Optimum OPTImill F 80 Betriebsanleitung Seite 378

Brief instruction 808D 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========
808D
Sample Program
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==
Page 378
OPTIMUM
M A S C H I N E N - G E R M A N Y
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==
Operating and Programming — Milling