Cycle "Tapping Without Compensating Chuck" (G84) - Siemens Sinumerik 840D sl Programming Manual

Additional functions
4.1 Program supporting functions
Example
M3 S150
G90 G0 Z100
G90 G99 G89 X200. Y-150. Z-100.
R50. P1000 F150.
Y-500.
Y-700.
X950.
Y-500.
G98 Y-700.
G80
G28 G91 X0 Y0 Z0
M5
4.1.11

Cycle "Tapping without compensating chuck" (G84)

The tool drills at the programmed spindle speed and feedrate to the entered final thread
depth. With G84 you can produce rigid tapping.
Note
G84 can be used if the spindle to be used for the drilling operation is technically able to be
operated in the position-controlled spindle mode.
Format
G84 X... Y... Z... R... P... F... K... ;
X,Y: Drilled hole position
Z: Distance from point R to the bottom of the hole
R: Distance from the initial plane to plane R
P: Dwell time at the bottom of the hole and at point R during return
F: Cutting feedrate
K: Number of repetitions (if necessary)
98
;Rotary motion of stem
;Positioning, drilled hole 1,
;then 1 s stop at the bottom of a hole
;Positioning, drilled hole 2,
;then return to point R
;Positioning, drilled hole 3,
;then return to point R
;Positioning, drilled hole 4,
;then return to point R
;Positioning, drilled hole 5,
;then return to point R
;Positioning, drilled hole 6,
;then return to initial plane
;Deselection of the fixed cycle
;Return to reference position
;Spindle stop
Programming Manual, 06/09, 6FC5398-7BP10-1BA0
ISO Milling