image.png

ngspice does issue this warning

@Rana Muhammad Shahid Jamil @Christoph Maier simulation works if you remove the '`AREA=1`' parameter in diode lines. Try manually editing the

test_diode.spice

file after xschem generates the netlist and before doing the simulation. My understanding is that you should give the layout area of the diode with an AREA parameter, and since the skywater has a

.option scale=1e-6

a value of AREA=1 should correspond to 1um^2 diode. However in model definition default value for area is

area = 1.0e+12

. I don't know what does

1e12

area diode correspond to in physical dimensions. Is it a 1um^2 area? or a 1 square meter (1000000um x 1000000um = 1e12um^2)? @Tim Edwards In order to make simulation produce realistic data i have changed the default AREA to 1e12, same as the default value in model files. Thank you for pointing out this issue.

@Tim Edwards It looks that the AREA parameter in diodes is not scaled by .option scale, Following example...

** test diode scaling with area and .option scale **
.option scale=1
vvcc vcc 0 0.65
d1 vcc 0 D1N4148 area=1
.control
op
print vvcc#branch
quit
.endc

.MODEL D1N4148 D
+ IS = 4.352E-9 N = 1.906 BV = 110 IBV = 0.0001 RS = 0.6458 CJO = 7.048E-13
+ VJ = 0.869 M = 0.03 FC = 0.5 TT = 3.48E-9
.end

...with diode

area=1

and

.option scale=1

yields

-2.24933e-03

diode current. Same example with diode

area=100

and

.option scale=0.1

yields

-2.24933e-01

current. So the diode

area

parameter is taken as an absolute multiplier, not affected by

.option scale

. I don't remember (and i have no more access to) hspice behavior, so i don't know if above behavior is a bug or not.

@Tim Edwards in some hspice slides (i assume here hspice does the right thing, which is of course questionable) it is specified that .option scale should affect diodes too...

I think time has come to file a bug 🙂

I need to carefully write the bug fix requests, ngspice bug tracking is flooded with bugs that are not bugs, like: • ngspice updated the boltzman constant that in recent precise measures is more accurate and different from the k constant used in original spice2 40 years ago. Some users are complaining because they see microvolt differences. I find it very funny that someone asks to use a wrong physical constant (by today measuring standards) just to preserve compatibility with some 40 years old spice implementation. • Some users ask the unary - operator takes precedence over exponentiation, so that -1^2 should get 1 instead of ngspice result of -1. This, also according to operator precedence of mainstream authoritative programming languages is not a bug, ngspice does the right thing. (well,

awk -2^2 -->-4, tcl -2**2 -->4

so best thing to avoid ambiguity is use parenthesis) Anyway, this is the bug report.

By lurking into the code, ngspice has a diosetup.c file where:

...
here->DIOarea = here->DIOarea * scale * scale;
...

So diode should be scaled. Ngspice devs are looking into the issue.

@Rana Muhammad Shahid Jamil @Tim Edwards I have investigated the diode issue. Ngspice does scale diode geometric parameters (area, perimeter) if a

LEVEL=3

is present in the diode model, and we have that level parameter in diode models. I have manually changed the

.option scale=1e-6

to

.option scale=100e-6

in

.../share/pdk/sky130A/libs.tech/ngspice/all.spice

and I/V characteristics of diodes change considerably (bottom picture with .option

scale = 100e-6

show a much lower Vbe for both diodes, since they are now 10000 times bigger). Both simulations below are done with AREA=1e12 set on diode lines:

**.subckt test_diode
I1 net1 0 0
Vk1 net1 K1 0
.save  i(vk1)
D1 0 K1 sky130_fd_pr__diode_pw2nd_05v5 area=1e12
Vk2 net2 K2 0
.save  i(vk2)
D2 0 K2 sky130_fd_pr__diode_pw2nd_11v0 area=1e12
F1 0 net2 vk1 1
.control
save all
dc i1 0 50u 0.1u
plot k1 k2
.endc
.lib /home/schippes/share/pdk/sky130A/libs.tech/ngspice/sky130.lib.spice tt
.end

What is not clear to me is what AREA parameter do i need to specify on diode lines to simulate a 1um^2 diode. From the pictures it seems that AREA=1e12 yields an I/V characteristics that is compatible for a 1um^2 device, although considering the .option scale=1e-6 and AREA=1e12 this would be the specification of a 1 square meter diode.

Also i noticed that ngspice is aligned with HSPICE, from Hspice device models reference manual: Setting Scaling Options ■ Use the SCALE element option to scale LEVEL=2 and LEVEL=3 diode element parameters. ■ Use the SCALM (scale model) option to scale LEVEL=2 and LEVEL=3 diode model parameters. LEVEL=1 does not use SCALE or SCALM. So a diode without LEVEL=2 or LEVEL=3 is not scaled. This is probably to preserve models for discrete devices from unwanted scaling.