I am trying to simulate the resistance of a Pseudo-Resistor, but I keep having convergence problems in NGSPICE. I tried puting some resistor in parallel with my mosfet channels but I still cannot simulate the circuit. I understand the problem is because of the small voltages and current in this block, but anyway, I couldn't figure out a way to simulate this. Anyone can help me? (The simulation is from -0.9 to 0.9V).

Can you please provide the schematic file,

pseudo_tb.sch

and the

pseudo_tb.spice

netlist? Thanks!

Thanks for the anwser. Here they are

I got simulation running with no errors... Just replaced the model .includes with a single line:

.lib /path/to/sky130.lib.spice tt

ensure in the

~/.xschem/simulations/

directory (the directory where netlist is generated) a

.spiceinit

file is present with following lines inside:

set ngbehavior=hsa

set ng_nomodcheck

Also commented out the .options on gmin and itl* and the .nodeset

Thank you very much for your answer, Mr Schippers. The reason you were able to simulate is because you commented the option line that sets gmin. The default value for gmin is 1e-12 which is very high for the simulation I am doing, even if the simulator plots something, because of this gmin the result won't be realistic. The resistance I am trying to simulate has its maximum value around 1e-14, that is why I cannot use the default gmin value. I think a gmin value of 1e-16 would be suitable for this simulation, the problem is that, for some reason, the simulation is not converging. Anyway thanks for your answer, I will keep trying to figure out how to simulate that.

Thank you for the explanation. Yes, using a lower GMIN causes convergence issues. Don't know if this is a simulator issue or a problem with the MOS model equations.

Your workaround sounds good, even though I'm a bit worried of using it, since putting transistors in parallel affects the resistance in a non-linear way in this weak inversion situation. Skywater130 uses the BSIM model which has some known discontinuities in its higher order derivatives (not sure if that is the problem, but, in other pdks, sometimes I had to use the PSP model to simulate transistors in deep weak inversion), but, as far as I know, a PSP model is not available for the SKY130 pdk. Anyway, thank you very much for all your help.