Voltage of parallel components (RLC circuit)
SPICE, in general, when no special considerations apply to the simulation card, tries to solve the circuit prior to simulation, i.e. it considers that the circuit has been running since the dawn of time, has had time to settle all the transients, and when the user presses &quot;run&quot;, all that's left is the steady-state.
This is what happened here: you set the simulation card as .tran 10m, which has no special flags or settings, thus LTspice first tried to determine the steady-state before running the simulation.
Since you are interested in the dynamics of the circuit, then you have to tell that to the simulator, since it can't read minds. One of the conditions you mention is that the current source is switched on at t=0. I'll assume that the voltage source is DC only. You could add the uic flag, but that would force V1 to start from zero, too. It's more useful to modify the current source, only.
With these in mind, this is how you can try to model the circuit:

Notice how I've changed I1 to be a step source: PWL(0 0 1u 6). That means at t=0 it's 0, and in the course of 1 us it switches to a 6 A value. You cannot use a zero rise (or fall) time, since that would be a physical impossibility; no simulator would accept that. Those conditions are mathematical abstractions for the easyness of calculation (like the Dirac pulse). That's why there has to be a value for the rising time. There's also no need to exaggerate and make it 1 ps, partly because the differences in the output will be minimal, and also because all the SPICE engines use machine precision (usually double) to crunch numbers, so using extreme differences (1 ps vs fractions of a second time constants) might cause the matrix to be ill-conditioned.
If you say you need a derivative, you can right-click on V(x) in the waveform window and modify it to d(V(x)). Be careful: the waveform compression (default on) will affect the outcome. To turn off waveform compression add this to your schematic (reminder: press S): .opt plotwinsize=0. It will increase the size of the .raw file, but for this case, it shouldn't matter.
One other thing to know is that LTspice adds a default 1 mOhm series resitance to the inductors. This can be set to zero by right-clicking on the inductor and setting Rser=0 (or in the Control Panel &gt; Hacks! &gt; Supply a min. ..., which would make this setting permanent). One of the reasons for this is that many people added a voltage source straight across the inductors and then got voltage loop errors. There are other parasitics that are added behind the scenes, so if you really want to make the LC elements as ideal as possible, right-click on them and set to zero all the fields (except peak current for L, and voltage rating and RMS current rating for C -- thise are decorative, mostly).