数控铣加工与编程-06数控铣削编程与加工资源-课件

数控铣削编程与加工项目六配合件的加工图6.1配合件1零件图

在数控铣床上加工如图6.1、6.2所示的配合件零件。零件材料为45钢，已完成上下平面及周边侧面的预加工。项目任务图6.2配合件2零件图项目任务项目实施一、制定零件加工工艺1.零件结构及技术要求分析该零件为配合件，零件外轮廓为正方形，零件配合精度要求较高。2.零件加工工艺及工装分析

（1）加工机床的选择：用立式数控铣床，机床系统：FANUC0i系统或SIEMENS802D系统。

（2）工件的装夹：以底面和侧面作为定位基准，工件采用平口钳装夹，装夹时，钳口内垫上合适的高精度平行垫铁，垫铁间留出加工型腔时的落刀间隙，装夹后要进行工件的校正。工件装夹后所处的坐标位置应与编程中的工件坐标位置相同。

（3）加工方法及刀具的选择：在进行配合件加工时，要合理控制好首件凸、凹结构的尺寸大小，一般取尺寸偏差的上、下偏差，为加工配合工件尺寸精度和配合精度奠定基础。根据图样要求首先加工件1，然后加工件2。件2加工完成后，必须在拆卸之前与件1进行配合，若间隙偏小，可改变刀具半径补偿，将轮廓进行再加工，直至配合情况良好后方可取下件2。配合件1的加工方案为：1）铣削平面，保证尺寸10mm，选用Φ80mm面铣刀。2）钻两工艺孔，Φ11.8mm直柄麻花钻。3）粗加工两个凹型腔，选用Φ14mm三刃立铣刀。4）精加工两个凹型腔，选用Φ12mm四刃立铣刀。5）点孔加工，选用Φ3mm中心钻。6）钻孔加工，选用Φ11.8mm直柄麻花钻。7）铰孔加工，选用Φ12mm机用铰刀。项目实施配合件2的加工方案为：1）铣削平面，保证尺寸28.5mm，选用Φ80mm面铣刀。2）粗加工两个凸台外轮廓，选用Φ16mm三刃立铣刀。3)铣削边角料，选用Φ16mm三刃立铣刀。4）钻中间位置孔，选用Φ11.8mm直柄麻花钻。5）扩中间位置孔，选用Φ35mm锥柄麻花钻。6）精加工两个凸台外轮廓，并保证8mm和10mm的高度,选用Φ12mm四刃立铣刀。7）粗镗Φ38.5mm孔，选用Φ37.5mm粗镗刀。8）精镗Φ38mm孔，选用Φ38mm精镗刀。9）点孔加工，选用Φ3mm中心钻。10）钻孔加工，选用Φ11.8mm直柄麻花钻。11）铰孔加工，选用Φ12mm机用铰刀。12）孔口R5圆角，选用Φ14mm三刃立铣刀。项目实施（4）切削用量的选择：工件材料为45钢，主轴转速选择时，粗加工及去除余量时取较低值，精加工时选择最大值；粗加工时进给速度选择较大值，精加工进给速度应选择较小值；轮廓深度有公差要求时分两次切削，留一些精加工余量。3.数控加工工艺文件件1、件2数控加工工序卡如下表所示。项目实施2钻两个凹型腔工艺孔T02Φ11.8mm直柄麻花钻高速钢55080H023粗加工两个凹型腔（落料）T03Φ14mm粗齿三刃立铣刀高速钢50080H03D01=7.24精加工两个凹型腔T04Φ12mm细齿四刃立铣刀高速钢800100H04D02=5.9855点孔加工T05Φ3mm中心钻高速钢1200120H056钻孔加工T02Φ11.8mm直柄麻花钻高速钢55080H027铰孔加工T06Φ12mm机用铰刀高速钢30050H06编制审核批准第页共页注：H01～H06中的数值根据具体加工和对刀情况而定。项目实施表6.3件2零件数控加工工序卡数控加工工序卡片工序号工序内容单位零件名称零件图号材料夹具名称使用设备配合件22-6-245#钢精密平口虎钳数控铣床工步号工步内容刀具号刀具规格/mm主轴转速(r.min-1)进给速度(mm.min-1)长度补偿（FANUC）半径补偿（FANUC）项目实施1粗、精加工上表面T01Φ80mm面铣刀（5个刀片）硬质合金450/800300/160H012粗加工两个个凸台外轮廓面T07Φ16mm粗齿三刃立铣刀高速钢500120H07D03=8.23铣削边角料T07Φ16mm粗齿三刃立铣刀高速钢500120H07D03=8.24钻中间位置孔T02Φ11.8mm直柄麻花钻高速钢55080H025扩中间位置孔T08Φ35mm锥柄麻花钻高速钢15020H086精加工两个个凸台外轮廓面T04Φ12mm细齿四刃立铣刀高速钢800100H04D04=5.985项目实施7粗镗孔Φ37.5mmT09Φ37.5mm粗镗刀硬质合金85080H098精镗孔Φ38mmT10Φ38mm精镗刀硬质合金100040H109点孔加工T05Φ3mm中心钻高速钢1200120H0510钻孔加工T02Φ11.8mm直柄麻花钻高速钢55080H0211铰孔加工T06Φ12mm机用铰刀高速钢30050H0612孔口R5mm圆角T03Φ14mm粗齿三刃立铣刀高速钢8001000H03编制审核批准第页共页项目实施二、编制数控加工程序

1.坐标系的确定件1和件2编程坐标系原点设在工件上表面。利用寻边器或分中棒、Z轴设定器或量块对刀，确定工件坐标系原点O。2.编写加工程序FANUCOiM系统及SIEMENS802DM数控系统的指令及规则编写加工程序如下表6.6、6.7所示。项目实施程序（FANUC0iM系统）程序(SIEMENS802DM系统)注释粗加工上表面O0268G54G90G17G21G94G49G40M03S450G00G43Z150H01X125Y-30Z0.3G01X-125F300G00Y30G01X125G00Z150M05M00XK3211.MPFG54G90G17G71G94G40M3S450G0D2Z150X125Y-30Z0.3G1X-125F300G0Y30G1X125G0Z150M5M0建立工件坐标系，用Φ80mm面铣刀调用1号刀具长度补偿程序暂停（利用厚度千分尺测量厚度，确定精加工余量）表6.6件1数控加工参考程序精加工上表面M03S800G00X125Y-30M07Z0G01X-125F160G00Y30G01X125G00Z150M09M05M00M3S800G0X125Y-30M7G1X-125F160G0Y30G1X125G0Z150M9M5M0程序暂停（手动换刀，更换Φ11.8mm麻花钻）钻两个凹型腔工艺孔M03S550G00G43Z150H02X0Y0M07G83G99X0Y25Z-16Q5R2F80X-55Y35G00Z150M09M05M00M3S550F80G0D2Z150M7MCALLCYCLE83(10,0,2,-16,16,-5,5,0,0,1,1,1)X0Y25X-55Y35MCALLG0Z150M9M5M0调用2号刀具长度补偿程序暂停（手动换刀，更换Φ14mm粗齿立铣刀）项目实施粗加工两个凹型腔（落料）M03S500G00G43Z150H03X0Y25M07Z1G01Z-10.5F40G41G01X-13.381Y40D01F80M98P1G00Z5X-55Y35Z1G01Z-10.5F40G41X-73.944Y28.447D01F80M98P2G00Z150M09M05M00

M3S500G0D2Z150X0Y25M7Z1G1Z-10.5F40G41G1X-8.381Y40D1F80X-13.381L1G0Z5X-55Y35Z1G1Z-10.5F40G41X-63.944Y28.447D1F80X-73.944L2G0Z150M9M5M0调用3号刀具长度补偿引入1号刀具半径补偿值调用子程序O0001，加工中间凹型腔调用子程序O0002，加工键形腔项目实施精加工两个凹型腔M03S800F100G00G43Z150H04X0Y25M07Z-10.5G01G41X-13.381Y40D02M98P1G00Z5X-55Y35Z-10.5G01G41X-73.944Y28.447D02M98P2G00Z150M09M05M00M3S800F100G0D2Z150X0Y25M7Z-10.5G1G41X-8.381Y40D1X-13.381L1G0Z5X-55Y35Z-10.5G1G41X-63.944Y28.447D1X-73.944L2G0Z150M9M5M0调用4号刀具长度补偿引入2号刀具半径补偿值调用子程序O0001，加工中间凹型腔调用子程序O0002，加工键形腔程序暂停,更换Φ3mm中心钻项目实施点孔加工M03S1200G00G43Z150H05X0Y0G81G99X65Y0Z-5R2F120G00Z150M05M00M42M3S1200F120G0D2Z150X65Y0CYCLE81(10,0,2,-5,5)G0Z150M5M0主轴选用高速档（800~5300r/min）调用5号刀具长度补偿程序暂停（更换Φ11.8mm麻花钻）钻孔加工M03S550G43G00Z100H02X0Y0M07G83G99X65Y0Z-15Q5R2F80G00Z150M09M05M00

M41M3S550F80G0D2Z150X65Y0M7CYCLE83(10,0,2,-16,16,-5,5,0,0,1,1,1)G0Z150M9M5M0主轴选用低速档（50~800r/min）调用2号刀具长度补偿程序暂停（更换Φ12mm机用铰刀）项目实施铰孔加工M03S300G43G00Z100H06M07X0Y0G85G99X65Y0Z-15R2F50G00G49Z50M05M30

M3S300F50G0D2Z150M7X65Y0CYCLE85(10,0,2,-16,16,0,50,50)G0Z50M9M5M30调用6号刀具长度补偿程序结束回起始位置，机床复位（切削液关，主轴停转）项目实施子程序O0001（中间凹型腔）O0001G03X-20.309Y36R8G01X-48.928Y-13.569G03X-50Y-17.569R8G01Y-32G03X-42Y-40R8G01X42G03X50Y-32R8G01Y-23.664G03X47.576Y-17.928R8G02Y17.928R28G03X50Y23.664R8G01Y32G03X42Y40R8G01X-13.381G40X0Y25M99

L01.SPFG3X-20.309Y36CR=8G1X-48.928Y-13.569G3X-50Y-17.569CR=8G1Y-32G3X-42Y-40CR=8G1X42G3X50Y-32CR=8G1Y-23.664G3X47.576Y-17.928CR=8G2Y17.928CR=28G3X50Y23.664CR=8G1Y32G3X42Y40CR=8G1X-13.381G40X0Y25RET

子程序名子程序结束，返回主程序项目实施子程序O0002（键形腔）O0002G03X-58.623Y15.519R-10G01X-39.34Y38.572G03X-54.66Y51.428R-10G01X-73.944Y28.447G40X-55Y35M99L02.SPFG3X-58.623Y15.519CR=-10G1X-39.34Y38.572G3X-54.66Y51.428CR=-10G1X-73.944Y28.447G40X-55Y35RET

子程序名子程序结束，返回主程序项目实施表6.7件2数控加工参考程序程序（FANUC0i系统）程序(SIEMENS802D系统)注释粗加工上表面G55G90G17G21G94G49G40M03S450G00G43Z150H01X125Y-30Z0.3G01X-125F300G00Y30G01X125G00Z150M05M00

G55G90G17G71G94G40M3S450G0D2Z150X125Y-30Z0.3G1X-125F300G0Y30G1X125G0Z150M5M0

建立工件坐标系，用Φ80mm面铣刀调用1号刀具长度补偿程序暂停（利用厚度千分尺测量厚度，确定精加工余量项目实施精加工上表面M03S800G00X125Y-30M07Z0G01X-125F160G00Y30G01X125G00Z150M09M05M00

M3S800G0X125Y-30M07Z0G1X-125F160G0Y30G1X125G0Z150M9M5M0程序暂停（手动换刀，更换Φ16mm粗齿立铣刀）项目实施粗加工两个凸台外轮廓面M03S500F120G00G43Z150H07X92Y0M07Z-10G41G01X50Y-14D03M98P3G41G01X58.623Y15.591D03M98P4G01X73Y-60X65Y-46Y-53X-81X-65Y-46X-73Y0X-63Y-10Y10X-73Y6Y60X-65Y46Y53X25Y70G00X75G01Y50G00Z150M09M05M00M3S500F120G0D2Z150X92Y0M7Z-10G41G1X60Y-14D3X50L3G41G1X58.623Y10.591D3Y15.591L4G1X73Y-60X65Y-46Y-53X-81X-65Y-46X-73Y0X-63Y-10Y10X-73Y6Y60X-65Y46Y53X25Y70G0X75G1Y50G0Z150M9M5调用7号刀具长度补偿引入3号刀具半径补偿值调用子程序O0003，加工中间凸台调用子程序O0004，加工键形凸台程序暂停（更换Φ11.8mm麻花钻）项目实施钻中间位置孔M03S550F80G00G43X0Y0Z150H02X0Y0M07G83G99X0Y0Z-35Q5R2F80G00Z150M09M05M00

M3S550F80G0D2Z150X0Y0M7CYCLE83(10,0,2,-35,35,-5,5,0,0,1,1,1)G0Z150M9M5M0调用2号刀具长度补偿程序暂停（更换Φ35mm麻花钻）扩中间位置孔M03S150F20G00G43Z150H08X0Y0M07G83G99X0Y0Z-40Q-5R2F20G00Z150M09M05M00

M3S150F20G0D2Z150X0Y0M7CYCLE83(10,0,2,-40,40,-5,5,0,0,1,1,1)G0Z150M9M5M0调用8号刀具长度补偿程序暂停（更换Φ12mm立铣刀）项目实施精加工两个凸台外轮廓面M03S800F100G00G43Z150H04X92Y0M07Z-10G41G01X50Y-14D04M98P3G41G01X58.623Y15.591D04M98P4G00Z5X32Y55.098Z-2G01X68.881Y11.144X76.542Y17.572X40.941Y60G00Z150M09M05M00M3S800F100G0D2Z150X92Y0M7Z-10G41G1X60Y-14D4X50L3G41G1X58.623Y10.591D4Y15.591L4G0Z5X32Y55.098Z-2G1X68.881Y11.144X76.542Y17.572X40.941Y60G0Z150M9M5M0调用4号刀具长度补偿引4号入刀具半径补偿值调用子程序O0003，加工中间凸台调用子程序O0004，加工键形凸台程序暂停（手动换刀，更换Φ37.5mm粗镗刀）项目实施粗镗孔Φ37.5mmM03S850G43G00Z100H09M07X0Y0G85G99X0Y0Z-30R2F80G00Z100M09M05M00

M42M3S850F80G0D2Z150X0Y0M7CYCLE85(10,0,2,-30,30,0,80,100)G0Z150M9M5M0

主轴选用高速档（800~5300r/min）调用9号刀具长度补偿程序暂停（手动换刀，更换Φ38mm精镗刀）精镗孔Φ38mmM03S1000G43G00Z100H10M07X0Y0G85G99X0Y0Z-30R2F40G00Z100M09M05M00

M3S1000F40G0D2Z150X0Y0M7CYCLE85(10,0,2,-30,30,0,40,60)G0Z150M9M5M0

调用10刀具号长度补偿程序暂停（更换Φ3mm中心钻）项目实施点孔加工M03S1200G00G43Z150H05X0Y0G81G99X-65Y0Z-12R2F120G00Z150M05M00

M3S1200F120G0D2Z150X-65Y0CYCLE81(10,0,2,-12,12)G0Z150M5M0调用5号刀具长度补偿程序暂停（更换Φ11.8mm麻花钻）钻孔加工M03S550G43G00Z100H02X0Y0M07G83G99X-65Y0Z-35Q5R2F80G00Z150M09M05M00M41M3S550F80G0D2Z150X-65Y0M7CYCLE83(10,0,2,-35,35,-5,5,0,0,1,1,1)G0Z150M9M5M0主轴选用低速档（50~800r/min）调用刀具2号长度补偿程序暂停（更换Φ12mm机用铰刀）项目实施铰孔加工M03S300G43G00Z100H06M07X0Y0G85G99X-65Y0Z-35R2F50G00Z150M09M05M00

M3S300F50G0D2Z150M7X-65Y0CYCLE85(10,0,2,-30,30,0,50,50)G0Z150M9M5M0

调用6号刀具长度补偿程序暂停（更换Φ14mm立铣刀）项目实施孔口R5mm圆角M03S800G43G00Z100H03X0Y0M07Z0G01X17F60#1=0#2=-7#3=7+#1#4=SQRT[7*7-#3*#3]#5=17-#4G01X[#5]Y0Z[#1]F1000G02I[-#5]J0#1=#1-0.02IF[#1GE#2]GOTO123G00G49Z50M30M3S800G0D2Z150X0Y0Z0G1X17F60R1=0R2=-5MARKE1:R3=5+R1R4=SQRT(5*5-R3*R3)R5=17-R4G1X=R5Y0Z=R1F1000G2I=-R5J0R1=R1-0.02IFR1>=R2GOTOBMARKE1G0Z50D0M9M5M30调用刀具3号长度补偿程序结束回起始位置，机床复位（切削液关，主轴停转）项目实施子程序O0003（中间凸台）OO003G01Y-32G02X42Y-40R8G01X-42G02X-50Y-32R8G01Y-23.664G02X-47.576Y-17.928R8G03Y17.928R28G02X-50Y23.664R8G01Y32G02X-42Y40R8G01X13.381G02X20.309Y36R8G01X48.928Y-13.569G02X50Y-17.569R8G40G01X60Y0M99L03.SPFG1Y-32G2X42Y-40CR=8G1X-42G2X-50Y-32CR=8G1Y-23.664G2X-47.576Y-17.928CR=8G3Y17.817CR=28G2X-50Y23.664CR=8G1Y32G2X-42Y40CR=8G1X13.381G2X20.309Y36CR=8G1X48.928Y-13.569G2X50Y-17.569CR=8G40G1X60Y0RET子程序名子程序结束，返回主程序项目实施子程序O0003（键形凸台）OO004G01X39.34Y38.572G02X54.66Y51.428R-10G01X73.944Y28.447G02X58.623Y15.519R-10G40G01X55Y0M99L04.SPFG1X39.34Y38.572G2X54.66Y51.428CR=-10G1X73.944Y28.447G2X58.623Y15.519CR=-10G40G1X55Y0RET

子程序名子程序结束，返回主程序项目实施1．选择机床、数控系统并开机。2．机床各轴回参考点。3．安装工件。4．安装刀具并对刀。5．输入加工程序，并检查调试。6．手动移动刀具退至距离工件较远处。7．自动加工。8．测量工件，优化程序，对工件进行误差与质量分析。三、加工中心加工项目实施四、形位精度和配合精度分析1.形位精度

形位精度