13. Program Support Functions
13.2 Special Fixed Cycle
283
Bolt hole circle (G34)
G34 X x
1
Y y
1
I r J
θ
K n ;
X, Y
:Positioning of bolt hole cycle center. This will be affected by G90/G91.
I
:Radius r of the circle. The unit follows the input setting unit, and is given with a
positive number.
J :Angle
θ
of the point to be drilled first. The CCW direction is positive.
(The decimal point position will be the degree class. If there is no decimal point,
the unit will be 0.001
°
.)
K
:No. of holes n to be drilled. 1 to 9999 can be designated, but 0 cannot be
designated. When the value is positive, positioning will take place in the CCW
direction, and when negative, will take place in the CW direction.
If “0” is designated, the program error (P221) will occur.
Drilling of n obtained by dividing the circumference by n will start at point created by the Z axis and
angle
θ
. The circumference is that of the radius R centering on the coordinates designated with XX
and Y. The hole drilling operation at each hole will hold the drilling data for the standard canned
cycle such as G81.
The movement between hole positions will all be done in the G00 mode. G34 will not hold the data
even when the command is completed.
(Example)
With 0.001mm least command increment
Position prior to excution
of G34 command
G0 command in
N005
N001 G91 ;
N002 G81 Z – 10.000 R5.000 L0 F200 ;
N003 G90 G34 X200.000 Y100.000 I100.000 J20.000 K6 ;
N004 G80 ; .........................(G81 cancel)
N005 G90 G0 X500.000 Y100.000 ;
(500 mm, 100 mm)
20
°
n = 6 holes
I = 100 mm
X1 = 200 mm
Y1 = 100 mm
W
(Example)
As shown in the example, the tool position after the G34 command is completed is over
the final hole. When moving to the next position, the coordinate value must be
calculated to issue the command with an incremental value. Thus, use of the absolute
value mode is handy.
(Note 1)
If an address other than the selected plane's vertical axis, horizontal axis, G, N,
I, J, K, H, O, P, F, M, S or 2nd miscellaneous function is issued in the same
block as the G34 command, a program error (P32) will occur.
