Table of Contents
Advertisement
6-3.
Transverse Grooving/Drilling Fixed Cycle (G74)
In the G74 mode, a grooving cycle is performed as shown below.
Z
X
E
[Programming format]
G74 X__ Z__ I__ K__ D__ L__ F__ E__ T__
X
: X coordinate of target point
Z
: Z coordinate of target point
I
: Shift amount in X-axis direction
(as a diameter; if no I word is specified, the control assumes I = 0)
K
: Shift amount in Z-axis direction (if no K word is specified, the control assumes K = 0)
D
: Depth of cut (infeed amount)
L
: Total infeed amount for tool withdrawal motion
(The sequence is not performed when no L word is specified.)
D
: Retraction amount "a" is specified. When no DA word is specified, the amount set at Pecking
A
amount in grooving and drill cycle of optional parameter (OTHER FUNCTION 1) is used as
the retraction amount. This applies both in the G94 and G95 modes.
E
: Duration of dwell when target point on Z-axis is reached
(Command unit is the same as an F word in G04 mode.)
If no E word is specified, this sequence is not performed.
T
: Tool offset number determining the tool offset amount when target point on X-axis is reached.
(If no T word is specified, the tool offset number selected on positioning to the starting point
of the grooving cycle is selected. The T command after this block is the one designated when
positioning to the starting point is performed.)
α
D
D
L
L
SECTION 7 FIXED CYCLES
T when positioning to the
coordinates of the target point
End point
I/2
Starting point
T when positioning to the
coordinates of the starting point
D
K
5238-E P-128
LE33013R0300900210001
Advertisement
Table of Contents
