关 键 词：

双面 型腔件 三维 造型 编程 仿真 数控 铣削 加工 工艺 NX CAD

资源描述：

双面型腔件三维造型、编程仿真及数控铣削加工工艺含NX三维及CAD图.zip,双面,型腔件,三维,造型,编程,仿真,数控,铣削,加工,工艺,NX,CAD

内容简介：

摘要本次毕业设计是通过应用UG软件、机械设计资料和所学的知识对双面型腔件进行工艺分析、三维建模、数控加工编程及加工。工艺分析是设计产品重点；三维建模、数控加工编程是UG软件的重点所在，具有操作简单和修改方便等优点；加工是对所设计的产品进行检测。关键词: UG软件、工艺分析、建模、编程、加工IIIAbstractThe graduation project is through the application of UG software, mechanical design information and knowledge learned in the cavity of the double-sided documents for process analysis, three-dimensional modeling, NC programming and machining. Process analysis is to design product priorities; three-dimensional modeling, NC programming is the focus of UG software, is simple and easy and modified; processing of products is designed to detect.Keyword ：UG software ，Process Analysis，Modeling ，Programming，Processing目录摘要IIAbstractIII第一章 绪论11.1 UG介绍1第二章 双面型腔工艺分析与设计22.1计算零件的生产纲领、确定生产类型22.2零件图的工艺分析22.2.1读图和审图32.2.2数控加工内容的选择32.2.3零件结构的工艺性32.2.4重要部位加工精度分析42.3毛坯42.3.1毛坯种类的选择42.3.2加工余量42.4基准的选择52.5夹具的选择52.6机床的选择62.7刀具材料的选择62.8工艺路线72.8.1 工序、工步的划分72.8.2 加工顺序的安排72.8.3 工艺路线72.9切削用量、刀具及切削液92.9.1粗铣基准A、上表面92.9.2粗铣凸台112.9.3钻2-12通孔132.9.4切削液的选择14第三章UG造型编程及加工163.1三维造型163.2数控加工编程193.2.1凸台的数控加工编程193.2.2钻2-12（H7）通孔的数控加工编程223.3加工24结论25参考文献26致谢27外文翻译28第一章 绪论1.1 UG介绍Unigraphics（简称UG）是西门子公司推出的集CAX（CAD/CAM/CAE的总称）于一体的三维参数化软件。UG软件从20世纪70年代开发以来，经历了基于图样（1974年）、基于特征（1988年）、基于过程（1995年）和基于知识（2000年）的发展阶段，功能不断扩展，在CAX等领域的应用不断扩大。UG软件包括CAD/CAE/CAM计算机铺助工业设计、知识驱动自动化、数据交换和其他特殊应用等功能。UG软件在CAD方面的建模和造型分为两个模块实体造型和自由曲面造型。在造型功能方面，除其他软件所具有的通用功能外，它还拥有灵活的复合建模、齐备的仿真照相、细腻的动画渲染和快速的原型工具，仅复合建模就可以让用户在实体建模、曲面建模、线框建模和基于特征的参数建模中任意选择，使设计者可根据工程设计实际情况确定最佳建模方式，从而得到最佳设计效果。在加工功能方面，UG针对计算机铺助制造的实用性，适应性和效能性，通过覆盖制造过程，实现制造的自动化、集成化和用户化，从而在产品制造周期、产品制造成本和产品制造质量等方面提供了极大的效益。1第二章 双面型腔工艺分析与设计2.1计算零件的生产纲领、确定生产类型 企业在计划期内生产的产品数量和进度计划称为生产纲领。企业（或车间、工段、班组、工作地）生产专业化程度的分类称为生产类型。生产类型一般可分为单件生产、成批生产、大量生产三种类型。一、计算生产纲领本双面型腔件是某产品，该产品年产量400台，备品率10%，机械加工废品率大约2%，则零件的生产纲领为N=Qn（1+a%+b%） =4001（1+10%+2%） =448件/年二、确定生产类型 表2-3 生产纲领与生产类型的关系生产类型零件的年生产纲领/件重型零件（100kg）中型零件(10100kg)轻型零件(10kg)单件生产5101000500050000该零件的年产量为448件，其质量为2.64kg，根据表2-3，可以确定其生产类型为小批生产。2.2零件图的工艺分析在数控铣削加上中，对零件图的工艺分析的主要包括零件结构工艺性分析、选择数控铣削的加工内容、零件毛坯的工艺性分析和加工方案分析。目的在于，一是审查零件的结构形状及尺寸精度、相互位置精度、表面粗糙度、材料及热处理等的技术要求是否合理，是否便于加工；二是通过工艺分析，对零件的工艺要求有进一步的了解，以便制订出合理的工艺规程。2.2.1读图和审图(1)该零件图表达完整、清晰，尺寸、公差、表面粗糙度及有关技术要求齐全、明确。(2)该零件2-8.5和SR20表面粗糙度为Ra6.3um，38、20、上表面和底面表面粗糙度为Ra1.6um其余为Ra3.2um。参数合理，利于加工。(3)该零件的定位基准为底面，必须先满足该面的精度。(4)该零件选用的材料为45钢，价格低廉，加工难度不大，能够保证零件件的各方面要求。 零件的技术要求有未注尺寸公差为IT13。加工要素有平面、凸台、曲线、曲面、型腔和孔类加工。主要加上内容包括上下平面、内外型腔、孔类加工。2.2.2数控加工内容的选择该零件加工内容主要是平面、凸台、曲线、曲面、型腔和孔类等的加工，如果采用普通机床，像曲面（球面）、曲线等，难加工，质量难以保证，而且效率低，工人手工操作劳动强度大，故将全部采用数控机床加工。2.2.3零件结构的工艺性该零件的加工的各工艺性能良好，耗工不大。（零件的结构工艺性是指所设计的零件在满足使用要求的前提下，制造的可行性和经济性。好的结构工艺性会使零件易于加工，节省工时、材料；差的结构工艺性会使零件加工困难、浪费工时、材料，甚至无法加工。）2.2.4重要部位加工精度分析该零件结构虽然看似复杂，但是却易于加工。根据图纸上的标注，该零件的尺寸精度（尺寸精度:限制加工表面与其基准间的尺寸误差不超过一定的范围）在IT79之间；位置精度（位置精度:限制加工表面与其基准间的相互位置误差，如平行度、垂直度、同轴度、位置度等）是要保证38、20、50与基准A的垂直度，凸台底面与基准A的平行度。2.3毛坯2.3.1毛坯种类的选择制造机械零件（或产品）所选用的毛坯有铸件、锻件、冲压件、焊接件、型材等。该材料选用的是45钢，故该零件力学性能要求较高。45钢属于中碳钢，是优质碳素结构钢中应用最广泛的一类。该零件属于小批量生产故采用自由锻件（大量生产应选精度和生产率都较高的毛坯制造方法。如铸件应采用金属模机器造型或精密铸造;锻件应采用模锻或冷轧、冷拉型材等;单件小批量生产则用木模手工造型或自由锻件）。2.3.2加工余量加工余量（加工余量是指加工过程中从加工表面切除的金属层厚度）大小，直接影响零件的加工质量和生产率。加工余量过大，不仅增加机械加工劳动量，降低生产率，而且增加材料、工具和电力的消耗，增加成本。但若加工余量过小，又不能消除前工序的各种误差和表面缺陷，甚至产生废品。该零件采用查表修正法确定加工余量，余量如下:根据机械加工工艺手册表2.3-25毛坯尺寸定为14510529(长宽高)。表2.3-25 方块类锻件的机械加工余量及偏差 （mm）锻件高度H锻件截面边长A、B100101150abab5041415551100556262注：只截取部分工序余量：面（所有）加工：根据金属机械加工工艺人员手册表13-27（第1050页），当加工面长度小于等于300mm，加工面宽度小于等于100mm时，精铣余量为0.5mm，那么粗铣余量为2mm。孔加工：2-12（H7）根据金属机械加工工艺人员手册表13-14（第1050页），当加工孔的直径为12mm时，钻（工序尺寸为11mm，余量为1mm），扩孔钻（工序尺寸为11.85mm，余量为0.15mm），铰至尺寸；2-8.5查机械加工工艺手册表2.3-48（第495页），当加工孔的直径为8.5mm时，钻（工序尺寸为8.4mm，余量为0.1mm），铰至尺寸；2-15直接加工至尺寸。2.4基准的选择所谓基准是用来确定生产对象上几何要素间的几何关系所依据的那些点、线、面。 该零件的表面全部都需要加工，加工该零件的上平面、凸台、孔、球面、内圆时以基准A为定位基准，加工底面、型腔时，以上平面为定位基准。该零件既遵循了“基准重合”原则（为了较容易地获得加工表面对其设计基准的相对位置精度要求，应选择加工表面的设计为其定位基准。这一原则称为基准重合原则），“基准统一”原则（当工件以某一组精基准定位可以比较方便地加工其他表面时，应尽可能在多数工序中采用此精基准定位，这就是“基准统一”原则），又遵循了“互为基准”原则（为了获得均匀的加工余量或较高的位置精度，可采用互为基准反复加工的原则）2.5夹具的选择本零件采用铣床用平口虎钳装夹工件，型号为QH160参数如下：名称型号钳口宽度钳口最大张开量钳口高度定位键宽度铣床用平口虎钳（mm）QH1601601255018 2.6机床的选择机床的选择：(1)机床规格应与工件的外形尺寸相适应，及大件用大机床，小件用小机床。(2)机床精度应与工件加工精度要求相适应。 本零件选择加工选用XD-40数控立铣床 ，参数如下：1、工作台工作台规格 长宽（mm） 800400T型槽尺寸 槽宽(mm)18H71303(中央T型）工作台最大载重(kg)3002、坐标范围X坐标(mm) 600Y坐标(mm) 400Z坐标(mm) 540主轴中心线距Z向导轨面距离(mm) 460主轴断面距工作台上平面距离(mm)150-6903、进给X、Y、Z向切削进给速度(mm/min) 15000X、Y、Z向快速进给速度(m/min)20（X、Y） 15（Z）主轴最高转速(r/min) 5000（8000可选）4、主轴系统主轴功率(kW)7.5主轴锥孔7：24主轴前支承直径(mm)70主轴轴承润滑方式油脂润滑5、精度定位精度(mm) （国标） X、Z：0.020 Y：0.016重复定位精度(mm) （国标） X、Z：0.008 Y：0.0062.7刀具材料的选择刀具材料选用硬质合金，钻头、键槽刀、扩孔刀和铰刀选用高速钢。硬质合金的切削速度比高速钢高410倍，切削力强，但其冲击韧性与抗拉强度远比高速钢差，成本高。2.8工艺路线2.8.1 工序、工步的划分加工该零件按加工部位划分工序（对于加工内容很多的零件，可按其结构特点将加工部位分成几个部位，如内腔、外形、曲面或平面）。加工该零件，构成工步的任一要素（加工表面、刀具及加工连续性）改变后，都将视为另一个工步。2.8.2 加工顺序的安排 总的原则是前面的工序为后续工序创造条件，作为基准的准备。具体原则如下：（1）先粗后精（2）先主后次（3）先面后孔（4）先基准后其他2.8.3 工艺路线 根据以上本零件的工艺路线如下： 工艺路线方案一： 锻热（调质处理）铣（上、下平面）铣（四周边）铣（粗精铣凸台）铣（粗精铣内圆）铣（粗精铣孔）铣（粗精铣球面）钻（钻、扩、铰）铣（粗精铣型腔）铣（粗精铣孔）钳（清洗、去毛刺）检（检验入库） 工艺路线方案二：锻热（调质处理）铣（上、下平面）铣（四周边）铣（粗精铣凸台）铣（粗精铣内圆）铣（粗精铣球面）铣（粗精铣孔）铣（粗精铣型腔）铣（粗精铣孔）钳（清洗、去毛刺）检（检验入库）上述两个工艺方案特点在于：方案一的孔是采用钻、扩、铰加工，方案二所有的孔采用铣加工。如果采用方案二，孔小选择的刀具直径也小，很容易断刀，切削效率也不高，所以方案一比较合理。工艺过程方案：010锻1锻造成形020热1去应力退火030铣1粗铣底面，留余量0.5mm2精铣底面至尺寸3调面，粗铣上平面，留余量0.5mm040铣1粗铣10024两端面，留余量0.5mm2精铣10024两端面至尺寸3粗铣14024两端面，留余量0.5mm4精铣14024两端面至尺寸050铣1粗铣凸台，单边留余量0.5mm2精铣上平面至尺寸3精铣凸台至尺寸060铣1粗铣50内圆，留余量0.5mm2粗铣20mm、深度为10mm的内圆，留余量0.5mm3精铣50内圆至尺寸4精铣20mm、深度为10mm的内圆至尺寸070铣1粗铣26通孔，留余量0.5mm2精铣 26孔至尺寸080铣1粗铣球面，留余量0.5mm2精铣球面、R3圆弧至尺寸090钻1钻2-12（H7）通孔，留余量1mm2钻2-8.5通孔，留余量0.1mm3扩2-12（H7）通孔，留余量0.15mm4铰2-12（H7）通孔至尺寸5铰2-8.5通孔至尺寸6加工2-15mm、深度为8.5mm的沉孔至尺寸100铣1粗铣型腔，留余量0.5mm2精铣型腔至尺寸110铣1粗铣38mm、深度为15mm的孔，留余量0.5mm2精铣38mm、深度为15mm的孔至尺寸120钳1去除毛刺，锐边2清洗130检1检验入库2.9切削用量、刀具及切削液2.9.1粗铣基准A、上表面 1. 选择刀具（1） 根据表1.2（在切削用量简明手册第56页），选择YT15硬质合金刀片。根据表3.1（在切削用量简明手册第84页），铣削深度p4mm时，端铣刀直径d0为80mm，e为60mm。但已知铣削宽度100mm，故应根据铣削宽度e120mm，选择d0=200mm。由于选择标准硬质合金端铣刀，故齿数z=8（表3.15，在切削用量简明手册第9596页）。（2） 铣刀几何形状（表3.2，在切削用量简明手册第8486页）：由于b 650MPa，故选择kr=20,kr=5,a0=8，a0=9，s=-10，0=5。2.选择切削用量（1） 决定铣削深度p 由于加工余量不大，故可在一次走刀内完成，则 p =h=2mm （2） 决定每齿进给量fz 采用不对称端铣以提高进给量。根据表3.5（在切削用量简明手册第88页），当使用YT15,铣床功率为7.5KW（XD-40立式铣床）时，fz=0.090.18mm/z 但因采用不对称端铣，故取fz=0.18mm/z（3） 选择铣刀磨钝标准及刀具寿命 根据表3.7（在切削用量简明手册第8889页），铣刀刀齿后刀面最大磨损量为1.2mm，由于铣刀直经d0=200mm，故刀具寿命T=240min（表3.8，在切削用量简明手册第89页）（4） 决定切削速度vc和每分钟进给量vf 切削速度vc可根据公式计算，也可以直接由表中查出。根据表3.15（在切削用量简明手册第9596页），当d0=200mm，z=8，p 5mm，fz0.18mm/z时，vt=129m/min，nt=206r/min，vft=263mm/min。各修正系数为：kmv=kmn=kmvf=1.13 ksv=ksn=ksvf=0.8故 vc=vtkv=1291.130.8=116.616m/min117m/min n=ntkn=2061.130.8=186.224r/min187r/min vf=vftkvf=2631.130.8=237.752mm/min238mm/min（5）校检机床功率 根据表3.23（在切削用量简明手册第104页） ，当b 5601000MPa，e100mm，p 2mm，d0=200mm，z=8， vf=238mm/min，近似为Pcc=3.2kw XD-40立式数控铣床，机床主轴允许的功率为 Pcm=7.5kw 故PccPcm，因此所选的切削用量可以采用。（6）计算基本工时 tm=L/vf 式中，L=l+y+，l=140mm，根据表3.26（在切削用量简明手册第106页），不对称安装铣刀，入切量及超切量y+=60mm，则L=l+y+=140+60=200mm，故tm=200/238min0.84min精铣基准A、精铣上表面、粗精四周边与上相似得到的切削用量如下：粗铣上表面：p=2mm，n=187r/min，f=1.27mm/r，vc=117m/min，tm0.84min精铣基准A、上表面：p=0.5mm，n=275r/min，f=0.5mm/r，vc=173m/min，tm1.5min粗铣10024端面：用80硬质合金面铣刀加工，p=2mm， n=393r/minf=0.8mm/r，vc=123m/min，tm0.3min精铣10024端面：用80硬质合金面铣刀加工，p=0.5mm，n=498r/min，f=0.45mm/r，vc=157m/min，tm0.47min粗铣14024端面：用80硬质合金面铣刀加工，p=2mm，n=393r/min，f=0.8mm/r，vc=123m/min，tm0.46min精铣14024端面：用80硬质合金面铣刀加工，p=0.5mm，n=498r/min，f=0.45mm/r，vc=157m/min，tm0.65min刀具归结如下：刀具名称刀具号200硬质合金面铣刀TO180硬质合金面铣刀TO22.9.2粗铣凸台1选择刀具(1) 根据表10.102（在金属机械加工工艺人员手册第835页），选择YT15硬质合金刀。根据图选择d0=16mm的立铣刀，齿数z=6（表10-130，在金属机械加工工艺人员手册第864页）。(2)铣刀几何形状（表10-104，在金属机械加工工艺人员手册第837838页）：由于采用套齿圈的铣刀，故选择a0=20，a01=6，a00=30，0=-5，01=-30=25。2选择切削用量(1)决定铣削深度p 侧吃刀量e p =h=2mm ，e=5mm (2)决定每齿进给量fz 根据表10-131（在金属机械加工工艺人员手册第865页），当采用套齿圈的铣刀，d0=16mm，z=6，p 5mmfz=0.040.06mm/z但因粗铣，故取fz=0.06mm/z(3)选择铣刀磨钝标准及刀具寿命 根据表10-107（在金属机械加工工艺人员手册第843页），铣刀刀齿后刀面最大磨损量为0.3mm，由于铣刀直经d0=16mm，故刀具寿命T=120min（表10-130，在金属机械加工工艺人员手册第864页）(4)决定切削速度vc和每分钟进给量vf 切削速度vc可根据公式计算，也可以直接由表中查出。根据表10-130（在金属机械加工工艺人员手册第864页），当d0=16mm，z=6，p 5mm，e10mm，fz0.075mm/z时，vt=78m/min，Pcc=1.8kw各修正系数（表10-152，在金属机械加工工艺人员手册第885页）为：kcv=0.87， kcp=1.04故 vc=vtkv=780.87=67.86m/min68m/min Pc=Pcckcp=1.81.04=1.872kw（5）校检机床功率 XD-40立式数控铣床，机床主轴允许的功率为 Pcm=7.5kw故Pcc1013mm，b 570680MPa，d0=11mm时f=0.650.78mm/r从以上进给量比较可以看出，受限制的进给量是工艺要求，其值为f=0.1250.155mm/r，取f=0.155mm/r。（二）决定钻头磨钝标准及寿命 由表2.12（在切削用量简明手册第54页），当d0=11mm时，钻头后刀面最大磨损量取为0.5mm，寿命T=45min。（三）决定切削速度 由表2.14（在切削用量简明手册第5556页），b =600MPa的45钢加工性属5类。由表2.13（在切削用量简明手册第55页），当加工性为第5类，切削速度近似为vt=19m/min。切削速度的修正系数为（见表2.31）：ktv=1.0，kcv=1.0，kiv=1.0，kxv=0.87因此vc=vtkv=191.01.01.00.87=16.53m/min17m/min n=470.8r/min471r/min（四）校检机床功率 根据表2.22（在切削用量简明手册第63页），机床功率近似为Pcc=1.1kwXD-40立式数控铣床，机床主轴允许的功率为 Pcm=7.5kw故PccPcm，因此所选的切削用量可以采用。 （五）计算基本工时 tm=L/nf 式中，L=l+y+，l=19mm，根据表2.29（在切削用量简明手册第68页），入切量及超切量y+=5mm，则L=l+y+=19+5=24mm，故tm=24/（4710.155）min0.3min其他孔的加工与上相似切削用量如下：铰2-12通孔：用12H7铰刀， n=213r/min，f=0.7mm/r，vc=8m/min，tm0.2min钻2-8.5通孔：8.4高速钢麻花钻头，n=836r/min，f=0.11mm/r，vc=21m/min，tm0.3min扩2-12通孔：用11.85扩孔刀，a0=8，=20，2=118，T=30min，n=524r/min，f=0.7mm/r，vc=19.5m/min，tm0.2min铰2-8.5通孔：用8.5铰刀，n=375r/min，f=0.6mm/r，vc=10m/min，tm0.1min加工2-15mm、深度为8.5mm的沉孔：用15高速钢键槽铣刀，n=800r/min，f=0.013mm/r，vc=36m/min，tm1.2min刀具归结如下：刀具名称刀具号11.5高速钢麻花钻头T078.4高速钢麻花钻头T0812H7铰刀T098.5铰刀T1015高速钢键槽铣刀T1111.85扩孔刀T122.9.4切削液的选择切削液有水溶液、切削油和乳化液三种。其起到冷却、润滑、清洗、防锈等作用。切削该工件时使用的硬质合金刀具，由于它的耐热性好，所以一般不使用切削液。若要使用，则必须大量注射，以免硬质合金刀具因冷热不均产生裂纹；使用的高速钢刀具选用水溶液作为切削液。15第三章UG造型编程及加工3.1三维造型先建立新文件，文件名只能是英文和数字组成。在主菜单中依次单击“起始”“建模”命令，进入实体建模环境。单击工具栏中的“长方体”按钮，弹出“长方体”对话框，按照默认的构建模式，在“长度”内输入“140”、在“宽度”内输入“100”、“高度”内输入“19”，如图3-1所示，单击“确定”按钮，构建了一个长方体实体建模。图3-1以长方体上平面为绘制平面，进入草图绘制图3-2，完成草图后，向上拉伸5mm，并求和。图3-2以图3-2绘制好的实体的上表面为绘制平面，进入草图分别绘制图3-3、图3-4，完成草图后，分别向下拉伸求差6mm、10mm。图3-3图3-4以XZ为绘制平面，进入草图绘制图3-5，完成草图后，回转360并求差。图3-5以长方体上表面为绘制平面，进入草图绘制图3-6，完成草图后，向下拉伸4mm，并求差。图3-6以长方体上表面为绘制平面，单击工具栏中的“孔”按钮，分别完成两个通孔和两个沉头孔的绘制，对话框如图3-7、3-8 。图3-7图3-8以长方体的底面为绘制平面，绘制双面型腔件的底面，与上相似，具体步骤省略。完成所有造型后，所生成的模型如图3-9 。 图3-93.2数控加工编程铣六面一次走刀完成，可以直接手动编程，这里不做详诉。3.2.1凸台的数控加工编程在标准工具条中选择“开始”“加工”，系统将弹出“加工环境”对话框，在CAM设置选择栏中选择“mill-contour”模板，单击“初始化”按钮，系统将进入型腔铣加工环境。（一）创建几何体 在操作导航器的几何视图中，设置加工坐标系、零件和毛坯，为创建操作做准备。（1）设置加工坐标系。 先将操作导航器转换到几何体视图。 在“操作导航器-几何体”中选择“MCS-MILL”，单击右键，在其快捷菜单中选择“编辑”命令。 在弹出对话框中的“机床坐标系”中的“指定MCS”栏中，单击“自动判断”图标，然后在图形区域选择毛坯的顶面，之后单击“确定”，系统将自动在毛坯的顶面中心位置创建加工坐标系，如图3-10所示。图3-10（2）设置几何体 在“操作导航器-几何体”中，双击“WORKPIECE”图标，将弹出“几何体”对话框。 指定部件几何体。在“几何体”对话框中，单击“指定部件”按钮，将弹出“部件几何体”对话框，在图形区域选择零件， 点击“确认”返回“几何体”对话框，如图3-11所示。图3-11 指定毛坯几何体，在“几何体”对话框中，单击“指定毛坯”图标按钮，将弹出“毛坯几何体”对话框，选择“自动块”，单击“确定”后，返回“几何体”对话框，如图3-12所示。图3-12 在“几何体”对话框中单击“确认”，结束几何体的设置操作。（二）创建刀具（1）在“创建操作”工具条中选择“创建刀具”命令，进入“创建刀具”对话框。（2）先在“创建刀具”对话框中的类型选择项内选择“mill-contour（铣型腔）”，然后在“刀具子类型”选项栏中选择“立铣刀（MILL）”图标，并输入刀具名称LIXIDAO16，然后单击“应用”，进入“刀具参数”对话框，设置参数后单击“确定”，完成刀具的创建。（三）创建操作（1） 在加工创建工具条中，单击“创建操作”命令，系统将弹出“创建操作”对话框。（2） 在“创建操作”对话框中，选择“类型”中选择“mill-contour（铣型腔）”，然后在“操作子类型”中，选择型腔铣模板图标CAVITY-MILL铣型腔。（3） 在“创建操作”对话框中设置其他参数：程序、刀具、几何体、方法、名称。（4） 在“创建操作”对话框中单击“确定”，选择切削区域、设置切削层、进给率。（5） 生成操作，如图3-13所示。图3-13（6） 加工仿真。例如，图3-14。图3-14（四）后处理先在操作导航器中选中各铣削图标，然后在“加工操作”工具条中单击“后处理”按钮，在“后处理”对话框中，后处理选择“MILL-3-AXIS”，单位选择“公制/部件” ，单击“确定”后，系统就会生成型腔铣操作的NC加工代码。例如，图3-15 。 图3-153.2.2钻2-12（H7）通孔的数控加工编程（一）创建刀具（1）在“创建操作”工具条中选择“创建刀具”命令，进入“创建刀具”对话框。（2）先在“创建刀具”对话框中的类型选择项内选择“drill”，然后在“刀具子类型”选项栏中选择“麻花钻头（DRILLING-TOOL）”图标，并输入刀具名称DRILLING-TOOLD11，然后单击“应用”，进入“刀具参数”对话框，设置参数后单击“确定”，完成刀具的创建。（二）创建操作（1）在加工创建工具条中，单击“创建操作”命令，系统将弹出“创建操作”对话框。（2）在“创建操作”对话框中，选择“类型”中选择“drill”，然后在“操作子类型”中，选择型腔铣模板图标PECK-DRILLING啄钻。在“创建操作”对话框中设置其他参数：程序、刀具、几何体、方法、名称。在“创建操作”对话框中单击“确定”，指定孔、指定部件表面、指定底面、指定循环方式、进给和速度，如图3-16所示。图3-16（3）生成操作，如图3-17所示。图3-17 （4）加工仿真，如图3-18所示。图3-18（三）后处理先在操作导航器中选中各铣削图标，然后在“加工操作”工具条中单击“后处理”按钮，在“后处理”对话框中，后处理选择“MILL-3-AXIS”，单位选择“公制/部件” ，单击“确定”后，系统就会生成型腔铣操作的NC加工代码，如图3-19所示 。图3-19该零件其他的数控加工编程与上相似，这里不作详述。3.3加工（1）开机检查主轴运转、各功能是否正常，然后将各坐标轴回到机床零点。（2）装工件、对刀建立坐标系。（3）将程序输入机床后进行相应修改，再将机床处于单段运行状态，检验刀具在机床中运行的位置是否正确，主要是Z轴，当位置确定后释放单段运行状态，自动运行。43结论本论文通过对零件图形的结构分析，拟定出工艺方案。在加工时要特别注意位置精度。刀具直径的选择要注意根据零件图选择，特别是立铣刀不要选择够大，否则会过切，影响加工精度。利用UG软件对零件进行三维造型及数控加工编程，减少了烦琐的计算过程，大大缩短了编程的时间。参考文献1 李洪主编 机械加工工艺手册 北京出版社 2 赵如福主编 金属机械加工工艺人员手册 上海科学技术出版社 3 焦建民主编 切削用量 电子工业出版社 4 吴国梁主编 铣工 江苏科学技术出版社5 过小容 李坤 编著 辽宁科学技术出版社 UG三维造型与数控加工编程 6 倪森寿主编 无锡职业技术学院 机械技术基础7 倪森寿主编 化学工业出版社 机械制造工艺与装配8 李锦标 钟平福 等编著 机械工业出版社 UG NX 从数控加工编程到CNC加工实战致谢通过这次毕业设计让我学到了很多知识、所学的知识都得到了应用，提高了综合应用能力。王自建老师，给予了精心的指导，提出了宝贵的经验。感谢王自建老师给予的支持和帮助。同时要感谢在百忙之中来参加我毕业答辩的评审老师。外文翻译（一）Production and meaning of CNC machine toolsTraditional mechanical manufacturing industry, manufacturers of what kind of machine tool equipment, depending on its type of production. For mass production, the use of special machine tools, machine tool, production line and the corresponding tooling. This mode of production, investment, and product is not easy replacement cycle is long. For single and in small batch production type, using a common universal machine and copying machine, and this mode of production need to make adjustments by mold and machine tools, spend a lot of manual labor hours, and require workers with high technical level, Also need a longer preparation period of production, processing, accuracy is also difficult to meet higher demand.The current world has entered the information age, technological advances. Production areas and high-tech field of increased competition, product and technological progress, accelerating the pace of upgrading. Now single and small batch production machining of parts have been accounted for more than 80% of the total, and with the requirements of parts of higher quality, higher accuracy, the shape are becoming increasingly complex, which is placed in front of the machine tool industry, a problem. In order to solve complex, sophisticated, single and small batch and the changing shape of the parts processing problems, a new type of machine - digital control machine tool production is inevitable. In 1952, the United States and the Massachusetts Institute of Technology Parsons the first company successfully developed the worlds first CNC machine tools.Numerical control of machines referred to as CNC machine tools, is a kind of digital information as a form of instruction, through a dedicated or general-purpose electronic computer-controlled machine tools. It can be said, CNC machine tools is under the control of the CNC system, accurate process by pre-arranged, and automate the processing requirements of machine tool movements.（二）The choice of locating datumPositioning reference base with coarse and fine of reference points. Starting in the processing processes, can only be used on rough surfaces not processed as a positioning reference, the surface is called rough benchmark. The surface has been processed using a locating datum, is called precision benchmark.Select benchmark crude, the main consider two questions: First, do not guarantee processing surface and machined surface accuracy of mutual location: the second is a reasonable allocation of the allowance of the machined surface. Reference to the following principles when specific choices.1.For both the surface of the machined surface and non-processing parts, in order to ensure processing between the surface and not the location of the machined surface accuracy, surface finish should be chosen not as a rough benchmark. If there are multiple parts are not machined surface, places where the surface of each location and processing high precision surface as a rough benchmark.2.For a more finished surface of the workpiece .select the coarse reference should be considered a reasonable allocation of the allowance of the machined surface. Rational allocation of allowances refer to the following two points.a. should ensure that all of the major surface has a sufficient allowance. To meet this requirement, should choose the smallest margin rough surface as a rough benchmark.b. For certain important on the surface of the workpiece (such as rail and important holes, etc.), uniform allowance to as much as possible to the surface, the surface should be chosen as an important benchmark crude.3.Rough benchmarks should avoid repeated use. Direction in the same size, the crude base is usually used only once to avoid large position error.4.Chosen as the benchmark crude should be flat plane, or the flash is not casting defects such as riser for positioning and reliable.Reference should be fine selection of departure to ensure precision parts, taking into account the clamping convenient, simple fixture. Precision reference select the following principles should be considered normal.a.coincidence basis principleIn order to more easily access the machined surface the relative position of the design basis of their accuracy, the design should be selected for processing positioning reference surface. This principle is called the principle of reference coincide.b.unified basis principleWhen the workpiece to a group of fine benchmarking process can be more convenient to the other surface, as far as possible the use of this procedure in most intensive benchmarking, this is the benchmark unity principle.c. as the base from the principleWhen the workpiece finishing or finishing process requirements and uniform margin as small as possible should be selected when processing the surface of positioning itself as the benchmark, this is the self as a benchmark principle.d. mutual basis principleIn order to obtain a uniform allowance or a higher position accuracy, can be processed again the principle of mutual reference.e. Fine reference selection should ensure that accurate workpiece positioning, clamping, reliable, easy to operate.The coarse and fine reference selection principle, and often can not be fully met, the actual application will always be a conflicting situation, which requires comprehensive consideration, prioritize, focus on solving the principal contradiction.（三） Positioning method(1)Directly to locate lawDirectly to the Law-rectification is the use of dial indicator positioning, visual planning methods such as needle or on the machine directly to the workpiece surface is the design basis to obtain the correct position to the positioning method.This method of positioning accuracy and speed of alignment depends on the level of the workers to find are, in general, this method is time-consuming, and more for single and small batch production or require particularly high positional accuracy of the workpiece.(2)Crossed to find law positioningLaw position is crossed to find on the machine by using the program needle or semi-finished blanks to be processed on the pre-draw the line at the workpiece alignment, the location to obtain the correct positioning method. This method is crossed by the alignment accuracy and precision limitations, the positioning accuracy is not high. Mainly for low-volume precision embryos hairs and large parts, which are not easy to use rough fixture for processing.(3)The use of fixtureFixture that is the direct use of the fixture positioning device to obtain the correct position of the workpiece positioning method. The positioning of the fixture components and the relative position of machine tools and cutting tools are pre-adjusted, so the workpiece positioning no longer individually adjusted. This method is targeting rapid, reliable, high accuracy, widely used in the production of finished products and a large number.（四）Workpiece clampingThe purpose is to prevent the workpiece clamped in the cutting force, gravity, inertia under the action of such displacement or vibration, so that the positioning of the workpiece. Basic requirements:1.Clamping force does not destroy the correct positioning of the workpiece;2.Clamping device should have sufficient rigidity;3.Clamping should not damage the surface, should not exceed the allowable range workpiece deformation;4.Less clamping force can be used to obtain the necessary clamping effect;5.Technology is good, the premise of ensuring the survival of the structure should be simple, easy to manufacture, maintenance and operation. Manual clamping structure should be self-locking performance.According to the above basic requirements, the correct clamping force to determine the three elements (direction, the role of point size) is very important.1.To determine the direction of clamping forcea.The direction of the clamping force should not undermine the work piece positioning.b.Clamping force should point to the main orientation direction of the surface.2.To determine the point of clamping forcea.Clamping force acting point should fall within the scope of support.b.Clamping force should fall on the workpiece rigid point of a good site.c.Point of clamping force should be close to the workpiece processing site.Estimate the size of the clamping force approach:a.To identify the worst of the transient clamp to estimate the state of clamping force required.b. For convenience, only the main factors considered in the force system in the effects of factors omitted in the system of forces in the secondary impact.c. According to the work of the state, listing force (moment) of the equilibrium equations to solve the size of the clamping force should also give due consideration to safety factors.（5） Select type of rough（1）According to the drawings and mechanical properties of the material provisions of selected rough. Drawing on the basic material required to determine the type of blank. For example: material is cast iron, is necessary to use casting blank; materials for the steel, if the mechanical performance requirements of high-forging is optional, if the mechanical performance requirements of the optional low-profile or cast steel.（2）According to the rough part of the function selection. According to the working conditions of parts, materials, structural features of all three into account, such as materials for the 45 steel, the main axis of the forging; medium and small gear and more to do with the rough forging, steel casting gear used to do rough.（3）According to the production of type selection blank. Mass production should be selected with higher precision and productivity are blank manufacturing methods. Should be used, such as casting or molding metal mold casting machine; should be forging or cold forging, cold-drawn profiles, etc.; single and small batch is handmade with a wooden mold or shape forgings.（4）According to the specific choice of rough production conditions. Blank must be combined to determine the specific production conditions, such as the actual field blank manufacturing level and ability, the possibility of outsourcing. Conditions, should actively organize specialized production areas, unified supply of rough.（六）The choice of blank shape and sizeRough shape and size composition of the surface mainly by the shape of parts, structure, size and other factors to determine allowance, and close to as much as possible with the parts in order to reduce the amount of machining work, and strive to achieve little or no cutting. But there are the following four cases.（1）By forging, casting blank, because of the amount of forging die voltage when the fault with the allowed range modulus, also due to sand casting error, shrinkage, and poor flow of liquid metal filled the cavity and so can not cause more thanranging from the amount, in addition, forging, casting, the rough amount of deflection and distortion can also cause the different allowances are not sufficient, unstable, so, in addition to sheet metal, but whether it is forging, casting or molding, as long asready to use CNC machining, the processing tables should have a more full margin.For hot-rolled, the thick aluminum plate, after quenching and aging and easily processed in the processing of the deformation and, therefore, need to consider whether the added layer cutting, sub-layers of cutting, generally try to do all the processing tablesmargin uniform cutting to reduce the internal stress caused by deformation.（2）Small or thin parts, for ease of clamping and to reduce the chuck, the workpiece can be more connected together by a system out of the rough.（3）Formed the same work surface assembly of two related parts, in order to ensure processing quality and to processing convenience, often the two together as a whole blank, processing, and then cut to a certain stage.（4）Clamping of the blank for the inconvenience, consider an additional fixture in the rough on the margin or process bosses, lugs and other auxiliary craft basis.（七）AllowanceAllowance size, a direct impact on the machining quality and productivity. Allowance is too large, not only increase the amount of machining work, reduced productivity, and increase the materials, tools, and power consumption, increase costs. However, if the allowance is too small, before the process can not eliminate all errors and surface defects, and even waste. Therefore, we must determine with a reasonable margin. The established method is as follows. 1. Experience estimation method Estimation method is based on the experience the experience of technology to determine the allowance. For the avoidance of waste, as determined by combined general larger margin. Suitable for single and small batch production. 2.Look-up table correction methods The method according to the manual, look up the value allowance, and then make the appropriate amendments to the actual situation. This is a widely used method.3.Analysis and Calculation Method This is the allowance of the various factors affecting the analysis, then some formula to calculate the allowance method. Allowance for this method to determine a more reasonable, but requires a comprehensive test data, calculations are more complex, it is rarely used.（八）The division processNC divided according to characteristics:(1)To an installation process as a process. This method is suitable for processing the contents of small parts.(2)The contents of the same division of the tooling process. Although some parts installation process a lot of time to be processed surface, but considering the program is too long, such as memory capacity and other constraints, in addition, will also increase the error and retrieval difficulties. Therefore, programs can not be too long, the contents of a process can not be too much.(3)Procedures by processing parts. For processing the contents of many of the parts, can be part of its structural features will be processed into several parts, such as bore, shape, surface or plane.(4)Rough, finishing division process. For the processing of parts prone to distortion, due to the deformation that may occur after roughing the need for sizing, so generally speaking, anyone who will be rough, finishing the process should be separated.（九）The division of work stepsGenerally speaking, constitute a step in any work elements (machined surface, tool and process continuity) to change, it becomes another process step. However, that situation should be considered following a process step.(1)A fixture for those in the same continuous work of a number of steps should be considered a process step.(2)In order to increase productivity, and sometimes a few to several surface processing tool at the same time, this time should also be considered as a process step, called the complex working steps.（十）The choice of the content of CNC machiningWhen you select and decide on a CNC machining parts, after processing all of its contents are not using CNC machining, CNC machining parts machining processes may be just a part of. Therefore, it is necessary to carefully analyze the part design, based on solving problems, improving productivity, attention to give full play to the advantages of CNC, to select those most appropriate content and processes needed for NC machining. The following general principles can be selected NC content:（1）General machine tools can not process the contents of the selection should be the focus.（2）General machine tools difficult to machine, difficult to guarantee the quality of the contents of the selected content should be the focus.（3）General machine tools, low efficiency, labor-intensive manual workers in the content, you can still processing capacity of CNC machine tools on the basis of selection.In contrast, a number of processing the contents of the following should not choose NC.（1）The need to account for machine use more time to adjust the processing content.（2）Allowance unstable, and the CNC machine tool parts and can not automatically adjust the coordinates of the location of the processing of content.（3）Can not be completed in the first installation in the processing of parts scattered sites, the use of CNC machining is very convenient, the effect is not obvious, can arrange for additional processing of general machine tools.In addition, the choice of NC content, but also to consider the production volume, production cycle, process between the working conditions and other factors, make rational use of CNC machine tools to achieve product quality, productivity and overall economic efficiency indicators have significantly improved the purpose of preventing CNC machine tools will be reduced to ordinary use.(十一)Moving PathMoving Path is the tool in the whole trajectory in machining operations, which includes not only the content of the process step should also be reflected on the order of working steps.Moving Path to note the following:(1)For the shortest processing line, to reduce air knife time to increase processing efficiency.(2)To ensure that the surface of workpiece surface roughness after processing, the final outline should be arranged at the last walk the knife out of the continuous process.(3)To consider the progress of the tool, back knife (cut, cut out) line, the tool should be cut out or entry points along the extension of the surrounding parts to ensure the smooth contours of the workpiece; the surface of the workpiece contour to avoid the vertical upper and lower knife to scratch the surface; minimizing the suspension of the contour machining (cutting force caused by a sudden change in elastic deformation), to avoid leaving marks.（一）数控机床的产生及含义传统机械制造业中，生产企业采用什么样的机床设备，主要取决于它的生产类型。对于大批量生产，采用专用机床、组合机床、生产线及其相应的工装。这种生产方式的投资大、周期长及产品不易更新换代。对于单件和中、小批量的生产类型，则采用通用万能机床和仿形机床，而这种生产方式需要制造靠模和调整机床，耗费大量的手工劳动工时，并要求工人技术等级高，同样需要较长的生产准备周期，加工精度也很难达到更高的要求。当前的世界已进入信息时代，科技进步日新月异。生产领域和高科技领域中的竞争日益加剧，产品技术进步、更新换代的步伐不断加快。现在单件小批生产的零件已占到机械加工总量的80%以上，而且与要求零件的质量更高、精度更高，形状也日趋复杂化，这是摆在机床工业面前的一个出问题。为了解决复杂、精密、单件小批量以及形状多变的零件加工问题，一种新型的机床数字控制机床的产生也就是必然的了。1952年，美国帕森公司和麻省理工学院率先研制成功世界第一台数控机床。数字控制机床简称数控机床，是一种以数字量作为指令信息形式，通过专用或通用的电子计算机控制的机床。也可以说，数控机床是在数控系统的控制下，准确按事先安排的工艺流程，而自动地实现规定加工动作的金属切削机床。（二）定位基准的选择定位基准有粗基准和精基准之分。在加工起始工序中，只能用毛柸上未曾加工过的表面作为定位基准，则该表面称为粗基准。利用已加工过的表面作为定位基准，则称为精基准。选择粗基准时，主要考虑两个问题：一是保证加工面与不加工面的相互位置精度要求：二是合理分配各加工面的加工余量。具体选择时参考下列原则。1对于同时具有加工表面和不加工表面的零件，为了保证加工表面与不加工表面之间的位置精度，应选择不加工表面作为粗基准。如果零件上有多个不加工表面，则以其中与加工表面相互位置精度要求较高的表面作为粗基准。2对于具有较多加工表面的工件，选择粗基准时，应考虑合理分配各加工表面的加工余量。合理分配加工余量是指以下两点。a.应保证各主要表面都有足够的加工余量。为满足这个要求，应选择毛柸余量最小的表面作为粗基准。b.对于工件上的某些重要表面（如导轨和重要孔等），为了尽可能使其表面加工余量均匀，则应选择重要表面作为粗基准。3粗基准应避免重复使用。在同一尺寸方向上，粗基准通常只能使用一次，以免产生较大的定位误差。4选作粗基准的平面应平整，没有浇冒口或飞边等缺陷，以便定位可靠。精基准的选择应从保证零件加工精度出发，同时考虑装夹方便、夹具结构简单。选择精基准一般应考虑如下原则。a“基准重合”原则为了较容易地获得加工表面对其设计基准的相对位置精度要求，应选择加工表面的设计为其定位基准。这一原则称为基准重合原则。b“基准统一”原则当工