Does the LT Spice monte carlo simulation definitely output the max and min voltage for any number of simulation runs?
A brute force solution can be implemented using the following number system.
This described method will cover the minimum and maximum result.
For example, using a decimal number system, you can specify the tolerance by 10 values.
The number of digits is the number of components you want to vary.

ABCD
0000  all components have their minimum value
0001  
0002
....
0009 components A,B and C have their minimum value and component D its maximum value
....
9999 all components have their maximum value


Now, using the LSpice directive .step param run 0 9999 1 you can use the run parameter to define the value of each component.  

Using floor() you can select the component, e.g. component C is selected by floor(run/10)-floor(run/100)*10.
(Note that the divisors are powers of 10, because a decimal number system is used. For other number systems, corresponding divisors must be used).  

In the decimal number system, we have 10 tolerance values. Spreading them evenly, the digit has to be subtracted and then divided by (10-1)/2. So, digit value "0" gives -1, digit value "9" gives +1.

With these notes, if the value for component B is e.g. 680&Omega; 1% the LTspice resistor value becomes R={ 680 * (1 + 0.01*( floor(run/10)- floor(run/100)*10 -4.5)/4.5 )}

Below is a comparative result. I didn't have the diode, so I left it out.
The first waveform is the total result, the second waveform zoomed in at the maximum values, the third waveform zoomed in at the minimum values, the last waveform is showing the values of the resistors.