Can someone please explain why I would get this error when trying to run the simulation on the tb schem? (error in the image attached)

@Tejas Nafde I think your M3 transistor size may be too big.

M3
L=1.5
W=226.45
nf=1

The spice models are bin’ed, which means that they are only valid for certain ranges of parameters. I imagine that this very wide transistor does not match of the bins. For example, the spice models for

pfet_01v8

are in

$PDK_ROOT/$PDK/libs.ref/sky130_fd_pr/spice/sky130_fd_pr__pfet_01v8.pm3.spice

There are over 60 bins - here is a sample with the parameter ranges:

.model sky130_fd_pr__pfet_01v8__model.0 pmos
* DC IV MOS Parameters
+ lmin = 1.45e-07 lmax = 1.55e-07 wmin = 1.255e-06 wmax = 1.265e-6
--
.model sky130_fd_pr__pfet_01v8__model.1 pmos
* DC IV MOS Parameters
+ lmin = 1.45e-07 lmax = 1.55e-07 wmin = 1.675e-06 wmax = 1.685e-6
--
.model sky130_fd_pr__pfet_01v8__model.2 pmos
* DC IV MOS Parameters
+ lmin = 9.95e-07 lmax = 1.005e-06 wmin = 9.95e-07 wmax = 1.005e-6
--
.model sky130_fd_pr__pfet_01v8__model.3 pmos
* DC IV MOS Parameters
+ lmin = 1.995e-06 lmax = 2.005e-06 wmin = 9.95e-07 wmax = 1.005e-6
--

Translating `M3`’s parameter units to the same scale gives

l=1.5e-06 w=2.2645e-04

What you might try is increasing the number of fingers,

nf

. This effectively splits the very wide transistor into multiple thinner transistors in parallel.

@Mitch Bailey that worked, thank you so much! :))