Mill. Contour G840 - HEIDENHAIN CNC PILOT 640 User Manual

4

Mill. contour G840

G840 – fundamentals
G840 mills or deburrs open or closed contours (figures or free
contours).
Plunge strategies: Depending on the cutter you are using, select one
of the following strategies:
Vertical plunge: The cycle moves the tool to the starting point; the
tool plunges and mills the contour
Calculate positions, predrill, mill. The machining process is
performed in the following steps:
Insert drill.
Calculate hole positions with G840 A1 ..
Predrill with G71 NF..
Call cycle G840 A0 .. The cycle positions the tool above the
hole; the tool plunges and mills the contour
Predrilling, milling. The machining process is performed in the
following steps:
Predrill with G71 ..
Position the cutter above the hole. Call cycle G840 A0 .. The
cycle plunges and mills the contour or contour section
If the milling contour consists of multiple sections, G840 takes all
the sections of the contour into account for predrilling and milling.
Call G840 A0 .. separately for each section when calculating the hole
positions without G840 A1 ...
Oversize: A G58 oversize shifts the contour to be milled in the
direction given in cycle type Q.
With inside milling and closed contour: Shifted inward
With outside milling and closed contour: Shifted outward
Open contour: Shifts to the left or right depending on Q
If Q = 0, oversizes are not taken into account
G57 and negative G58 oversizes are not taken into
account
416
DIN/ISO programming | Milling cycles
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017