Mitsubishi Electric M700V Series Programming Manual page 507

13. Program Support Functions
(12) Automatic operation handle interruption
Do not perform the automatic operation handle interruption during the tool center point control.
If performed, the tool moves off the programmed track.
(13) Manual / Automatic simultaneous
Manual / Automatic simultaneous cannot be executed to the axes related to the tool center
point control during the tool center point control.
(14) Tool handle feed & interruption
Do not perform the tool handle feed & interruption during the tool center point control. If
performed, the tool moves off the programmed track.
(15) Corner chamfering/Corner R
When the corner chamfering/corner R is performed during the tool center point control, the tool
center point control becomes valid to the track after the corner chamfering/corner R.
(16) Mirror image by parameter setting / external mirror image input
When the tool center point control command is issued during the mirror image by
parameter/external input, a program error (P941) occurs. Also, do not turn the mirror image by
parameter/external input ON during the tool center point control.
(17) Linear angle command
When A axis is used as a rotary axis, the linear angle command cannot be executed. When A
axis is not used as a rotary axis, tool center point control becomes valid to the shape after the
linear angle command.
(18) Geometric command
When A axis is used as a rotary axis, the geometric command cannot be executed. If executed,
a program error When A axis is not used as a rotary axis, tool center point control becomes
valid to the shape after the geometric command.
(19) Figure rotation
The tool center point control becomes valid to the shape after the figure rotation.
(20) Coordinate rotation by parameter
When the tool center point control command is issued during the coordinate rotation by
parameter, a program error (P941) occurs. Also, do not turn the coordinate rotation by
parameter ON during the tool center point control.
(21) Chopping
Chopping operation for the 3 orthogonal axes and 2 rotary axes cannot be performed during
the tool center point control.
(22) Macro interruption
If the macro interruption command is executed during the tool center point control, a program
error (P941) occurs.
(23) Tool life management
The compensation amount of the tool center point control during the tool life management is
equal to the compensation amount of the tool subjected to the tool life management.
(24) G00 non-interpolation
Functions as "G00 interpolation".
13.24 Tool Center Point Control; G43.4/G43.5
495