The way mastercam outputs the toolpaths with the comp options is basically this,
-computer (no comp command, coordinates are tool centreline)
-wear (comp command g41/42, coordinates are also tool centreline, but tool shifts to the proper side by the amount of wear comp in control, usually a very small number), leave the geometry (rad/diameter) column to zero on the control of the machine)
- control (comp command g41/42, outputs coordinates of the geometry, this is used when you are entering the tool radius or diameter (depending on control settings of machine) into the tool geometry, this allows you to change the tool from say 3/4" to 1/2" at the control rather than by changing the toolpath. this can cause issues though if you allow the operator to decide what tool diameter to use. This can also use the wear comp on the machine to make minor adjustments with this method.
You can tell mastercam that the tool is a smaller size to adjust the toolpath with comp set to computer, however the next time you run it with a brand new tool, you might overcut your part.
use wear comp with a lead in motion on the helix and you can make minor adjustments while still retaining the proper programmed coordinates. That is pretty much the industry standard way. Most of my customers use it that way anyways
also one of the previous comments suggested that an option may not be available. That would not matter as you can easily output point to point code that will do the same thing. all the helical or tornado option is, is a macro canned cycle that does the cycle with a one line call. Very nice for when you want to punch a quick hand program on the control, but not necessary when using a CAM system.