HEIDENHAIN TNC 640 (34059x-02) Cycle programming - Manual (Page 206)

Fixed Cycles: Cylindrical Surface
8.3 CYLINDER SURFACE Slot milling (Cycle 28, DIN/ISO: G128,
software option 1)
8
206
TNC 640 | User's Manual Cycle Programming | 5/2013
8.3 CYLINDER SURFACE Slot milling
(Cycle 28, DIN/ISO: G128, software
option 1)
Cycle run
This cycle enables you to program a guide notch in two dimensions
and then transfer it onto a cylindrical surface. Unlike Cycle 27,
with this cycle the TNC adjusts the tool so that, with radius
compensation active, the walls of the slot are nearly parallel. You
can machine exactly parallel walls by using a tool that is exactly as
wide as the slot.
The smaller the tool is with respect to the slot width, the larger the
distortion in circular arcs and oblique line segments. To minimize
this process-related distortion, you can define in parameter Q21
a tolerance with which the TNC machines a slot as similar as
possible to a slot machined with a tool of the same width as the
slot.
Program the midpoint path of the contour together with the tool
radius compensation. With the radius compensation you specify
whether the TNC cuts the slot with climb milling or up-cut milling.
1 The TNC positions the tool over the cutter infeed point.
2 At the first plunging depth, the tool mills along the programmed
slot wall at the milling feed rate Q12 while respecting the
finishing allowance for the side.
3 At the end of the contour, the TNC moves the tool to the
opposite wall and returns to the infeed point.
4 Steps 2 to 3 are repeated until the programmed milling depth
Q1 is reached.
5 If you have defined the tolerance in Q21, the TNC then
remachines the slot walls to be as parallel as possible.
6 Finally, the tool retracts in the tool axis to the clearance height
or to the position last programmed before the cycle.