240
PROGRAMMING EXAMPLES
96-8000
June 1999
GENERAL P URPOSE P OCKET M ILLING
The general purpose pocket milling program is included in the Haas control. This program is used to mill
irregular shapes and is capable of leaving islands and bosses within a contour. With the G150, there is a main
program for technical input and a subprogram for contour definition.
PROGRAM LINE REQUIREMENTS:
X = X-axis position of the starting hole
Y = Y-axis position of the starting hole
Z = Final depth of the hole
F = Feed rate
R = Reference plane
Q = Incremental Z-axis cut depth per pass
I = X-axis cut increment
J = Y-axis cut increment
K = finish cut allowance
P = Subprogram number
D = Geometry offset number
G41 or G42 = Cutter compensation turn ON
G150 FORMAT EXAMPLE:
%
O4500
T1 M06
G00 G90 G54 X0 Y0 S3500 M03
G43 H01 Z.1 M08
G150 X__ Y__ Z__ F__ R__ Q__ I__ OR J__ K__ P4600 D__ G41 OR G42
G00 Z1.0 M09
G28 G40 G91 Y0 Z0
M30
%
%
O4600
G01 X__ Y__
X__
Y__
X__ Y__
M99
%
The shape of the pocket to be cut must be defined by a series of motions within a subprogram. One of either I
or J must be specified. If I is used, the pocket is cut from a series of strokes in the X-axis. If J is used, the
pocket is cut from a series of strokes in the Y-axis. The value entered with the I or J will be the shift amount or
cutter overlap. The K amount is the finishing allowance for the walls of the pocket.
To Next Page
Loading...
Need help?
General
