Special Canned Cycle; G34, G35, G36, G37.1 - Mitsubishi Electric MELDAS C6 Programming Manual

13. Program Support Functions

13.2 Special canned cycle; G34, G35, G36, G37.1

Function and purpose
The special canned cycle is used with the standard canned cycle. Before using the special canned
cycle, program the canned cycle sequence selection G code and hole machining data to record
the hole machining data. (If there is no positioning data, the canned cycle will not be executed, and
only the data will be recorded.)
Even after the special canned cycle is executed, the recorded standard canned cycled will be held
until canceled.
If the special canned cycle is designated when not in the canned cycle mode, only positioning will
be executed, and the hole drilling operation will not be done.
Bolt hole circle (G34)
G34 X x
X, Y
I
J
K
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)
I r J θ K n ;
Y y
1 1
:Positioning of bolt hole cycle center. This will be affected by G90/G91.
:Radius r of the circle. The unit follows the input setting unit, and is given with a
positive number.
: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 ° .)
: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 alarm P221 Special Canned Holes Zero will occur.
When input setting unit is 0.001mm
N001 G91 ;
N002 G81 Z − 10000 R5000 L0
N003 G90 G34 X200000 Y100000 I100000 J20000 K6 ;
N004 G80 ; ............... (Cancel of G81)
N005 G90 G0 X500000 Y100000 ;
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.
13.2 Special canned cycle
F200 ;
x
y =100mm
1
(500mm, 100mm)
Position before
G34 is executed
168
=200mm
1
n = 6 holes
I=100mm
N005 G0 command
20 °