What takes precedence? 

Using the NFS wizards for drilling some holes, it didn't seem to matter what R value I entered, it always wanted to retract 0.1".  Do I need to go the the "Mill Options" and "General Options" and adjust this value to change what Mach 3 is going to use?

I've found that G73 Pullback IS governed by the setting in Mill Options and it is only intended to break the chip, not retract clear of the hole.
Perhaps you should use G83 which is used to retract clear of the hole to clear the chips. There is an option in the Circular Hole Pattern wizard.
RC

EDIT:  Just noticed you said NFS....but it has the option as well.

Ok, I think I was confusing the R value in the G73 code with the retraction distance.  The R value is the safe starting distance above the job, not the retraction distance.  So the retraction distance used in G73 code is only controlled with the setting in Mach3.

Here's what I was wanting to do:  I'm drilling a 1.75" deep hole.  I wanted to use the G73 for 0.5 inches, then retract full amount, then rapid back down, use peck drilling for another 0.5", then full retract, etc.  The G83 just takes too long to finish the hole.

Will this work?

G73 X1 Y1 Z-.5 R0.1 Q0.05 F4
G80
G0 Z-.5
G73 X1 Y1 Z-1 R-.5 Q0.05 F4
G80
G0 Z0.1
G0 Z-1
G73 X1 Y1 Z-1.5 R-1 Q0.05 F4
G80
G0 Z0.1
G0 Z-1.5
G73 X1 Y1 Z-1.75 R-1.5 Q0.05 F4
G80

I'd like to change my Mach setting for the retraction distance to make it smaller as well.  I just need to break the chip, no use in going any farther.  Maybe 0.025"?

Here's the code I got to do what I needed...  HOWEVER, Mach3 will not let me change the G73 retraction amount in the ports and pins configuration area?  It won't save the change?  I'm stuck with a 0.1" retraction after each peck??

M6 T15
M03 S4000
M9
G00G43 H15 Z0.1
G73 X0 Y0 Z-0.25 Q0.025 R0 F11.9
G80
G90
(***** Linear Hole Pattern *****)
G73 X0 Y0 Z-0.5 Q0.025 R-0.25 F11.9
G80
G90
(***** Linear Hole Pattern *****)
G73 X0 Y0 Z-0.75 Q0.025 R-0.5 F11.9
G80
G90
(***** Linear Hole Pattern *****)
G73 X0 Y0 Z-1 Q0.025 R-0.75 F11.9
G80
G90
M5 M9
M30

The changes work fine here. Make your entry in the DRO then hit OK...not ENTER.
RC

JUST a word for the wise. The R value in the G73 is only used to start and park the Z when the cycle is complete. If you leave the Rvalue at -.75 when the cycle ends that is as far as it will retract up the hole. IT leaves the bit in a dangerous position as any xy move will snap the bit and damage the hole(;-)

ALSO it is good to have the drill cycle clear all the chips as you progress downward in a deep hole to keep the chips from LOCKING up the bit SO to use a safeZ as a Rvalue is a good thing to use to clear chips.  AS you drill deeper it becomes more important to keep the chips cleared out of the hole.

Also IF you have to do a run from here right after the last drill cycle. The Z will cycle all the way down into the hole to restart at the last Rvalue(-.75) AND the new tooll may crash into the part doing so.

JUST a thought, (;-) TP

The changes work fine here. Make your entry in the DRO then hit OK...not ENTER.
RC

Thanks!

Very good point Vmax549, I figured that was the case when I ran it.  Thinking about it some more, would this be a better way to do the above?  I simply added a G0 Z0.1 and G0 Z-(X) where X is the last drill depth.  This should cause it to rapid back out of the hole completely then rapid back down to where it left off.

M6 T15
M03 S4000
M9
G00G43 H15 Z0.1
G73 X0 Y0 Z-0.25 Q0.025 R0 F11.9
G80
G0 Z0.1
G0 Z-0.25
G90
(***** Linear Hole Pattern *****)
G73 X0 Y0 Z-0.5 Q0.025 R-0.25 F11.9
G80
G0 Z0.1
G0 Z-0.5
G90
(***** Linear Hole Pattern *****)
G73 X0 Y0 Z-0.75 Q0.025 R-0.5 F11.9
G80
G0 Z0.1
G0 Z-0.75
G90
(***** Linear Hole Pattern *****)
G73 X0 Y0 Z-1 Q0.025 R-0.75 F11.9
G80
G0 Z0.1
G90
M5 M9
M30