808D Page 91 Operating and Programming — Milling
Sample
Program
s
Machining Process
Drawing
Tool information
T1 Milling tool D50 T5 Milling tool D5
T2 Milling tool D12 T6 Drilling tool D10
T3 Milling tool D10 T7 Drilling tool D5
T4 Milling tool D16 T8 Tap D6
Milling
program 3
Part of the cycles in the program are
taken as examples in Section 5, “Create
Part Program Part 2”!
N10 G17 G90 G54 G71
N20 SUPA G00 Z300 D0
N30 SUPA G00 X300 Y300
N40 T1 D1
N50 MSG ("Please change to Tool No 1")
N60 M05 M09 M00
N70 S4000 M3
; =======Face milling start========
N80 CYCLE71( 50, 2, 2, 0, 0, 0, 70, 100,
0, 2, 40, 2, 0.2, 500, 41, 5)
N90 S4500 M3
N100 CYCLE71( 50, 2, 2, 0, 0, 0, 70, 100,
0, 2, 40, 2, 0.2, 300, 22, 5)
; ========Face milling end========
N110 SUPA G00 Z300 D0
N120 SUPA G00 X300 Y300
; =======Path milling start========
N130 T3 D1
N140 MSG( "Please change to Tool No 3")
N150 M05 M09 M00
N160 S5000 M3 G94 F300
N170 G00 X-6 Y92
N180 G00 Z2
N190 G01 F300 Z-10
N200 G41 Y 90
N210 G01 X12 RND=5
N220 G01 Y97 CHR=2
N230 G01 X70 RND=4
N240 G01 Y90
N250 G01 G40 X80
N260 G00 Z50
; ========Path milling end========
N10
N20
N30
N40
N50 hint:change to tool 1
N60
N70
; =======Face milling start=======
N80 start point (X0,Y0), machining length: X
→70 mm, Y→100 mm, angle between verti-
cal axis and X axis is 0º, finishing allow-
ance 0.2 mm, feedrate 500 mm/min, along the
alternate direction parallel to the Y axis to
perform the finishing
N90
N100 repeat N80 contour process, the
difference in the feedrate is 300 mm/min along
the single direction parallel to the Y axis to
perform the finishing
; =========Face milling end=======
N110
N120
; ======Path milling start=========
N130
N140 hint:change to tool 3
N150
N160 feedrate 300 mm/min
N170
N180
N190
N200 left side radius compensation
N210 circle, milling radius is 5 mm
N220 incline, milling side length is 2 mm
N230
N240
N250 cancel tool radius compensation
N260
; =========Path milling end======
To Next Page
Loading...
Need help?
General
