Please Note While Programming - HEIDENHAIN TNC 620 User Manual

Fixed Cycles: Contour Pocket | SIDE FINISHING (Cycle 24, DIN/ISO: G124, software option 19)

Please note while programming:

The sum of allowance for side (Q14) and the radius
of the finish mill must be smaller than the sum of
allowance for side (Q3, Cycle 20) and the radius of the
rough mill.
If no allowance has been defined in Cycle 20, the control
issues the error message "Tool radius too large".
The allowance for side Q14 is left over after finishing.
Therefore, it must be smaller than the allowance in
Cycle 20.
This calculation also holds if you run Cycle 24 without
having roughed out with Cycle 22; in this case, enter "0"
for the radius of the rough mill.
You can use Cycle 24 also for contour milling. Then you
must:
define the contour to be milled as a single island
(without pocket limit), and
enter the finishing allowance (Q3) in Cycle 20 to be
greater than the sum of the finishing allowance Q14
+ radius of the tool being used
The TNC automatically calculates the starting point for
finishing. The starting point depends on the available
space in the pocket and the allowance programmed in
Cycle 20.
The starting point calculated by the TNC also depends
on the machining sequence. If you select the finishing
cycle with the GOTO key and then start the program,
the starting point can be at a different location from
where it would be if you execute the program in the
defined sequence.
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
227