Ansys练习非线性分析

Click to edit Master title style,Click to edit Master text styles,Second level,Third level,Fourth level,Fifth level,January 30, 2001,Inventory #001444,W7-,January 30, 2001Inventory #001444W7-*,INTRODUCTION TO ANSYS 5.7 - Part 2,专题,Supplement,大挠度拱梁,练习 7,非线性分析,7. 非线性分析 - 大挠度拱梁,说明,浅拱受到跨中载荷为,20,000,N,的作用。用线性和非线性（大挠度）两种分析分别确定跨中位移，比较它们的结果。,January 30, 2001,7. 非线性分析 - 大挠度拱梁,载荷和材料属性,January 30, 2001,7. 非线性分析 - 大挠度拱梁,1.按教师指定的工作目录用,“,beamarch”,作为作业名，进入,ANSYS。,2.,我们建议您按步骤,3-12,建立模型,如果您不愿意这样做的话，可以恢复已存在的数据库,(,beamarch.db1),，直接跳到步骤13。,Utility Menu File Resume from ,或使用命令:,RESUME,beamarch,db1,3.,在整体柱坐标系中定义四个关键点,:,关键点1的坐标,(1270,75),关键点,2,的坐标,(1270,90),关键点,3,的坐标,(1270,105),关键点,4,的坐标,(1270sin45, 90).,关键点,4,是方向关键点,.,Utility Menu WorkPlane Change Active CS to Global Cylindrical,Main Menu Preprocessor -Modeling- Create Keypoints In Active CS ,Utility Menu Parameters Angular Units .,或用命令:,/PREP7,CSYS,1,K,1,1270,75,K,2,1270,90,K,3,1270,105,*AFUN,DEG,K,4,(1270*SIN(45),90,January 30, 2001,7. 非线性分析 - 大挠度拱梁,4.在关键点1和关键点2间定义线（弧），在关键点2和3间定义线,:,Main Menu Preprocessor -Modeling- Create -Lines- Lines In Active Coord +,或用命令:,L,1,2,L,2,3,5.,定义单元类型为,BEAM189,定义材料特性,(,EX=210e3 MPa, PRXY=0.3):,Main Menu Preprocessor Element Type Add/Edit/Delete ,Main Menu Preprocessor Material Props Material Models Structural Linear Elastic - Isotropic,或用命令:,ET,1,BEAM189,MP,EX,1,210E3,MP,PRXY,1,0.3,6.,约束关键点1和3,UX, UY,和,UZ,位移,约束关键点2,UZ,位移,:,Main Menu Preprocessor Loads -Loads- Apply -Structural- Displacement On,keypoints,+,或用命令:,DK,1,UX,0,UY,UZ,DK,3,UX,0,UY,UZ,DK,2,UZ,0,January 30, 2001,7. 非线性分析 - 大挠度拱梁,7.在关键点2的-,Y,方向上施加20000,N,的力,:,Main Menu Preprocessor Loads -Loads- Apply -Structural- Force/Moment On keypoints +,或用命令:,FK,2,FY,-20000,January 30, 2001,7. 非线性分析 - 大挠度拱梁,8.定义梁的截面,:,Main Menu Preprocessor Sections -Beam- Common Sectns .,ID = 1,Sub-Type = ,Offset = Centroid,B = 25,H = 12.5,按 ,OK,或用命令:,SECTYPE,1,BEAM,RECT,SECOFFSET,CENT,SECDATA,25,12.5,January 30, 2001,7. 非线性分析 - 大挠度拱梁,9.指定线的属性,包括线的定位关键点,:,Main Menu Preprocessor -Attributes- Define All Lines .,MAT = 1,TYPE = “1 BEAM189”,SECT = 1,选择定位关键点为,“yes”,按 ,OK,拾取关键点,然后按,OK,或用命令:,LATT,1, ,1, ,4, ,1,January 30, 2001,7. 非线性分析 - 大挠度拱梁,10.在所有线上设置单元分割数为10,:,Main Menu Preprocessor -Meshing- Size Cntrls -ManualSize- -Lines- All Lines .,或用命令:,LESIZE,ALL,10,11.,对所有线进行网格划分,:,Main Menu Preprocessor -Meshing- Mesh Lines +,或用命令:,LMESH,ALL,12.,设置,/,ESHAPE,为“,on”,/,EFACET,为2,然后画出单元,:,Utility Menu PlotCtrls Style Size and Shape .,或用命令:,/ESHAPE,1,/EFACET,2,EPLOT,January 30, 2001,7. 非线性分析 - 大挠度拱梁,13. 存储数据库并进行线性求解：,Pick the “SAVE_DB” button in the Toolbar (or select: Utility Menu File Save as Jobname.db),Main Menu Solution -Solve- Current LS,或用命令:,SAVE,/SOLU,SOLVE,14.,选择节点2,(,跨中节点,),进入通用后处理器,POST1,并列出节点位移,:,Utility Menu Select Entities .,Main Menu General Postproc List Results Nodal Solution .,或用命令:,NSEL,S,2,/POST1,PRDISP,January 30, 2001,7. 非线性分析 - 大挠度拱梁,15.选择全部实体，进入求解器，进行非线性求解,:,Utility Menu Select Everything,Main Menu Solution Soln Control .,在分析选项中激活,“L,arge Displacement Static,”,选项,设定子步数,= 10,按 ,OK,Main Menu Solution -Solve- Current LS,或用命令:,ALLSEL,/SOLU,NLGEOM,1,NSUBST,10,SOLVE,收敛控制图,January 30, 2001,7. 非线性分析 - 大挠度拱梁,16.列出节点2的位移,:,Utility Menu Select Entities .,Main Menu General Postproc List Results Nodal Solution .,或用命令:,NSEL,S,2,/POST1,PRDISP,January 30, 2001,7. 非线性分析 - 大挠度拱梁,17.选择全部实体，设置位移缩放比例为,5,然后画出,UY,位移,:,Utility Menu Select Everything,Utility Menu PlotCtrls Style Displacement Scaling ,Main Menu General Postproc Plot Results -Contour Plot- Nodal Solu ,或用命令:,ALLSEL,/DSCALE,1,5,PLNSOL,U,Y,January 30, 2001,7. 非线性分析 - 大挠度拱梁,18.画出位移,UY,的动画,:,Utility Menu PlotCtrls Animate Deformed Results ,或用命令:,ANCNTR,10,0.5,19.,存储并退出,ANSYS:,Pick the “QUIT” button,in the Toolbar,或用命令:,FINISH,/EXIT,January 30, 2001,