In a structural finite element model, why doesn’t the calculated maximum stress always converge with mesh refinement? Is it caused by a stress singularity? If so, how do I minimize the singularity effect?


April 13, 2023 at 7:33 amSolutionParticipant
All finite element (FE) models are simplifications of the actual geometry and loading. Common simplifications are: •linearelastic material model, •point loads/restraints applied at a single node, •sharp corners in the CAD model – no fillet. These simplifications are valid modeling techniques used to create practical FE models, but they can cause mathematical singularities, which produce artificially high local stresses. The calculated FE singularity stress will not converge to a specific value, because the theoretical singularity stress limit is infinity. Increasing the mesh refinement will increase the singularity stress. A stress singularity does not necessarily indicate an invalid FE model. Singularities are local affects. Even though the calculated singularity stress does not reflect the actual stress, the displacements should be correct, and the nearby stresses should be correct. Refining the FE model to remove all singularities may not be practical or even possible. It is often more practical to leave singularities in the FE model and then use engineering judgement to assess their effect on structural integrity. Techniques that commonly used to assess the effect of a stress singularity are: 1.Ignore linearelastically calculated FE stress at a singularity and base engineering decisions on calculated nearby stress. The singularity stress is not real. It is a numerical artifact. The calculated stress in nearby elements is more representative of the actual stress. The nearby stresses should converge to specific values with increased mesh refinement. Engineers can often make sound design decisions using the more realistic nearby stresses. To visualize the nearby stress without including the effect of the stress singularity, you can plot results using a Named Selection/Component that contains the nodes/elements surrounding the singularity but does not contain the nodes/elements at the singularity. 2.Remove (or reduce) the model feature causing the stress singularity. For example, if the CAD model includes a sharp corner, you can revise the CAD model to include a radius and then use a fine mesh to capture the true local geometry. This approach requires revising the CAD model and using a refined mesh to capture the curvature. Thus, it will require extra modelling effort and will be computationally more expensive. This approach can produce mathematically more precise FE results, but it is often unfeasible for large models with multiple discontinuities. a.a variation of this approach is to use a submodel to create a refined mesh near the singularity that more accurately represents the local geometry. Using a submodel requires additional effort, but it should not significantly increase the computational expense, because the submodel mesh should be small. 3.Numerically evaluate the stress distribution to estimate a more accurate stress at the singularity. One technique is to “linearize” the stress distribution along paths through the thickness and then apply a theoretical stress concentration factor (SCF) to the linearized stresses to predict the total stress. SCFs for various geometries are available in engineering reference manuals (e.g., “Peterson’s Stress Concentration Factors”). Stress linearization is a numerical technique that decomposes the stress field into membrane, bending, and peak stress components. Commercial design codes such as the ASME Boiler and Pressure Vessel Code use it to establish design limits. It integrates the stress along the path to obtain the net membrane force and moment, and in turn the membrane (P/A) and bending (Mc/I) stress on that path. The peak stress is the difference between the linearized membrane plus bending stress and the total calculated stress. Stress linearization removes a local stress concentration effect from the calculated stress in a model without singularities. It will not remove a singularity stress, but a singularity will not affect the linearized stresses as much as it affects the calculated nodal stress because the singularity acts over a small area. Unlike the nodal singularity stress, the linearized stresses will tend to converge with mesh refinement. Linearization requires more postprocessing to define paths, calculate the linearized stresses, and adjust the linearized stresses for a theoretical SCF (plus the contour plots do not capture the predicted total stress); but it does not require modifying the CAD model or using a more refined mesh. 4.Use a nonlinear FE model with an elastic, nearlyperfectly plastic material model to limit the singularity effect. With an elastic, nearlyperfectly plastic material model, elements with a calculated stress above the yield stress cannot carry any additional load. The singularity elements will experience permanent plastic strain, but the effect is local. If a singularity causes a high local stress, the developed plastic zone will be small. The surrounding elastic material will contain the plastic zone growth. Additional load will increase the nearby elastic stress, but it will not significantly increase the plastic zone size. This approach requires a computationally more expensive, nonlinear FE, but it does not require modifying the CAD model or the mesh. Even if the FE model includes a radius and a refined mesh, there might still be a singularity effect if the radius is small. Also, if the actual radius is small, the component might experience true local yielding. Typically, local yielding caused by a discontinuity stabilizes after several loading cycles and does not affect the structural integrity (unless the component is subject to cyclic service). A nonlinear analysis can help quantify the magnitude of any local yielding. If you know the actual postyield material behavior, you can use it to create a more precise material model. However, using an elastic, nearlyperfectly plastic material model is common, because it is simple to define (e.g., setting the tangent modulus to be 1/100 of the elastic modulus might be sufficient) and it is conservative because it ignores strain hardening. Do not use an elasticperfectly plastic material model (tangent modulus = 0), because it can be numerically unstable. You may need to adjust the assumed tangent modulus value to develop a representative, numerically stable model. This KM does not detail all techniques used to assess stress singularity affects. It just identifies four commonly used techniques. The “best” approach to assess a singularity is model dependent. You must evaluate the FE model (e.g., number of singularities, complexity of CAD model/FE mesh, magnitude of nearby stresses, mission critical nature of the affected region, and cyclic service requirement) and apply the most appropriate approaches.
Attachments:
1. KM_2067559.pdf

Introducing Ansys Electronics Desktop on Ansys Cloud
The Watch & Learn video article provides an overview of cloud computing from Electronics Desktop and details the product licenses and subscriptions to ANSYS Cloud Service that are...
How to Create a Reflector for a Center HighMounted Stop Lamp (CHMSL)
This video article demonstrates how to create a reflector for a center highmounted stop lamp. Optical Part design in Ansys SPEOS enables the design and validation of multiple...
Introducing the GEKO Turbulence Model in Ansys Fluent
The GEKO (GEneralized KOmega) turbulence model offers a flexible, robust, generalpurpose approach to RANS turbulence modeling. Introducing 2 videos: Part 1 provides background information on the model and a...
Postprocessing on Ansys EnSight
This video demonstrates exporting data from Fluent in EnSight Case Gold format, and it reviews the basic postprocessing capabilities of EnSight.
 What is the difference between secant and instantaneous coefficients of thermal expansion (CTE)?
 Does ECAD trace mapping support more than one type of trace material (usually copper) in the same layer?
 How to use the NewtonRaphson residuals option under Solution Information?
 How can I understand Beam Probe results?
 ANSYS Mechanical: Fatigue Crack Growth Analysis using SMART Crack Growth
 How to find total heat flowing through a surface in Mechanical?
 How to define frictional coefficient as a function of relative sliding velocity
 Difference Between Environment Temperature and Reference Temperature in Mechanical
 How to plot stresses of a beam connection in Workbench?
 How to reduce contact penetration?
© 2024 Copyright ANSYS, Inc. All rights reserved.