HEIDENHAIN TNC 640 User Manual page 154

4
Fixed Cycles: Tapping / Thread Milling | OUTSIDE THREAD MILLING (Cycle 267, DIN/ISO: G267)
Q358 Sinking depth at front? (incremental):
Distance between tool point and the top surface
of the workpiece for countersinking at the front of
the tool. Input range -99999.9999 to 99999.9999
Q359 Countersinking offset at front?
(incremental): Distance by which the TNC moves
the tool center away from the center. Input range
0 to 99999.9999
Q203 Workpiece surface coordinate? (absolute):
Coordinate of the workpiece surface. Input range
-99999.9999 to 99999.9999
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
Q254 Feed rate for counterboring?: Traversing
speed of the tool in mm/min during counterboring.
Input range 0 to 99999.9999 alternatively FAUTO,
fu
Q207 Feed rate for milling?: Traversing speed of
the tool in mm/min while milling. Input range 0 to
99999.999 alternatively FAUTO
Q512 Feed rate for approaching?: Traversing
speed of the tool in mm/min while approaching.
For smaller thread diameters you can decrease
the approaching feed rate in order to reduce
the danger of tool breakage. Input range 0 to
99999.999 alternatively FAUTO
154
NC blocks
25 CYCL DEF 267 OUTSIDE THREAD
MLLNG
Q335=10 ;NOMINAL DIAMETER
Q239=+1.5 ;THREAD PITCH
Q201=-20 ;DEPTH OF THREAD
Q355=0 ;THREADS PER STEP
Q253=750 ;F PRE-POSITIONING
Q351=+1 ;CLIMB OR UP-CUT
Q200=2 ;SET-UP CLEARANCE
Q358=+0 ;DEPTH AT FRONT
Q359=+0 ;OFFSET AT FRONT
Q203=+30 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP CLEARANCE
Q254=150 ;F COUNTERBORING
Q207=500 ;FEED RATE FOR MILLNG
Q512=0 ;FEED FOR APPROACH
HEIDENHAIN | User's manual for cycle programming | 10/2017