Siemens SINUMERIK User Manual page 161

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:
● Approaching the position of safety distance relative to the reference plane with G0
● Oriented spindle stop (value in the parameter POSS) and switching the spindle to axis mode
● 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 and direction reversal
● Retraction to the retraction plane with G0; spindle mode is reinitiated by reprogramming the spindle speed active before
the cycle was called and the direction of rotation programmed under SDAC
Explanation of the parameters
For more information about the parameters RTP, RFP, SDIS, DP, DPR, see Section "Drilling, centering - CYCLE81
(Page 152)".
See the following parameters for CYCLE84:
DTB (dwell time)
The dwell time must be programmed in seconds. When tapping blind holes, it is recommended that you omit the dwell time.
SDAC (direction of rotation after end of cycle)
Under SDAC, the direction of rotation after end of cycle is programmed.
For tapping, the direction is changed automatically by the cycle.
Programming and Operating Manual (Turning)
161
01/2017