Drilling A Right-Hand Thread Without Any Compensating Chuck" Cycle (G84) - Siemens SINUMERIK 808D Programming And Operating Manual

Restrictions
None.
Changeover of the axes
Before changing over the drilling axis, one must first deselect the fixed cycle.
Drilling
The drilling cycle is executed only if an axis motion, e.g. is programmed with X, Y, Z or R.
R
Always program R only in one block with an axis motion, otherwise the programmed values are not stored modally.
Deselection
The G functions of Group 01 (G00 to G03) and G89 should not be used together in one block, as otherwise G89 is
deselected.
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
4.4.1.11

"Drilling a right-hand thread without any compensating chuck" cycle (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)
140
;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 and Operating Manual (ISO Turning/Milling)
01/2017