Table of Contents
Advertisement
5
RECTANGULAR POCKET (Cycle 251, DIN/ISO: G251)
5.2
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 deined
Q218 First side length? (incremental): Pocket
length, parallel to the reference axis of the working
plane Input range 0 to 99999.9999
Q219 Second side length? (incremental): Pocket
length, parallel to the minor axis of the working
plane Input range 0 to 99999.9999
Q220 Corner radius?: 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
Q368 Finishing allowance for side? (incremental):
Finishing allowance in the machining plane Input
range 0 to 99999.9999
Q224 Angle of rotation? (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
Q367 Position of pocket (0/1/2/3/4)?: 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 corner top
Q207 Feed rate for milling?: Traversing speed of
the tool in mm/min during 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 pocket Input range
-99999.9999 to 99999.9999
133
HEIDENHAIN | TNC 320 | User's manual for cycle programming | 9/2016
Advertisement
Table of Contents
