HEIDENHAIN TNC 320 (34055x-06) Cycle programming - Manual (Page 129)

SLOT MILLING (Cycle 253, DIN/ISO: G253) 5.4
5
TNC 320 | User's Manual Cycle Programming | 5/2013
129
Cycle parameters
Machining operation (0/1/2) Q215: 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
Slot length Q218 (value parallel to the reference
axis of the working plane): Enter the length of the
slot. Input range 0 to 99999.9999
Slot width Q219 (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
Finishing allowance for side Q368 (incremental):
Finishing allowance in the working plane. Input
range 0 to 99999.9999
Angle of rotation Q374 (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
Slot position (0/1/2/3/4) Q367: 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
Feed rate for milling Q207: Traversing speed of
the tool in mm/min while milling. Input range 0 to
99999.999 alternatively
FAUTO, FU, FZ
Climb or up-cut Q351: Type of milling operation
with M3
+1 = climb
–1 = up-cut
PREDEF: The TNC uses the value from the GLOBAL
DEF block
Depth Q201 (incremental): Distance between
workpiece surface and bottom of slot. Input range
-99999.9999 to 99999.9999