Cycle Parameters - HEIDENHAIN TNC 640 User Manual

5
Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | SLOT MILLING (Cycle 253, DIN/ISO: G253)

Cycle parameters

Q215 Machining operation (0/1/2)?: Define
machining operation:
0: Roughing and finishing
1: Only roughing
2: Only finishing
Side finishing and floor finishing are only machined
when the specific allowance (Q368, Q369) is
defined
Q218 Length of slot? (value parallel to the
reference axis of the working plane): Enter the
length of the slot. Input range 0 to 99999.9999
Q219 Width of slot? (value parallel to the
secondary axis of the working plane): Enter the
slot width. If you enter a slot width that equals the
tool diameter, the TNC will carry out the roughing
process only (slot milling). Maximum slot width for
roughing: Twice the tool diameter. Input range 0 to
99999.9999
Q368 Finishing allowance for side? (incremental):
Finishing allowance in the machining plane. Input
range 0 to 99999.9999
Q374 Angle of rotation? (absolute): Angle by
which the entire slot is rotated. The center of
rotation is the position at which the tool is located
when the cycle is called. Input range -360.000 to
360.000
Q367 Position of slot (0/1/2/3/4)?: Position of the
slot in reference to the position of the tool when
the cycle is called:
0: Tool position = slot center
1: Tool position = left end of slot
2: Tool position = center of left slot arc
3: Tool position = center of right slot arc
4: Tool position = right end of slot
Q207 Feed rate for milling?: Traversing speed of
the tool in mm/min while milling. Input range 0 to
99999.999 alternatively FAUTO, fu, FZ
Q351 Direction? Climb=+1, Up-cut=-1: Type of
milling operation with M3:
+1 = Climb
–1 = Up-cut
PREDEF: The TNC uses the value from the
GLOBAL DEF block (if you enter 0, climb milling is
performed)
Q201 Depth? (incremental): Distance between
workpiece surface and bottom of slot. Input range
-99999.9999 to 99999.9999
172
HEIDENHAIN | User's manual for cycle programming | 10/2017