pyNgSpice/examples/osdi

A 'quick and dirty' howto for OpenVAF and OSDI:



Example BSIMBULK

Tested under MS Windows 10 and OpenSUSE 15.4



Have OpenVAF compiler available.

    Executables for download are available at https://openvaf.semimod.de/download/

    for Linux and MS Windows.

Download BSIMBULK model from http://www.bsim.berkeley.edu/models/bsimbulk/

Open bsimbulk.va in a text editor

Search for the module name, here: 

    module bsimbulk(d, g, s, b, t);

The module name 'bsimbulk' will become the new model type in the .model statement

    .model mname type ( pname1 = pval1 pname2 = pval2 ... ).

Compile  bsimbulk.va with OpenVAF to obtain bsimbulk.osdi

Put bsimbulk.osdi into directory bsimbulk/osdi_libs

Search for suitable model parameters

    BSIMBULK107 distro does not contain any parameters

    BSIMBULK106 does contain a model parameter file model.l among the benchmark tests

    Put model.l into directory bsimbulk/Modelcards

    Edit model.l:

        Check if model type is 'bsimbulk' (it is already)

        Choose a model name for mname (nch or pch may be o.k., or BSIMBULK_osdi_N or ...)

        There are NMOS and PMOS parameters in the same file here.



Create a ngspice netlist in directory bsimbulk, e.g. bb_IDvsVG.cir.



*** BSIMBULK107 Id versus Vgs ***

* the voltage sources

Vd dd 0 50m

Vg gg 0 1

Vs ss 0 0

Vb bb 0 0



* load the model parameter sets

.include Modelcards/model.l



* the call to the transistor (OSDI devices always start with N !)

NMN1 dd gg ss bb  BSIMBULK_osdi_N W=500n L=90n



* the .control section

.control

* load the model dynamically

pre_osdi osdi_libs/bsimbulk.osdi

* the dc simulation

dc Vg 0 1.5 0.01 Vb 0 -1.6 -0.4

* plotting

set xbrushwidth=3

plot I(Vs)

.endc

.end

*********************************



So we have two OSDI specific actions in the netlist:

load the model by 

    pre_osdi osdi_libs/bsimbulk.osdi

instantiate the transistor by

    NMN1 dd gg ss bb BSIMBULK_osdi_N W=500n L=90n