·208·
Programming manual
CNC 8055
CNC 8055i
10.
MULTIPLE MACHINING
·M· & ·EN· MODELS
SOFT: V02.2X
G61: Multiple machining in rectangular pattern
10.2 G61: Multiple machining in rectangular pattern
The programming format for this cycle is:
[ A±5.5 ] Angle of the path with respect to the abscissa axis
Defines the angle that forms the machining path with the abscissa axis. It is expressed in degrees
and if not programmed, the value A=0 will be taken.
[ B±5.5 ] Angle between paths
Defines the angle formed by the two machining paths. It is expressed in degrees and if not
programmed, the value B=90 will be taken.
[ X5.5 ] Length of the path along the abscissa axis
Defines the length of the machining path according to the abscissa axis.
[ I5.5 ] Machining pass along the abscissa axis
Defines the pass between machining operations along the abscissa axis.
[ K5 ] Number of machining operations along the abscissa axis
Defines the total number of machining operations in the abscissa axis, including the machining
definition point.
Due to the fact that machining may be defined according to the abscissa axis with any two points
of the X I K group, the CNC allows the following definition combinations: XI, XK, IK.
Nevertheless, if format XI is defined, care should be taken to ensure that the number of machining
operations is an integer number, otherwise the CNC will show the corresponding error code.
[ Y5.5 ] Length of the path along the ordinate axis
Defines the length of the machining path according to the ordinate axis.
[ J5.5 ] Machining pass along the ordinate axis
Defines the pass between machining operations according to the ordinate axis.
[ D5 ] Number of machining operations along the ordinate axis
Defines the total number of machining operations in the ordinate axis, including the machining
definition point.
Due to the fact that machining may be defined according to the ordinate axis with any two points
of the Y J D group, the CNC allows the following definition combinations: YJ, YD, JD.
Nevertheless, if format YJ is defined, care should be taken to ensure that the number of machining
operations is an integer number, otherwise the CNC will show the corresponding error code.
G61 A B X I
X K
I K
Y J
Y D
J D
P Q R S T U V
To Next Page
Loading...
