Ansys谱分析技术详解

关于材料

材料属性  Material Prop(支柱)→Material Models→Strutural  EX=2e11、PRXY=0.3、Density=7800

单元类型  Element type→add  Beam189(梁) 、shell181(壳)

梁截面    Section→Beam→Common Sections  Name、ID=1、B=0.004、H=0.004

板的厚度  Section→Shell→Lay-up(储存)→add  Name、ID=2、Thiness=0.002

几何建模(距离是0.05)是      

建点Modeling→Create→Keypoints→In Active CS   1（0,0,0）2（0.05,0,0）3（0.05, 0.05,0）2（0, 0.05,0）

复制关键点（复制关键点建2面，再复制2面）Modeling→Copy→Keypoints  Pick all、DX=0、DY=0、DZ=0.05

压缩编号（合并编号）前→Numbering Ctrls→Compress Numbers  Keypoints

创建线

划分网格

划分的尺寸Meshing→MeshTool→SizeControls,Global,Set  Size=0.02

划分壳单元Meshing→MeshTool→Set  [TYPE]=SHELL、[SECNUM]=SHELL→Mesh  面积

划分梁单元Meshing→MeshTool→Set  [TYPE]=BEAM、[SECNUM]=BEAM→Mesh  梁

单元形状（看划分效果）PlotCtrls→Style→Size and Shape  ESHAPE:ON

模态分析 1

设置分析类型（模态应分析）Analysis Type→New Analysis  

设置求解方法             Analysis Type→Analysis Option  Subspace No.of modes extract=10

加约束（底端6个点全约束）Loads→Define loads→Apply→Structural→Displacement(移位)→On Node  选择 All DOF

求解F

模态分析 2

设置分析类型（谱分析）Analysis Type→New Analysis Spectrum

设置扩展模态数       Analysis Type→Analysis Option  Single-pt resp  No.of modes for solu=10

设置谱类型Solution→Load Step opts→Spectrum→single point→setting  Seismic displac  Coordinates og point=0,1,0

定义频率表Solution→Load Step opts→Spectrum→single point→Freq Table FREQ1-FREQ8=0.5 , 1 , 2.4 , 3.8 ,17,18,20,32

定义谱值表Solution→Load Step opts→Spectrum→single point→Spectr Values OK

SV1-SV8=0.001,0.0005,0.0009,0.0008,0.0012,0.00075,0.00086,0.0002s

求解F

扩展模态 3

设置分析类型（模态分析）Analysis Type→New Analysis Modal

设置扩展项             Analysis Type→ExpansionPass   Expansion Pass=On

设置扩展参数Solution→Load Step opts→ExpansionPass→Single Expand→Expand ModesNo.of modes to expand=10 yes SIGNIF=

求解

合并模态 4

设置分析类型（谱分析）Analysis Type→New Analysis Spectrum

设置扩展模态数       Analysis Type→Analysis Option  OK

模态合并参数设置Solution→Load Step opts→Spectrum→single point→Mode Significant threshold=0.15

Combine Mode Combination Method=SRSS  

求解F

数据后处理

结果概要          General Postproc→Results Summary  出图

列出节点解        General Postproc→Read results→Frist set

列出合位移的节点解General Postproc→List Results  Nodal solution DOF solution Dispalcement vector sum

列出反力解        General Postproc→List Results→Reaction Solu  All Items