How to use .step param with more than two parameters in LTSpiceIV
In LTSpice the table command really creates a kind of dictionary where you have to specify key value pairs. The proper directive for your case would then be:

.step param Rx list 1 2 3
.param R1 table(Rx,1,1k,2,1Meg,3,1k)
.param R2 table(Rx,1,10k,2,1Meg,3,10Meg)


and set the value of the resistors to {R1} and {R2} respectively.

If you want to have the values of a resistor near to it, you can also enter (instead of value, when right clicking onto it)

R=table(Rx,1,10k,2,1Meg,3,10Meg)


into the resistor value field. This works the same way for all kinds of components and with an external script to create .asc files it can be used as a crutch for LTspices missing monte carlo functonality.