HEIDENHAIN TNC 360 User Manual - Manual (Page 180)

8-27 TNC 360
8 Cycles
Fig. 8.30: Infeeds and distances for
CONTOUR MILLING
Fig. 8.31: Finishing allowance
8.3 SL Cycles
A
B
C
Y
X
D
CONTOUR MILLING (Cycle 16)
Cycle 16 CONTOUR MILLING is used to finish-mill the contour pocket.
This cycle can also be used generally for milling contours.
Process
• The tool is positioned above the first starting point.
• The tool then penetrates at the programmed feed rate to the first
pecking depth.
• On reaching the first pecking depth, the tool mills the first contour at
the programmed feed rate and in the specified direction of rotation.
• At the infeed point, the tool is advanced to the next pecking depth.
This process is repeated until the programmed milling depth is reached.
The remaining subcontours are milled in the same manner.
Required tool
This cycle requires a center-cut end mill (ISO 1641).
Input data
• SETUP CLEARANCE A
• MILLING DEPTH B
• PECKING DEPTH
C
• FEED RATE FOR PECKING:
Traversing speed of the tool during penetration.
• DIRECTION OF ROTATION FOR CONTOUR MILLING:
The following is valid for M3:
DR+: Climb milling for pocket and
island
DR–: Up-cut milling for pocket and
island
• FEED RATE:
Traversing speed of the tool in the machining plane.