Tapping - Cycle84, 840 - Siemens SINUMERIK 840D sl Operating Manual

4.4.7

Tapping - CYCLE84, 840

Function
You can machine an internal thread with the "tapping" cycle.
The tool moves to the safety clearance with the active speed and rapid traverse. The spindle
stops, spindle and feedrate are synchronized. The tool is then inserted in the workpiece with
the programmed speed (dependent on %S).
You can choose between drilling in one cut, chipbreaking or retraction from the workpiece for
stock removal.
Depending on the selection in the "Compensating chuck mode" field, alternatively the
following cycle calls are generated:
● With compensating chuck: CYCLE840
● Without compensating chuck: CYCLE84
When tapping with compensating chuck, the thread is produced in one cut. CYCLE84
enables tapping to be performed in several cuts, when the spindle is equipped with a
measuring system.
Approach/retraction - CYCLE840 - with compensating chuck
1. The tool moves with G0 to safety clearance of the reference point.
2. The tool drills with G1 and the programmed spindle speed and direction of rotation to
3. The direction of rotation is reversed.
4. Dwell time at final drilling depth.
5. Retraction to safety clearance with G1.
6. Reversal of direction of rotation or spindle stop.
7. Retraction to retraction plane with G0.
Approach/retraction - CYCLE84 - without compensating chuck
One cut:
1. Travel with G0 to the safety clearance of the reference point.
2. Spindle is synchronized and started with the programmed speed (dependent on %S).
3. Tapping with spindle-feedrate synchronization to Z1.
HMI sl Turning
Operating Manual, 01/2008, 6FC5398-7AP10-0BA0
depth Z1. The feedrate F is calculated internally in the cycle from the speed and pitch.
Programming a cycle
4.4 Drilling
165