Simulator

Eeschema provides an embedded electrical circuit simulator using ngspice as the simulation engine.

When working with the simulator, you may find the official pspice library useful. It contains common symbols used for simulation like voltage/current sources or transistors with pins numbered to match the ngspice node order specification.

There are also a few demo projects to illustrate the simulator capabilities. You will find them in demos/simulation directory.

Assigning models

Before a simulation is launched, components need to have Spice model assigned.

Each component can have only one model assigned, even if component consists of multiple units. In such case, the first unit should have the model specified.

Passive components with reference matching a device type in Spice notation (R** for resistors, C* for capacitors, L** for inductors) will have models assigned implicitly and use the value field to determine their properties.

Spice model information is stored as text in symbol fields, therefore you may either define it in symbol editor or schematics editor. Open symbol properties dialog and click on Edit Spice Model button to open Spice Model Editor dialog.

Spice Model Editor dialog has three tabs corresponding to different model types. There are two options common to all model types:

Disable symbol for simulation

When checked the component is excluded from simulation.

Alternate node sequence

Allows one to override symbol pin to model node mapping. To define a different mapping, specify pin numbers in order expected by the model. ‘Example:’ connections: 1: non-inverting input 2: inverting input 3: positive power supply 4: negative power supply 5: output .subckt tl071 1 2 3 4 5 To match the symbol pins to the Spice model nodes shown above, one needs to use an alternate node sequence option with value: “1 3 5 2 4”. It is a list of pin numbers corresponding to the Spice model nodes order.

Passive

Passive tab allows the user to assign a passive device model (resistor, capacitor or inductor) to a component. It is a rarely used option, as normally passive components have models assigned implicitly, unless component reference does not match the actual device type.

Model

Model tab is used to assign a semiconductor or a complex model defined in an external library file. Spice model libraries are often offered by device manufacturers.

The main text widget displays the selected library file contents. It is a common practice to put models description inside library files, including the node order.

Source

Source tab is used to assign a power or signal source model. There are two sections: DC/AC analysis and Transient analysis. Each defines source parameters for the corresponding simulation type.

Source type option applies to all simulation types.

Refer to the ngspice documentation, chapter 4 (Voltage and Current Sources) for more details about sources.

Spice directives

It is possible to add Spice directives by placing them in text fields on a schematic sheet. This approach is convenient for defining the default simulation type. This functionality is limited to Spice directives starting with a dot (e.g. “.tran 10n 1m”), it is not possible to place additional components using text fields.

Simulation

To launch a simulation, open Spice Simulator dialog by selecting menu Tools→Simulator in the schematics editor window.

The dialog is divided into several sections:

• Toolbar

• Plot panel

• Output console

• Signals list

• Cursors list

• Tune panel

Menu

File

Simulation

View

Toolbar

The top toolbar provides access to the most frequently performed actions.

Plot panel

Visualizes the simulation results as plots. One can have multiple plots opened in separate tabs, but only the active one is updated when a simulation is executed. This way it is possible to compare simulation results for different runs.

Plots might be customized by toggling grid and legend visibility using View menu. When a legend is visible, it can be dragged to change its position.

Plot panel interaction:

• scroll mouse wheel to zoom in/out

• right click to open a context menu to adjust the view

• draw a selection rectangle to zoom in the selected area

• drag a cursor to change its coordinates

Output console

Output console displays messages from the simulator. It is advised to check the console output to verify there are no errors or warnings.

Signals list

Shows the list of signals displayed in the active plot.

Signals list interaction:

• right click to open a context menu to hide signal or toggle cursor

• double click to hide signal

Cursors list

Shows the list of cursors and their coordinates. Each signal may have one cursor displayed. Cursors visibility is set using the Signals list.

Tune panel

Displays components picked with the Tuner tool. Tune panel allows the user to quickly modify component values and observe their influence on the simulation results - every time a component value is changed, the simulation is rerun and plots are updated.

For each component there a few controls associated:

• The top text field sets the maximum component value.

• The middle text field sets the actual component value.

• The bottom text field sets the minimum component value.

• Slider allows the user to modify the component value in a smooth way.

• Save button modifies component value on the schematics to the one selected with the slider.

• X button removes component from the Tune panel and restores its original value.

The three text fields recognize Spice unit prefixes.

Tuner tool

Tuner tool lets the user pick components for tuning.

To select a component for tuning, click on one in the schematics editor when the tool is active. Selected components will appear in the Tune panel. Only passive components might be tuned.

Probe tool

Probe tool provides an user-friendly way of selecting signals for plotting.

To add a signal to plot, click on a corresponding wire in the schematics editor when the tool is active.

Simulation settings

Simulation settings dialog lets the user set the simulation type and parameters. There are four tabs:

• AC

• DC Transfer

• Transient

• Custom

The first three tabs provide forms where simulation parameters might be specified. The last tab allows the user to type in custom Spice directives to set up a simulation. You can find more information about simulation types and parameters in the ngspice documentation, chapter 1.2.

An alternative way to configure a simulation is to type Spice directives into text fields on schematics. Any text field directives related to simulation type are overridden by the settings selected in the dialog. It means that once you start using the simulation dialog, the dialog overriddes the schematics directives until the simulator is reopened.

There are two options common to all simulation types: