北航宇航学院飞设实验
报告
软件系统测试报告下载sgs报告如何下载关于路面塌陷情况报告535n,sgs报告怎么下载竣工报告下载
飞行器
设计
领导形象设计圆作业设计ao工艺污水处理厂设计附属工程施工组织设计清扫机器人结构设计
工程实验报告
——圆柱壳体结构有限元分析
ZY1315228 张晶 1.圆柱加筋壳体结构有限元分析介绍
圆柱加筋壳结构如图1所示,一端固定,表面有分布载荷。结构、材料特性、约束与载荷的具体形式将在后面给出。试用MSC.Patran/Nastran建立圆柱加筋壳的有限元模型并计算它的位移与应力。
图 1 圆柱加筋壳结构
2.模型描述
2.1 结构
1)壳
,2Lm,6Rmm,,,,3100.50.53圆柱壳半径为,长为。它由两部分组成,,,
一部分是复合材料结构,从固定端到中部,长3m,厚6.2mm;另一部分是金属
材料结构,从中部到自由端,长3m,厚2mm。
2)加筋梁
有纵向加筋与环向加筋,沿壳分布如图2所示,均为金属材料。
图 2 圆柱壳上加筋梁分布
纵向加筋共八条沿周向对称分布如图3所示,截面形状为L型,具体尺寸与指向如图4所示。
图 3 周向对称分别L型梁 R=0.53m 图 4 L型梁截面尺寸 w=h=10mm t=3mm
环向加筋共3条,分别位于壳的两端与中部,截面形状为矩形,具体尺寸如图5所示。
图 5 矩形梁截面尺寸 w=h=10mm 2.2 材料
1)金属材料
2,,0.33即copper,,。 EeNm,,1.011/,,
2)复合材料
22面板(facesheet):,,EeNm,,1.011/EeNm,,1.010/,,,,1122
2,。 GeNm,,1.510/,,0.1,,1212
222芯(core):,,,ENm,100/ENm,100/GNm,50/,,,,,,221211
22GeNm,,1.06/,GeNm,,1.06/,,,0.3。 ,,,,231213
层合板:由面板和芯组成,具体铺层形式和方向如图6所示。其中每层面板厚0.3mm,芯厚5mm。
45º
-45º
0ºcorefacesheet
-45º
45º
图 6 复合材料铺层
2.3 约束与载荷
圆柱壳一端固定,如图7所示。
图 7 固定端
2壳的内表面有分布载荷PyNm,200/(Y轴如图3所示)。 ,,
3.建模过程
3.1几何模型的建立
1.建立新的数据库,输入全局参数,最大尺寸为6米
File/new
New database name: sylindrical shell structure
Ok
, Based on model
Approximate maximun model
Dimesion: 6.0 Analysis code: MSC.Nastran Analysis type: structure
Ok
2.建立名为”shell”的一个新组
Group/create
New group name: shell , Make current
Apply
Cancle
3.绘制一半径为0.5m的圆,并通过面拉伸命令形成壳体
, Geometry
Action creat Object curve Method 2D Circle Circle radius 0.5 Construction plane list coord 0.3 Center point list [0 0 0] Apply
Action create Object surface Method extrude Tanslation vector <0 0 3> Curve list curve 1 Apply
4.复制刚刚生成的圆柱壳体
Action tranform Object surface Method translate Surface list surface 1 Direction vector <0 0 1> Vector magnitude 3 Repeat count 1 Apply
5.建立一个新的组取名为”circular_beam”
Group/create
New group name: circular beams , Make current
Apply
Cancle
6.通过复制生成另外两个圆形梁曲线
Action tranform Object circle Method translate Curve list curve 1 Direction vector <0 0 1>
Vector magnitude 3 Repeat count 2 Apply
7.纵向筋的绘制,建立一个名为” longitudinal beams”的新组
Group/create
New group name: longitudinal beams , Make current
Apply
Cancle
8.沿长度方向创建一条直线
Action creat Object curve Method point Starding point point 1 Ending point point 3 Apply
9.通过旋转的方法创建8条直线,旋转角度为45?
Action transform Object curve
Method rotate Rotation angle 45 Repeat count 7 Curve list curve 4 Apply
图 错误~文档中没有指定样式的文字。-8几何模型建立完成
1.1 显示组”shell”,并设置为当前组
Group/post
Select group to post: shell Apply
Cancle
3.2有限元网格划分
1.将组”shell”设置为当前组
Group/post
Select group to post: shell
Apply
Cancle
2.生成”mesh seed”
, Elements
Action create
Object mesh seed
Type uniform
Number of elements:
Number= 32
Curve list curve 1
Apply
Number of elements:
Number= 30
Curve list surface 1.1 2.1
Apply
3. 选择”isomesh”,生成四边形单元
Action creat
Object mesh
Type surface Elem shape quad Mesher IsoMesh Topology Quad4 Surface list surface 1 2 Apply
4.显示组“longitudinal beams” 并且设置为当前组
Group/post
Select group to post: longitudinal beams
Apply
Cancle
5.用curve的方式划分longitudinal beams的网格
Action creat Object mesh Type curve Topology bar2 curve list curve 4:11 Apply
6.显示组“cicular beams” 并设置为当前组
Group/post
Select group to post: circular beams Apply
Cancle
7.用curve的方式划分circular beams的网格
Action creat Object mesh
Type curve
Topology bar2
curve list curve 1:3 Apply
8.节点等效
在面的边上重复创建了节点,因此需要将节点等效
Action: equivalence Object: all Type: tolerance cube Equivalence tolerance: 0.004 Apply
图3-2 有限元网格划分完成
3.3 材料属性添加
3.3.1 复合材料的添加
1.facesheet和core材料添加
, Material
Action: create Object: 2d orthotropic Method: manual input Material name: facesheet Input properties
Constitutive model: linear elastic Elastic modulus 11: 1e11 Elastic modulus 22: 1e10 Poisson ratio 12: 0.1 Shear modulus 12: 1.5e10 Apply
Material name: core
Input properties
Constitutive model=: inear elastic Elastic modulus 11=: 100 Elastic modulus 22=: 100 Poisson ratio 12: 0.3
Shear modulus 12: 50 Shear modulus 23: 1e6 Shear modulus 13: 1e6 Apply
图3-3 core材料属性
图3-4 facesheet材料属性
2.复合材料属性添加,用core和facesheet材料铺成复合材料
Action: create Object: composite Method: laminate Material name: compsite_layers Laminated composite
Input date
Material name thichness orientation
1 facesheet 3e-4 45
2 facesheet 3e-4 -45
3 core 5e-3 0
4 facesheet 3e-4 -45
5 facesheet 3e-4 45
图3-5 复合材料建立完成
3.铜的材料属性添加
Action: create Object: isotropic Method: manual input Material name: copper Input properties
Elastic modulus= 1e11 Poission ratiao= 0.33 Ok
Apply
4.创建单元属性并将单元属性赋给壳单元
Group/post
Select group to post: shell Apply
Cancle
, Properties
Action: create Object: 2D Type: shell Property set name: composite shell Options: lanminlate Input properties
Material name: m:composite_layers Ok
Select members: ele 1:960 Ok
Apply
Action: create Object: 2D Type: shell Property set name: copper shell Options: homogenous Input properties
Material name: m:copper Thickness: 2E-3
Ok
Select members: ele 961:1920 Ok
Apply
5.建立本地坐标圆柱系
在壳的地步中心点建立一个本地圆柱坐标系,编号1,用于定义纵向L型
梁的指向。
, Geometry
Action create
Object coord Method 3point Coord ID list 1 Type cylindrical Refer. Coordinate frame coord 1 Origin [0 0 0] Point on axis 3 [0 0 1] Point on plan1-3 [1 0 0] Apply
6.创建L型的单元属性并将其赋给L型梁单元
Action: create Object: 1D
Type: beam Property set name copper_beam
Material name: m:copper Input properties
Beam library
Action create Object standard shape Method nastran standard New section name L
L
W= 10e-3
H= 10e-3
t1= 3e-3
t2= 3e-3
Ok
Section name L
Material name m:copper
Bar orientation <-1 0 0>coord 1 Ok
Select application region: ele 1921:2400
Ok
Apply
Action: create Object: 1D
Type: beam
Property set name: L-beam Material name: m:copper Input properties
Beam library
Action create Object standard shape Method nastran standard
New section name rectangle
W= 10e-3 H= 10e-3
Ok
Section name rectangle
Material name m:copper
Bar orientation <-1 0 0>coord 1 Ok
Select application region: ele 2401:2496
Ok
Apply
3.4 固定边界条件建立
, Loads/BCs
Action: create
Object: displacement
Method: nodal
New set name: fixed_node
Input data
Translation
<0,0,0>
Rotations < , , >
Analysis coordinate frame: coord 0
Ok
Selet applicaytion region…
, FEM
Application region: node 1:29:4
Add
Ok
Apply
图3-6固定边界加载完成 3.5 建立壳内表面压力场
1.创建一个变化的标量场
, Field Action: create
Object: spatial
Method: pcl function Field name: linear_load Field type: scalar
Coordinate system type: Real Coordinate system: coord 0 Scalar function: 200*abs(„Y)
Apply
Create the pressure load that will reference the field function.
, Loads/BCs
Action: create
Object: pressure
Method: element uniform
New set name: surface_load Target element type: 2D Input data
Loads/BCs set scale factor 1 Pressure:
Bot surf pressure f:linear_load Analysis coordinate frame: coord 0 Ok
Selet applicaytion region…
, FEM
Application region: ele 1:1920
Add
Ok
Apply
图3-7 内表面加变化的压力载荷
2.压力载荷和边界条件组装到名为“shell_loads”的工况里面。 , Load cases Action: create
Load case name: shell_load Type static
Assign/prioritize load/BCs: Disp_fixed_node
Press_shell_load
Ok
Apply
3.6 将建好的模型提交给Nastran分析
, Analysi
Action: analyze
Object: entire modle
Method: full run
Job name: cylindrical_shell Solution type: linear static Subcase select
Available load cases: shell_load Ok
Apply
3.7 读取并查看分析结果
, Analysis Action: access results
Object: attach XDB
Method: result entities
Available jobs: cylindrical_shell Select results file…
Select results file: cylindrical_shell.XDB
, Results
Action: create
Object: quick plot
Select results cases: cylindracal_shell Select fringe result: stress tensor Quanlity: magnitude
Select deformation result: displacements translational
Apply
4.结果分析
各部位各层应力—变形图如下
图4-1 z1层
图4-2 z2层
图4-3 复合材料第1层
图4-4 复合材料第2层
图4-5 复合材料第3层
图4-6 复合材料第4层
图4-7 复合材料第5层