Cycle Parameters - HEIDENHAIN TNC 620 User Manual

7
TROCHOIDAL SLOT (Cycle 275, DIN ISO G275, software option 19) 7.10

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 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
Infeed per rev. Q436 absolute: Value by which the
TNC moves the tool in the machining direction per
revolution. Input range 0 to 99999.9999
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
Feed rate for milling Q12: Traversing speed of
the tool in the working plane. Input range 0 to
99999.9999, 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
Plunging depth Q202 (incremental): Infeed per
cut. Enter a value greater than 0. Input range 0 to
99999.9999
193
TNC 620 | User's Manual Cycle Programming | 3/2014