ANSYS Mechanical APDL Substructure Analysis Tutorial Step By Step

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

The substructure analysis technique in ANSYS involves creating a super-element for the localized area of interest and combining it with non-super elements to form a complete model for computation. After solving the complete model, the results on the interface between super and non-super elements are mapped to a single super-element, simplifying the calculation process and keeping errors within a controllable range.

Generally, the steps for substructure analysis are as follows:

1. Super-element generation

This involves defining the super-element by partitioning the area of interest and connecting it to external non-super elements through primary degrees of freedom. The main challenge in defining the super-element is ensuring that the nodes in the super and non-super elements are coincident. This can be achieved in two ways: using the same node numbering system or coupling nodes. The latter method is recommended.

2. Super-element usage

After defining the super-element, the external non-super elements are connected, and the complete model is solved.

3. Super-element expansion

After solving the complete model, the results on the interface between super and non-super elements are mapped to a single super-element, which is used to calculate the results for the area of interest.

For example, let’s consider a steel plate measuring 500mm in length, 200mm in width, and 10mm in thickness, with a 10mm diameter hole in the middle. The left side of the plate is fixed, and the right side is subjected to a uniform tensile load of 10KN/m. We can use substructure analysis to determine the stress distribution in the plate at the location of the hole.

If we are only interested in the total horizontal displacement of the plate due to the uniform load on the right side, we can use a coarser mesh around the hole to save computational resources. However, if we are interested in the stress distribution around the hole, we need to use a finer mesh. For complex models, over-meshing the area around the hole can result in an uncoordinated mesh with the rest of the model and can consume a large amount of computational resources.

In this example, we are interested in the stress concentration around the hole. Thus, we can aggregate the elements within a 100mm radius of the hole into a super-element for analysis.

Step1:Creating a Super Element

We’ll name the file S_1 and use shell181 elements to simulate the physical model of a plate with a 100mm hole in the middle.

First, create the physical model of the plate with the hole.

Then, perform local mesh refinement to divide the mesh into smaller sections. Note that to ensure the main degrees of freedom of the super element overlap with the external nodes, we need to specify the number of partition sections on both sides of the straight lines for later coupling.

Enter the solution module, define the analysis type as substructure, select the two side nodes as the main nodes, choose all degrees of freedom for constraint, solve, and save as S_1.db.

Step2 :Using the Super Element

After creating the super element, we’ll create other non-super elements and then assemble and solve them.

1. Create a new file named S_2 and create the geometry models on both sides.

2. Specify the number of partition sections along the boundary line that overlaps with the super element, and divide the mesh.

3. Add a new element type: matrix50, which is a special element for super elements.

4. Load the super element. Once loaded successfully, the super element will be displayed as an outline.

5. Couple the main degrees of freedom of the super element with the external node connection points of the non-super element. The overall model is now assembled.

6. Apply constraints to the entire model, load and solve.

7. Check the results of the non-super element calculations.

Structural von Mises stress distribution map

Structural displacement map in the X direction

Step3: Expanding the Super Element and Checking Internal Cohesive Element Results

1. Create a new file named S_1 and resume the previous work.

2. Enter the solution module, turn on Expass.

3. Write the file name of the super element and the main structure in the designated path.

4. Solve the mapping results.

5. Check the results of the internal cohesive element of the super element:

Super element displacement map in the X direction

Super element von Mises stress distribution map

Finally, here are the overall calculation results using the same mesh

X-direction stress distribution map

Overall von Mises stress distribution map

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！