Verilog-A Compilation

Once OpenVAF is installed, compilation of Verilog-A models to an OSDI library suitable for circuit simulation is easy. Simply run

openvaf <file>.va

in a terminal and the compilation should complete quickly. OpenVAF offers options which are displayed when executing openvaf --help, but these won't usually be required.

If there are no errors in the Verilog-A source, a file called <file>.osdi will be generated that can be used by circuit simulators that implement the OSDI interface, such as Ngspice.

Ngspice Integration

Loading OSDI Files

Once you have a compiled an OSDI file as described above, it can be loaded by Ngspice using a simple Ngspice simulator command.

osdi <path>.osdi

To load a model in a netlist, one must add pre to the osdi command for ensuring that the model is loaded before the netlist is resolved:

pre_osdi <file>.osdi
*other control commands
  • The path to the file can be an absolute path like /home/folder/example.osdi.
  • The path can be a relative path like folder/example.osdi, it is then resolved in the netlist directory.
  • You can also omit the path and just write example.osdi if the file is located in the lib/ngspice directory. To activate this feature you must comment out unset osdi_enabled in share/ngspice/scripts/spinit . This method is recommended if you want to make this model permanently available to Ngspice.

Using Verilog-A Modules

Once an OSDI file has been loaded, Verilog-A modules can be initiated in a netlist as shown below. Note that the N prefix of the device name is important for ensuring correct behavior.

.model <model name> <Verilog-A module name> <model parameters>*

N<instance name> <nodes>* <model name> <instance parameters>*

A minimal example netlist that creates a single instance of the HICUM/L2 model is shown below. Further examples can be found here.

OSDI Example

.model hicum_model hicuml2va c10=1e-30

N1 C B E S hicum_model

pre_osdi hicumL2V3p0p0.osdi