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.
Several modifiers can be placed on the .tran line.