Cycle Parameters - HEIDENHAIN TNC 620 User Manual

5
RECTANGULAR POCKET (Cycle 251) 5.2

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
1st side length Q218 (incremental): Pocket length,
parallel to the reference axis of the working plane.
Input range 0 to 99999.9999
2nd side length Q219 (incremental): Pocket length,
parallel to the minor axis of the working plane. Input
range 0 to 99999.9999
Corner radius Q220: Radius of the pocket corner. If
you have entered 0 here, the TNC assumes that the
corner radius is equal to the tool radius. 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 Q224 (absolute): Angle by which
the entire machining is rotated. The center of
rotation is the position at which the tool is located
when the cycle is called. Input range -360.0000 to
360.0000
Pocket position Q367: Position of the pocket in
reference to the position of the tool when the cycle
is called:
0: Tool position = pocket center
1: Tool position = left corner below
2: Tool position = right corner below
3: Tool position = right corner top
4: Tool position = left top corner top
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 (If you enter 0, climb milling is used for
machining)
Depth Q201 (incremental): Distance between
workpiece surface and bottom of pocket. 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
139
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 9/2015