I tried testing all the models listed in the continuous

models_diodes.spice

. The only devices that don't show this behavior are

diode_pd2nw_05v5_esd

,

diode_pd2nw_05v5_esd_v5

,

diode_pw2nd_05v5_esd

, and

diode_pw2nd_05v5_esd_v5

. These are modeled as a diode with a parameter

rs_int

set to 0, its area parameter increased by 54%, and a 1.1101-Ohm resistor on the anode.

rs_int

is used to set the diode model's

rs

parameter, and is by default 600 pOhm for

pd2nw_05v5/11v0

devices and 981 pOhm for

pw2nd_05v5/11v0

devices. Just adding a resistor on the anode isn't enough to eliminate this current noise, so I will try playing with the model parameters.

OKAY. It's related to

rs

. I would need to look deeper into ngspice to understand how the circuit model works.

All the

sky130_fd_pr__diode

models use

rs

scaled down to the pico-Ohm region, except for the

_esd_*

models, which set it equal to zero. This is not typical. Most real diodes have ohmic resistance on the order of 1-1000 mOhms. I created custom diode models in my sky130 install directory to verify that using

rs=0

produces no step-to-step current fluctuations on the anode. Alternatively, using

rs>5e-3

produces current fluctuations at the anode that are of the fA magnitude, which is still usable for simulating high-impedance nodes. I was originally thinking the diode model

rs

parameters were mistakenly given with a factor of `1e-12`~, and should be scaled to Ohms to interact properly with ngspice~. But I don't yet understand where this current fluctuation issue is arising in the simulator. If

rs

is being scaled by 1/area first, then the units start to make sense and there's some other simulation issue related to

rs

that isn't the parameter value itself.

As a follow-up, here are my simulation results with custom diode models based on the ESD devices that change

rs_int = {0*1e-12}

to

rs_int = 600e-3

or

rs_int = 981e-3

and remove the series 1.11-Ohm resistors. These are behaving the way the diode models should behave in reverse bias, but I don't yet have a proposal for a permanent fix.

Ngspice definitely scales

rs

. Forward current at 10uA with

AREA = 1e-12 m

and my modified diode model generates 6MV, so 600 GOhms.

ESR= rs/A

. But this means

rs

must be zeroed out to have reasonable forward-bias behavior without huge reverse-bias current noise on the anode. I will try and track down why non-zero

rs

parameters with these PDK models cause transient noise on a single diode terminal with ngspice. Fortunately, I have loads of time today.

More nuggets to solve the mystery. The issue does not affect anodes at 0 potential. Changing a series voltage source from 0 to +/- 1mV is enough to cause the current fluctuations at the anode again. I haven't yet found relevant code snippets, looking through the ngspice-42 repo. If there are any experts on the simulation theory of operation, I'd be interested to identify the root cause.