Drilling A Left-Hand Thread Without Any Compensating Chuck" Cycle (G74) - Siemens SINUMERIK 808D Programming And Operating Manual

S command
An error message is displayed if the specified gear stage is one step higher than the maximum permissible value.
F function
An error message is displayed if the value specified for the cutting feedrate exceeds the maximum permissible value.
Unit of the F command
G function Metric input
G94 1 mm/min
G95 0.01 mm/rev
Example
Feedrate for the Z axis 1000 mm/min
Spindle speed 1000 rev/min
Thread lead 1.0 mm
<Programming as feedrate per minute>
S100 M03S1000
G94
G00 X100.0 Y100.0
G84 Z-50.0 R-10.0 F1000
<Programming as revolutional feedrate>
G95
G00 X100.0 Y100.0
G84 Z-50.0 R-10.0 F1.0
4.4.1.12

"Drilling a left-hand thread without any compensating chuck" cycle (G74)

The tool drills at the programmed spindle speed and feedrate to the entered final thread depth. With G74 you can produce
left rigid tapping.
Note
G74 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
G74 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 point 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)
142
Input in inch
0.01 inch/min
0.0001 inch/rev
;Feedrate per minute
;Positioning
;Tapping without compensating chuck
; Rev. feedrate
;Positioning
;Tapping without compensating chuck
Remarks
Decimal point programming is permitted
Decimal point programming is permitted
Programming and Operating Manual (ISO Turning/Milling)
01/2017