Bore Milling (Cycle 208); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 320 User's Manual For Cycle Programming

3.9

BORE MILLING (Cycle 208)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse
FMAX 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 F.
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 setup clearance at FMAX. If
programmed, the tool moves to the 2nd set-up clearance at
FMAX.

Please note while programming:

Program a positioning block for the starting point
(hole center) in the working plane with radius
compensation R0.
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
of milling defined in the cycle.
Note that if the infeed distance is too large, the tool
or the workpiece may be damaged.
To prevent the infeeds from being too large, enter
the maximum plunge angle of the tool in the ANGLE
column of the tool table. The TNC then automatically
calculates the max. infeed permitted and changes
your entered value accordingly.
Danger of collision!
Enter in machine parameter displayDepthErr whether
the TNC should output an error message (on) or not
(off) if a positive depth is entered.
Keep in mind that the TNC reverses the calculation
for pre-positioning when a
entered. This means that the tool moves at rapid
traverse in the tool axis to set-up clearance
the workpiece surface!
HEIDENHAIN | TNC 320 | User's manual for cycle programming | 9/2016
does not influence the type
positive depth is
below
BORE MILLING (Cycle 208)
3
3.9
85