叶轮叶片练习2A耦合INTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-22A.耦合叶轮叶片说明•对叶轮的30°扇区使用耦合。•确定叶片在绕Z轴1000弧度/秒角速度载荷下的vonMises应力分布。INTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-32A.耦合叶轮叶片载荷和材料特性INTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-42A.耦合叶轮叶片1.按教师指定的工作目录,用“cp-blade”作为作业名,进入ANSYS。2.恢复“cp-blade.db1”数据库文件:–UtilityMenuFileResumefrom…–或使用命令:RESUME,cp-blade,db13.进入前处理器,分别定义单元类型1为SOLID95,单元类型2为MESH200。对MESH200单元设置KEYOPY(1)=5:–MainMenuPreprocessorElementTypeAdd/Edit/Delete…•[Add...]–选择“StructuralSolid”和“Brick20node95”,然后按[Apply]–选择“NotSolved”and“MeshFacet200”,然后按[OK]•选择[Options...]•SetK1=“TRIA6-NODE”,然后按[OK]•[Close]–或使用命令:/PREP7ET,1,SOLID95ET,2,MESH200KEYOPT,2,1,5INTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-52A.耦合叶轮叶片4.使用VSWEEP对体volume2进行网格剖分:–MainMenuPreprocessorMeshTool…•选择“Hex”(六面体)和“Sweep”(扫掠),然后选择[Sweep]–或使用命令:VSWEEP,25.选择“智能尺寸”等级4并用MESH200单元对1号面剖分网格(扇区底侧边界):–MainMenuPreprocessorMeshTool…•智能尺寸”等级置为4•Mesh置为Areas•选择“Tri”和“Free”,然后按[Mesh]–或使用命令:SMRT,4AMESH,1INTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-62A.耦合叶轮叶片6.拷贝1号面的网格到11号面(扇区高段一侧边界):–MainMenuPreprocessor-Modeling-CopyAreaMesh+•拾取1号面(或者在ANSYS输入窗口键入“1”后按[Enter]键)•[OK]•拾取11号面(或者在ANSYS输入窗口键入“11”后按[Enter]键)•在拾取对话框中选择[OK]•设置KCN=1•设置DY=30•按[OK]–或使用命令:MSHCOPY,AREA,1,11,1,0,30INTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-72A.耦合叶轮叶片7.使用SOLID95对1号体剖分网格:–MainMenuPreprocessorMeshTool…–或使用命令:VMESH,18.将SOLID95退化为SOLID92单元:–MainMenuPreprocessor-Meshing-ModifyMeshChangeTets...–或使用命令:TCHG,95,92,3INTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-82A.耦合叶轮叶片9.在柱坐标系(CSYS,1)中,把边界低侧节点自由度耦合到边界高侧节点的自由度:–MainMenuPreprocessorCoupling/CeqnOffsetNodes…•设置KCN=1•设置DY=30•选择[OK]–或使用命令:CPCYC,ALL,0.0001,1,0,30INTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-92A.耦合叶轮叶片10.在X=0(或者在柱坐标系中r=0)的节点上约束UX和UY:10a.在X=0选择节点:–UtilityMenuSelectEntities...–或使用命令:NSEL,S,LOC,X,010b.约束节点UX、UY自由度:–MainMenuPreprocessorLoads-Loads-Apply-Structural-DisplacementOnNodes+–或使用命令:D,ALL,UX,,,,,UY11.为了防止在Z方向的刚体运动(轴向),约束坐标原点处节点(2426号节点)UZ自由度:11a.再选择Z=0处节点子集:–UtilityMenuSelectEntities...–或使用命令:NSEL,R,LOC,Z,011b.约束所选节点UX,UY,和UZ自由度:–MainMenuPreprocessorLoads-Loads-Apply-Structural-DisplacementOnNodes+–或使用命令:D,ALL,UZINTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-102A.耦合叶轮叶片12.选择所有节点并把节点的坐标系改变到总体柱坐标系:12a.选择所有节点:–UtilityMenuSelectEverything–或使用命令:NSEL,ALL12b.把激活坐标系设置为总体柱坐标系:–UtilityMenuWorkPlaneChangeActiveCStoGlobalCylindrical–或使用命令:CSYS,112c.改变节点坐标系到总体柱坐标系:–MainMenuPreprocessor-Modeling-Move/Modify-RotateNodeCS-ToActiveCS+•[PickAll]–或使用命令:NROTAT,ALLINTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-112A.耦合叶轮叶片13.关闭节点耦合符号:–UtilityMenuPlotCtrlsSymbols…•在对话框中选择“ForIndividual:”和“Miscellaneous”,然后选择[Ok]•设置CP=“Off”•选择[OK]–或使用命令:/PBC,CP,,014.检查单元:–MainMenuPreprocessor-Meshing-CheckMeshSelBadElems…•在对话框中选择[OK]•选择[Close]–UtilityMenuPlotElements•选择[Close]–UtilityMenuSelectEverything–UtilityMenuPlotElements–或使用命令:CHECK,ESEL,WARNEPLOTESEL,ALLEPLOTINTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-122A.耦合叶轮叶片15.存储数据库并获取解答:–Pickthe“SAVE_DB”buttonintheToolbar(orselect:UtilityMenuFileSaveasJobname.db)–MainMenuSolution-Solve-CurrentLS•查看“/STATUSCommand”然后关闭对话框•选择[OK]•选择[Close]-关闭黄色信息框完成求解–或使用命令:SAVE/SOLUSOLVEINTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-132A.耦合叶轮叶片16.进入后处理器,画出vonMises应力:–MainMenuGeneralPostprocPlotResults-ContourPlot-NodalSolu...–或使用命令:/POST1PLNSOL,S,EQVINTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-142A.耦合叶轮叶片17.画出2号体(叶片)的vonMises应力:–UtilityMenuSelectEntities–SeleBelow(toselecteverythingbelowselectedvolumes)–MainMenuGeneralPostprocPlotResults-ContourPlot-NodalSolu...–或使用命令:VSEL,S,,,2ALLSEL,BELOW,VOLUPLNSOL,S,EQVINTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-152A.耦合叶轮叶片18.画出1号体(基座)的vonMises应力:–UtilityMenuSelectEntities–SeleBelow(toselecteverythingbelowselectedvolumes)–Replot–或使用命令:VSEL,S,,,1ALLSEL,BELOW,VOLUPLNSOL,S,EQVINTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-162A.耦合叶轮叶片19.选择全部实体并把结果扩展360度:–UtilityMenuSelectEverything–UtilityMenuPlotCtrlsStyleSymmetryExpansionUser-SpecifiedExpansion…•设置NREPEAT=12•设置TYPE=Polar•设置DY=30,然后选择[OK]–UtilityMenuPlotCtrlsPan,Zoom,Rotate...•选择[ISO]•选择[Fit]–或使用命令:/EXPAND,12,PLOAR,FULL,,30/VIEW,1,1,1,1/AUTO,1/REPLOT20.存储并退出ANSYS:–Pickthe“QUIT”buttonintheToolbar–或使用命令:SAVEFINISH/EXIT涡轮叶片练习2B约束方程INTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-182B.约束方程涡轮叶片说明•使用约束方程连接涡轮叶片和叶片支座,然后施加X方向1000in/sec2的加速度进行应力分析。INTRODUCTIONTOANSYS5.7-Part2WorkshopSupplementJanuary30,2001Inventory#001444W2-192B.约束方程涡轮叶片载荷与材料特性INTRODUCTIONTOANSYS5.7-Part2Worksh