HEIDENHAIN TNC 640 User Manual page 101

Fixed Cycles: Drilling | UNIVERSAL PECKING (Cycle 205, DIN/ISO: G205)
Q257 Infeed depth for chip breaking?
(incremental): Plunging depth after which the TNC
breaks the chip. No chip breaking if 0 is entered.
Input range 0 to 99999.9999
Q256 Retract dist. for chip breaking?
(incremental): Value by which the TNC retracts
the tool during chip breaking. Input range 0.000 to
99999.999
Q211 Dwell time at the depth?: Time in seconds
that the tool remains at the hole bottom. Input
range 0 to 3600.0000
Q379 Deepened starting point? (incremental
with respect to Q203 SURFACE COORDINATE,
takes Q200 into account): Starting position
of actual drilling. The TNC moves at Q253 F
PRE-POSITIONING to the value Q200 SET-UP
CLEARANCE above the deepened starting point.
Input range 0 to 99999.9999
Q253 Feed rate for pre-positioning?: Defines
the traversing speed of the tool when returning to
Q201 DEPTH after Q256 DIST FOR CHIP BRKNG.
This feed rate is also in effect when the tool is
positioned to Q379 STARTING POINT (not equal
0). Entry in mm/min. Input range 0 to 99999.9999
alternatively fmax, FAUTO
Q208 Feed rate for retraction?: Traversing speed
of the tool in mm/min when retracting after the
machining operation. If you enter Q208 = 0, the
TNC retracts the tool at the feed rate Q206. Input
range 0 to 99999.9999, alternatively fmax,FAUTO
Q395 Diameter as reference (0/1)?: Select
whether the entered depth is referenced to the
tool tip or the cylindrical part of the tool. If the TNC
is to reference the depth to the cylindrical part
of the tool, the point angle of the tool must be
defined in the T ANGLE column of the tool table
TOOL.T.
0 = Depth referenced to the tool tip
1 = Depth referenced to the cylindrical part of the
tool
HEIDENHAIN | User's manual for cycle programming | 10/2017
3
101