HEIDENHAIN SW 54843x-02 DIN Programming - Manual (Page 346)

346 DIN programming
4.26 Milling cy
cles
Contour milling 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.