PROGRAMMING16. HIGH SPEED CUTTING FUNCTIONS
B–63664EN/02
306
Minimum
feedrate
Interpolation period:
8 msec
Interpolation period:
4 msec
(IS–B, metric input) 4 mm/min 8 mm/min
(IS–B, inch input) 0.38 inch/min 0.76 inch/mim
(Minimum feedrate) = 4
(interpolation period)
8
(IS–B, metric input)
In high–speed linear interpolation mode, the NC interpolation period can
be changed. As the interpolation period decreases, the machining speed
and precision increase.
IT2, IT1, and IT0 bits (bits 6, 5, and 4 of parameter 7501)
IT2 IT1 IT0 Interpolation period
0
0
0
0
1
0
1
0
1
1
0
0
1
1
1
8 msec in high–speed linear interpolation mode
4 msec in high–speed linear interpolation mode
2 msec in high–speed linear interpolation mode
1 msec in high–speed linear interpolation mode
0.5 msec in high–speed linear interpolation mode
Up to four axes can be controlled. The names of the controlled axes are
X, Y, Z, and C. Any other axis name is ignored. Set X, Y, Z, then C in
axis name setting parameter 1020.
Only the linear interpolation function can be executed. Circular
interpolation and other interpolation functions cannot be executed.
Movement cannot be specified by absolute values. A specified travel
distance is always considered as an incremental travel distance, regardless
of the G90/G91 mode setting.
The feed per revolution command cannot be specified. Feed per minute
is always assumed, regardless of the G94/G95 mode setting.
High–speed linear interpolation commands cannot be specified in cutter
compensation mode (G41/G42). If the high–speed linear interpolation
start command is specified in cutter compensation mode, P/S alarm No.
178 is issued.
The high–speed interpolation commands cannot be specified in polar
coordinate interpolation mode (G12.1), scaling mode (G51), or
coordinate system rotation mode.
D Interpolation period
Limitations
D Controlled axes
D Enabled interpolation
D Absolute command
D Feed per revolution
D Cutter compensation
D Modes related to the
coordinate system