HEIDENHAIN CNC PILOT 640 User Manual page 409

DIN/ISO programming | Milling cycles
Q: Cycle type (default: 0) – Depending on U, the following applies:
Contour milling (U = 0)
Q=0: Center of milling cutter on the contour
Q=1, closed contour: Inside milling
Q=1, open contour: Left in machining direction
Q=2, closed contour: Outside milling
Q=2, open contour: Right in machining direction
Q=3, open contour: Milling location depends on H and the
direction of tool rotation—see help graphic
Pocket milling (U > 0)
Q=0: From the inside toward the outside
Q=1: From the outside toward the inside
O: Roughing/Finish
0: Roughing
1: Finishing
Milling depth: The cycle calculates the depth from
the milling top edge and the milling floor—taking the
oversizes into account
Milling cutter radius compensation: Effective (except
for contour milling with Q = 0)
Approach and departure: For closed contours, the
point of the surface normal from the tool position to
the first contour element is the point of approach and
departure. If no surface normal intersects the tool
position, the starting point of the first element is the
point of approach and departure. For contour milling
and finishing (pocket milling), define with the approach
radius whether the tool is to approach directly or in an
arc.
G57/G58 oversizes are taken into account if the
oversizes I, K are not programmed:
G57: Oversize in X, Z direction
G58: The oversize shifts the milling contour as
follows:
With inside milling and closed contour: The
contour is contracted
With outside milling and closed contour: The
contour is expanded
With open contour and Q=1: Left in machining
direction
With open contour and Q=2: Right in machining
direction
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
409