Simulating large circuits may take an considerable amount of CPU time. If this is of importance, you should compile ngspice with the flags for optimum speed, set during configuring ngspice compilation. Under Linux, MINGW, and CYGWIN you should select the following option to disable the debug mode, which slows down ngspice:

./configure --disable-debug

Adding --disable-debug will set the -O2 optimization flag for compiling and linking.

Under MS Visual Studio, you will have to select the release version, which includes optimization for speed.

If you have selected XSPICE (see Chapt. 12 and II) as part of your compilation configuration (by adding the option --enable-xspice to your ./configure command), the value of trtol (see 15.1.4) is set internally to 1 (instead of default 7) for higher precision if XSPICE code model 'A' devices included in the circuit. This may double or even triple the CPU time needed for any transient simulation, because the amount of time steps and thus iteration steps is more than doubled. For MS Visual Studio compilation there is currently no simple way to exclude XSPICE during compilation.

You may enforce higher speed during XSPICE usage by setting the variable xtrtol in your .spiceinit initialization file or in the .control section in front of the tran command (via set xtrtol=2 using the set command 17.5.63) and override the above trtol reduction. Beware however of precision or convergence issues if you use XSPICE 'A' devices, especially if xtrtol is set to values larger than 2.

If your circuit comprises mostly of MOS transistors, and you have a multi-core processor at hand, you may benefit from OpenMP parallel processing, as described next (16.10).