Siemens sinumerik 808d Programming And Operating Manual page 124

Cycles
2.4 Drilling cycles
Function
The tool drills at the programmed spindle speed and feedrate to the entered final thread
depth.
CYCLE84 can be used to make tapped holes without compensating chuck. For tapping with
compensating chuck, a separate cycle CYCLE840 is provided.
Note
CYCLE84 can be used if the spindle to be used for the boring operation is technically able to
be operated in the position-controlled spindle operation.
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:
● Approach of the reference plane brought forward by the safety clearance by using G0
● Oriented spindle stop (value in the parameter POSS) and switching the spindle to axis
● Tapping to final drilling depth and speed SST
● Dwell time at thread depth (parameter DTB)
● Retraction to the reference plane brought forward by the safety clearance, speed SST1
● Retraction to the retraction plane with G0; spindle mode is reinitiated by reprogramming
programmed under SDAC
Explanation of the parameters
For the parameters RTP, RFP, SDIS, DP, DPR, refer to the topic "Drilling, centering -
CYCLE81 (Page 112)".
124
mode
and direction reversal
the spindle speed active before the cycle was called and the direction of rotation
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0