Modeling with a Spice Netlist

This tutorial explores the Spice Netlist block in Simba.

This block allows you to include any SPICE netlist, such as:

• a custom netlist you have previously created,
• a Spice model of a powersemiconductor switch, provided by a manufacturer, for example.

Two cases are considered:

1. Write a Spice netlist from scratch
2. Get a Spice netlist from a manufacturer

For each case, the Simba circuit can be built step by step. I you prefer, the final circuit can be downloaded with the link below:

Download Simba Model of the tutorial

Case #1: Write a Spice netlist from scratch

For this first case, let's consider the circuit below.

It is composed of:

• an AC voltage source of 10 V, 50 Hz,
• a Spice netlist which includes:
• a resistance $R_{load}$ of 1 kΩ,
• a switch controlled by a pulse waveform.

Select Spice Netlist block (#1)

First, select the Spice Netlist block from the library.

Enter Spice Netlist (#1)

Edit the Spice netlist block and enter your spice netlist

✔ Let's start with the power circuit elements:

• the load resistance of 1 kΩ connected between the nodes vdd and n,
• the voltage-controlled switch connected between the nodes n and the ground.

This leads to the following lines:

* Power
Rload vdd n 1k
S4    n 0 in 0 SW_VT

✔ Let's now define the control signal that drives the controlled switch.

This control is defined with a PULSE signal.

which leads to:

Vctrl in 0 PULSE(0 1 5m 1u 1u 20m 40m)

✔ Let's now define the switch model with:

• a on-state resistance of 0.5 Ω,
• a off-state resistance of 1 MΩ,
• a switch voltage threshold of 0.5 V,
• and no hysteresis voltage.

* Options
.model SW_VT SW(Ron=0.5 Roff=1e6 Vt=0.5 Vh=0)

It is possible to define the parameters of a transient analysis.

✔ Finally, let's define the variables to be saved:

• the control voltage,
• the switch voltage,
• and the switch current.

* Scopes
.save V(in,0) V(n,0) I(S4)

Define nodes (#1)

Define the nodes and the scopes of the Spice Netlist block. These nodes will be connected to the other elements of the Simba circuit.

It is also possible to define a list of scope names corresponding to the variables defined in the Spice netlist with the .save directive.

Build Simba circuit (#1)

Let's complete the circuit with a 10 V, 50 Hz AC voltage source and a voltage meter to measure the switch voltage, as shown below:

Simulate & Results (#1)

Once the simulation has been run, the following scopes are available, including the scopes defined in the Spice Netlist block, named N1 here.

The different scopes can be plotted has shown below:

• the AC voltage and the switch voltage in a first graph,
• the switch current in a second graph,
• the switch control voltage ($V_{in}$) in third graph.

Case #2: Get a Spice netlist from a manufacturer

For this second case, let's consider the Spice model of a 1200 V SiC mosfet which has been downloaded on Infineon website.

Select Spice Netlist block (#2)

As illustrated in first step of case #1, select the Spice Netlist block from the library.

Enter Spice Netlist (#2)

Edit the Spice netlist block and paste the spice netlist from the infineon model. The Spice mosfet model from infineon has been defined as a subcircuit using the .subckt directive. Therefore, the nodes that will be connected to this subcircuit must be defined in the main Spice netlist.

Define nodes (#2)

Define the nodes the Spice netlist block which will be connected to the other elements of the Simba circuit.

No scopes are defined in this case.

Build the Simba circuit (#2)

Let's complete the circuit with:

• a 600 V DC voltage source,
• a series resistance of 1Ω,
• a temperature source of 89°C modelled by voltage source connected to the junction temperature pin,
• and a gate driver composed of a 15 V 1 kHz AC voltage source.

Simulate & Results (#2)

Define solver settings (here, a minimum time of 1 µs and an end-time of 50 ms have been chosen), run the simulation and plot results as shown below:

• the $V_{GS}$ voltage in a first graph,
• the current $i_{DS}$ through the mosfet (which has been observed through the resistance $R_1$)

This concludes this tutorial on the Spice netlist block.