The Transient analysis computes the transient output variables as a function of time over a user-specified time interval. An Operating Point analysis is automatically performed prior to a Transient analysis to determine the DC bias of the circuit, unless the UIC option is enabled. All sources which are not time dependent (for example, power supplies) are set to their dc value.

# Description

Enter a brief description of the type of analysis. The text entered is the title of the document in which the simulation results will be stored.

# Analysis Range

## Start Time

Is the initial time. A Transient analysis always begins at time zero. In the time interval between zero and Start Time, the simulator analyzes the circuit but does not store the results.

## Stop Time

Is the final time.

## Max Step Time

Specifies the maximum time interval between two successive simulation steps. Generally it is not necessary to specify this parameter because the algorithm used by the program is sufficiently accurate in the choice of the interval of simulation. In some cases to improve the accuracy of the results it can be necessary to limit the maximum interval of simulation keeping in mind that a smaller interval of simulation will assure a greater precision to expenses of a greater time of simulation; while a greater interval will reduce the accuracy of the simulation and the profile of the signal can be distorted or even omitted.

## Setting parameters automatically

To automatically set the parameters relating to the analysis interval,
click on the **Set Defaults** button. The initial time is set to zero
while the remaining parameters are calculated based on the value of the
frequencies related to the signals of the generators present in the
circuit and the options
**TRANDEFCYCLES** and **TRANPTSXCYCLE**
defined between the options of the simulator. The parameter values are calculated as follows:

Stop Time = (1/freqMin)*TRANDEFCYCLES

Max Step Time = (1/freqMax)/TRANPTSXCYCLE

# UIC

The UIC (Use Initial Conditions) option specified in this box indicates how the initial conditions are to be determined (at time t = 0).
If this box is not checked, an Operating Point analysis is automatically performed before a transient analysis, which determines the initial solution at t = 0.
If this box is checked, the preliminary Operating Point analysis is not performed and the value of each voltage and current is zero except
for those voltages and currents initialized by the IC parameter belonging to the corresponding circuit element or by the instruction **.IC**.
For more information on the initial conditions for transient analysis, see the **.IC** instruction in the Simulator Reference Guide.

# Temperature

Specify the temperature at which the simulation will be performed.

# Fourier

Opens the dialog box where you specify the parameters for Fourier analysis. Specify the fundamental frequency of the signal on which the Fourier decomposition is based and the signals for which the spectral components are desired. Fourier analysis calculates the spectral components of all specified signals.

The Fourier analysis is performed together with the Transient analysis, in fact, considering the periodicity of the signal, the results of the Fourier analysis are calculated based on the results for the last period of the Transient analysis (StopTime-1/freq and StopTime). The vectors whose spectral components are to be calculated are interpolated on a scale corresponding to a period of the fundamental frequency.

In order to have an accurate spectral analysis, the simulation must extend for a number of periods such that the circuit reaches its steady state operation. It may also be convenient to limit the maximum simulation interval by specifying a value for the Max Step Time parameter.

The interpolation function is regulated by the options: **Polynomial degree for interpolation function** and **Number of interpolated points for Fourier analysis**.
The continuous component and the number of harmonics specified by the **Number of harmonics for Fourier analysis** option are calculated.
The numerical format and number of decimal places of the analysis results are defined by the options: **Number of decimal places** and **Numerical format**.

Tip: |
---|

The options can be set in the tab Vectors in the Application properties dialog box. The dialog can be activated by selecting the Settings » Application Properties command or via the key combination CTRL+ALT+A. |

## Output

In the SimResults folder, a document is generated that contains detailed information on the magnitude and phase of each harmonic in the Fourier analysis, for each specified signal.

## Graphic representation of the Fourier analysis

Normally the results of the Fourier analysis are reported in text mode. To obtain a graphical representation, the vectors generated by the analysis must be included in the diagrams. The names of the vectors generated by the Fourier analysis are of the following type: FOUR(signal name)

Perform the following operations in the diagram dialog box:

Set the Plot Type parameter to Comb.

As the scale vector for the X axis, select the

*Frequency*vector containing the frequency scale for Fourier analysis.Add the FOUR(signal name) vector to the list of vectors for the Y-axis.

# Analysis Mode

Specify whether a single or multiple analysis should be performed.
The multiple analysis performs several consecutive simulations, varying the value of some parameters at each step.
When a multiple analysis is selected, the **Setup** button is activated.
Click on the button to activate the dialog in which to set the specific parameters for the selected analysis mode.

The following analysis modes are supported, click a link to learn more about that analysis mode:

# Collect Data For

Specifying the simulation data to be collected. Simulations, especially multiple simulations, can produce a large amount of data, causing excessive memory usage and lower simulation speed. This section allows you to specify which information resulting from the simulation should be stored. Select one of the following options:

**Voltages, Currents, Probes**: Saves data for the voltage at each node and the current in each supply in addition to the signals specified via the Probe objects included in the schematic.**Voltages, Currents**: Saves data for the voltage at each node and the current in each supply;**Signals specified by Probe objects**: Stores only the signals specified via the Probe objects included in the schematic.**The specified signals**: To reduce the amount of data stored during a simulation it may be convenient to specify the names of only the vectors of interest, in this case only the data relating to the specified vectors will be stored. When this option is selected, the**Setup**button is activated; click on the button to activate the Vectors dialog box in which to specify the names of the vectors.

# Options

Click on this button to activate the dialog box in which to set the options of the simulator. The options set are only valid for the current analysis and replace those defined in the general tab of the simulator options.

# Plot

Click on this button to activate the dialog box in which to set the diagrams and the list of vectors to be included in the diagrams. See the Plot dialog box.