Siemens SINUMERIK 840D Manual page 75

Key functions for 5-axis machining
ORID
ORIC
Face milling
CUT3DFS
CUT3DFF
CUT3DF
3D circumferential milling with limitation surface (combined circumferential/face mill-
ing)
CUT3DCC
CUT3DCCD
Programming example for circumferential milling
A workpiece contour needs to be milled at the circumference. It is a question of programming
from the top edge of the workpiece and the engaged length ISD is taken into account. In the
example, compensation is performed to the right based on an ISD of 20.
Example involving
CUT3DC
© Siemens AG All rights reserved. SINUMERIK, Manual, 5-axis machining
No changes in orientation in inserted circular blocks at external
corners. Orientation motion is performed in the linear blocks.
Travel path is extended by means of circles. The change in orien-
tation is also performed proportionately in the circle.
Constant orientation (3-axis). Tool points in the Z direction of the
coordinate system defined via G17 - G19. Frames do not have
any effect.
Constant orientation (3-axis). Tool in Z direction of the coordinate
system currently defined via the frame.
5-axis with variable tool orientation
CNC program relates to the contour on the machining surface.
The CNC program relates to the tool center point path.
N10 A0 B0 C0 X0 Y0 Z0 F5000
N15 T1 D1 ISD=20
N20 ; Call tool and apply tool offset
N25 TRAORI
N30 ; Activate transformation
N35 CUT3DC
N40 ; 3D tool radius compensation
N45 G42 X10 Y10 G1
N50 ; Tool radius compensation and ISD selec-
tion
N55 X60
N60 A3=-1 B3=1 C3=1
N65 Y100
N70 ...
N90 G40
N95 ; Tool radius compensation and ISD dese-
lection
N100 ...
3.7
75