HEIDENHAIN iTNC 530 (340 49x-04) ISO programming - Manual (Page 325)

HEIDENHAIN iTNC 530 325
8.3 Cy
cles f
o
r Dr
illing, T
a
pping and Thr
ead Milling
BORE MILLING (Cycle G208)
1 The TNC positions the tool in the tool axis at rapid traverse to the
programmed set-up clearance above the workpiece surface and
then moves the tool to the bore hole circumference on a rounded
arc (if enough space is available).
2 The tool mills in a helix from the current position to the first
plunging depth at the programmed feed rate.
3 When the drilling depth is reached, the TNC once again traverses
a full circle to remove the material remaining after the initial
plunge.
4 The TNC then positions the tool at the center of the hole again.
5 Finally the TNC returns to the set-up clearance at rapid traverse. If
you have entered a 2nd set-up clearance, the tool subsequently
moves to that position in rapid traverse.
Before programming, note the following
Program a positioning block for the starting point (hole
center) in the working plane with radius compensation
G40.
The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program
DEPTH = 0, the cycle will not be executed.
If you have entered the bore hole diameter to be the same
as the tool diameter, the TNC will bore directly to the
entered depth without any helical interpolation.
An active mirror function does not influence the type of
milling defined in the cycle.
Enter in MP7441 bit 2 whether the TNC should output an
error message (bit 2=1) or not (bit 2=0) if a positive depth
is entered.
Danger of collision!
Keep in mind that the TNC reverses the calculation for pre-
positioning when a positive depth is entered. This
means that the tool moves at rapid traverse in the tool axis
at safety clearance below the workpiece surface!