Ansys练习 应力分析.ppt

车床刀具,练习2A应力分析,January20,2001Inventory#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)画位侈2)列反力3)画vonMises应力4)动态显示vonMises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。,January20,2001Inventory#001442W2-3,2A.应力分析车床刀具,第一次求解载荷及材料特性:,January20,2001Inventory#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：,January20,2001Inventory#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”:MainMenuPreferences选择“Structural”,然后按OK,January20,2001Inventory#001442W2-6,2A.应力分析车床刀具,3.选择“Nodefeaturing”，输入“cutter.igs”IGES文件:UtilityMenuFileImportIGES选择“Nodefeaturing”,然后按OK选择“cutter.igs,然后按OK或用命令:/AUX15IOPTN,IGES,NODEFEATIGESIN,cutter,igs,January20,2001Inventory#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：MainMenuPreprocessorOperateScaleVolumes+按PickAll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,1/2.54,1/2.54,1/2.54,0,1UtilityMenuPlotVolumes或用命令:VPLOT,January20,2001Inventory#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:UtilityMenuFileReadInputfrom选择“cutter-area.inp”,然后按OK或用命令:/INPUT,cutter-area,inp,January20,2001Inventory#001442W2-9,2A.应力分析车床刀具,6.确定单元类型：MainMenuPreprocessorElementTypeAdd/Edit/Delete按Add.选择“StructuralSolid”和“Tet10node92”,然后按OK按Close或用命令:ET,1,SOLID92,January20,2001Inventory#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):MainMenuPreprocessorMaterialPropsMaterialModelsStructural-Linear-Elastic-Isotropic输入EX=10e6(铝的弹性模量，以psi为单位)输入PRXY=.32按OKSelectMaterialExit或用命令:MP,EX,1,10e6MP,PRXY,1,.32,January20,2001Inventory#001442W2-11,2A.应力分析车床刀具,8.激活智能网格，用四面体单元划分实体：MainMenuPreprocessorMeshTool激活“SmartSize”设置SmartSize为4按Mesh拾取PickAll按Close或用命令:SMRT,4MSHAPE,1,3DMSHKEY,0VMESH,January20,2001Inventory#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：UtilityMenuPlotAreasMainMenuSolution-Loads-Apply-Structural-Displacement-SymmetryB.C.-OnAreas+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,January20,2001Inventory#001442W2-13,2A.应力分析车床刀具,10.在顶端施加压力:MainMenuSolution-Loads-Apply-Structural-PressureOnAreas+拾取面1,然后按OKVALUE=10000按OK或用命令:SFA,1,1,PRES,10000,January20,2001Inventory#001442W2-14,2A.应力分析车床刀具,11.保存数据库并求解:Clickthe“SAVE_DB”buttonintheToolbar(orselect:UtilityMenuFileSaveasJobname.db)MainMenuSolution-Solve-CurrentLS观察“/STATUSCommand”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,January20,2001Inventory#001442W2-15,2A.应力分析车床刀具,12.观察结果：12a.画出位侈：MainMenuGeneralPostprocPlotResults-ContourPlot-NodalSolu.选择“DOFsolution”和“TranslationUSUM”,选择“Def+undefedge”,然后按OK或用命令:/POST1PLNSOL,U,SUM,2,1,January20,2001Inventory#001442W2-16,2A.应力分析车床刀具,January20,2001Inventory#001442W2-17,2A.应力分析车床刀具,12b.列出反力:MainMenuGeneralPostprocListResultsReactionSolu.选择“Allitems”,然后按OK或用命令:PRRSOL,January20,2001Inventory#001442W2-18,2A.应力分析车床刀具,January20,2001Inventory#001442W2-19,2A.应力分析车床刀具,12c.画出vonMises应力:MainMenuGeneralPostprocPlotResults-ContourPlot-NodalSolu.选择“Stress”和“vonMisesSEQV”,然后按OK或用命令:PLNSOL,S,EQV,January20,2001Inventory#001442W2-20,2A.应力分析车床刀具,12d.对模型进行“捕捉”并将其最小化：UtilityMenuPlotCntrlsCaptureImage在以后的比较中把窗口最小化,January20,2001Inventory#001442W2-21,2A.应力分析车床刀具,12e.动画显示vonMises应力：UtilityMenuPlotCtrlsAnimateDeformedResults.选择“Stress”和“vonMisesSEQV”,然后按OK或用命令:PLNSOL,S,EQVANCNTR,10,0.5,January20,2001Inventory#001442W2-22,2A.应力分析车床刀具,January20,2001Inventory#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CloseUtilityMenuPlotAreasMainMenuSolution-Loads-Delete-Structural-DisplacementOnAreas+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:MainMenuSolution-Loads-Apply-Structural-DisplacementOnAreas+拾取面18,19,和26,然后按OK选择“AllDOF”,然后按OK或用命令:DA,18,ALLDA,19,ALLDA,26,ALL,January20,2001Inventory#001442W2-24,2A.应力分析车床刀具,改变标题:UtilityMenuFileChangeTitle键入标题:LatheCutter-withALLDOFconstraintonareasathole按OK16.保存数据库并求解:在工具条上拾取“SAVE_DB”(或选择:UtilityMenuFileSaveasJobname.db)MainMenuSolution-Solve-CurrentLS按OK按Close或用命令:SAVE/SOLUSOLVE17.观察结果:MainMenuGeneralPostprocPlotResults-ContourPlot-NodalSolu.选择“Stress”和“vonMisesSEQV”按OK或用命令:PLNSOL,S,EQV,January20,2001Inventory#001442W2-25,2A.应力分析车床刀具,打开前面分析最小化的结果以比较结果,January20,2001Inventory#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:UtilityMenuFileExit.)选择“SaveEverything”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,January20,2001Inventory#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。,January20,2001Inventory#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：UtilityMenuHelpANSY