Is this a used machine for you guys? The code looks OK except for a few things and I'll go over those:
M49 is a commanded code to not allow the use of the speed/feed overrides on the control. This is used in case you have a problem or the program is in a state of constant set up for example. Basically, in case the overrides are active, the M49 will ignore the overrides and force the program commanded speed and feed. M48 returns the control to the overrides.
Code:
N70 G84 R0.2 Z-1.0 F32.0 H100
H100: This is a program select for synchronous or asynchronous tapping. With G84, you have two ways of tapping... by Feed or by Pitch. H100 (or any value greater than 0) puts the machine into synchronous mode. Which is why you're not tapping. Your feed of 32.0 is telling the machine that your thread pitch is 32" per revolution. The control is smart enough to know that such a thread/tap doesn't exist. Try changing the feed to .0313 (for a 32 pitch thread) and see if it feeds. If you want to use Feed instead, then change the "H" value to "H0" or remove it from the line. Then @ 320rpm, you can set a feed of 10ipm.
Also, if your machine parameter is set to synchronous, then the "H" becomes a retract feed override. In otherwords, you can set an "H" value to adjust the speed of the retract from 1-100 of commanded feed. So, at 100, the retract feed/speed is double of the entry speed/feed.
If I were to guess, this should work for you: For a 32 pitch thread.
N30 T20
N35 M6
N40 G80 G90 G54 G49 G00 G17 G40 G98
N45 G91G28 Z0
N50 G28 Y0
N55 G90 G00 X11.7252 Y16.408 S382 T20 M3
N60 G43 H20 Z0.2
N65 M49
N70 G84 G98 R0.2 Z-1.0 F.0313
N75 X10.4021 Y11.6344
N80 X8.145 Y7.717
N85 X5.7064 Y9.5071
N90 X5.2913 Y6.4198
N95 X14.2677 Y3.7995
N100 X15.2017 Y11.6085
N105 X4.02 Y15.8632
N110 G80
N112 M48
N115 G91 G28 Z0
N120 G28 Y0
N125 M06
N130 M30
You may want to check your "OPTIONS" page to make sure you have Synchronous tapping turned on.
It's just a part..... cutter still goes round and round....