.TRAN -- Perform a Nonlinear Transient Analysis

Perform a transient analysis. This is the most direct simulation of a circuit. It basically computes what happens when the circuit is powered up. Test signals are often applied as independent sources.

Syntax: .TRAN <Tstep> <Tstop> [Tstart [dTmax]] [modifiers]
        .TRAN <Tstop> [modifiers]

The first form is the traditional .tran SPICE command. Tstep is the plotting increment for the waveforms but is also used as an initial step-size guess. LTspice uses waveform compression, so this parameter is of little value and can be omitted or set to zero. Tstop is the duration of the simulation. Transient analyses always start at time equal to zero. However, if Tstart is specified, the waveform data between zero and Tstart is not saved. This is a means of managing the size of waveform files by allowing startup transients to be ignored. The final parameter dTmax, is the maximum time step to take while integrating the circuit equations. If Tstart or dTmax is specified, Tstep must be specified.

Supported modifiers that can be placed on the .tran line:

startup: Solve the initial operating point with independent voltage and current sources at global scope turned off. Then start the transient analysis and turn these sources on over the first 20μs of the simulation.

UIC: Skip the D.C. operating solution.

steady: Stop the simulation when steady state has been reached. Steady state detection is written into the SMPS macromodels. If the circuit contains a signal voltage source and current source these will be identified as the input and output respectively and the efficiency will be computed.

nodiscard: Don't delete the part of the transient simulation before steady state is reached.

step: Compute the step response of the circuit. Requires a SMPS macromodel that include steady state detection and a stepped load current.