HEIDENHAIN TNC 640 (34059x-04) Cycle programming - Manual (Page 186)

Fixed Cycles: Contour Pocket
7.4 CONTOUR DATA (Cycle 20, DIN/ISO: G120)
7
186
TNC 640 | User's Manual Cycle Programming | 3/2014
Cycle parameters
Milling depth Q1 (incremental): Distance between
workpiece surface and bottom of pocket. Input
range -99999.9999 to 99999.9999
Path overlap factor Q2: Q2 x tool radius = stepover
factor k. Input range -0.0001 to 1.9999
Finishing allowance for side Q3 (incremental):
Finishing allowance in the working plane. Input
range -99999.9999 to 99999.9999
Finishing allowance for floor Q4 (incremental):
Finishing allowance in the tool axis. Input range
-99999.9999 to 99999.9999
Workpiece surface coordinate Q5 (absolute):
Absolute coordinate of the workpiece surface. Input
range -99999.9999 to 99999.9999
Set-up clearance Q6 (incremental): Distance
between tool tip and workpiece surface. Input range
0 to 99999.9999
Clearance height Q7 (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
Inside corner radius Q8: 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!
Input range 0 to 99999.9999
Direction of rotation? Q9: 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.
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 ;DIRECTION OF
ROTATION