulator. Again here is the ISCAS85 c7552_ann circuit for running a simulation comparison using the IHP PDK. You will need to compile the PSP103.6 nqs model with OpenVAF and load it into ngspice (see chapter 9 of the ngspice manual). Bipolar transistors are modelled with the native ngspice VBIC model.
Google/GlobalFoundries GF180MCU Open Source PDK
Another Open Source PDK has been published in 2022 as the Google/GlobalFoundries PDK for the 180 nm GF180MCU CMOS process from GF. ngspice is supported with parameters for native and high voltrage devices as an analog simulator.
KiCad/ngspice example circuits
KiCad is a powerful frontend to ngspice. It allows schematic entry of your circuit and control of the simulator. More than 35 examples are presented at the KiCad info forum, ranging from audio power amplifiers over power supplies (linear and SMPS) and some miscellanious applications (CMOS, tubes, other).
The ngspice distribution provides a lot of example circuits. These consist of netlists and models and cover various aspects of ngspice analog, digital and mixed signal simulation. They are also a very good study source if you are interested in the ngspice control language.
Device model parameters for simulation
For simulation you need as input the netlist, device model parameters, simulation commands, and out commands. The ngspice distribution does not provide such model parameters, but you may find many of them either in the web or on this web site. The Model Parameter Page does offer some further info and links.
