(testing it now Pepijn)

yes this .option scale=1e-6 is present in sky130_fd_pr/models/all.spice:

* SKY130 Spice File.
.option scale=1.0u
.include "parameters/lod.spice"
.param
+ lv_dlc_rotweak = .00e-9
+ lvhvt_dlc_rotweak = .00e-9
...
...

@User: SkyWater has a "built-in" ".option scale 1e-6" in the model files for the process, which means that all dimensions are automatically in units of microns; e.g., "w=1" means a 1 micron width. But magic (like a number of tools) wants to output dimensions with a "u" at the end, and scale things to microns itself. My (definitely somewhat kludgy) workaround for this was to multiply the dimensions up by 1E6 in magic, so that "W=1.0E6u" would then come out to 1 micron. My preferred solution is to get rid of the .option scale in the model files, but that's a lot easier said than done. Posted in #sky130

well I tried the treshold test you suggested Pepijn, and changed the scale to 1e3x and 1e6x as big and it doesn't change the output of the calcualation

@User your screenshot reports L=30, W=130 and similar for p-fet, these numbers are too big. there is no model binning for this size.

Yes i tried, you should remove scale and set W and L smaller

I was about to say, remove the scale line and multiply all lengths with 5000e-6, so 130=0.65

Also a question, does ngspice consider first line as comment?

yes 1st line is the circuit title

* Transistor Vth and I-V characteristic .param TEMP=27 .option scale=1E-6 * Include SkyWater sky130 device models .include "sky130_fd_pr/models/r+c/res_typical__cap_typical__lin.spice" .include "sky130_fd_pr/models/r+c/res_typical__cap_typical.spice" .include "sky130_fd_pr/models/corners/tt.spice" * Netlist Description X1 vdd n1 0 0 sky130_fd_pr__nfet_01v8 l=0.13 w=0.195 R1 in n1 55 * DC source for current measure Vin in 0 DC 3.3V Vdd vdd 0 DC 3.3V *simulation commands .op .dc Vdd 0 3.3 0.1 Vin 0 3.3 0.3 .end

i just got an error saying could not find a valid model name

how to give this w and l values as i am using a subcircuit here which taken from the file that was included.

looked into the models of 1.8V cells, Smallest L is 0.15 and smallest W 0.42. For maximum W and L you can use larger values than these specified in the models, up to 99

so that limit we have follow right?

like we have to choose values between lmin and lmax as stated in the models

not sure, i just binary searched for what works.

then how do we get 130nm i.e., 0.13u

nm name is just a marketing thing. in lower processes the difference is even larger

so L=0.15 and W=0.42 doesn't mean 150nm

also notice that in spice is different than channel length, a bit bigger

image.png

@User: Sorry, I've been buried in work and meetings and not tracking this conversation. But: Use "ext2spice lvs" to set various options to a "sane" state. Magic sets ".option scale" by default, but that should not be used with sky130A. I don't exactly have a way for magic to determine that a .option scale is already buried somewhere in the model files. "ext2spice lvs" sets "ext2spice hierarchy on; ext2spice format ngspice; ext2spice scale off" and several others. For the purpose of LVS, it sets the parasitic capacitance threshold to "infinity"; if you want parasitics, I suggest using "ext2spice lvs" anyway and then following that with "ext2spice cthresh <value>", as it is easier to remember that sequence than all of the ext2spice options you would otherwise need to set.

@User: Also use "extract do local" before "extract" to prevent dropping .ext files in the PDK space.

@User: "then how do we get 130nm i.e., 0.13u" : Note that this process is advertised as a "hybrid 180nm / 130nm". A number of aspects are either very close to a 180nm process or somewhere between 180 and 130. The typical minimum length low-voltage transistor is 150nm.

How to resolve "segmentation fault(core dumped problem)" ? as I got it as a result of my ngspice simulation.

@User -- You might want to fix your name appearing being in all capitals in the slack profile, it keeps feeling like someone is shouting your name! :-P

Ok I'll change it.

Probably just noticing it because your name is rather long and you have been active a lot recently....

BTW -- If anyone on the channel is interested in a project, I would love to see test benches for each primitive which confirm the spice simulation gets the same output as the electrical test parameters described in the documentation at https://skywater-pdk.readthedocs.io/en/latest/rules/device-details.html

There are a bunch of potentially interesting spice templates at http://www.idea2ic.com/NGSPICE_TEMPLATES/NGSPICE%20TEMPLATES.html