SpiceBind

SpiceBind is a lightweight bridge that enables co-simulation of analog ngspice circuits alongside HDL simulators. This tool allows design engineers to seamlessly integrate SPICE-accurate analog models into their existing digital verification flows.

⚠️ Note: This is an early release. We welcome feedback and contributions from the community.

Key Benefits

• Preserve Your Existing Flow: Keep your RTL, testbenches, and waveform viewers unchanged
• SPICE Accuracy: Replace any module with a SPICE-based analog model for accurate analog simulation
• Unified Timeline: Analog and digital domains run in synchronization
• Zero Vendor Lock-in: Works with open-source tools like Icarus Verilog up to commercial simulators (to be tested)
• Verification Ready: Compatible with cocotb for Python-based verification

Use Cases

Perfect for ASIC designers working on:

• Mixed-signal SoCs with analog IP blocks
• ADCs, DACs, and data converters
• PLLs, oscillators, and clock generation circuits
• Power management units
• Sensor interfaces and analog front-ends

How It Works

SpiceBind enables you to write Verilog source code that includes an empty Verilog module and have it implemented by ngspice. Here's how the magic happens:

The Process

1. Create a Verilog Module Shell: Write a Verilog module with the desired interface (inputs and outputs). The module body can be empty - it will be implemented in SPICE.

2. Design the SPICE Implementation: Create a corresponding SPICE netlist that implements the analog behavior of your module.

3. Name-Based Connection:

   • Verilog input ports appear in the SPICE circuit as external voltage sources
   • Selected SPICE circuit nodes drive the Verilog output ports
   • Connections are established by matching names between Verilog ports and SPICE nodes

4. VPI Integration: A VPI (Verilog Procedural Interface) module links to ngspice's shared library, enabling communication between the digital simulator and the analog engine.

Example Flow

Verilog: input real vin    →    SPICE: Vvin external_node 0 0 external
Verilog: output [3:0] code ←    SPICE: circuit nodes code[3], code[2], code[1], code[0]

During simulation, the VPI module:

• Reads values from Verilog input ports and sets corresponding SPICE voltage sources
• Runs SPICE analysis for the current time step
• Reads SPICE node voltages and drives corresponding Verilog output ports

This creates a co-simulation where analog and digital domains remain synchronized on a unified timeline.

Installation

Prerequisites

• C++ compiler with C++17 support
• ngspice library and development headers
• Verilog VPI compatible simulator (tested with Icarus Verilog)
• Python 3.6+ (optional)

Build Instructions

Clone the repository:

git clone https://github.com/themperek/spicebind.git
cd spicebind

Option 1: Standalone VPI Module

mkdir build && cd build
cmake ..
cmake --build .
cmake --build . --target debug  # Optional: builds debug version

Option 2: Python Integration

pip install -e .

Quick Start

1. Define Your Analog Block

Create a Verilog module with matching SPICE netlist with external voltage sources and ouptut ports.

Verilog module (e.g., adc.v):

module adc(
    input  real vin,
    output reg [3:0] code
);
endmodule

SPICE netlist (e.g., adc.cir):

* External voltage source for input
Vvin adc_in 0 0 external

* ADC subcircuit instantiation
Xadc adc_in code[3] code[2] code[1] code[0] sar_adc

* Simulation settings
.tran 1ns 1

2. Configure Environment

Set the required environment variables:

export SPICE_NETLIST=adc.cir
export HDL_INSTANCE=tb.adc
export VCC=3.3

3. Run Simulation

For Icarus Verilog:

vvp -M $(spicebind-vpi-path) -m spicebind_vpi tb.vvp

See the examples/ directory for complete working examples.

Multiple Instance Support

For designs with multiple analog blocks, configure each instance in your SPICE netlist with full hierarchical paths:

SPICE netlist:

* First ADC instance
Vtb.adc.vin vin 0 0 external
Xadc vin tb.adc.code[3] tb.adc.code[2] tb.adc.code[1] tb.adc.code[0] sar_adc

* Inverter instance
Vtb.inv.A inv_a 0 0 external
Xinv inv_a tb.inv.Y inv

.tran 1ns 1

Environment configuration:

export HDL_INSTANCE=tb.adc,tb.inv

Configuration Options

• SPICE_NETLIST: Path to your SPICE netlist file
• HDL_INSTANCE: Comma-separated list of HDL instance paths
• VCC: Supply voltage for analog simulation
• Additional options available in the documentation

Documentation

For detailed documentation, examples, and API reference, visit: https://themperek.github.io/spicebind/

Contributing

We welcome contributions! Please see our contributing guidelines and feel free to:

• Report bugs and request features via GitHub Issues
• Submit pull requests for improvements
• Share your use cases and examples

Roadmap

• Enhanced testing and validation
• Bidirectional bus support
• Automatic SPICE wrapper generation