Need Help!- tap cycles not posting properly from McV8

[firekoe]

i am trying to get master cam V8 to post a tap cycle to a fadal mill using the MPFADAL post but it post this:

N138 T3 M06 (T3 - DRILL/MISC - .375 DIA)
N140 S713.2 M5 M90
N142 E1 G00 X0. Y0.
N144 H3 Z.1 M08
N146 G84.2
N148 G84.1 G98 X0. Y0. Z-.5 R0.1 S713 Q-.0028 F713.
N150 G80
N152 M09
N154 G00 Z0 H0
N156 M01

i do not want the Q (peck) value and why does the feed the same as the ss. dose anyone know how to modify the post to fix this
the post look like this:

ptapfr # calculate tapping feed rate
if peck1 < 8, peck1 = ss / fr
tpi = peck1
# tapfr = ss/tpi
pitch = 1/tpi
tapfr = ss
*pitch, *tapfr, !frplunge

ptapmatic # calculate tapmatic feedrate
tpi = peck1
tapfr = (ss/tpi)*.95
*tapfr, !frplunge

[Neal]

First remove the G84.2, it was for very old machines. The newer ones include it within the G84.1. Second you are posting for Format 1 in which the Q is the lead of the thread and the F is the RPM. Format 2 programs like the Fanuc control of the 6m thru 11M series.

Neal

[firekoe]

i changed the post to post G84.2 but it still post the same any other suggestion

[Neal]

N144 H3 Z.1 M08
N146 G84.2--REMOVE THIS LINE
N148 G84.1 G98 X0. Y0. Z-.5 R0.1 S713 Q-.0028 F713.--REMOVE THE "S" CODE
N150 G80
Also change the format of the "R" word to R0+.01 and change your "Q" word to be the lead of the thread and you will be programmed for FORMAT 1.
If you want FORMAT 2 the remove line N146 and remove the "Q" word from line N148

NOTE: Format 1 The "F" code is the RPM and the "Q" word is the LEAD of the thread
(1"/threads per inch). The "S" code is NOT used.

FORMAT 2: The "F" code is a calculated feed rate based in the RPM. The "S" code is the RPM. The "Q" word is NOT used.

Neal