@Stefan Schippers I dont know whats the issue here the testbench is not recognizing the symbol I have created. Can you please help

message has been deleted

Still getting the same error

replace your testbench with this one.

message has been deleted

OK, found the issue. In the same directory where the

rp1-tb.spice

file is located create a

.spiceinit

file with following content:

set ngbehavior=hsa
set ng_nomodcheck 
# set filetype=ascii
set num_threads=4
# set strict_errorhandling=1
set skywaterpdk

This is needed for ngspice to correctly recognize device models.

It works now thank you 🙏

@Jnanapurushothama (cc @Tim Edwards) It appears that

Rp1

is an unfortunate choice for the component name. Looks like there is some

Rp1

definition somewhere in the models and ngspice gets confused. The

set skywaterpdk

will make ngspice work on your example because all parameter references in the circuit must be done with

{param}

and not

param

, so ngspice does not get confused by your subcircuit instance line. But if you rename

Rp1

to something different simulation runs fine even without the

set skywaterpdk

option in the

.spiceinit

file (I added myself this option only recently, it merely speeds up the loading of pdk data).

@Stefan Schippers https://github.com/iic-jku/IIC-OSIC-TOOLS/issues/69 Please report this bug to ngspice too

@Jnanapurushothama for the report above why not just use print?

ngspice 208 -> print @m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[l] = 3.000000e-07
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[w] = 2.000000e-06
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[m] = 1.000000e+00
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[nf] = 1.000000e+00
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[sa] = 0.000000e+00
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[sb] = 0.000000e+00
...
...
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[gmbs] = 1.644872e-05
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[gm] = 1.153455e-04
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[gds] = 1.804085e-06
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[vdsat] = 8.898804e-02
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[vth] = 6.135211e-01
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[id] = 6.617659e-06
...
...
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[vdseff] = 8.776572e-02
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[cgso] = 5.110275e-16
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[cgdo] = 4.998776e-16
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[cgbo] = 2.757858e-21
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[weff] = 1.948000e-06
@m.x2.xm1.msky130_fd_pr__nfet_01v8_lvt[leff] = 2.759500e-07
ngspice 209 ->

Display command used to work properly in previous version unlike now

display

as per ngspice manual does only display the active vectors and types, not their values,

print

does that. If

display

did show values in previous versions it is an undocumented feature.