Groove (Cycle930) - Siemens SINUMERIK 840D SL Operating Manual

Parameter
α1
α2
* Unit of feedrate as programmed before the cycle call
8.4.3

Groove (CYCLE930)

Function
You can use the "Groove" cycle to manufacture symmetrical and asymmetrical grooves on
any straight contour elements.
You can machine outer or inner grooves in the longitudinal or transverse directions. Use the
"Groove width" and "Groove depth" parameters to determine the shape of the groove. If a
groove is wider than the active tool, it is machined in several cuts. The tool is moved by a
maximum of 80% of the tool width for each groove.
You can specify a finishing allowance for the groove base and the flanks; roughing is then
performed down to this point.
The dwell time between recessing and retraction is stored in a setting data element.
Approach/retraction during roughing
Infeed depth D > 0
1. The tool first moves to the starting point calculated internally in the cycle at rapid traverse.
2. The tool cuts a groove in the center of infeed depth D.
3. The tool moves back by D + safety clearance with rapid traverse.
4. The tool cuts a groove next to the first groove with infeed depth 2 · D.
5. The tool moves back by D + safety clearance with rapid traverse.
6. The tool cuts alternating in the first and second groove with the infeed depth 2 · D, until
7. All subsequent groove cuts are made alternating and directly down to the final depth T1.
Milling
Operating Manual, 02/2012, 6FC5398-7CP40-3BA0
Description
Angle of the 1st edge
Angle of the 2nd edge
Machine manufacturer
Please also refer to the machine manufacturer's specifications.
the final depth T1 is reached.
Between the individual grooves, the tool moves back by D + safety clearance with rapid
traverse. After the last groove, the tool is retracted at rapid traverse to the safety
distance.
Between the individual grooves, the tool moves back to the safety distance at rapid
traverse.
Programming technological functions (cycles)
8.4 Turning - only for G code programs
Unit
Degrees
Degrees
395