Circuit stable in the Bode diagram, unstable in step-response
There's a fundamental methodology flaw in your simulation: frequency response in spice works by doing a DC working point analysis (cap open, ind shorted) and then a linearized small signal analysis in frequency domain. This is fine with opamps and properly biased transistors of many kinds. Diodes work 'above the knee'. The basic rule is 'all signals are small amplitude sines' (that's the premise of Bode and 99% of linear system tools)
However you are using a comparator which is a totally not linear device at all. spice decides the output of the comparator at the .op point and then does a linear analysis with that (no idea of what the linear model of a comparator would be). The bode plot became suspicious if not outright wrong.
Even if the lt1216 has a linear model, when used as a comparator it needs a large signal analysis, i.e. a transient simulation.
The kind of circuit you are modeling is actually a switching mode regulator (in hysteretic mode, controlled by the open loop gain of U2). There are actually ways to model it (look for 'average switching mode model'), just not a simple spice frequency analysis.
For educational purposes you could remove the comparator and turn it in a pass linear regulator (which is a mighty fine circuit to design in itself)