I have updated `open_pdks` now to enable both mism...
# analog-design
I have updated
now to enable both mismatch and process variation statistical analysis for sky130. The major change for the end-user is that ngspice testbenches will require the line
.param mc_mm_switch=0
.param mc_mm_switch=1
at the top to disable or enable device mismatch. Process variation is enabled by a corner-model-like specification using
.lib _<path>_/sky130.lib.spice mc
and then requires
.option SEED=random
.option SEED=_<value>_
to ensure that every run of ngspice will produce another set of random parameter values.
πŸ™Œ 2
πŸŽ‰ 2
πŸ‘ 1
What's the difference between the
choice and other choices like
, etc.?
means "monte carlo". Instead of values being tuned to a specific process corner like
, all the process variables are randomized with a normal distribution. With
you will get a different set of parameters every time you do a run. So you can do 1,000 simulations and get a statistical distribution of circuit behavior over a statistically significant set of possible process runs. Since it is hard, with a random distribution or in real life, for all variables to be at extremes, the monte carlo distributions tend to be less severe than the process corners, and so are more representative of real circuit behavior from a real fabrication run.
I selected the
library and when trying to simulate a design with
, I get the following error:
Copy code
Error: unknown subckt: x0.x10 x0.amplifier_0/vq x0.amplifier_0/vx 0 0 x0.0.0+mc_pr_switch*agauss 0 x0.1.0 x0.1 <http://x0.ad|x0.ad>=5.6e+11p x0.pd=4.00207e+06u as=7.38427e+12p ps=4.18992e+07u w=2e+06u l=2e+06u
    Simulation interrupted due to error!
The subckt should be:
Copy code
X10 amplifier_0/Vq amplifier_0/Vx GND GND sky130_fd_pr__nfet_01v8_lvt ad=5.6e+11p pd=4.00207e+06u as=7.38427e+12p ps=4.18992e+07u w=2e+06u l=2e+06u
It looks like
was replaced with
0.0 + MC_PR_SWITCH*AGAUSS(0,1.0,1)
. I checked
and saw there's a
.param sky130_fd_pr__nfet_01v8_lvt = 0.0 + MC_PR_SWITCH*AGAUSS(0,1.0,1)
. I saw in the commented out section a corresponding
vary sky130_fd_pr__nfet_01v8_lvt dist=gauss std=1.0
. The latter format looks like it's for a different SPICE simulator, so do I need the
.param sky130_fd_pr__nfet_01v8_lvt = 0.0 + MC_PR_SWITCH*AGAUSS(0,1.0,1)
at all? I tried commenting that line out and saw that it's referenced by other .param statements, so it's gotta be there. My model names in the .spice aren't in quotes or braces, so I'm confused as to why the substitution of
.param sky130_fd_pr__nfet_01v8_lvt = 0.0 + MC_PR_SWITCH*AGAUSS(0,1.0,1)
is happening in the first place.
I noticed the collision between the parameter names and the device names and since that was true of the original SkyWater decks I assumed it would not be an issue. It could be that ngspice is treating the parameter by doing a wholesale search-and-replace, which would be an incorrect implementation, but would match what you're seeing.
I can confirm this error, which looks like an issue with the way ngspice handles parameters. Not sure whether it should be called a "bug" or an "incompatibility". If there's a limited number of such conflicting parameter names in the PDK, then I can probably just make a list of them and fix them with yet another patch script.
I think there's a limited number of conflicts. It looks like model names appear throughout lines 51 to 68 of
Now I have two mysteries, because some of those entries add in the random variable twice, which looks like a parsing error in my patch script.
Those parameters don't even appear to exist anywhere else. . . it's like they were put there to screw up ngspice.
🀣 1
A nice little surprise
After spending much more of the day than I intended on this problem, open_pdks now converts the offending parameter names, and I confirmed that it works with the
device now. The list of parameter names to correct was hand-compiled from inspecting the file, but I think it's comprehensive.
πŸ™Œ 1
That's awesome. Thanks so much Tim!!!
Sorry it took more time than you'd hope...