Table of Contents
Advertisement
(12) M32, M33, M34 (thread cutting mode; straight, zigzag, straight (reversed))
These M codes are used to specify the thread cutting mode in the compound fixed cycle and
LAP; M32 for infeed along one side of the thread face to be cut (straight), M33 for zigzag infeed,
and M34 for straight infeed along the opposite thread face from the one in the M32 mode
(straight (reversed)).
(13) M40, M41, M42, M43, M44 (spindle drive gear range; neutral, gear 1, gear 2, gear 3, gear 4)
These M codes are used to select the spindle drive gear range; neutral (M40), gear 1 (M41),
gear 2 (M42), gear 3 (M43), and gear 4 (M44).
(14) M48, M49 (spindle speed override ignore)
When the spindle speed override ignore function is valid, the spindle speed override rate is
fixed at 100% regardless of the setting of the spindle override switch. The spindle speed
override ignore function is canceled by specifying the cancel M code, resetting the CNC, or
changing the operation mode.
< M codes >
Spindle speed override ignore⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅ M49
Spindle speed override ignore cancel⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅M48
(15) M55, M56 (tailstock spindle retract, advance)
These M codes specify tailstock retract/advance operation.
(16) M60, M61 (fixed surface speed arrival ignore OFF, ON)
These M codes are used to specify whether or not a program with constant surface speed
control is executed continuously without waiting for attainment of the specified surface speed;
M61 specifies advance to the next block without waiting for attainment of the specified surface
speed, and M60 specifies advance to the next block only after attainment of the specified
surface speed.
(17) M63 (spindle rotation answer signal ignore)
The M codes relating to spindle control (M03, M04, M05, M19, M40 - M44) and S command are
executed at the same time with axis move commands specified in the same block.
(18) M73, M74, M75 (thread cutting pattern 1, 2, 3)
In multi-machining fixed cycle and thread cutting cycle in LAP, the cutting pattern (infeed
pattern) is specified by these M codes. M73 for pattern 1, M74 for pattern 2, and M75 for
pattern 3.
(19) M83, M84 (chuck clamp, unclamp)
Regardless of the chuck clamp direction (I.D. or O.D.), the M code used to specify the clamping
of a workpiece is always M83.
(20) M85 (no return to the start point after the completion of LAP roughing cycle)
In LAP4, a roughing cycle is called by G85 or G86. When this M code is specified, the cutting
tool does not return to the reference point of the cycle after the completion of the called
roughing cycle, and the next block is executed continuously.
(21) M86, M87 (turret clockwise rotation ON, OFF)
These M codes are used to specify whether or not the turret rotation direction is fixed in the
clockwise direction; M86 specifies turret clockwise rotation ON, and M87 specifies turret
clockwise rotation OFF.
SECTION 5 S, T, AND M FUNCTIONS
5238-E P-48
LE33013R0300700050001
Advertisement
Table of Contents
