Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Fixed Cycles: Contour Pocket | CONTOUR TRAIN (Cycle 25, DIN/ISO: G125)

Cycle parameters

Q1 Milling depth? (incremental): Distance
between workpiece surface and contour bottom.
Input range -99999.9999 to 99999.9999
Q3 Finishing allowance for side? (incremental):
Finishing allowance in the machining plane. Input
range -99999.9999 to 99999.9999
Q5 Workpiece surface coordinate? (absolute):
Absolute coordinate of the workpiece surface.
Input range -99999.9999 to 99999.9999
Q7 Clearance height? (absolute): Absolute height
at which the tool cannot collide with the workpiece
(for intermediate positioning and retraction at the
end of the cycle). Input range -99999.9999 to
99999.9999
Q10 Plunging depth? (incremental): Infeed per
cut. Input range -99999.9999 to 99999.9999
Q11 Feed rate for plunging?: Traversing speed
of the tool in the spindle axis. Input range 0 to
99999.9999, alternatively FAUTO, fu, FZ
Q12 Feed rate for roughing?: Traversing speed
of the tool in the working plane. Input range 0 to
99999.9999, alternatively FAUTO, fu, FZ
Q15 Climb or up-cut? up-cut = -1:
Climb milling: Input value = +1
Up-cut milling: Input value = –1
Climb milling and up-cut milling alternately in
several infeeds: Input value = 0
HEIDENHAIN | User's manual for cycle programming | 10/2017
NC blocks
62 CYCL DEF 25 CONTOUR TRAIN
Q1=-20 ;MILLING DEPTH
Q3=+0 ;ALLOWANCE FOR SIDE
Q5=+0 ;SURFACE COORDINATE
Q7=+50 ;CLEARANCE HEIGHT
Q10=+5 ;PLUNGING DEPTH
Q11=100 ;FEED RATE FOR PLNGNG
Q12=350 ;FEED RATE F. ROUGHNG
Q15=-1 ;CLIMB OR UP-CUT
Q18=0 ;COARSE ROUGHING
TOOL
Q446=+0.01;RESIDUAL MATERIAL
Q447=+10 ;CONNECTION DISTANCE
Q448=+2 ;PATH EXTENSION
7
239