open-source-silicon.dev

You need to use an Nfet input diffamp, otherwise `vctrl` can not go high enough to regulate the output pfet.
The following schematic works. Ngspice has some problems at converging in a DC sweep, however a similar transient simulation with a slow ramp on V1 shows correct behavior.
Some notes:
• If you place dummy components in a schematic tie at least one node to a net, like GND. Don't leave all-floating components, as these create a singular matrix and simulators have problems at solving ill-conditioned systems.
• This schematic still exposes M1 and M2 input transistors of the Diffamp to voltages that are greater than 1.8V. If you have a higher reference voltage you can replace these transistors with `nfet_g5v0d10v5.sym`

If I replace the res_xhigh_po_1p41 resistors of the feedback divider with ideal resistances the DC simulation works and shows same results as the transient ramp simulation.

<@U07JY7WG2KH> here the modified circuit. Replaced the current source load with a resistor that gives equivalent current. This makes convergence easier.
Also add the following in your `.spiceinit` file in the directory where ngspice runs (`~/.xschem/simulations`):
`# optran noopiter gminsteps srcsteps tstep tstop supramp`
`optran 0 0 0 100n 10u 0`
This tells ngspice to go directly to optran simulation to find the DC OP of the circuit, skipping OP iterations, gimin stepping, source stepping.
Changes:
• changed corner from tt to tt_mm (Montecarlo variation)
• replaced I load with equivalent resistor
• rewritten mean, variance, distrib procedures
• changed the size of M1 and M2 cascode devices to allowed sizes (circuit won't simulate with the "binned" models (ngspice/ instead of combined/ model dir)

<@U01819B63HP> im going to put this in an IC in upcoming tt-10 along with other blocks im adding. If its ok with you?

<@U07JY7WG2KH> note the `setseed` command in the command block. This can be used to change the random number generator to simulate with a diffferent set of variations.