HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 212)

8 Programming: Cycles 196
X
Z
CONTOUR MILLING (Cycle G58/G59)
Application
Cycle G58/G59 CONTOUR MILLING serves for finishing the contour
pocket.
Before programming, note the following:
Program a positioning block for the starting point in the
tool axis (set-up clearance above the workpiece surface).
Direction of rotation during contour milling
■ In clockwise direction: G58
■ In counterclockwise direction: G59
The TNC finishes each subcontour separately, even at several
infeed depths.
ú Setup clearance (incremental value): Distance
between tool tip (at starting position) and workpiece
surface
ú Milling depth (incremental value): Distance between
workpiece surface and pocket floor
ú Plunging depth (incremental value):
Infeed per cut. The TNC will go to depth in one
movement if:
■ The plunging depth equals the milling depth
■ The plunging depth is greater than the milling depth
The milling depth does not have to be a multiple of
the plunging depth.
ú Feed rate for plunging: Traversing speed of the tool in
mm/min during penetration
ú Feed rate: Feed rate for milling in mm/min
8.6 SL Cycles Group I
Example NC blocks:
N54 G58 P01 2 P02 -15 P03 5 P04 250
P05 500*
...
N71 G59 P01 2 P02 -15 P03 5 P04 250
P05 500*
Kkap8.pm6 29.06.2006, 08:06 196