OPTIMUM
M A S C H I N E N - G E R M A N Y
808D
Page 137
Sample Program
Brief instruction 808D Milling
Operating and Programming — Milling
Machining Process
N270
SUPA G00 Z300 D0
N280
SUPA G00 X300 Y300
N290
T4 D1
N300
MSG ("Please change to Tool No 4")
N310
M05 M09 M00
; ===Circular pocket milling start====
N320
S5000 M3
N330
POCKET4( 50, 0, 2, -5, 22, 38, 70, 2.5,
0.2, 0.2, 300, 250, 0, 21, 10, 0, 5, 2, 0.5 )
N340
S5500 M3
N350
POCKET4( 50, 0, 2, -5, 22, 38, 70, 2.5,
0.2, 0.2, 250, 250, 0, 22, 10, 0, 5, 2, 0.5 )
; ===Circular pocket milling end====
N360
SUPA G00 Z300 D0
N370
SUPA G00 X300 Y300
N380
T5 D1
N390
MSG ("Please change to Tool No 5")
N400
M05 M09 M00
; ========Slot milling start========
N410
M3 S7000
N420
SLOT2( 50, 0, 2, , 3, 3, 30, 6, 38, 70,
20, 165, 90, 300, 300, 3, 3, 0.2, 0, 5, 250,
3000, )
; ========Slot milling end========
N270
N280
N290
N300
hint:change to tool 4
N310
; ====Circular pocket milling start===
N320
N330
milling circular groove(depth 5 mm, radius
22 mm, groove center coordinate (X38,Y70),
finishing allowance 0.2 mm, plane machining
feedrate 300 mm/min, depth machining feedrate
250 mm/min, milling in positive direction, along
helical path insert to do rough machining, helical
path radius 2 mm, insert depth 0.5 mm)
N340
N350
repeat N370 milling process, the difference
is the machining allowance.
; ====Circular pocket milling end===
N360
N370
N380
N390
hint:change to tool 5
N400
; ========Slot milling start=======
N410
N420
milling slot(depth 3 mm, machining 3 slots,
slot angle 30º, slot width 6 mm, basic circle center
point coordinate(X38,Y70), basic circle radius 20
mm, start angle 165º, slot incremental angle 90º,
depth machining feedrate 300 mm/min, plane
machining feedrate 300 mm/min, milling direction
G3, slot edge finishing allowance 0.2 mm, complete
machining ways, finishing machining feedrate 250
mm/min, spindle speed rate 3000 r/min
; ========Slot milling end=======
N430
SUPA G00 Z300 D0
N440
SUPA G00 X300 Y300
; ======Contour milling start======
N450
T2 D1
N460
MSG ("Please change to Tool No 2")
N470
M05 M09 M00
N480
S5000 M3
N490
CYCLE72( "SUB_PART_3", 50, 0, 2, -5,
5, 0, 0, 300, 100, 111, 41, 12, 3, 300, 12, 3 )
; ======Contour milling end=======
N500
SUPA G00 Z300 D0
N510
SUPA G00 X300 Y300
; =Rectangular pocket milling start==
N520
T2 D1
N530
MSG ("Please change to Tool No 2")
N540
M05 M09 M00
N550
S6500 M3
N560
POCKET3( 50, 0, 1, -3, 40, 30, 6, 36,
24.1, 15, 3, 0.1, 0.1, 300, 300, 0, 11, 12, 8, 3,
15, 0, 2 )
N570
POCKET3( 50, 0, 1, -3, 40, 30, 6, 36,
24.1, 15, 3, 0.1, 0.1, 300, 300, 0, 12, 12, 8, 3,
15, 0, 2 )
; ==Rectangular pocket milling end==
N430
N440
; ======Contour milling start======
N450
N460
hint:change to tool 2
N470
N480
N490
contour cutting depth 5 mm, surface
machining feedrate 300 mm/min, cutting direction
feedrate 100 mm/min, use G41 to activate
compensation, use G1 to do rough machining, back
to the machining plane at the end of the contour,
approach path is along 1/4 circle in space, length 3
mm, the parameters of feedrate//path/length for
retraction and approach are equal.
; ======Contour milling end=======
N500
N510
; =Rectangular pocket milling start==
N520
N530
hint:change to tool 2
N540
N550
N560
milling rectangle groove (depth 3 mm,
length 40 mm, width 30 mm, corner radius 6
mm,groove base point coordinate (X36,Y24.1),
angle between groove vertical axis and plane X
axis is 15º), finishing allowance 0.1 mm, feedrate
surface machining and cutting direction machining
is 300 mm/min, milling in positive direction, rough
machining, use G1 vertical groove center to insert.
N570
repeat N600 milling process, the difference
is the machining allowance.
; ==Rectangular pocket milling end==
