·206·
Programming manual
CNC 8055
CNC 8055i
10.
MULTIPLE MACHINING
·M· & ·EN· MODELS
SOFT: V02.2X
G60: Multiple machining in a straight line
10.1 G60: Multiple machining in a straight line
The programming format for this cycle is:
[ A±5.5 ] Angle of the path
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.
[ X5.5 ] Path length
Defines the length of the machining path.
[ I5.5 ] Step between machining operations.
Defines the pass between machining operations.
[ K5 ] Number of machining operations.
Defines the number of total machining operations in the section, including the machining definition
point.
Due to the fact that machining may be defined 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.
[ P Q R S T U V ] Points where no drilling takes place
These parameters are optional and are used to indicate at which points or between which of those
programmed points it is not required to machine.
Thus, programming P7 indicates that it is not required to do machining at point 7, and programming
Q10.013 indicates that machining is not required from point 10 to 13, or expressed in another way,
that no machining is required at points 10, 11, 12 and 13.
When it is required to define a group of points (Q10.013), care should be taken to define the final
point with three digits, as if Q10.13 is programmed, multiple machining understands Q10.130.
The programming order for these parameters is P Q R S T U V, it also being necessary to maintain
the order in which the points assigned to these are numbered, i.e., the numbering order of the points
assigned to Q must be greater than that assigned to P and less than that assigned to R.
Example:
Proper programming P5.006 Q12.015 R20.022
Correct programming P5.006 Q12.015 R20.022
If these parameters are not programmed, the CNC understands that it must perform machining at
all the points along the programmed path.
radius X I
X K
I K
P Q R S T U V
To Next Page
Loading...
