Please Note While Programming - HEIDENHAIN TNC 620 User Manual

Fixed Cycles: Contour Pocket | ROUGHING (Cycle 22, DIN/ISO: G122, software option 19)

Please note while programming:

This cycle requires a center-cut end mill (ISO 1641) or
pilot drilling with Cycle 21.
You define the plunging behavior of Cycle 22 with
parameter Q19 and with the tool table in the ANGLE and
LCUTS columns:
If Q19=0 is defined, the TNC always plunges
perpendicularly, even if a plunge angle (ANGLE) is
defined for the active tool.
If you define the ANGLE=90°, the TNC plunges
perpendicularly. The reciprocation feed rate Q19 is
used as plunging feed rate.
If the reciprocation feed rate Q19 is defined in Cycle
22 and ANGLE is defined between 0.1 and 89.999
in the tool table, the TNC plunges helically at the
defined ANGLE.
If the reciprocation feed is defined in Cycle 22 and no
ANGLE is in the tool table, the TNC displays an error
message.
If geometrical conditions do not allow helical
plunging (slot), the TNC tries a reciprocating plunge.
The reciprocation length is calculated from LCUTS
and ANGLE (reciprocation length = LCUTS / tan
ANGLE).
If you clear out an acute inside corner and use an
overlap factor greater than 1, some material might be
left over. Check especially the innermost path in the test
run graphic and, if necessary, change the overlap factor
slightly. This allows another distribution of cuts, which
often provides the desired results.
During fine roughing the TNC does not take a defined
wear value DR of the coarse roughing tool into account.
If M110 is activated during operation, the feed rate
of compensated circular arcs within will be reduced
accordingly.
Danger of collision!
If you set the parameter posAfterContPocket to
ToolAxClearanceHeight, the TNC positions the tool after the end
of the cycle only in the tool axis direction to the clearance height.
The TNC does not position the tool in the working plane.
After the end of the cycle, position the tool with all
coordinates of the working plane, e.g.
After the cycle, program the absolute position (not an
incremental traversing movement)
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
NOTICE
L X+80 Y+0 R0 FMAX
7
221