The small signal(linear) AC analysis of LTspice computes the AC complex node voltages as a function of frequency. First, the DC operating point of the circuit is found. Next, linearized small signal models for all of the nonlinear devices in the circuit are found for this operating point. Finally, using independent voltage and current sources as the driving signal, the resultant linearized circuit is solved in the frequency domain over the specified range of frequencies.
This mode of analysis is useful for filters, networks, stability analyses, and noise considerations. You can find a basic example here.
Syntax: .ac <oct, dec, lin> <Nsteps> <StartFreq> <EndFreq>
.ac list <FirstFreq> [<NextFreq> [<NextFreq> ...]]
The frequency is swept between frequencies StartFreq and EndFreq. The number of steps is defined with the keyword "oct", "dec", or "lin" and Nsteps according to the following table:
| Keyword | Nsteps |
| oct | No. of steps per octave |
| dec | No. of steps per decade |
| lin | Total number of linearly spaced steps between StartFreq and EndFr |
The syntax ".ac list <Freq>" with a single analysis frequency useful in combination with .step. It allows you to plot complex data as a function of a stepped parameter as shown in this example.