Setting up a simulation | InfineonSpice Documentation

Simulations are set up by specifying the desired parameters for them in the Simulation Environment view.

About this task

Setting up a simulation includes specifying the desired result categories, simulation parameters, and output options. While it is possible to run a simulation with default settings, getting the information required in a particular stage of the development usually requires an appropriate setup for the simulation.

Specifying a setup includes entering numerous values. Options for doing so are described in Values and expressions.

Before you begin

The circuit that you want to simulate must be available in the project as a schematic.

Procedure

Open the schematic to be simulated.
The tab displaying it must be the frontmost tab.
In the Simulation Environment view’s Analyses tab, check the areas that the simulation should analyze.

For each of the areas – transients, operating points, DC, AC – a subtab is displayed where you can specify basic settings for the analysis.

These settings are explained in detail in Simulation Environment view.

You can set up multiple analyses at the same time. In that case, running the simulation opens a separate Waveform Viewer window for each specified type of analysis.

Note that an AC analysis requires the power source of the schematic to have an ACM setting.
Specify the desired accuracy and temperature at the bottom of the Analyses tab.

Note that higher accuracy slows down the simulation. What SPICE settings correspond to each choice is displayed when you hover the mouse over the corresponding radio button.
In the Parameters tab, specify the settings for any parameters that you have defined.

Any values that depend on parameters (see Values and expressions) are calculated for the simulation using the parameter settings in this tab.

For example, when a value is specified as 2*baseRate+1 and baseRate is set to 5, the value is 11 during this simulation. If you set baseRate to 5.5, the value calculated from it is 12.

Note that the value assigned to a parameter can be static values or expressions (see Values and expressions) and can include other parameters.
In the Plot Setup tab, specify which voltages and currents are recorded for evaluation.

All

Every voltage or current, including in subcircuits

Top-level

Every voltage or current in the schematic itself, but not those in subcircuits

Signal only

Only voltages or currents on the specified signal

Recording more voltages or currents gives you more flexibility in the evaluation of the simulation, but the simulation takes longer to run.

You can define additional signals in the schematic using the Select Output tools and (standard and differential, respectively). You can also define expressions to plot based on signals by double-clicking the New expression entry, which opens the Expression dialog.

The AC analysis requires special signal setups, as described in Setting up an AC analysis.

If you set up multiple analyses, you can specify the same signal for more than one of them. To do so, add the signal once for each analysis and select the desired type of analysis for each of them in the Analysis column.
From the tab’s Plot Mode list, choose how the simulation results are to be displayed.

This setting determines just the initial display of the results. You can always add, remove, and rearrange plots during evaluation. For details, see Working with plots.
If external libraries for subcircuits in the schematic are required, specify them in the Model Libraries tab.

Enter the path of each library file, either as an absolute path or a relative path.
In the Settings tab, specify how floating nodes are to be handled.

By default, a floating node is handled as if it were connected to ground through a 1 GΩ resistor.
If you want to add custom netlist commands to the simulation, enter them In the Additional Netlist Commands tab.

Any netlist code you enter here is appended to the end of the netlist that InfineonSpice creates for the simulation.

Results

The simulation is now ready to run.

What to do next

You can run the simulation, as described in Running a simulation.