Single-Lip Deep-Hole Drilling (Cycle 241, Din/Iso: G241, Software Option 19); Cycle Run - HEIDENHAIN TNC 620 User Manual

Fixed Cycles: Drilling | SINGLE-LIP DEEP-HOLE DRILLING (Cycle 241, DIN/ISO: G241, software option 19)
3.10 SINGLE-LIP DEEP-HOLE DRILLING (Cycle
241, DIN/ISO: G241, software option 19)

Cycle run

1 The TNC positions the tool in the spindle axis at rapid traverse
FMAX to the programmed Safety clearance Q200 above the
SURFACE COORDINATE Q203
2 Depending on the "Position behavior when working with
Q379", Page 94, the TNC switches the spindle speed either
to the Safety clearance Q200 or to a specific value above the
coordinate surface. see Page 94
3 The TNC executes the approach motion with the direction of
rotation defined in the cycle, with clockwise, counterclockwise
or stationary spindle.
4 The tool drills to the hole depth at the feed rate F, or to the
plunging depth if a smaller infeed value has been entered. The
plunging depth is decreased after each infeed by the decrement.
If you have entered a dwell depth, the TNC reduces the feed
rate by the feed rate factor after the dwell depth has been
reached.
5 If programmed, the tool remains at the hole bottom for chip
breaking.
6 The TNC repeats this process (4 to 5) until the hole depth is
reached.
7 After the TNC has reached the hole depth, it switches off the
coolant and resets the drilling speed to the value defined in
Q427 ROT.SPEED INFEED/OUT.
8 The TNC positions the tool at the retraction feed rate to the
retraction position. Refer to the following document for the
value of the retraction position in your case: see Page 94
9 If programmed, the tool moves to the 2nd set-up clearance at
FMAX
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
3
101