LM311 imported from TI spice model has very slow simulation speed. Fast (less accurate) math is checked in options.
https://www.ti.com/lit/zip/slcm011
lm311 test.qsch (14.4 KB)
LM311 TI spice model use transmission line (T-device) as a delay element. This represent signal delay with 125ns. If a circuit with transmission line, simulation timestep will always be forced to at least 50 times less than this delay parameter, i.e. ~2.5ns in this case.
Now, simulate 2ms with 2.5ns timestep, this represents total 800k simulation points and that why simulation force to run slowly.
lm311 test (timestep monitor).qsch (15.3 KB)
A i had a similar problem with a SMPS IC LM5046 it had some odd current source that sharply changed behaviors at a certain voltage and it was borderline unstable i often even had problems with simulation convergence. tho this was in LTspice.
1 Like
I was trying to simulate the oscillator of AADE LC meter. (cant post link but it is a popular design). But the simulation fail to start.
Starting Gmin stepping.
Warning: Gmin stepping failed.
Starting source stepping.
Warning: Source stepping failed at 0.88572(2.27374e-16)
Starting pseudo transient analysis.
ocillator.qsch (17.6 KB)
For oscillator, you better to force an initial condition for its output as oscillator has no steady state stable solution and present a challenge in resolving .op (that why solver fail with Gmin stepping and source stepping etc…)
I changed C1 to speed up the startup of this oscillator (just to get the result faster in this demo).
oscillator(KSK).qsch (22.6 KB)
