PNP model is missing to run test_bandgap.

I believe Stefan's xschemrc files points to the combined models by default, which don't seem to have the bjt models? If you modify these lines the xscehmrc file, it should run

set SKYWATER_MODELS ${PDK_ROOT}/${PDK}/libs.tech/ngspice

#set SKYWATER_MODELS ${PDK_ROOT}/${PDK}/libs.tech/combined

The combined models have changed the transistor subcircuit definition from a 3 pin device (

c, b, e

) to a 4 pin device (

c, b, e, s

) If you manually edit the netlist and find the

XQ

device instances, add a '`0`' (ground) as 4th pin, simulation should run. I will wait for @Tim Edwards advice for this. If we plan to move on 4 pin bjt for pnp I will update the symbol and add the substrate pin. Old binned models:

.subckt  sky130_fd_pr__pnp_05v5_W0p68L0p68 Collector Base Emitter  mult = 1.0

New 'combined models:

.subckt  sky130_fd_pr__pnp_05v5_W3p40L3p40 c b e s mult=1

@Stefan Schippers: Thanks for pointing this out. I had not noticed the change in the bipolar definition. I think that even if a PNP is placed in a deep nwell structure, the "substrate" terminal is still the p-well and not the (global) substrate. I do not think there is any way to separate the substrate terminal from the collector. So my opinion is that the best solution is to just change the subcircuit definition back to a 3-terminal device (it can call the BJT model with

c b e c

instead of

c b e s

).

Ok, Thanks. so I will leave the symbol as it is (so it won't break existing designs 🙂 )

Thanks all! 👍

@Stephen, @Stefan Schippers: I just pushed an update to the

sky130_fd_pr

library. This (I hope) fixes the bipolar problem by removing the substrate terminal from the two PNP devices. I also made an update to the older models to add subcircuit definitions for the diodes so that they become forwards-compatible with the continuous models, which only have the subcircuit definitions. Now I only need to figure out what needs to be done about the subthreshold parameters for the pFET devices. . .