练习I-02A(应力分析-车床刀具).ppt
车床刀具,练习 2A应力分析,January 20,2001Inventory#001442W2-2,2A.应力分析 车床刀具,说明下面求解一个车床刀具模型的 3-D应力分析。通过下列步骤在通用后处理器中查看结果：1)绘位侈2)列反力3)绘 von Mises 应力4)动态显示von Mises应力施加不同的约束重新求解，并与第一次的结果进行比较。,January 20,2001Inventory#001442W2-3,2A.应力分析 车床刀具,第一次求解荷载及材料特性:,January 20,2001Inventory#001442W2-4,2A.应力分析 车床刀具,第二次求解时的荷载及材料特性：,January 20,2001Inventory#001442W2-5,2A.应力分析 车床刀具,1.按教师指定的工作目录，用“cutter”作为作业名，进入ANSYS。2.设置 GUI 优先选择 为“结构”:Main Menu Preferences 选择“Structural”,然后按OK,January 20,2001Inventory#001442W2-6,2A.应力分析 车床刀具,3.选择“No defeaturing”，输入“cutter.igs”IGES 文件:Utility Menu File Import IGES 选择“No defeaturing”,然后按 OK选择“cutter.igs,然后按OK或用命令:/AUX15 IOPTN,IGES,NODEFEAT IGESIN,cutter,igs,January 20,2001Inventory#001442W2-7,2A.应力分析 车床刀具,4.按一定比例转换模型，把厘米单位转换英寸：Main Menu Preprocessor Operate Scale Volumes+按Pick All对RX,RY,和 RZ输入 1/2.54 设置 IMOVE为“Moved”,然后按 OK或用命令:VLSCAL,ALL,1/2.54,1/2.54,1/2.54,0,1Utility Menu Plot Volumes或用命令:VPLOT,January 20,2001Inventory#001442W2-8,2A.应力分析 车床刀具,5.读入文件“cutter-area.inp”，建立一个小的面，在面上施加荷载:Utility Menu File Read Input from 选择“cutter-area.inp”,然后按 OK或用命令:/INPUT,cutter-area,inp,January 20,2001Inventory#001442W2-9,2A.应力分析 车床刀具,6.确定单元类型：Main Menu Preprocessor Element Type Add/Edit/Delete 按Add.选择“Structural Solid”和“Tet 10node 92”,然后按 OK按Close或用命令:ET,1,SOLID92,January 20,2001Inventory#001442W2-10,2A.应力分析 车床刀具,7.定义第一组材料的弹性模量为 10e6(铝):Main Menu Preprocessor Material Props Material Models Structural-Linear-Elastic-Isotropic输入 EX=10e6(铝的杨氏模量，以psi为单位)输入PRXY=.32按OKSelect Material Exit或用命令:MP,EX,1,10e6MP,PRXY,1,.32,January 20,2001Inventory#001442W2-11,2A.应力分析 车床刀具,8.激活灵活网格，用四面体单元划分实体：Main Menu Preprocessor MeshTool 激活“Smart Size”设置 Smart Size为4按Mesh拾取Pick All按Close或用命令:SMRT,4MSHAPE,1,3DMSHKEY,0VMESH,January 20,2001Inventory#001442W2-12,2A.应力分析 车床刀具,9.在面上施加对称约束，约束附加区域：Utility Menu Plot AreasMain Menu Solution-Loads-Apply-Structural-Displacement-Symmetry B.C.-On Areas+拾取面 18,19,25,和 26,然后按 OK或用命令:DA,18,SYMMDA,19,SYMMDA,25,SYMMDA,26,SYMM,January 20,2001Inventory#001442W2-13,2A.应力分析 车床刀具,10.在顶端施加压力:Main Menu Solution-Loads-Apply-Structural-Pressure On Areas+拾取面 1,然后按OKVALUE=10000按OK或用命令:SFA,1,1,PRES,10000,January 20,2001Inventory#001442W2-14,2A.应力分析 车床刀具,11.保存数据库并求解:Click the“SAVE_DB”button in the Toolbar(or select:Utility Menu File Save as Jobname.db)Main Menu Solution-Solve-Current LS观察“/STATUS Command”窗口，然后关闭它按OK按Close-求解完成后关闭黄色信息窗口或用命令:/SOLUSOLVE,January 20,2001Inventory#001442W2-15,2A.应力分析 车床刀具,12.观察结果：12a.画出位侈：Main Menu General Postproc Plot Results-Contour Plot-Nodal Solu.选择“DOF solution”和“Translation USUM”,选择“Def+undef edge”,然后按 OK或用命令:/POST1PLNSOL,U,SUM,2,1,January 20,2001Inventory#001442W2-16,2A.应力分析 车床刀具,January 20,2001Inventory#001442W2-17,2A.应力分析 车床刀具,12b.列出反力:Main Menu General Postproc List Results Reaction Solu.选择“All items”,然后按 OK或用命令:PRRSOL,January 20,2001Inventory#001442W2-18,2A.应力分析 车床刀具,January 20,2001Inventory#001442W2-19,2A.应力分析 车床刀具,12c.画出von Mises 应力:Main Menu General Postproc Plot Results-Contour Plot-Nodal Solu.选择“Stress”和“von Mises SEQV”,然后按 OK或用命令:PLNSOL,S,EQV,January 20,2001Inventory#001442W2-20,2A.应力分析 车床刀具,12d.对模型进行“拍照”并将其最小化：Utility Menu Plot Cntrls Capture Image在以后的比较中把窗口最小化,January 20,2001Inventory#001442W2-21,2A.应力分析 车床刀具,12e.动画显示 von Mises 应力：Utility Menu PlotCtrls Animate Deformed Results.选择“Stress”和“von Mises SEQV”,然后按 OK或用命令:PLNSOL,S,EQVANCNTR,10,0.5,January 20,2001Inventory#001442W2-22,2A.应力分析 车床刀具,January 20,2001Inventory#001442W2-23,2A.应力分析 车床刀具,13.关闭动画显示，删除面对称约束：按CloseUtility Menu Plot AreasMain Menu Solution-Loads-Delete-Structural-Displacement On Areas+拾取面 18,19,25,和26,然后按 OK按OK或用命令:DADELE,18,ALLDADELE,19,ALLDADELE,25,ALLDADELE,26,ALL14.对面18,19,和26施加 全部自由度 约束:Main Menu Solution-Loads-Apply-Structural-Displacement On Areas+拾取面18,19,和 26,然后按OK选择“All DOF”,然后按OK或用命令:DA,18,ALLDA,19,ALLDA,26,ALL,January 20,2001Inventory#001442W2-24,2A.应力分析 车床刀具,改变标题:Utility Menu File Change Title 键入标题:Lathe Cutter-with ALL DOF constraint on areas at hole按OK16.保存数据库并求解:在工具条上拾取“SAVE_DB”(或选择:Utility Menu File Save as Jobname.db)Main Menu Solution-Solve-Current LS按OK按Close或用命令:SAVE/SOLUSOLVE17.观察结果:Main Menu General Postproc Plot Results-Contour Plot-Nodal Solu.选择“Stress”和“von Mises SEQV”按OK或用命令:PLNSOL,S,EQV,January 20,2001Inventory#001442W2-25,2A.应力分析 车床刀具,Open minimized plot from previous analysis to compare results,January 20,2001Inventory#001442W2-26,2A.应力分析 车床刀具,17.存储并退出ANSYS:在工具条上拾取“QUIT”(或选择:Utility Menu File Exit.)选择“Save Everything”按OK或用命令:FINISH/EXIT,ALL,2-D 角型支架分析指南,练习 2B应力分析,January 20,2001Inventory#001442W2-28,2B.应力分析2-D角型支架分析指南,说明本练习向你逐步介绍有关ANSYS指南一步一步求解的例子，它们以HTML格式显示。这个问题是一个用二维平面应力单元模拟的角型支架的静力分析。,January 20,2001Inventory#001442W2-29,2B.应力分析2-D角型支架分析指南,按教师指定的工作目录，用“bracket”作为作业名，进入ANSYS。进入ANSYS在线帮助指南：Utility Menu Help ANSYS Tutorials打开“Structural Tutorial”文件夹选择“Static Analysis of a Corner Bracket”文件架执行 步骤1 至 26或用命令 在您的浏览器窗口选择以下路径:Unix:ansys57docuenglishansyshelpHlp_UI_Tutorials.htmlIntel-PC:D:/ansys57/docu/english/tuthelp.chm(注意，向您的教师询问您的计算机中TUTORToc.htm文件的路径）,
