Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Fixed Cycles: Contour Pocket | CONTOUR DATA (Cycle 20, DIN/ISO: G120)

Cycle parameters

Q1 Milling depth? (incremental): Distance
between workpiece surface and bottom of pocket.
Input range -99999.9999 to 99999.9999
Q2 Path overlap factor?: Q2 x tool radius =
stepover factor k. Input range: -0.0001 to 1.9999
Q3 Finishing allowance for side? (incremental):
Finishing allowance in the machining plane. Input
range -99999.9999 to 99999.9999
Q4 Finishing allowance for floor? (incremental):
Finishing allowance for the floor. 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
Q6 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface. Input
range 0 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
Q8 Inside corner radius?: Inside "corner" rounding
radius; entered value is referenced to the path of
the tool center and is used to calculate smoother
traverse motions between the contour elements.
Q8 is not a radius that is inserted as a separate
contour element between programmed
elements!
Q9 Direction of rotation? cw = -1: Machining
direction for pockets
Q9 = –1 up-cut milling for pocket and island
Q9 = +1 climb milling for pocket and island
You can check the machining parameters during a program
interruption and overwrite them if required.
HEIDENHAIN | User's manual for cycle programming | 10/2017
Input range 0 to 99999.9999
NC blocks
57 CYCL DEF 20 CONTOUR DATA
Q1=-20 ;MILLING DEPTH
Q2=1 ;TOOL PATH OVERLAP
Q3=+0.2 ;ALLOWANCE FOR SIDE
Q4=+0.1 ;ALLOWANCE FOR FLOOR
Q5=+30 ;SURFACE COORDINATE
Q6=2 ;SET-UP CLEARANCE
Q7=+80 ;CLEARANCE HEIGHT
Q8=0.5 ;ROUNDING RADIUS
Q9=+1 ;ROTATIONAL DIRECTION
7
225