4 - Fagor Automation

2.
MULTIPLE MACHINING
CNC 8065
(REF: 1209)
·66·
G160. Multiple machining in straight line
2.1 G160. Multiple machining in straight line
Canned cycles (·M· model)
The programming format for this cycle is. When defining the machining operation, only use
two parameters of the group "X", "I" and "K".
G160 A X I K P Q R S T U V
A Angle, in degrees of the machining path with respect to the abscissa axis.
If not programmed, a value of A = 0 is assumed.
When defining the machining operation, only two of parameters "X", "I" and "K" are required.
X Length of the machining path.
I Step between machining operations.
K Total number of machining operations in the section, including that of the machining definition
point.
X I X K I K
When selecting the "X-I" format, bear in mind that the resulting number of machining
operations must be an integer, otherwise, the CNC will issue the relevant error message.
P,Q,R,S,T,U,V These parameters are optional and are used to indicate at which points or between
which points of the ones programmed the machining operation will NOT be carried
out. If these parameters are not programmed, the CNC executes the machining
operation at all the points of the programmed path.
Thus, programming "P7" means that no machining operation takes place at point 7.
Programming "Q10.013" means that no machining takes place at points 10, 11, 12 and
13.
When defining a set of points (Q10.013), bear in mind that the last point must be defined
with three digits because, for example, "Q10.13" is the same as programming "Q10.130".
The programming order for these parameters is "P" "Q" "R" "S" "T" "U" "V" and the
numbering sequence for the points assigned to them must also be respected; In other
words, the numbering sequence of the points assigned to "Q" must be greater than the
one of those assigned to "P" and smaller than the one for those assigned to "R".
Example of proper programming: P5.006 Q12.015 R20.022
Example of wrong programming: P5.006 Q20.022 R12.015