HEIDENHAIN TNC 640 User Manual page 201

Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | FACE MILLING (Cycle 233, DIN/ISO: G233)
Q200 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface. Input
range 0 to 99999.9999; alternatively PREDEF
Q204 2nd set-up clearance? (incremental):
Coordinate in the spindle axis at which no collision
between tool and workpiece (fixtures) can occur.
Input range 0 to 99999.9999; alternatively PREDEF
Q347 1st limit?: Select the side of the workpiece
where the plan surface is bordered by a side wall
(not possible with helical machining). Depending
on the position of the side wall, the TNC limits the
machining of the level surface to the respective
coordinate of the starting point or to the side
length: (not possible with helical machining):
Input 0: No limiting
Input -1: Limiting in negative principal axis
Input +1: Limiting in positive principal axis
Input -2: Limiting in negative secondary axis
Input +2: Limiting in positive secondary axis
Q348 2nd limit?: See Parameter 1st limit Q347
Q349 3rd limit?: See Parameter 1st limit Q347
Q220 Corner radius?: Radius of a corner at limits
(Q347 to Q349). Input range 0 to 99999.9999
Q368 Finishing allowance for side? (incremental):
Finishing allowance in the machining plane. Input
range 0 to 99999.9999
Q338 Infeed for finishing? (incremental):
Infeed in the spindle axis per finishing cut.
Q338=0: Finishing in one infeed. Input range 0 to
99999.9999
HEIDENHAIN | User's manual for cycle programming | 10/2017
5
201