Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014
121
●
During retraction, the roles of the modally effective feedrate from the previous block and the feedrate programmed in the
SAR block are changed, i.e. the actual retraction contour is traversed using the old feedrate, and a new velocity
programmed using the F word will apply correspondingly from P2 to P0.
Programming example: Approach along a quadrant, infeed using G341 and FAD
N10 T1 D1 G17 G90 G94
; Activate tool, X/Y plane
N20 G0 X0 Y0 Z30
; Approach P0
N30 G41 G341 G247 DISCL=5 DISR=13 FAD=500 X40 Y-10 Z=0 F800
N40 G1 X50
N50 G40 G1 X20 Y20
N60 M30
Explanation with regard to N30:
By using G0 (from N20), the point P1 (starting point of the quadrant, corrected by the tool radius) is approached in the plane
Z=30, then lowering to the depth (P2) with Z=5 (DISCL). Using a feedrate of FAD=500 mm/min, it is lowered to a depth of
Z=0 (P3) (G341). Then, the contour is approached at point X40,Y-10 along a quadrant in the plane (P4) using F=800
mm/min.
Intermediate blocks
A maximum of five blocks without moving the geometry axes can be inserted between an SAR block and the next traversing
block.
Information
Programming when retracting:
●
With an SAR block with a geometry axis programmed, the contour ends at P2. The positions on the axes that constitute
the machining plane result from the retraction contour. The axis component perpendicular to this is defined by DISCL.
With DISCL=0, the motion will run completely in the plane.
●
If in the SAR block only the axis is programmed vertically to the machining plane, the contour will end at P1. The
positions of the remaining axes will result, as described above. If the SAR block is also the TRC disable block, an
additional path from P1 to P0 is inserted such that no motion results at the end of the contour when disabling the TRC.
●
If only one axis on the machining plane is programmed, the missing second axis is modally added from its last position in
the previous block.
9
Cycles
9.1
Overview of cycles
Cycles are generally applicable technology subroutines that can be used to carry out a specific machining process, such as
drilling of a thread (tapping) or milling of a pocket. These cycles are adapted to individual tasks by parameter assignment.
Drilling cycle, drilling pattern cycles and milling cycles
The following standard cycles can be carried out using the SINUMERIK 808D ADVANCED control system:
●
Drilling cycles
CYCLE81: Drilling, centering
CYCLE82: Drilling, counterboring
CYCLE83: Deep-hole drilling
CYCLE84: Rigid tapping
CYCLE840: Tapping with compensating chuck
CYCLE85: Reaming 1
CYCLE86: Boring
CYCLE87: Drilling with stop 1
CYCLE88: Drilling with stop 2
CYCLE89: Reaming 2
