LTSpice Simulation Problem - Controlled Rectifier Single Phase Dual Converter
It looks like V2 has the same phase as V1, which is causing the pi/3 overlap.

That aside, a schematic would have been a good idea, to avoid people wishing to simulate it recreating the whole thing. Also, you probably modified your symbol for SCR, because the default one (residing in [Misc]) has A G K as a pin order, so you'd have to modify to .subckt SCR 1 3 2 for it to work. As a side note, it's better to leave Cjo set to something minimal, 0.1p or less, because it helps convergence, and it might also be better to use the LTspice native Vt and Vh for the switch, because then you can make it clear to specify a negative hysteresis (Vt=0.25 Vh=-0.25) which also improves convergence. Just some tips, nothing more.



Edit: Meant to say it but fogot: instead of specifying brute numbers for your commanding sources, it would be better to have them parametrized, what if you need to change the timings? So, something like this would be much better: pulse 0 10 {td1} {1m*T} {1m*T} {Ton} {T} (and td2,3,4), where T=1/60, Ton=200u, td1=T/6, td2=T/2+td1, td3=T/3, td4=T/2+td3, while the rise/fall times are set to 0.1% of T, just enough to not matter, while also large enough to not slow down the simulation, or cause hiccups.