LTSpice multiple load iteration
The problem with spice is it doesn't work this way, there isn't a good way to change text statements from simulation to simulation (that I know of anyway, I would love for someone to prove me wrong, as it would make my life a little simpler)

There is a way this can be done, is it elegant? Heck no. If you really want to change the way a source behaves, a b-source is the way this is to be done, you can use if statements in b-source blocks. 

You create a parameter that defines the simulation, in this case sim is -1 for the first run and 1 for the second. 

So you say, if first simulation, use a constant 2A (or whatever), on the second simulation, use a different value for current. 

The problem is, you can't insert a PWL statement in an if statement.

I=if(sim&gt;0,2,PWL(0 5 2 0)) &lt;= does not work


but you can insert a different time varying node (either a voltage or current)

I=if(sim&gt;0,2,V(node))


So then you create a voltage pwl and use it's node as the varying current for the second simulation

And there you have it (as pictured below), the red line is the constant 2A (through the R3 resistor) and the pink from the varying PWL in two simulations. You could do this for more than two simulations with nested if statements 



I thought about using variable resistors with if statements, but this will not work with current sources, as they can still source current through any amount of resistance. An approach below would work with voltage sources however.