How to Customize or Create Beam Sections in Ansys Workbench

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

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:

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.

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

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

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.

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

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.

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.

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

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.

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.

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.

Good Luck!

欢迎搜索关注本站微信公众号：ANSYS结构院

欢迎给网站捐助，您的捐助是我坚持下去的动力！