4 - Fagor Automation

Canned cycles (·M· model)
2.4 G163. Multiple machining in a full circle
The programming format for this cycle is. When defining the machining operation, only use
one parameter of the group "I" and "K".
G163 X Y I K C F P Q R S T U V
Parameters "X" and "Y" define the center of the circle, same as "I" and "J" in circular
interpolations (G02, G03).
X Distance from the starting point to the center along the abscissa axis.
Y Distance from the starting point to the center along the ordinate axis.
When defining the machining operation, only one of parameters "I" and "K" is required. If the
angular step is programmed, bear in mind that the total angular movement must be 360º,
otherwise, the CNC will issue the relevant error message.
I Angular step between machining operations.
When the movement between points is done in G00 or G01, the sign indicates the direction:
"I+" counterclockwise and "I-" clockwise.
K Total number of machining operations including that of the machining definition point.
When the movement between points is done in G00 or G01, the machining operation is carried
out counterclockwise.
C It indicates how it will move between the machining points. If not programmed, a value of C
= 0 is assumed.
C=0 In rapid (G00).
C=1 Linear interpolation (G01).
C=2 In clockwise circular interpolation (G02).
C=3 In counterclockwise circular interpolation (G03).
F Feedrate for the movement between points. It will only be valid for "C" values other than zero.
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
2.
MULTIPLE MACHINING
G163. Multiple machining in a full circle
CNC 8065
(REF: 1209)
·75·