 # Why ANSYS Maximum Equivalent Stress (Von-Mises) is Higher Than the Material Ultimate Strength

Many people who conduct nonlinear material analysis encounter a problem: when examining the final structure stress, they often find that the von Mises stress is greater than the material’s yield strength. In this article, we will discuss the reasons for this phenomenon and how to avoid it.

Before we dive into the specifics, let’s first discuss the concept of integration points.

As we all know, the finite element method involves solving a matrix equation: [K]x[U]=[F].

[K] represents the stiffness matrix, [F] represents the load matrix. For simple situations, we can easily assemble them, such as using the matrix displacement method in structural mechanics. However, for complex models, when calculating the stiffness matrix and load matrix of isoparametric elements, we need to use integration in the following form: Here, the function being integrated is too complex to obtain its explicit expression, and even if we could, the integration would still be very complicated. Additionally, general computer resources are not enough to support such a large amount of calculations. In order to solve this integration more effectively, numerical integration is typically used to replace function integration.

Numerical integration means selecting integration points within the integration domain according to certain rules, calculating the numerical value of the integrated function at the integration points, multiplying by the corresponding weighting coefficients, and summing them to obtain the integral value of the function. For example, the formula for one-dimensional numerical integration is: There are many numerical integration methods, with common algorithms including Gaussian integration and Simpson’s rule. Gaussian integration is more commonly used, mainly because it can achieve higher accuracy with the same number of integration points. When using Gaussian integration, the integration points are called Gaussian integration points.

It’s important to note the difference between element nodes and integration points. They are two different concepts. Element nodes are points defined when we define the element and actually exist. They are mainly used to construct element shape functions. Integration points, on the other hand, are introduced for the purpose of using numerical integration methods. They take on different forms depending on the numerical integration method used. For example, when using Gaussian integration, the integration points are different from the node positions, but when using Newton-Cotes method, the nodes are the element nodes, and the two positions coincide.

Now that we understand what integration points are, let’s take a look at the finite element calculation process.

When solving the equation 【K】x【U】=【F】 to obtain node displacement solutions, finite element analysis yields the most fundamental and precise solution. Once the node displacement solution is obtained, the next step is to solve for strain and stress, which are not directly obtained at the nodes but rather at the integration points.

ANSYS software mainly uses Gaussian integration to calculate strain and stress, and the following process exemplifies how the software computes them:

• Compute strain at the integration point by using the equation 【e】=【B】【U】.
• Use Hooke’s law and geometric equations to derive the stress at the integration point: 【v】=【D】【B】【U】.

Therefore, the integration point value is the most precise in calculating stress and strain. By using the specific element shape function and the stress and strain values at the Gaussian points, these values are extrapolated to the nodes of the element to obtain the stress and strain values at the nodes.

For elements with common nodes, the extrapolated stress and strain values at the common nodes from the integration points of different elements are generally not the same. Therefore, an averaging process is usually performed to represent the stress and strain values of that node. During this process, since extrapolation is used, it is inevitable that there will be instances where the node stress values exceed the material yield stress, which is a common situation.

How can we change this situation? The software provides an option to turn off the extrapolation of integration points. In the solution module, click the following path and the corresponding dialog box will appear. By default, the software extrapolates the stress and strain values, but we can choose “No – Copy them,” which means that the node stress and strain values will be copied from the integration points without extrapolation. Then, the node cloud map we create will be based on the integration point cloud map, which is the most accurate. Of course, in this case, there will be no instance where the calculated stress exceeds the material yield stress. The relevant command and help are as follows: Below is an example of calculating a perforated plate. The plate is made of Q235B material and uses the ideal elastic-plastic BKIN bilinear model. The left side is fixed and the right side is subjected to a uniformly distributed line load that is large enough to make the plate yield. When the extrapolation of integration points is not turned off, the node stress cloud map is as follows:

``````Mp,ex,1,3.0e4

Mp,prxy,1,0.2

Mp,dens,1,2500e-12

tb,bkin,1

tbdata,1,235`````` As shown in the input for the structural material, the yield strength of the material is 235 MPa. From the cloud map, the maximum von Mises stress is 236.553 MPa, which exceeds the yield strength of the material. This is the result of the extrapolation of integration point stress. Next, we turn off the extrapolation of integration points and copy the stress of the integration points. We add the following command during the solution phase:

``````/solu
Allsel,all
time,1
nsubst,1000
eresx,no
Solve`````` From the cloud map, the maximum stress value is now 234.983 MPa, which is very close to the yield strength of the material set at 235 MPa. The value is the result of copying the integration point.

Good Luck!   