Drilling, Counterboring - Cycle82 - Siemens SINUMERIK User Manual

Programming example: Drilling_centering
This program produces three drill holes using the CYCLE81 drilling cycle. The drilling axis is always the Z axis.
See the following example for drilling centering_drilling on turning center without tool:
N10 G0 G17 G90 F200 S300 M3
N20 D1 T3 Z110
N30 X0
N40 CYCLE81(110, 100, 2, 35,)
M30
12.4.4

Drilling, counterboring - CYCLE82

Programming
CYCLE82 (RTP, RFP, SDIS, DP, DPR, DTB)
Parameters
Parameter Data type
RTP REAL
RFP REAL
SDIS REAL
DP REAL
DPR REAL
DTB REAL
Function
The tool drills at the programmed spindle speed and feedrate to the entered final drilling depth. A dwell time can be allowed
to elapse when the final drilling depth has been reached.
Sequence
Position reached prior to cycle start:
The drilling position is the position in the two axes of the selected plane.
The cycle creates the following sequence of motions:
● Approaching the position of safety distance relative to the reference plane with G0
● Traversing to the final drilling depth with the feedrate (G1) programmed prior to the cycle call
154
Description
Retraction plane (absolute)
Reference plane (absolute)
Safety clearance (enter without sign)
Final drilling depth (absolute)
Final drilling depth relative to the reference plane (enter without sign)
Dwell time at final drilling depth (chip breakage)
; Specification of technology values
; Approach retraction plane
; Approach drilling position
; Cycle call with absolute end drilling depth, safety
clearance and incomplete parameter list
; Program end
Programming and Operating Manual (Turning)
01/2017