FANUC T系列 Macro自動C軸循圓粗銑

     今天早上改了FANUC車床C軸自動循圓粗銑如下，順便用DIA畫了個流程圖，在文章最下面可以參考一下。注意 : 所有G65呼叫之變數皆以直徑值指示。因為沒有CNC車床可試，等過幾天我再拿到太平市給朋友試試看，因為他的車床是FANUC 18iT 64刀以下TYPE B，所以這個程式用在64刀以上時需要改。

可通孔可不通空孔，不通孔時粗銑圓鼻刀、精銑用平刀。這一個程式要試一下，因為我還沒試過。

O2266 (MAIN PROGRAM)
(CALLS MACRO O8888 by Shih Yu Chung )
N1 G21
N2 M66 T0101
N3 G12.1
N4 G00 X0 C0 S1200 M33
N5 Z25.0 M08
N6 G65 P8106 X50.0 C3.75 Z7.5 D49.0 K2.5 W4.0 T5 F500.0
N7 G28 Z0
N8 M67 T0100 M9
N9 G13.1 M05
N10 M01
...
%

O8888 (ROUGHING CIRCULAR POCKET MACRO)
(*** DO NOT CHANGE SEQUENCE NUMBERS ***)
IF[#7 EQ #0] GOTO9101
IF[#20 EQ #0] GOTO9102
IF[#23 EQ #0] GOTO9103
IF[#26 EQ #0] GOTO9104
IF[#9 EQ #0] GOTO9105
#10 = #4003
#120 = [ABS[#[2200+#20]+#[2900+#20]]]
#77 = ABS[#7/2]
IF[#120 GE #77] GOTO9106
#26 = ABS[#26]
#126 = #4006
IF[#126 EQ 20.0] THEN #126 = 0.1
IF[#126 EQ 21.0] THEN #126 = 2.0
G00 X#24 C#3
Z#126
G01 Z0 F[#9/2]
#16 = #26
IF[#6 EQ #0] GOTO1
#6 = ABS[#6]
GOTO2
N0001 #6 = #26
N0002 #4 = [#7-#120*2]
WHILE [#16 GE #6] DO1
#33 = #23
G01 Z-#6 F[#9/2]
WHILE [#33 LT #4] DO2
G01 X[#24+#33] F#9
G03 I-#33
#33 = #33+#23
END2
G01 X[#24+#4] F#9
G03 I-#4
G01 X#24 F[#9*3]
#16 = #16-#6
END1
IF[#16 LE 0] GOTO9000
G01 Z-#16 F[#9/2]
#33 = #23
WHILE[#33 LT #4] DO1
G01 X[#24+#33] F#9
G03 I-#33
#33 = #33+#23
END1
G01 X[#24+#4] F#9
G03 I-#4
G01 X#24 F[#9*3]
N9000 G00 Z#126
GOTO9999
N9101 #3000=101 (NO POCKET DIAMETER)
N9102 #3000=102 (NO T-OFFSET)
N9103 #3000=103 (NO CUTTING WIDTH)
N9104 #3000=104 (NO POCKET DEPTH)
N9105 #3000=105 (NO FEEDRATE)
N9106 #3000=106 (TOOL RADIUS TOO LARGE)
N9999 G#10
M99

%

流程圖

                                                                        update : 2010/4/15