Siemens SINUMERIK 828D Operating Manual page 323

Clamping the spindle
For ShopTurn, the "Clamp spindle" function can be set up by the machine manufacturer.
Input simple (only for G code)
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.
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.
Approach/retraction CYCLE84 - without compensating chuck in the "1 cut" mode
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.
4. Spindle stop and dwell time at drilling depth.
5. Spindle reverse after dwell time has elapsed.
6. Retraction with active spindle retraction speed (dependent on %S) to safety clearance
7. Spindle stop.
8. Retraction to retraction plane with G0.
Turning
Operating Manual, 01/2015, 6FC5398-8CP40-5BA2
Machine manufacturer
Please refer to the machine manufacturer's specifications.
Machine manufacturer
Various defined values can be pre-assigned using setting data.
Please refer to the machine manufacturer's specifications.
Programming technology functions (cycles)
9.1 Drilling
323