How to Customize or Create  Beam Sections in Ansys Workbench

How to Customize or Create Beam Sections in Ansys Workbench

Please Share Us

点击此处查看 ✿水哥原创ANSYS视频教程清单 ✿

When conducting structural analysis using beam elements in ANSYS Workbench, the software provides us with commonly used cross-sectional types, and users only need to input corresponding parameters based on the cross-sectional form. However, for structures with non-standard cross-sections, users need to define their own cross-sectional types.

In ANSYS APDL, if users need to define their own cross-sections, the typical process is to first create a plane based on the cross-sectional dimensions, then use a plane element, usually Plane82, to mesh it, and finally use the secwrite command to write out the cross-section file for later use. Then, a new model is created, and the beam element geometry model is built. The cross-sectional file written earlier is loaded using the secread command.

As seen above, defining custom cross-sections with APDL is slightly more complicated, but the benefit is that users can freely control the cross-sectional form and mesh division, and the definition of variable cross-sections is also relatively free.

So, can custom cross-sections be defined in Workbench?

This article will use the example of a cable-stayed bridge to demonstrate the steps:

The cross-sectional dimensions of the main beam are shown below:

图片[1]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

图片[2]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

The steps are as follows:

1. First, draw the cross-sectional shape in AutoCAD based on the dimension diagram, and align the center line of the cross-sectional vertices with the original coordinates.

图片[3]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

Open Workbench, create a new project, and open SpaceClaim. Import the cable-stayed bridge wireframe model.

图片[4]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

3. Create a new SC file and import the main beam CAD cross-section as shown below.

图片[5]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

4. Use the fill command to fill the main beam and stretch it appropriately. Because SC reads in the cross-section by recognizing faces of different colors, stretching is necessary.

图片[6]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

5. Select the end face, choose Face in the display menu, and specify a different color.

图片[7]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

6. Click on Design, select Create New Coordinate System, locate it at the midpoint of the cross-sectional top plate, and save it to the software working directory as Beamsection.scdoc. Note that it must be saved in SCDM format, otherwise it cannot be read.

图片[8]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

 

7. Open the cable-stayed bridge main file, click on Prepare, under the beam category, scroll down to Profiles, select More Profiles, choose the SC file Beamsection saved earlier, and read in the cross-sectional file.

图片[9]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

图片[10]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

8. After a successful read-in, the approximate cross-sectional form will be displayed under the beam project type.

图片[11]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

9. If you did not follow the previous steps, you may encounter two types of errors below. It means that you need to create a local coordinate system and a single colored face for the cross-section.

Profile must have a coordinate system.

Profiles must have a single colored face.

10. Select the main beam’s straight line, then choose the cross-section for cross-sectional assignment, and click on Display – Solid Beams under the beam element project.

图片[12]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

11. During the assignment process, if the cross-section position does not match the actual position, the main reason is the influence of the straight line direction. Select the non-matching straight line, and rotate the cross-section in the properties until it matches the actual situation. For example, select the left straight line here, and change the orientation in Properties to 180 degrees, and so on.

图片[13]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

图片[14]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

12. After the assignment of the main beam is completed, assign the cross-sections to other components, then open Mechanical, and now you can happily perform meshing and loading operations.

图片[15]-How to Customize or Create  Beam Sections in Ansys Workbench-峰设教育

Good Luck!

更多即时资讯,欢迎扫描如下二维码关注本站微信公众号:ANSYS结构院

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…