< Stefan Schippers> Trying to plot Id Vd curve for NMOS with open-source-silicon.dev #xschem

<@U01819B63HP> Trying to plot Id-Vd curve for NMOS...

vks

05/01/2023, 12:31 PM

@Stefan Schippers Trying to plot Id-Vd curve for NMOS with sweeping Vgs. But not able to plot waveform inside xschem window. Please see attached gif file and suggest what might be wrong here.

nmos.spice screen-capture.webm

Stefan Schippers

05/01/2023, 12:45 PM

The reason is that the circuit is called

nmos.sch

and the raw file is saved as

nmos2.raw

. Save the simulation data as

nmos.raw

. Alteratively give this comand at the xschem console:

xschem raw_read $netlist_dir/nmos2.raw

vks

05/02/2023, 5:37 AM

Hi @Stefan Schippers, raw file was renamed same as schematic file name i.e. nmos but still the issue is persisting. Please check attached gif.

screen-capture (1).webm

Stefan Schippers

05/02/2023, 8:03 AM

Move save and simulation commands inside the .control:

Copy code

.options savecurrents
.control
  save all
  dc Vd 0 1.8 0.1 Vg 0 1.2 0.01
  write nmos.raw
.endc

Stefan Schippers

05/02/2023, 8:09 AM

... or place a

run

instruction into your .control:

Copy code

.save all
.dc Vd 0 1.8 0.1 Vg 0 1.2 0.01
.control
  run
  write nmos.raw
.endc

vks

05/02/2023, 10:01 AM

Thanks @Stefan Schippers, I am able to get plots on xschem window. Little confuse on use of .control block. I have worked on HSPICE and though ngspice is similar; but it's not. Any guidelines how to use .control block?

Stefan Schippers

05/02/2023, 11:01 AM

I think the best source is the ngspice user manual, chapter 17.

Stefan Schippers

05/02/2023, 11:04 AM

ngspice has an interactive mode (the ngspice prompt) where you can write commands to run a simulation, plot results and so on. the .control ... .endc blocks allow to put commands as they were typed on the terminal in interactive mode. ngspice has also a batch mode (

ngspice -b file.cir -r file.raw

) where .control / .endc is not used at atll.

vks

05/02/2023, 11:38 AM

Ok...can you please confirm that netlist syntax for ngspice batch mode will be same or similar to HSPICE batch mode. I believe that ngspice batch mode provides all features as interactive mode.

Stefan Schippers

05/02/2023, 12:24 PM

ngspice netlist is simialr to hspice but not all hspice devices are supported in the exact way. In some cases ngspice has a different equivalent device/syntax. For sky130 the

.spiceinit

file is set to:

set ngbehavior=hsa

to read hspice format .lib files.

27 Views

Open in Slack

Previous Next