Modal analysis of a frame using ANSYS (ANSYS框架模态分析)

ANSYS 框架结构模态分析练习。(This is a small example to outline the steps required to do a simple modal analysis of a frame structure using ANSYS.)

  • 算例(Example

ProblemDescription_Blog

  • ANSYS有限元模拟(FEM Analysis with ANSYS

这个问题可以很简单的通过命令流的方式进行建模,如下给出具体的命令流:

FINISH
/CLEAR
/TITLE,Modal analysis of a frame
/PREP7

!Element type
ET,1,BEAM4

!Material
MP,EX,1,32500
MP,PRXY,1,0.2
MP,DENS,1,2.403E-09

!Real for beam 200X500
!R,NO,AREA,IZZ,IYY,TKZ,TKY,THETA
R,1,100000,3.333E+08,2.083E+09,500,200,
!ISTRAIN,IXX,SHEARZ,SHEARY
RMORE,0,9.981E+08,0,0

!Real for Column 600X600
!R,NO,AREA,IZZ,IYY,TKZ,TKY,THETA
R,2,360000,1.080E+10,1.080E+10,600,600,
!ISTRAIN,IXX,SHEARZ,SHEARY
RMORE,0,1.825E+10,0,0

!Nodes
N,1,-3000,-3000,0
N,2,-3000,-3000,3000
N,3,-3000,-3000,6000
N,4,-3000,-3000,9000
N,5,-3000,3000,0
N,6,-3000,3000,3000
N,7,-3000,3000,6000
N,8,-3000,3000,9000
N,9,3000,-3000,0
N,10,3000,-3000,3000
N,11,3000,-3000,6000
N,12,3000,-3000,9000
N,13,3000,3000,0
N,14,3000,3000,3000
N,15,3000,3000,6000
N,16,3000,3000,9000

!Direction Nodes
N,41,-3000,-3000,12000
N,161,3000,3000,12000
N,91,6000,-3000,0
N,131,6000,3000,0

!Column elements
REAL,2
EN,1,1,2,91
EN,2,2,3,91
EN,3,3,4,91
EN,4,5,6,131
EN,5,6,7,131
EN,6,7,8,131
EN,7,9,10,91
EN,8,10,11,91
EN,9,11,12,91
EN,10,13,14,131
EN,11,14,15,131
EN,12,15,16,131

!Beam elements
REAL,1
EN,13,2,10,41
EN,14,3,11,41
EN,15,4,12,41
EN,16,6,14,161
EN,17,7,15,161
EN,18,8,16,161
EN,19,2,6,41
EN,20,3,7,41
EN,21,4,8,41
EN,22,10,14,161
EN,23,11,15,161
EN,24,12,16,161

!Displacement boundary conditions
D,1,UX,0
D,1,UY,0
D,1,UZ,0
D,1,ROTX,0
D,1,ROTY,0
D,1,ROTZ,0

D,5,UX,0
D,5,UY,0
D,5,UZ,0
D,5,ROTX,0
D,5,ROTY,0
D,5,ROTZ,0

D,9,UX,0
D,9,UY,0
D,9,UZ,0
D,9,ROTX,0
D,9,ROTY,0
D,9,ROTZ,0

D,13,UX,0
D,13,UY,0
D,13,UZ,0
D,13,ROTX,0
D,13,ROTY,0
D,13,ROTZ,0

FINISH

!Analysis options
/SOLU
ANTYPE,2
MODOPT,LANB,12,,,,1
MXPAND,12,,,YES
LUMPM,ON

!Solve
SOLVE
FINISH

!Post process
/POST1
SET,LIST
SET,1,1
PLDISP,1

输入以上命令流,运行分析,即可获得分析结果。

  • 查看分析结果(Check Results

MODE1

MODE2

MODE3 ModeList

  • 与SAP2000分析结果对比(Comparison with SAP2000 results 

SAP2000中建立欧拉梁单元模型,参见博文 :《Modal analysis of a frame using Abaqus (Abaqus框架模态分析)

SAP2000分析结果:

SAP2000Freq

从以上对比可见,SAP2000的分析结果与ANSYS的分析结果一致。

  • 相关博文( Related Posts)

[01]. Torsion analysis by thermal analogy with ANSYS (ANSYS热比拟扭转应力分析)

[02]. Analysis of a Euler–Bernoulli beam with ANSYS [ANSYS 欧拉-伯努利梁分析]


You already voted!

  • 注释 ( Comments )

  (  大家一起学习有限元!!!! 如有错漏,欢迎批评指正。邮箱:jidong_cui@163.com . 如果你喜欢这篇博文,请在上面给我 点个赞 吧! 🙂   🙂   :-)

  ( If  you have found any problem about this post, please don’t hesitate to contact me directly.Email : jidong_cui@163.com. If you like this posts, please give me a thumbs up rating on the above button! )

  • 微信公众号 ( Wechat Subscription)

WeChat_QRCode

欢迎关注 “结构之旅” 微信公众号

 

3 thoughts on “Modal analysis of a frame using ANSYS (ANSYS框架模态分析)

  1. Pingback: Influence line analysis using ANSYS (ANSYS影响线分析) | 崔济东的博客 - JiDong Cui's Blog

  2. Pingback: TABLE type array parameters in ANSYS (ANSYS中的表格型数组参数) | 崔济东的博客 - JiDong Cui's Blog

  3. Pingback: Array parameter in ANSYS (ANSYS中的数组参数) | 崔济东的博客 - JiDong Cui's Blog

Leave a Reply

Your email address will not be published. Required fields are marked *

This site uses Akismet to reduce spam. Learn how your comment data is processed.