How to Use INISTATE Command In ANSYS Workbench

How to Use INISTATE Command In ANSYS Workbench

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

In engineering structures, pre-stress must often be considered, especially in civil engineering, such as in bridge,  shell structures,  initial stress analysis of soil and rock. In this article, we will briefly introduce how to use the INISTATE command in Workbench.

In the ANSYS Help, the usage of this command is as follows:

INISTATE, Action, Val1, Val2, Val3, Val4, Val5, Val6, Val7, Val8, Val9

Firstly, Action specifies the type of INISTATE operation, which is mainly divided into six types: Set, Define, Write, Read, List, and Delete. Each type represents a different pre-stress input parameter, defining pre-stress, writing out initial stress, reading initial stress, listing stress, or deleting pre-stress.

For example, when specified as Set, the specific parameter values that follow are the parameters for pre-stress input. As shown in the Help, there are mainly two parameters, one specifies the coordinate system for pre-stress input, and the other is the type of pre-stress input, whether it is stress, strain, or plastic strain.

图片[1]-How to Use INISTATE Command In ANSYS Workbench-峰设教育

When specified as Define, the data inputted through INISTATE is the specific stress or strain data. ID represents the element number, EINT, K LAYER, PARMINT represent the Gauss integration point, layer number, and layer integration point, and the subsequent CXX~CXZ represent the specific pre-stress value. Usually, it is unnecessary to specify EINT, KLAYER, and PARMINT for further operation.

图片[2]-How to Use INISTATE Command In ANSYS Workbench-峰设教育

When specified as Write and Read, they respectively represent writing out pre-stress and reading stress operations. It is generally used more in the initial ground stress analysis of soil and rock. The usage is simple, and you can follow the Help prompt to operate. Please note that the file extension for initial ground stress written out is an “ist” file.

A typical “ist” file format is shown below, which includes unit number, integration point, layer number, and six-directional stress information.

图片[3]-How to Use INISTATE Command In ANSYS Workbench-峰设教育

Below are the command flow demonstrations for defining pre-stress for a single element and reading and writing initial ground stress for a batch of elements:

1. Defining pre-stress for a single element

!Define initial stress applied along the element coordinate system

Inistate, Set, -2, Stre

!Apply a pre-stress of size 20 in the X direction to element 2.

Inistate, Define, 2, , , , 20

2. Reading and writing initial ground stress for a batch of elements

Allsel, all

!Write stress data for all units

Inistate, Write, 1, , , , 0, S

!Read the initial stress data with the file name “file0”

Inistate, Read, file0

In Workbench, a good habit before applying initial stress through the INISTATE command is to first establish Named Selection for the elements to be pre-stressed, and then select the elements directly through the selection group when inserting the command later to prevent problems caused by changes in node numbering due to changes in the mesh.

Here is an example to illustrate the usage method:

For a two-dimensional structure similar to a canopy, the lower beam is a steel tube with a diameter of 180 and a thickness of 10, and the upper cable has a diameter of 20. The left side is fixed, and the materials are all steel.  To analyze the structural response, we will apply an initial axial stress of 50 MPa to the cables, using rod elements, and beam elements for the beams.

图片[4]-How to Use INISTATE Command In ANSYS Workbench-峰设教育

Before we start, it is important to note that when creating a named selection for the cables, it should be done for the element group rather than the geometric group. This is because the subsequent application of the initial stress will be done on the individual elements.

图片[5]-How to Use INISTATE Command In ANSYS Workbench-峰设教育

To apply the initial stress using the INISTATE command, follow the steps below:

1.Insert the command snippet as shown below:

图片[6]-How to Use INISTATE Command In ANSYS Workbench-峰设教育

2. To verify if the initial stress has been applied, constrain all the nodes of the structure, and then draw the axial stress cloud diagram. Check if it matches the initial stress applied. To do this, insert a beam tool in the results view and draw the direct stress diagram. If the result matches the initial stress, it means that the stress has been applied correctly.

图片[7]-How to Use INISTATE Command In ANSYS Workbench-峰设教育

图片[8]-How to Use INISTATE Command In ANSYS Workbench-峰设教育

Alternatively, you can use a method where the initial stress is applied by reading in a file. This method is useful when dealing with large-scale initial stress applications. To do this, follow these steps:

1. Write the data file in the standard format, as shown below:

图片[9]-How to Use INISTATE Command In ANSYS Workbench-峰设教育

2. In ANSYS Workbench, insert the following command snippet, where the INISTATE command uses the read operation and is followed by the path to the file:

图片[9]-How to Use INISTATE Command In ANSYS Workbench-峰设教育

Note that /dtype and /csys respectively represent the type and coordinate system. Here, we are applying an initial stress using the element coordinate system, and the stress value is SX=50, which means an axial stress of 50.

图片[11]-How to Use INISTATE Command In ANSYS Workbench-峰设教育

In conclusion, the Define operation type is suitable for small-scale initial stress applications, while the Read operation type is suitable for large-scale applications. You can choose the method that is best suited for your engineering project’s complexity.

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…