HEIDENHAIN TNC 640 User Manual page 90

3
Behavior with chip breaking and with decrement
1 The TNC positions the tool in the spindle axis at rapid traverse
FMAX to the programmed set-up clearance above the workpiece
surface
2 The tool drills at the programmed feed rate for plunging Q206
to the first plunging depth Q202
3 The TNC then disengages the tool by the value of Retraction
rate for chip breaking Q256
4 An infeed is then again machined by the value of plunging
depth Q202 minus decrement Q212 at feed rate for plunging
Q206. The continuously declining difference from the updated
plunging depth Q202 minus decrement Q212 must never
be less than the minimum plunging depth Q205 (example:
Q202=5, Q212=1, Q213=4, Q205= 3: The first plunging depth
is 5 mm, the second plunging depth is 5 - 1 = 4 mm, the third
plunging depth is 4 - 1 = 3 mm and the fourth plunging depth is
also 3 mm)
5 The TNC repeatedly infeeds until achieving the number of chip
breaks Q213 or until the hole has the desired depth Q201.
If the defined number of chip breaks is achieved but the hole
does not yet have the desired depth Q201, the TNC retracts the
tool from the hole at feed rate for retraction Q208 to set-up
clearance Q200
6 If programmed, the TNC now waits in accordance with the
dwell time at top Q210
7 Then the TNC plunges at rapid traverse into the hole to the
value retraction rate for chip breaking Q256 above the last
infeed depth
8 Procedure 2-7 is repeated until depth Q201 is achieved.
9 If programmed, the TNC now waits in accordance with the
dwell time at depth Q211
10 When Depth Q201 is achieved and dwell time at depth Q211
has expired, the TNC removes the tool with Fmax from the hole
to the 2nd set-up clearance Q204
90
Fixed Cycles: Drilling | UNIVERSAL DRILLING (Cycle 203, DIN/ISO: G203)
HEIDENHAIN | User's manual for cycle programming | 10/2017