HEIDENHAIN TNC 640 User Manual page 195

Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | FACE MILLING (Cycle 233, DIN/ISO: G233)
Strategies Q389=0 and Q389 =1
The strategies Q389=0 and Q389=1 differ in the overtravel during
face milling. If Q389=0, the end point lies outside of the surface. If
Q389=1, it lies at the edge of the surface. The TNC calculates the
end point 2 from the side length and the safety clearance to the
side. If the strategy Q389=0 is used, the TNC additionally moves
the tool beyond the level surface by the tool radius.
4 The TNC moves the tool to the end point
feed rate for milling.
5 Then the TNC offsets the tool to the starting point in the next
pass at the pre-positioning feed rate. The offset is calculated
from the programmed width, the tool radius, the maximum path
overlap factor and the safety clearance to the side.
6 The tool then returns at the feed rate for milling in the opposite
direction.
7 The process is repeated until the programmed surface has been
completed.
8 The TNC then positions the tool at rapid traverse FMAX back to
the starting point 1.
9 If more than one infeed is required, the TNC moves the tool in
the tool axis to the next plunging depth at the positioning feed
rate.
10 The process is repeated until all infeeds have been machined. In
the last infeed, only the finishing allowance entered is milled at
the finishing feed rate.
11 At the end of the cycle, the tool is retracted at FMAX to the 2nd
set-up clearance.
HEIDENHAIN | User's manual for cycle programming | 10/2017
2 at the programmed
5
195