Openvaf

OpenVAF + ngspice: Compile and Simulate Verilog-A Models

This skill covers the full flow: write a Verilog-A compact model → compile it with OpenVAF → load the compiled .osdi plugin in ngspice → run simulations.

Scope: What OpenVAF Can and Cannot Compile

OpenVAF implements the analog subset of the Verilog-AMS LRM 2.4.0. It is designed for compact device models (MOSFETs, BJTs, diodes, varactors, resistors, capacitors) — the kind of models that define I-V and C-V relationships.

Supported features

• analog begin / end blocks
• I(), V() branch access, <+ contributions
• ddt(), idt(), idtmod(), ddx()
• $vt, $temperature, $abstime
• @(initial_step), @(final_step)
• $strobe, $display, $bound_step
• limexp(), ln(), exp(), sqrt(), pow(), abs(), min(), max()
• $param_given(), parameter ranges
• Noise: white_noise(), flicker_noise()
• All math from constants.vams

NOT supported (will cause compile errors)

Bottom line: If your .va file uses @(cross), arrays, or genvar, it is a behavioral model and cannot be compiled with OpenVAF. Use a full Verilog-AMS simulator (Cadence AMS, Synopsys HSPICE, Mentor AFS) instead. The veriloga skill covers writing both behavioral blocks and compact models; this skill covers compiling and simulating the compact-model subset.

1. Installation

OpenVAF (the compiler)

Read references/install.md for detailed step-by-step instructions for Windows and Linux. The short version:

1. Download the prebuilt binary from https://openvaf.semimod.de/download/
   • Windows: rename the downloaded file to openvaf.exe
   • Linux: make executable with chmod +x
2. Place on PATH (e.g., C:\tools\ on Windows, /usr/local/bin/ on Linux)
3. Windows only: install Microsoft Visual C++ Build Tools ("Desktop development with C++" workload) — OpenVAF needs the MSVC linker
4. Verify: openvaf --help should print usage info

ngspice (the simulator)

Requires ngspice 39 or later for OSDI support. Read the ngspice skill for general ngspice setup, or see references/install.md for the OSDI-specific parts.

2. The Workflow

  .va file ──→ openvaf ──→ .osdi file ──→ ngspice loads it ──→ simulation

Step 1: Compile

On Linux (or if MSVC is in PATH):

openvaf mymodel.va

On Windows, the MSVC linker environment must be loaded first. Use this one-liner from any shell:

cmd.exe /c "call \"C:\Program Files (x86)\Microsoft Visual Studio\<ver>\BuildTools\VC\Auxiliary\Build\vcvarsall.bat\" x64 >nul 2>&1 & openvaf.exe mymodel.va"

Replace <ver> with your VS version (e.g., 18, 2022). Without this, OpenVAF crashes because it can't find the MSVC link.exe.

Produces mymodel.osdi in the same directory. Compilation typically takes under 1 second for simple models.

Step 2: Write an ngspice netlist that loads the model

* Test circuit for mymodel
V1 in 0 DC 1.0

.control
pre_osdi mymodel.osdi
dc V1 0 5 0.01
plot -i(V1)
.endc

.model m1 mymodel paramA=1.0 paramB=2.0
Nr1 in 0 m1

.end

Step 3: Run

ngspice test.spice

3. Netlist Rules for OSDI Models

These rules are specific to OSDI-loaded models in ngspice. Getting any of them wrong causes cryptic errors.

Rule 1: Use pre_osdi, not osdi

The pre_ prefix tells ngspice to load the model before parsing the netlist. Without it, ngspice won't recognize the model type and will fail.

.control
pre_osdi mymodel.osdi
.endc

Rule 2: Instance names start with N

All OSDI device instances must have names beginning with the letter N:

Nr1 in out mymod            ✓ correct
Nq1 col base emit sub mymod ✓ correct
R1  in out mymod            ✗ wrong — ngspice treats it as a built-in resistor
M1  d g s b mymod           ✗ wrong — ngspice treats it as a built-in MOSFET

Rule 3: .model uses the exact Verilog-A module name

The .model statement must reference the exact module name from the .va source:

// In myresistor.va:
module myresistor(p, n);    // ← this name

.model r1k myresistor r=1000    ✓ matches module name
.model r1k resistor r=1000      ✗ wrong — conflicts with ngspice built-in

Rule 4: Avoid module names that clash with ngspice built-ins

Do NOT name your module resistor, capacitor, inductor, diode, nmos, pmos, npn, pnp, or other ngspice built-in type names. Use a unique name like myresistor, custom_diode, nmos_sq, etc.

Rule 5: Path resolution for .osdi files

For portable projects, keep the .osdi file next to the netlist and use ./.

4. Complete Examples

Example A: Simple resistor

See assets/example_resistor.va and assets/test_resistor.spice for the complete files. This is the simplest possible round-trip: a two-terminal resistor model.

Example B: Square-law MOSFET

See assets/example_mosfet.va and assets/test_mosfet.spice for a basic MOSFET with linear/saturation regions and body effect — demonstrates a 4-terminal device.

Example C: Voltage-dependent capacitor (varactor)

See assets/example_varactor.va and assets/test_varactor.spice for a C(V) model using ddt() — demonstrates dynamic (charge-based) modeling.

5. Troubleshooting

Read references/troubleshooting.md for a comprehensive list. The most common issues:

6. Pre-compiled Model Library

The VA-Models repository provides pre-compiled .osdi files for standard compact models (BSIM-CMG, PSP, HICUM, EKV, MEXTRAM, etc.) for both Windows and Linux, ready for ngspice 39+. Consider using these instead of compiling from source when working with standard models.

Further Reading

• references/install.md — Detailed installation instructions
• references/troubleshooting.md — Extended troubleshooting guide
• references/supported_features.md — Full feature support table
• assets/ — Complete example files ready to compile and run