Verilog-A models in NGspice
Introduction
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:
Translate the Verilog-A code into a .osdi file that can be interpreted by NGspice
Create a component in Qucs-S such that your .osdi model can be used in schematics in the Qucs-S gui
Requirements
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.
Verifying the installation of OpenVAF and Qucs-S
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
Translating the Verilog-A model into an .osdi file
NGspice, and therefore Qucs-S, cannot directly interpret the Verilog-A file. Instead, OpenVAF is used to translate your model into an .osdi file. This can then be referenced in Qucs-S. The steps are as follows:
Make a folder named “\library_prj\” in the Qucs Workspace: “…\Users\$your_username\QucsWorkspace\library_prj\”
Place your “XXXX.va” and spice “.lib” model description file in the folder “…\Users\$your_username\QucsWorkspace\library_prj\”
The folder should contain the two files shown in the picture below
3. Open a terminal in this folder
4. Type the command: “openvaf .\XXXX.va”
5. Success. The folder should now contain a few extra files, among which a “XXXX.osdi” file. See the screenshot below.
6. From now on, we only need the “XXXX.osdi” file and your spice “.lib” model description file. Keep these in the “…\library_prj\” folder.
If step 4 fails due to a linker error, check whether the MSVC build tools were correctly installed (including the “Desktop development with C++” plugin). Otherwise, it can also be that your Verilog-A file contains errors, such as integer parameters initialized as real, or external parameters which are not flagged as such.
You now have an NGspice-compatible model file!
Verifying the .osdi file
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.
Including the model in the Qucs-S GUI
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:
Create a .lib file which describes a spice subcircuit containing 1 instance of the component described by your model
Create a schematic in Qucs-S containing the .lib subcircuit as a spice subcircuit block
Create a symbol from the Qucs-S schematic
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.
- Create a .lib file which describes a spice subcircuit
Again, in the “…\library_prj\” folder, open a text editor and manually write the netlist describing the subcircuit. The only thing this netlist needs to do is make available one instance of your component to higher level schematics. The netlist describing my NMOS component is shown below. Please note:
The order of the terminals of your model file depend on the definition in the Verilog-A file.
In my case, the verilog-A module definition is: “module bsim470sic(drain, gate, source, bulk);”
To find the definition, open the verilog-A file and search for a line with the same format
The “SiC_CMOS_500dC_model_spectreSyntax.lib” file is my “.lib” model description file. It contains a spice model statement describing all the parameters that need to be supplied to the BSIM4SIC model.
In my case, the model statement is: “model BSIM4SIC_n bsim470sic type_spice = 1 version = 4.7.0 param1=2.3 param2= …”
The bsim470sic refers to the Verilog-A module name
The BSIM4SIC_n is the name of the model, and is used in the subcircuit below
You should always use N as a prefix for an instance based on a .osdi model file.
Note the correct syntax for passing a parameter from a higher level schematic to the model: “L = {L} W = {W}”
For more examples on how to place an .osdi instance in a netlist, see the OpenVAF website.
The figure below shows the contents of the “…\library_prj\” folder after the creation of the .lib files. There is a .lib file for both the NMOS and PMOS transistors. Each file describes a subcircuit as can be seen in the netlist above. The unnecessary files generated by OpenVAF have been removed.
2. Create a schematic in Qucs-S
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.
2. In a blank schematic (it should already be open), place a SPICE library device block (can be found under “Components ⇾ file components”)
The SPICE library device block will look like a small blue square, and have a label X1.
3. Double-click the SPICE library device block to configure which files to attach to the block.
Select the “.lib” file from the previous step. It should be located in the “…\library_prj\” folder.
The window will show the contents of the lib file in the bottom right
Select “Automatic symbol” and click “OK” to close the window.
4. Place as many ports as you need and connect them to the SPICE library device block
Give them a name as indicated below. Ensure the names match the port order from the Verilog-A module description. For example, the Source is pin 3 in my Verilog-A file.
Leave the port numbers unchanged, and ensure the port numbers match the pin numbers on the SPICE library device block.
See the figure below on the left as to how the SPICE library device block looks when connected with ports to each of its pins
5. Save the schematic.
The name you give it here will be the name of the component in your component library once the setup is done.
3. Create a symbol in Qucs-S
Right-click on the schematic, and select “Edit Symbol F9”.
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.
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.
Below, you can see the contents of the “…\library_prj\” folder after the schematics and symbols are created and saved. Note that both the schematic and the symbol are saved in the “.sch” file.
4. Create a Qucs-S library component
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”.
The image below shows the contents of the “…\user_lib\” folder after the library has been created. This is the folder where user library components are stored. However, you cannot delete the “…\library_prj\” folder, since its contents are being referenced by the files in the user library.
Note the “SiC_MOSFETS” file, which describes the schematics and symbols of your components. The folder “SiC_MOSFETS” holds the .lib files that link your components to the .osdi file in the “…\library_prj\” folder.
Use your components in schematics
You can now close the project containing your symbols. If you create a new project, you should be able to place your component in a schematic by navigating to “Libraries ⇾ User Libraries”. Below you can see a schematic that uses one of the MOSFETs from my SiC library.
