First and foremost: SPICE is a numeric solver and all its models only approximate their real life counterparts, if modelled. What you have there is a MESFET which can only try to come close to some real-life counterpart, but who has two of the parameters null, and a bunch of LC filters that, most likely, have no parasitics modelled/added.
Next are the values:
ms simulation time. Now, that's not a problem in itself, you can simulate until the end of time, but it's about the dynamic range involved. You have time constants there that are many magnitudes smaller than the simulation time, and an imposed timestep of
1 ns, which is comparable to the LC values:
At this point, I have to ask: what is your purpose when simulating this circuit? I see no
uic, no initial conditions, and all the sources are DC. Yet you are simulating a heavily filtered circuit. If the operating point is what interests you,
.OP will do. If a dynamic behaviour is what you're after, then DC sources can hardly be called dynamic.
At any rate, if accuracy is needed, then you need some
1k ... 10k times less time resolution, at least. That means
2.5 ps ... 0.25 ps or less. Are you sure you want to simulate for
10 ms like this?
Why do those oscillations appear? Numerical accuracy, and chaos. Think Lorentz attractor. You have complex feedback in a very complex schematic (transfer function wise). Combine that with nonlinear elements and you get a possible oscillator. Use them with a very linear (and quite ideal) LC network and you get a simulation that can go fast, unless a timestep is imposed -- in this case,
1n is not enough. All you have to do is run the circuit for long enough.
As for the various solvers, the two main contenders are gear and trapezoidal. Gear typically has very strong damping, and it's used where parasitic oscillations are of not needed. It will damp even your ideal LC oscillator. It's inherently stable, which means using it to simulate oscillators is not such a good idea. Maybe switching applications, if transients are of no importance. Trapezoidal is meant to try to reproduce as accurately as possible for a 2nd degree implicit solver, even at the cost of oscillations. And these will come if proper conditions exist: a high order LC network, multiple feedback paths, an uncontrolled timestep, these can contribute.
But, again, your circuit doesn't make sense to be simulated for
10 ms with DC sources. Either choose
.DC, or use other types of sources that add some dynamics and make sense for choosing
PS: I didn't try to reproduce manually your schmatic. If you can post the source, I'll give it a try, but you have to say first what is the purpose of the simulation.