At the netlist level the Simulation Command is simply a line of text that begins with any of the following Dot Commands:
.tran .ac <oct, dec, lin> <Nsteps> <StartFreq> <EndFreq> .dc .noise .tf .op
At the schematic level these commands may be entered directly as a SPICE Directive (ctrl-right-click on the text to edit) or may be entered via the drop down menu item: Simulate => Edit Simulation Cmd.
|Transient||AC Analysis||DC sweep||Noise||DC Transfer||DC op pnt|
|Various options for the active Tab|
Perform a small signal AC Analysis linearized about the DC Operating Point.
The small signal (linear) ac portion 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.
Syntax: .ac <oct, dec, lin> <Nsteps> <StartFreq> <EndFreq>
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:
|Oct||steps per octave|
|Dec||steps per decade|
|Lin||steps between |
StartFreq and EndFreq