Why does LTSpice sometimes stop printing midway through a simulation?
LTspice uses a solver that is based on convergence. It also uses a variable time step, meaning the time step is based on accuracy parameters.
If the next time step is not converging it 'backs up' and tries again, to explain this in detail would require a knowledge of numerical methods (of which I only understand the basics). If it fails to converge again and doesnt meet the tolerance requirements it backs up and tries again, which results in the simulation failing to solve for new timesteps.
If you having convergence issues try this (SOURCE: LT spice wiki)

Add a small conductance of 1e10(=10GOhm) parallel to every diode of transistors and diodes.

.options gmin=1e-10   


Increase the allowed tolerance from 1e-12 to 1e-10 for the convergence criteria.

 .options abstol=1e-10  


Increase the allowed tolerance from 0.0001 to 0.003 for the convergence criteria. Never larger than 0.003!

.options reltol=0.003  


Capacitance added from each node to ground. Adding a small CSHUNT to each node can solve some &quot;internal timestep too small&quot; problems caused by high-frequency oscillations or numerical noise. Default = 0.

.options cshunt=1e-15 

Edit:
Odds are the cshunt in conjunction with another resistance in the circuit will create an RC circuit and help to limit bandwidth (its hard if the solver wants to simulate more than GHz of bandwidth because it needs to use lots of time steps). A resistor can help reduce floating nodes or nodes that have high impedance but need to be referenced to ground. Both of these methods truncate numerical errors in the solver and reduce the time it needs to solve. A lot of times adding pFs and Mohms are fine because those values are close to that of air or from plane to plane in FR4. In doing so you simulate parasitics and make the circuit behave more like it would in the real world.
If we did have circuit superconductors and could construct ideal circuit elements it would create a lot of problems, like resonators past the GHz range, in all of our PCB's. The real world isn't like that but LT spice is, unless you watch the parasitics.