![一日一例——子程序加工蝸桿](http://p2.ttnews.xyz/loading.gif)
左端程序參考:
O0001;
G0 G40 G97 G99 S500 T11 M03 F0.2;
X42.0 Z2.0;
G71 U2.0 R0.5;
G71 P10 Q11 U0.4 W0.03;
N10 G0 G42 X20.0;注意刀具不要與頂夾干涉注意刀具不要與頂夾干涉注意刀具不要與頂夾干涉
G01 Z0;
X24.0C1.5;
Z-15.0;
X28.0C1.5;
Z-25.0;
X38.0 A110.0;
Z-130.0;
N11 G01 G40 X40.0;
G0 X200.0 Z2.0;粗加工完成後,刀具的退刀點及換刀點
M05;
切10mm寬的蝸桿退刀槽
G0 G40 G97 G99 S300 T66 M03 F0.05;
X42.0 Z-80.0;
G75 R0.5;
G75 X29.0Z-85.0 P2000 Q2000;
G0 X200.0 Z2.0;
M05;
左端外形輪廓精加工
G0 G40 G97 G99 S800 T22 M03 F0.1;
X42.0 Z2.0;
G70 P10Q11;
G0 X200.0 Z2.0;
M05;
蝸桿分度圓以上粗加工,刀寬3.0mm,刀刃中心對刀
G0 G40 G97 G99 S200 T33 M03;
X42.0 Z-15.0;
G76 P020000 Q50 R0.05;直進法切削
G76 X34.0 Z-85.0 P2000 Q300 F6.283;
G0 X200.0 Z2.0;
M05;
蝸桿齒根圓至分度圓之間粗加工,刀寬1.1mm,刀刃中心對刀
G0 G40 G97 G99 S200 T44 M03 ;
X42.0 Z-15.0;
G76 P020000 Q50 R0.05;直進法切削
G76 X29.3 Z-85.0 P2350 Q300 F6.283;蝸桿底徑留0.1mm的加工餘量
G0 X200.0 Z2.0;加工完成後,刀具的退刀點及換刀點加工完成後,刀具的退刀點及換刀點加工完成後,刀具的退刀點及換刀點
M05;
蝸桿右端精加工,刀寬1.1mm,單面成形刀,刀刃中心對刀,斜進法
G0 G40 G97 G99 S200 T55 M03;
X53.2;
Z-15.0;
W1.785;
M98 P180002;調用蝸桿右端精加工子程序18次
G0 X200.0 Z2.0;
M05;
蝸桿左端精加工,刀寬1.1mm,單面成形刀,刀刃中心對刀,斜進法
G0 G40 G97 G99 S200 T77 M03;
X53.2 Z-15.0;
W-1.785;
M98 P180003;調用蝸桿左端精加工子程序18次
G0 X200.0 Z2.0;
M05;
M30;
蝸桿右端精加工子程序
O0002;
G0 U-15.0;
U-0.5 W-0.091;
G32 W-70.0 F6.283;
G0 U15.0;
W70.0;
M99;
蝸桿左端精加工子程序
O0003;
G0 U-15.0;
U-0.5 W0.091;
G32 W-70.0 F6.283;
G0 U15.0;
W70.0;
M99;
閱讀更多 機械首條 的文章