For Spectre / ngspice Users¶

This guide maps familiar SPICE simulator concepts to VAJAX equivalents.

Analysis Types¶

Spectre	ngspice	VAJAX	Status
`.tran`	`.tran`	`engine.run_transient()`	Available
`.ac`	`.ac`	`engine.run_ac()`	Available
`.noise`	`.noise`	`engine.run_noise()`	Available
`.dc`	`.dc`	`engine.run_dc_sweep()`	Coming soon
`.op`	`.op`	Internal (computed automatically)	Available
`dcinc`	-	`engine.run_dcinc()`	Available
`dcxf` / `xf`	-	`engine.run_dcxf()`	Available
`acxf` / `xf`	-	`engine.run_acxf()`	Available
Corner / Monte Carlo	-	`engine.run_corners()`	Available (PVT sweep)

Netlist Conversion¶

VAJAX can convert netlists from ngspice, HSPICE, LTspice, and Spectre formats:

# Convert a Spectre netlist
vajax convert input.scs output.sim --dialect spectre

# Convert an ngspice netlist (default dialect)
vajax convert input.sp output.sim

# Other dialects
vajax convert input.sp output.sim --dialect hspice
vajax convert input.sp output.sim --dialect ltspice

What Gets Converted¶

Instance statements (resistors, capacitors, transistors, subcircuit calls)
Model definitions and parameters
Subcircuit definitions with parameters
.lib "file" section library inclusion
SI prefix notation (1k, 1u, 1n, 1p, etc.)
Analysis statements (.tran, .ac)

Spectre-Specific Features¶

The Spectre dialect handles: - library ... section ... endsection ... endlibrary blocks - Statistics blocks (statistics { process { ... } mismatch { ... } }) - Spectre instance syntax (name (nodes) model param=value) - Spectre SI prefixes (e.g., M for milli vs Meg for mega)

Known Limitations¶

Some advanced Spectre features (ocean scripts, Maestro setup) are not converted
Mixed-signal (Verilog-AMS) wrappers are not supported
Conversion may require manual review for complex designs

Device Models¶

VAJAX supports Verilog-A compact models compiled at runtime via OpenVAF. If your PDK provides Verilog-A sources (most modern PDKs do), VAJAX can use them directly.

Bundled Models¶

Model	Type	Notes
`resistor`	R	SPICE resistor with temperature coefficients
`capacitor`	C	Ideal capacitor
`inductor`	L	Ideal inductor
`diode`	D	SPICE diode model
`psp103`	MOSFET	PSP103 production MOSFET
`bsimbulk`	MOSFET	BSIM-BULK 106
`bsimcmg`	MOSFET	BSIM-CMG (FinFET)
`bsimimg`	MOSFET	BSIM-IMG (FD-SOI)
`ekv`	MOSFET	EKV model
`hisim2`	MOSFET	HiSIM2
`asmhemt`	HEMT	ASM-HEMT
`mvsg_cmc`	HEMT	MVSG CMC

Using Your PDK Models¶

To use a custom Verilog-A model, reference it in your netlist with a load statement:

load "path/to/your_model.va"
model mymod your_model_module_name (param1=value1 ...)

The load path is resolved relative to the netlist file location.

Output Formats¶

Format	Command	Compatible With
Raw (binary)	`vajax circuit.sim -o results.raw`	ngspice, gwave
CSV	`vajax circuit.sim -o results.csv --format csv`	Excel, Python
JSON	`vajax circuit.sim -o results.json --format json`	Custom tools

The default .raw format is binary-compatible with ngspice, so you can view waveforms using ngspice's built-in plotter or external viewers like gwave.

Key Differences from Spectre¶

No GUI — VAJAX is a command-line and Python API tool. Use matplotlib for plotting, or export .raw files to your preferred waveform viewer.
GPU acceleration — Large circuits (1000+ nodes) benefit significantly from GPU acceleration. Use engine.prepare(use_sparse=True) for circuits over ~1000 nodes.
JAX backend — Jacobians are computed via automatic differentiation rather than hand-coded derivatives. This means any Verilog-A model works without modification.
Python-first API — While the CLI works for simple runs, the Python API gives you full control over simulation setup and post-processing.

Quick Example: Spectre to VAJAX¶

Spectre netlist (amp.scs):

// Simple common-source amplifier
simulator lang=spectre

include "pdk_models.scs" section=tt

subckt cs_amp (out in vdd vss)
  M0 (out in vss vss) nmos w=10u l=0.18u
  M1 (out bias vdd vdd) pmos w=20u l=0.18u
  R0 (vdd bias) resistor r=10k
ends cs_amp

I0 (out in vdd vss) cs_amp
V0 (vdd 0) vsource dc=1.8
V1 (in 0) vsource dc=0.9

myac ac freq=1k stop=1G dec=100

Convert and run:

# Convert to VAJAX format
vajax convert amp.scs amp.sim --dialect spectre

# Run the simulation
vajax amp.sim -o amp.raw

Or use the Python API:

from vajax import CircuitEngine

engine = CircuitEngine("amp.sim")
engine.parse()

# AC analysis
ac_result = engine.run_ac(
    freq_start=1e3,
    freq_stop=1e9,
    mode='dec',
    points=100,
)