Operator`s manual

Advanced Haas Mill Programming Techniques Training Manual Page 44
The following code may be used to program all five slots. First the tool is called up, a 5/8 carbide end mill in
the main program. Then the sub program O03904 is called which describes the tool path of the slot at 3
o’clock. That slot will be machined ending with the tool 1 inch above the part. Then the sub program
O3905 is call up 4 times using L4. Program O03905 incrementally rotates the coordinate 72° counter
clockwise around the part zero (X0, Y0) then calls up the tool path program O03904. Then all the rest of the
slots are created.
O03903 (CLOSED SLOT G68 MAIN PROG)
G28
T1 M06 (5/8 END MILL)
M98 P3904 (CALL TOOL PATH SUB)
M98 P3905 L4 (CALL ROTATION SUB 4 TIMES)
G91 G28 Z0 M05
G69 (CANCEL G68)
M30
O03904 (CLOSED SLOT TOOL PATH SUB)
N3 G90 G54 G00 X3. Y0 S9165 M03
N4 G43 Z0.1 H01 M08
N5 G01 Z0 F80.
N6 X1. Z-0.07 F183.
N7 X3. Z-0.14
N8 X1. Z-0.2
N9 X3.
N10 G41 X2.65 Y-0.025 D01 F90.
N11 G03 X3. Y-0.375 R0.35
N12 Y0.375 R0.375
N13 G01 X1.
N14 G03 Y-0.375 R0.375
N15 G01 X3.
N16 G03 X3.35 Y-0.025 R0.35
N17 G40 G01 X3. Y0
N18 G00 Z1. M09
M99
O03905 (INC G68 SHIFT SUB)
G91 G68 X0 Y0 R72.
M98 P3904
M99
Graphic screen shot of above program