Multipass Milling (Cycle 230, Din/Iso: G230, Software Option 19); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 620 User Manual

MULTIPASS MILLING (Cycle 230, DIN/ISO: G230, software option
10.2 MULTIPASS MILLING (Cycle 230, DIN/
ISO: G230, software option 19)

Cycle run

1 From the current position in the working plane, the TNC
positions the tool in rapid traverse FMAX to the starting point 1;
the TNC moves the tool by its radius to the left and upward.
2 The tool then moves in at FMAX in the spindle axis to set-up
clearance. From there it approaches the programmed starting
position in the spindle axis at the feed rate for plunging.
3 The tool then moves as the programmed feed rate for milling
to the end point2. The TNC calculates the end point from the
programmed starting point, the programmed length, and the
tool radius.
4 The TNC offsets the tool to the starting point in the next pass
at the stepover feed rate. The offset is calculated from the
programmed width and the number of cuts.
5 The tool then returns in the negative direction of the first axis.
6 Multipass milling is repeated until the programmed surface has
been completed.
7 At the end of the cycle, the tool is retracted in FMAX to set-up
clearance.

Please note while programming:

From the current position, the TNC positions the tool
at the starting point, first in the working plane and
then in the spindle axis.
Pre-position the tool in such a way that no collision
between tool and fixtures can occur.
TNC 620 | User's Manual Cycle Programming | 3/2014
10
10.2
19)
231