第9章受内外压筒体的有限元建模与应力变形分析(Project 2)计算分析模型如图9-1 所示, 习题文件名: cylinder。

X(a)σO=100N/mm2σI =200N/mm2γ =7.85g/cm3µ =0.3E =210000N/mm2(b)图9-1 计算分析模型9.1进入ANSYS程序→ANSYSED 6.1ed →Interactive →change the working directory into yours→input Initial jobname: cylinder→Run9.2 设置计算类型ANSYS Main Menu: Preferences…→select Structural →OK9.3 选择单元类型ANSYS Main Menu: Preprocessor → Element Type →Add/Edit/Delete… → Add… →select Solid Quad 4node 42 →Apply →select Solid Brick 8node 45 → OK → Close (the ElementTypes window)9.4定义材料参数ANSYS Main Menu: Preprocessor →Material Props →Materials Models →Structural→Lineal →Elastic→Isotropic…→input EX:2.1e5, PRXY:0.3→ OK 关闭材料定义窗口9.5构造筒体模型➊生成模型截平面ANSYS Main Menu: Preprocessor →Modeling→Create →Keypoints →In Active CS… →按次序输入横截平面的十个特征点和旋转对称轴上两点坐标（十个特征点：(300,0,0), (480,0,0), (480,100,0), (400,100,0), (400,700,0), (480,700,0), (480,800,0), (300,800,0), (300,650,0), (300,150,0)，对称轴上两点：(0,0,0), (0,800,0)）（每次输入完毕，用Apply结束，0可以不输入）→Cancel (back to Create window) →-Areas- Arbitrary → Through KPs →依次连接截面边线上的十个特征点(注意在选完第10点后结束，不要再选第1点)→ OK➋对平面进行网格划分ANSYS Main Menu: Preprocessor →Meshing→Mesh Tool →(Size Controls) Globl: Set →input SIZE (element edge length): 50 →OK (back to MeshTool window)→Mesh → Pick All (in Picking Menu) → Close( the MeshTool window)➌用旋转法生成筒体模型ANSYS Main Menu: Preprocessor →Modeling→Operate →Extrude→Elem Ext Opts→select TYPE:SOLID 45→Element sizing options for extrusion No. Elem divs: 1→OK (back to Extrude window)→Areas →About Axis →Pick All(in Picking Menu)→OK→Pick the two keypoints (11,12) of the Symmetrical Axis → OK→input ARC: 90; NSEG: 3→ OK9.6 模型加位移约束ANSYS Main Menu: Solution→Define Loads →Apply→Structural→Displacement➊两截面分别加Z, X方向的约束ANSYS Utility Menu: Select → Entities…→Nodes → By Location →select X coordinates →input 0→ OK (back to Displacement window)→On Nodes → Pick All(in Picking Menu) → select Lab2:UX →OK →ANSYS Utility Menu: Select → EverythingANSYS Utility Menu: Select → Entities…→ Nodes → By Location →select Z coordinates →input 0→ OK (back to Displacement window)→On Nodes →Pick All(in Picking Menu) → select Lab2:UZ →OK →ANSYS Utility Menu: Select →Everything➋底面加Y方向的约束ANSYS Utility Menu: Select → Entities… → Nodes → By Location →select Y coordinates →input 0→ OK (back to Displacement window)→On Nodes →Pick All(in Picking Menu) →select Lab2:UY → OK →ANSYS Utility Menu: Select →Everything9.7 模型加载荷ANSYS Main Menu: Solution→ Define Loads→Apply→Structural→Pressure →On Areas →pick the Internal Load Surface of model (Total 6 areas) → OK→input V ALUE:200 → Apply →(忽略警告信息)pick the External Load Surface of model → OK→input V ALUE:100→ OK9.8 分析计算ANSYS Main Menu: Solution→ -Solve- Current LS→OK (to close the Solve Current Load Step window)9.9 结果显示ANSYS Main Menu: General Postproc →Plot Results→Deformed Shape…→select Def + Undeformed→OK (back to Plot Results window)→ -Contour Plot- Nodal Solu…→select: Stress, Von Mises, Def + Undeformed→OK9.10 退出系统ANSYS Utility Menu: File→Exit…→ Save Everything→OK9.11完全的直接命令输入方式操作finish !finish the last case/clear,start !restart/prep7 !preprocessoret,1,plane42 !define the elementset,2,solid45mp,ex,1,210000 !define materials parametersmp,prxy,1,0.3k,1,300,,, !define key points of section framek,2,480,,,k,3,480,100,,k,4,400,100,,k,5,400,700,,k,6,480,700,,k,7,480,800,,k,8,300,800,,k,9,300,650,,k,10,300,150,,k,11,,,, !define key points of revolving axisk,12,,800,0a,1,2,3,4,5,6,7,8,9,10 !link the key points to an areaesize,50,, !define element edge lengthamesh,all !meshing the areatype,2 !define the following element typeextopt,esize,1,0 !define element division number when extruding vrotat,all,,,,,,11,12,90,3 !extrude (sweep) the area with meshes/solution !define the load and run this casensel,s,loc,x,0 !select all nodes whose x coordinate are 0d,all,ux,0 !constrain the node's x DOFallsel,allnsel,s,loc,z,0 !select all nodes whose z coordinate are 0d,all,uz,0 !constrain the node's z DOFallsel,allnsel,s,loc,y,0 !select all nodes whose y coordinate are 0d,all,uy,0 !constrain the node's y DOFallsel,allsfa,10,1,pres,200 !define pressure on the inner area of cylinder sfa,21,1,pres,200sfa,32,1,pres,200sfa,5,1,pres,100 !define pressure on the outter area of cylinder sfa,16,1,pres,100sfa,27,1,pres,100solve !runfinish/view,1,1,2,3/post1 !postprocessorplnsol,s,eqv,0,1 !plot the contour of von-Mises stressfinish !end。