10.1.8
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, chip breaking or retraction from the workpiece for
swarf 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.
Input simple (only for G code programs)
For simple machining operations, you have the option to reduce the wide variety of parameters
to the most important parameters using the "Input" selection field. In this "Input simple" mode,
the hidden parameters are allocated a fixed value that cannot be adjusted.
Machine manufacturer
Various defined values can be pre-assigned using setting data.
Please refer to the machine manufacturer's specifications.
If the workpiece programming requires it, you can display and change all of the parameters
using "Input complete".
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 depth
Z1. The feedrate F is calculated internally in the cycle from the speed and pitch.
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.
Programming technological functions (cycles)
10.1 Drilling
Milling
396
Operating Manual, 08/2018, 6FC5398-7CP41-0BA0
