Did some one got this CACE example running? I tried to run the xschem and got this error:

Error on line:

m.x1.xm20.msky130_fd_pr__pfet_g5v0d10v5 out x1.pdrv1 vdd3v3 vdd3v3 x1.xm20:sky130_fd_pr__pfet_g5v0d10v5__model l= 5.000000000000000e-01 w= 2.000000000000000e+02 nf= 2.000000000000000e+02 ad= 2.900000000000000e+01 as= 2.929000000000000e+01 pd= 2.580000000000000e+02 ps= 2.605800000000000e+02 nrd= 1.450000000000000e-03 nrs= 1.450000000000000e-03 sa= 0.000000000000000e+00 sb= 0.000000000000000e+00 sd= 0.000000000000000e+00 m= 1.000000000000000e+00 could not find a valid modelname Simulation interrupted due to error!

@Or Dicker: How are you running this? Through CACE, or from xschem? It appears that ngspice parded through the first five devices in the netlist and got stuck on XM20 with W=200, which suggests that there is a missing

.spiceinit

file. By default, ngspice uses an interpretation of

W

meaning "width per finger", while the BSIM model documentation says

W

is "total width". The mode that switches between these interpretations is in the

.spiceinit

file. If you are running directly from CACE, it should find that file from the PDK and use it. However, if you just run xschem directly on the schematic, then you'll need to copy the file yourself. It's in

$PDK_ROOT/sky130A/libs.tech/ngspice/spinit

. If you are using defaults in xschem, then it will simulate from

~/.xschem/simulations/

, so copy the file there and rename it from

spinit

to

.spiceinit

.

Hi, I'm trying to run it directly from xschem first. I fixed some path issues and copied all the files(xschemrc, .magicrc, .spiceinit) to the main folder. I ran xschem from the main folder and got the error 😞 How can I debug it?

@Or Dicker: Note what I said above, that unless you configure xschem to run simulations from the local directory, then the

.spiceinit

file needs to be in the directory

~/.xschem/simulations/

, which is where ngspice is launched from. From the error, it is nearly certain that the problem is the lack of the

set ngbehavior=hsa

option, which gets set from

.spiceinit

.

works! thank you!