Fagor 8055 M, Programming Manual

Page: 217 / 482

Programming manual
CNC 8055
CNC 8055i
MULT
IPL
E
MAC
H
INI
N
G
10.
·M· & ·EN· M
ODELS
S
OFT
: V02.2
X
·217·
G6
4
:
Mu
lt
ip
le
ma
ch
in
in
g
in
a
n
a
rc
10.5 G64: Multiple machining in an arc
The programming format for this cycle is:
[ X±5.5 ] Distance from the first machining point to the center along the abscissa axis
Defines the distance from the starting point to the center along the abscissa axis.
[ Y±5.5 ] Distance from the first machining point to the center along the ordinate axis
Defines the distance from the starting point to the center along the ordinate axis.
With parameters X and Y the center of the circle is defined in the same way that I and J do this in
circular interpolations (G02, G03).
[ B5.5 ] Angular travel
Defines the angular stroke of the machining path and is expressed in degrees.
[ I±5.5 ] Angular pass between machining operations
Defines the angular pass between machining operations. When moving from point to point in G00
or G01, the sign indicates the direction, "+" counterclockwise, "-" clockwise.
[ K5 ] Total number of machining operations
Defines the total number of machining operations along the circle, including the machining definition
point.
It will be enough to program I or K in the multiple machining definition block. Nevertheless, if K is
programmed in a multiple machining operation in which movement between points is made in G00
or G01, machining will be done counterclockwise.
[ C 0/1/2/3 ] Type of move from point to point
Indicates how movement is made between machining points. If not programmed, a value of C=0
is assumed.
C=0: Movement is made in rapid feedrate (G00).
C=1: Movement is made in linear interpolation (G01).
C=2: Movement is made in clockwise circular interpolation (G02)
C=3: Movement is made in counterclockwise circular interpolation (G03)
[ F5.5 ] Feedrate to move from point to point
Defines the feedrate that is used for moving from point to point. Obviously, it will only apply for "C"
values other than zero. If it is not programmed, the value F0 will be taken, maximum feedrate selected
by the "MAXFEED" axis machine parameter.
G64 X Y B I
K C F P Q R S T U V