Simulators are first and foremost, numerical solvers. They only represent reality to the extent that you, the modeler, have created a model that will produce realistic numerical results.
Ground is absolute, so you have to add a GND symbol (net 0) somewhere. Preferably on a common net, so all your voltage measurements are relative to it, without having to connect a pair of wires to read the difference. (In SPICE, there IS such a thing as absolute voltage -- 0 is global ground. In reality, you always need two wires.)
There are two kinds of components, for example: SPICE standard R, L, C are pure abstract components. On the other hand, real components, can be modeled as an infinite network of abstract RLC parts!
How far into that network you go, determines how good (accurate over a given frequency range or time scale) your model will be.
The analyses you will be most interested in, are Transient (the "play" button, or select it from the menu), and AC Steady State.
To use Transient, use pulse signal voltage sources to represent your amplifier's switching output. The rise and fall times will be short, 10ns perhaps. You specify the pulse width (say 0.5us) and period (say 1us, thus giving about 50% duty at 1MHz -- representative enough), and the voltages when 'on' and 'off'. You can also assign an AC Magnitude, which does nothing in Transient.
To use AC Steady State, at least one voltage source has to have an AC Magnitude and Phase assigned (otherwise, they default to zero). This performs an AC frequency sweep, using the assumption that the circuit's DC operating point is linear. (This won't matter, because your network is linear. It does matter for nonlinear circuits, like amplifiers, where the DC condition varies with signal level.) On the sim dialog, enter a range of frequencies, usually a fair amount below and above the cutoff frequency (say, 10k to 100M). You'll want a decade plot with 200-500 points/dec. Go to the "Output" tab and pick a few circuit nodes to plot. (If you haven't named the circuit nodes, they will have default numberings. Hit OK on the dialog and double-click a wire to see what name it has, and set a user-defined name if you like.)
Once you've picked the outputs, press the Simulate button. The graph view will open, and you should see something resembling a lowpass filter.
Note that, since the SPICE components are ideal, your filter will also be ideal. Adding ESR to inductors and capacitors is a good first step. Inductors also have EPR (i.e., a modest sized resistor in parallel) and C, and capacitors have ESL also. A real filter will have many humps and valleys at high frequencies (because real components are complicated); in the simulator, you only get as many humps and valleys as you have reactive (L or C) components.
You can also determine power dissipation. If you do a Transient simulation (from the menu), you can pick outputs. If you write an expression for power (such as VSRC[ i] * V(VSRC), the power generated by a source VSRC), you will get a plot of that. You can do this for sources and loads, and subtract to find the difference: losses.
Tim