Cut3Df/Cut3Dfd Face Milling - Siemens SINUMERIK 828D Manual

3.8
CUT3DCD programming
example
122
Important functions for 3- to 5-axis machining
Finishing NC program, 5-axis program
N1 G17 G40 G90
N2 CYCLE800()
N3 TRAFOOF
N4 T="CUTTER_10"
N5 M6
N6 S15061 M3
N7 CYCLE800(0,"TISCH",100000,27,0,0,0,288.079,0,-10.196,0,0,0,-1,0,1)
N8 G00 X-13.532 Y-24.856 M03
N9 TRAORI
N10 ORIWKS ORIAXES
N11 G54
N12 TOFFL=0
N13 TOFFR=0
N14 CYCLE800()
N15 CYCLE832(0.05,_TOP_SURFACE_SMOOTH_ON+_ORI_SEMIFIN,0.1)
N16 G0 X0 Y0 Z100.0
N17 CUT3DCD
N18 G41
N19 G1 X-5.945 Y-60.546 A3=0.021144 B3=0.341366 C3=0.939693 F2500
N20 Z5.502 A3=0.021144 B3=0.341366 C3=0.939693
N21 G1 Z0.502 A3=0.021144 B3=0.341366 C3=0.939693 F2500
N22 G1 X-5.743 Y-59.698 A3=0.021144 B3=0.341366 C3=0.939693 F500
......
N17525 g40 X0 Y0
N17526 CYCLE832(0,_OFF,1)
N17528 TRAFOOF
N17529 M17

3.8.3 CUT3DF/CUT3DFD face milling

The situation is also more complicated with face milling. Since the tool is not always
perpendicular to the plane to be machined as with two dimensions, a constant offset is no longer
sufficient. The compensation value and the compensation direction now depend on the tool
radius, the rounding radius and of course on the tool orientation relative to the workpiece surface.
This means that we require additional information about the surface. This is defined by
programming the normal vectors A4, B4, C4 (start of block) and A5, B5, C5 (end of block -
recommended programming).
The compensation is defined with CUT3DF/CUT3DFD and activated with G41/G42, whereby
there is no difference between G41 and G42 in this case.
The activation must be performed in a linear block (G0/G1). Switching off with G40 can be made
in a linear block or in a separate NC block. A change of the 3D TRC variant with active tool radius
compensation is ignored without alarm.
Before switching on CUT3DFD with G41/G42, Top Surface / COMPSURF / CYCLE832 must be
activated, not immediately before tooling, but rather approximately 1000 x CTOL = path before
the tooling or G41/G42 programmed, e.g. 1000 x 0.01 mm = 10 mm.
For traversing motions in the orientation direction of the tool, alarm 10769 is triggered and
machining stopped. As workaround, a G40 and then a G41/G42 can be programmed again for
the machining.
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling