Changing parameter values from a value list file in SPICE
Re-reading this now I think I understand what OP wants: to use a custom sequence of numbers that can be used in a .step command. If this is the case, I'll try to answer.
Normally, for a non-linear sequence of numbers that is not logarithmic, the keyword list is used. Unfortunately, it doesn't allow evaluations, i.e. the values must be numeric, {cos(1)} or {2*5} will fail. So about the only solution would be to generate the numbers externally, in a plain text file, as a single line, or as a concatenated line (with +  in front of each new line), and add:
.step param x list &lt;sequence_of_numbers&gt;

at the beginning. This file can then be added to the schematic with the .inc (or .include) command. Don't forget that LTspice XVII sorts the numbers in ascending order prior to simulation start. You may, or may not like it, but that's how it is now. The only way to circumvent this is to use LTspice IV.
To test this, the text file's contents looks like this:
.step param x list 7.254322142991044e-12 2.974321522582202e-10
+ 5.94864415973779e-9 7.733237831307738e-8 7.346575989515156e-7
+ 5.436466237528063e-6 3.261879742903331e-5 1.630939871486926e-4
+ 6.931494453849666e-4   0.02292014166076882 0.05730035415192529
+ 0.1278238669542985 0.2556477339086 0.4601659210354829 0.7477696216826623
+ 1.099661208356858 1.466214944475812 1.774891774891774 1.952380952380952

and the schematic gives this after a .op:

The numbers are some would-be Gaussian bell shape. The output looks like a straight line, but using the View &gt; Mark Data Points shows that the distribution is nonlinear. Using .tran will show different DC levels, as expected.