Introduce to ANSYS  Cable280 –Get a Thorough Understanding of This Element

Introduce to ANSYS Cable280 –Get a Thorough Understanding of This Element

Please Share Us

点击此处查看 ✿水哥原创ANSYS视频教程清单 ✿

水哥专属答疑服务已开通,点此此处查看详情

ANSYS has released a new single element in the 2020R1 version called Cable280. This element is suitable for simulating cable structures ranging from medium to very fine. In civil engineering, it is particularly useful for simulating stay cables, especially for stay cables of cable-stayed bridges and cable-supported domes. This article will briefly introduce the characteristics of the Cable280 element and demonstrate its usage through a simple example of a tensioned beam.

It is worth noting that in the current 2021R1 version, the classic interface cannot specify this element via GUI. It may be added in future versions, but it can still be called through command streams. However, in Workbench, the Cable type can be directly specified for the line body.

Cable280 can be understood as a special Link180 with unidirectional tensile function. Because it uses a higher-order form of shape functions, it has better convergence than Link180 under the same conditions. The element consists of four nodes (I, J, K, L), with the fourth node (L node) as the directional point, which can generally be ignored (because the axial force and area of the cable are the main concerns, and there are no special requirements for the cross-sectional direction). The element geometry is shown below:

图片[1]-Introduce to ANSYS  Cable280 –Get a Thorough Understanding of This Element-峰设教育

The Cable280 node degrees of freedom include three directions of translation (UX, UY, UZ) and can be subjected to element surface loads, i.e., the five directions mentioned above. They can be applied using the SFBEAM command:

  1. Surface 1: I-J surface, Z-axis downward perpendicular to the element
  2. Surface 2: I-J surface, Y-axis downward perpendicular to the element
  3. Surface 3: I-J surface, X-axis positive direction, element tangential
  4. Surface 4: Surface of I, X-axis positive direction, element axial
  5. Surface 5: Surface of J, X-axis negative direction, element axial

The element supports various techniques, including birth-death element, initial state, large deformation, large strain, linear perturbation, nonlinear stability, and stress stiffening.

For this element type, here are three things you should keep in mind:

1、The input of the section area is through the definition of the Link section type with APDL command Sectype and Secdata, which is different from other Link elements.

This element does not support the input of real constants. A typical definition is as follows:

Et,1,Cable200

sectype,1,link

secdata,500

type,1

secnum,1 …

2、As this element is a unidirectional tensile element, in many cases, pre-stress needs to be input to ensure model convergence. The input of pre-stress is through the Inistate command.

A typical command is as follows:

esel,s,ename,,280

inistate,set,csys,elem i

nistate,set,dtyp,stre

inistate,define,,,,,100

allsel,all

The output of this element is through the element table output, and the output content is as follows:

图片[2]-Introduce to ANSYS  Cable280 –Get a Thorough Understanding of This Element-峰设教育

图片[3]-Introduce to ANSYS  Cable280 –Get a Thorough Understanding of This Element-峰设教育

3. When using this element, geometric nonlinearity needs to be turned on, i.e., Nlgeom needs to be set to “on”.

For more detailed information about this element, please refer to the latest Help document.

Here is an example of a simple tensioned beam to demonstrate its usage. The basic information of the example is as follows:

A particular tensioned stringer measures 2.6 meters in height and is supported by three strut rods. The longest strut rod measures 1.1 meters in length and the tensioning control stress is set at 100 megapascals. The cross-sectional area of the beam is a 203mm x 6mm circular pipe, while the strut rods measure 89mm x 3.5mm. The cross-sectional area of the cable is 346mm^2. The elastic modulus of the beam and strut rods is 206 gigapascals, and the elastic modulus of the cable is 180 gigapascals. The density of all components is 7850 kilograms per cubic meter.

图片

In this case, Beam188 is used for the beam, Link180 is used for the strut rods, and Cable280 is used for the cable. The command flow is as follows, and please note that it should be run on version 2020R1 or later, as earlier versions do not have the Cable280 element.

finish
/clear
/prep7
et,1,beam188
et,2,link180
et,3,Cable280
sectype,1,beam,ctube
secdata,203/2-6,203/2
sectype,2,link
secdata,234
sectype,3,link
secdata,346
!================
mp,ex,1,2.06e5
mp,dens,1,7850e-12
mp,prxy,1,0.3
mp,ex,2,1.8e5
mp,dens,2,7850e-12
mp,prxy,2,0.3
!==================
k,1
k,2,20000
k,3,10000,-1100
Larc,1,2,3,21000
L,1,3
L,3,2
wprota,,,90
wpoffs,,,5000
lsbw,all
wpoffs,,,5000
lsbw,all
wpoffs,,,5000
lsbw,all
L,4,5$L,3,6$L,8,7
lsel,s,,,6,10,4
lsel,a,,,2,5,3
secnum,1
latt,1,,1
lesize,all,,,10
lmesh,all
lsel,s,,,1,3,2
lsel,a,,,11
secnum,2
latt,1,,2
lesize,all,,,1
lmesh,all
allsel,all
lsel,u,mat,,1
secnum,3
latt,2,,3
lesize,all,,,1
lmesh,all
!=============
esel,s,ename,,280
inistate,set,csys,elem
inistate,set,dtyp,stre
inistate,define,,,,,100    
allsel,all
!=============
dk,1,ux,0,,,uy,uz
dk,2,uy,0,,,uz,ux
allsel,all
d,all,uz,0
/solu
allsel,all
nsubst,1000
nlgeom,on
time,1
cnvtol,m,-1
autots,on
acel,,9800
solve
/post1
set,last
/eshape,1
plnsol,u,y

The results:

图片[5]-Introduce to ANSYS  Cable280 –Get a Thorough Understanding of This Element-峰设教育

图片[6]-Introduce to ANSYS  Cable280 –Get a Thorough Understanding of This Element-峰设教育

Good Luck!

欢迎扫描如下二维码关注本站微信公众号:ANSYS结构院

有时间麻烦帮忙点击下公众号文末的广告哦, 权当码字的辛苦费,感谢大家!

Please Share Us
© 版权声明
THE END
喜欢就支持一下吧
点赞0赞赏 分享
评论 抢沙发
头像
欢迎您留下宝贵的见解!
提交
头像

昵称

取消
昵称表情代码

    暂无评论内容

YOU MAY LIKE…