G84 tapping cycle performs tapping operation, tapping is performed by rotating the spindle clockwise, when bottom of the hole has been reached, the spindle is rotated in the reverse direction for retraction. This whole operation creates threads.
G84 X... Y... Z... R... P... F... K...
|X||Hole position in x-axis.|
|Y||Hole position in y-axis.|
|Z||Depth, tapping from R-plane to Z-depth.|
|R||Position of the R plane.|
|K||Number of cycle repetitions (if required).|
Once given in program G84 tapping cycle is repeated at every axis movement until G80 is given in program to end tapping cycle.
Feedrate override is ignored during tapping.
Feed-hold does not stop the machine until the return operation is completed.
N150 M6 T2 N160 G90 G00 X60 Y28 Z12 S100 M03 N170 G99 G84 X60 Y28 Z-17 P300 R2 F120 N180 G98 Y12 N190 G91 G80 G28 X0 Y0 Z0 M05 N200 M30
Brief description of how G84 tapping cycle works,
0- CW Spindle rotation command (M03) must be given in part-program.
1- Rapid traverse to X, Y position (pre-drill hole position).
2- Rapid traverse to R-plane.
3- Tapping operation is done till Z-depth (with tapping feed given with G84).
4-1- Dwell for time specified with P
4-2- Spindle is rotated CCW
5- Tap is Retracted with the specified feed.
At R-plane spindle is rotated CW.
If G99 is specified then tapping for this hole ends here,
6- if G98 is given in program then tap is moved to Initial-level.
G98 G99 Modes
After completing tapping the return height can be controlled by using G98 or G99.
G98 Tap will return to the Initial level
G99 Tap will return to R-plane.
G98, G99 can be used multiple times during G84 tapping cycle.
G84 tapping cycle can be repeated multiple times if K value is given.
For working example see G81 drilling cycle.
N10 T1 M06 N20 G90 G54 G00 X30 Y25 N30 S100 M03 N40 G43 H01 Z5 M08 N50 G84 Z-20 R2 F1.25 N60 X80 Y50 N70 G80 G00 Z100 M09 N80 M30