This pane allows you to define the various defaults for LTspice. These defaults can be overridden in any simulation by specifying the options in that simulation. Usually you can leave these options as they are. If you have frequently updated the program over the web, you might want to press "Reset to Default Values" to reset to the current recommended settings.
One default you may want to change is Trtol. Most commercial SPICE programs default this to 7. In LTspice this defaults to 1 so that simulations using the SMPS macromodels are less likely to show any simulation artifacts in their waveforms. Trtol more affects the timestep strategy than directly affects the accuracy of the simulation. For transistor-level simulations, a value larger than 1 is usually a better overall solution. You might find that you get a speed of 2x if you increase trtol with out adversely affecting simulation accuracy. Your trtol is remembered between program invocations. However, most of the traditional SPICE tolerance parameters, gmin, abstol, reltol, chgtol, vntol are not remembered between program invocations. If you want to use something other than the default values, you will have to write a .option statement specifying the values you want to use and place it on the schematic or keep the settings in a file and .inc that file.
Also interesting is which solver is used. LTspice contains two complete versions of SPICE. One is called the normal solver and the other is called the alternate solver. The alternate solver uses a different sparse matrix package with reduced roundoff error. Typically the alternate solver will simulate at half the speed of the normal solver but with one thousand times more internal accuracy. This can be a useful diagnostic to have available. There is no .option to specify which solver is used, the choice must be made before the netlist is parsed because the two solvers use different parsers.
Check the box next to "Accept 3K4 as 3.4K" to force LTspice to understand a number written as 4K99 to be equal to 4.99K. Normal SPICE practice does not allow this, but it is available in LTspice by popular request.