GSK 980MDc, Руководство пользователя

Страница: 131 / 473

GSK980MDc Milling CNC System User Manual
112
I Programming
3.29.3 Limit
Plane selection
Linear chamfering and arc chamfering are executed in the specified planes (G17, G18, G19), and the
planes cannot be switched between their chamfering blocks.
Next block
A block with a specified chamfering can follow an interpolation block (G01, G02, G03), and can also
follow some non-movement commands (including G04, G90, G91, G94, G95, G98, G99, FMST and
non-movement commands which block numbers are N, it can command up to 10 blocks, among which M
commands do not include M02, M30, M98, M99, M9000~M9999). P/S alarm occurs when the next block
includes other commands except for the above commands.
Excessive motion range
P/S alarm occurs when the inserted chamfering length or arc radius is too big, or exceeds the specified
length in a program.
Polar coordinate command
Chamfering function cannot be specified when the system is in polar coordinate command mode.
Others: the blocks following coordinate change G92, G54~G59 or reference point return G28~G30 cannot
execute the chamfering.
Note: When a chamfering is specified, an alarm occurs when L and U are specified in the same block.
3.30 Rigid Tapping
The right-handed tapping cycle (G84) and left-handed tapping cycle (G74) may be performed in
standard mode or rigid tapping mode. In standard mode, the spindle is rotated and stopped along with a
movement along the tapping axis using miscellaneous functions M03 (rotating the spindle clockwise), M04
(rotating the spindle counterclockwise), and M05 (stopping the spindle) to perform tapping.
In rigid mode, tapping is performed by controlling the spindle motor as if it were a servo motor and by
interpolating between the tapping axis and spindle. When tapping is performed in rigid mode, the spindle
rotates one turn every time a certain feed (thread lead) which takes place along the tapping axis. This
operation does not vary even during acceleration or deceleration.