Step Subcircuit in LTSpice
It's not officially supported, since LTspice flattens the schematics prior to simulation. That is, all subcircuits, hierarchies, are expanded and flattened to fit in the matrix solver, so if, for example, a second circuit that is stepped doesn't coincide element by element and node by node with the first one, then LTspice may have problems expanding the circuit "mid-flight". 

A minor proof is using any stepped subcircuit and looking at the extended netlist format, in the log, after the simulation. You'll see that the expanded subcircuit is the first one, repeated over all the steps.

But that doesn't mean it's not impossible, only that, if it fails, you shouldn't complain. First, ako only works with models, which are well-defined internally, while subcircuits can have any topology. For this, rename your subcircuits with numerals, 1, 2, 101, etc, so that they can be used with a .step variable. Then you're set, but, again, don't expect miracles. Here's a quick example:



Alternatively, you can use switches and/or resistors that connect the subcircuits to the rest of the schematic, and step their values between 1m and 1g, for example, but that will make all the subcircuits count towards the matrix solver, even if they won't be used.