Verilog-A models in NGspice

As part of my thesis on silicon carbide integrated circuit design, I received transistor models in Verilog-A. Specifically, the transistor behavior was described in a modified version of the BSIM4 MOSFET model. Most SPICE simulators, such as LTspice or NGspice, have support for BSIM3 and BSIM4 transistors, because the BSIM model, which is originally written in Verilog-A, is translated and compiled as part of those spice engines. However, custom Verilog-A component libraries are not compatible with these spice engines. This post describes how I got a Verilog-A model description to work in NGspice.

The transistor models I received consist of two files:

• the BSIM4SIC Verilog-A model file, originally published as part of this publication. The original code is available here.

• the spice “.lib” or  “.mod”  model description file, which contains all the parameters that need to be supplied to the BSIM4SIC model.

Unfortunately, I cannot publicly share the actual Verilog-A model description file or the spice “.lib” model description file, since these are not owned by me. However, the process described below applies to all Verilog-A based models, such as those used for simulation in Cadence Virtuoso Spectre, HSpice or ADS. The BSIM4SIC model is a modified version of the BSIM4 model, although only the original BSIM4 model is natively supported in LTspice or NGspice.

The process will consist of two steps: 

1. Translate the Verilog-A code into a .osdi file that can be interpreted by NGspice

2. Create a component in Qucs-S such that your .osdi model can be used in schematics in the Qucs-S gui

• This tutorial was worked out on an x86 Windows PC

  • It will not work on arm laptops (as of 2025)

  • All the steps described below should also be possible on Linux systems (x86 only)

• You will need to install OpenVAF

  • OpenVAF requires MSVC build tools on Windows, including the “Desktop development with C++” plugin

  • Please read the OpenVAF installation documentation

  • Ensure that you add the OpenVAF executable to PATH

• You will need to install Qucs-S, which automatically includes an up-to-date NGspice installation

• Of course, you also need your Verilog-A model file and spice “.lib” model description file.

Before starting the whole process, we should verify whether all the programs are correctly installed. Open a terminal in any location, and type “openvaf --help”. If you receive the OpenVAF documentation, the installation was successful. Otherwise, ensure that the openvaf executable is added to your PATH.

Next, check whether the following folder exists: “…\Users\$your_username\QucsWorkspace\”

Additionally, you can add the NGspice executable (located in: “Program Files\Qucs-S\bin\”) to your PATH by editing the windows system variables. However, it is not a requirement

This step is optional. If NGspice is added to path, you can open an NGspice console in the “…\library_prj\” folder, and verify whether you can load your model using “.model” and pre_osdi statements. Examples on how to write a short NGspice netlist can be found on the OpenVAF website.

The crucial and difficult part is over, now starts the tedious and annoying part. Unfortunately, Qucs-S does not have an easy to follow .osdi model import wizard. However, we want to be able to use your model as a component in circuits. So the model needs to have a symbol. And when the symbol is placed in a schematic, it should simulate as expected. 

Therefore, I created the following workflow to import .osdi models as library components:

1. Create a .lib file which describes a spice subcircuit containing 1 instance of the component described by your model

2. Create a schematic in Qucs-S containing the .lib subcircuit as a spice subcircuit block

3. Create a symbol from the Qucs-S schematic

4. Create a Qucs-S library component from the schematic and symbol from step 2 and 3.

In my case, the component will have externally defined parameters for the length and width of my MOSFET. Additionally, I have to do the process for both the NMOS and PMOS variants.

1. Open Qucs-S and double-click “Projects ⇾ library_prj” to open the Library project. The files in this project will be the reference for the symbol of your component. If the project is opened, you will be forwarded to the “Content” tab.

1. Right-click on the schematic, and select “Edit Symbol F9”.

2. Draw the symbol as you like

•  Ensure the ports are placed on the symbol where you want them, since this is where wires connect in higher level schematics.

• Note that the empty symbol starts with a blue box. Remove it, since it can be interpreted as a wire connection in a higher level schematic.

3. double-click on the “SUB” to change the properties of the symbol

• Replace SUB with a more descriptive prefix of the symbol. I replaced SUB with NMOS.

• If you have parameters that need to be passed to your model, enter them here. Include a Default Value, Description, and Type (unit) if preferred.

Verify that all your desired components have a schematic within the project you created. For example, I want to include both a symbol for an NMOS transistor and for a PMOS transistor.

Then, navigate to “Projects ⇾ Create library”. Follow the steps until you can click “Create”.