During ANSYS limit load analysis, the Mises stress value exceeded the yield limit

Did the poster perform finite element analysis of the ring reinforcement structure using the limit method? My habit is to simply use thicker tubing for routine analysis. For those with reinforcement rings, conventional calculation methods can be used directly. If it exceeds the specifications, it is recommended to thicken the nozzle.

Is an ideal elastoplastic material being used?

It’s an old post from four years ago; I’ve been working on a similar issue recently, so I’m sharing my thoughts here for everyone’s discussion and reference. Criticism and suggestions are welcome. After setting the yield limit in ANSYS, theoretically, once the Mises stress at that point (ANSYS does not seem to support a third strength yield criterion) reaches the yield line, the local stress-strain relationship will change; the specific form of this change depends on the constitutive model used. I am using bilinear reinforcement with a tangent value set to 0; under such settings, no hardening occurs after the element yields – the stress no longer increases as strain increases, but remains constant at the yield level. During my own experiments, I also encountered situations where the Mises stress value was higher than the yield threshold, with a deviation of around 30%. This is because in finite element calculations, the numerical solutions at the integration points within the elements are calculated directly, and then these values are extended outward (analogous to interpolation) to obtain the node data. The stress values shown in the contour plot correspond exactly to those at the nodes, and errors in the extrapolation process may result in the stress at the nodes being higher than the stress values at the integration points on either side. In my opinion, the process of extrapolating integral points and the errors that arise from such extrapolation are inevitable. These errors can be reduced by refining the grid, thereby having more and closer local integral points of interest, which in turn reduces the extrapolation errors. In my own calculations, this method proved to be effective as well; even after refining the grid, the maximum stress still exceeded the yield limit, but the relative deviation was only around 1.5%.

If you manually add zones to the cloud icon scale and define a very narrow area near the yield line, it will be observed in the new cloud diagram that the stress areas above the yield line are primarily located in areas with poor grid quality or at the edges of the yield region; in such places, the stress variations are relatively large, resulting in greater errors in the extrapolation process. Ansys first calculates strain, and then stress. As can be seen after performing the above operations, the area where the stress reaches the yield value roughly coincides with the area where plastic strain occurs. This indicates that the stresses above the yield line shown in the stress map are due to calculation errors, and they have no effect on the deformation of the structure; after all, there is a sequence in which strain is calculated first and then stress. In other words, aside from the errors inherent in the simulation itself (caused by loads, boundary conditions, model simplifications, and the grid), although the stress values in some areas of the calculation results exceed the yield threshold, these local calculation errors do not affect the overall accuracy of the numerical simulation. The strain results of the structure under the calculated conditions are reliable.

Next is the issue of grid refinement. Due to the performance limitations of the office computer, I used the sub-model method during the refinement process; based on the results obtained from the master model, I continuously selected the specific local areas of the structure that were of interest for further calculation. Indeed, it was observed that the finer the sub-model grid, the smaller the relative deviation between the maximum stress and the yield line. However, with the sub-model method, it is also necessary to avoid stress concentration areas, in order to ensure that the data used as the boundary conditions for the sub-model are as accurate as possible. Therefore, the sub-models should not be too small. Furthermore, based on the relationship between strain and stress as shown above, it can be concluded that in practical calculations there is no need to refine the grid to the extent where the maximum stress exactly equals the yield limit; being relatively close to this value is sufficient to obtain sufficiently accurate strain and stress results. After all, errors are bound to exist in the simulation process; the choice of submodels and the level of grid refinement depend on your tolerance for such errors.

I forgot to mention earlier that by comparing the stress and plastic strain maps, it can be seen that in areas where the maximum stress far exceeds the yield threshold, there is likely no plastic deformation. In my understanding, when ANSYS determines values such as yield strength, it is likely to use the values at the integration points, while the values displayed in the cloud diagram are those at the nodes. Therefore, stress cloud maps are error-prone, but strain cloud maps should be relatively accurate; this is not contradictory. All of the above-mentioned topics, including the extrapolation error of integration points, the sub-model method, the setting of yield limits, and so on, can be easily found. If there are any mistakes, please feel free to point them out.

This post was last edited by Ou Lan on 2020-12-14 at 18:04. The internal pressure structure of the cylinder is simple, with a regular grid; the stress and strain distribution is quite ideal, so it’s unlikely that any of the problems I mentioned earlier will occur. If you try simple stretching, you will find that the yield of the specimen also matches the ideal scenario quite well.