

February 15, 2023 at 1:02 pmDario DenzlerSubscriber
Hello,
I am facing some trouble with result evaluation in areas (corner of pressfit) that show clear singularity effects. Decreasing mesh size leads to increased stress focused on just one node if looking at nodal stresses (average). Now the question is, if it is good practice to evaluate stresses by looking at elemental stress instead of nodal results?
As I would like to automate the postprocessing, I would like to extract the max/min values but in case of a stress concentration/singularity, I am forced to check the model manually. Using elemental results would probably help as it kind of average out the peaks. But is still a feasible approach?
Generally, we are looking at max./min. principal stress due to the material behaviour and not equivalents if that is of any importance.
Mesh size (0.0075 mm)
Nodal results (averaged)
Nodal results (unaveraged)
Elemental results

February 15, 2023 at 4:35 pmErik KostsonAnsys Employee
Hi
Perhaps this is of some help.
All the best
Erik

February 17, 2023 at 6:41 amDario DenzlerSubscriber
Thanks for sharing. Unfortunetly, the recommended radius is already included in my model and I also tweaked contact definition (such as penetration tolerance and contact stiffness) to “relax” the contact. However, I still see stress concentrations and wonder if taking element results is a valid way. Evaluating results away from the stress singularity is kind of hard to judge how far we away can go as the stress gradient is quite high and I do not want to miss actual material limits.

February 17, 2023 at 3:54 pmClaudio PedrazziSubscriber
my two cents: in my opinion even looking at the stresses in the elements you can't avoid stress concentrations. If you shrink the mesh even the stresses in the elements (which, by the way, are the ones that are calculated first, at the Gauss points, from the nodal deformations, which are the real "solution" of the FEM system of equation: then they are extrapolated to the nodes), they too will grow indefinitely.
If the real stress state at that location is important to you (i.e., you can't do your maximization excluding that location), I personally see no alternative but to use a material model that is a little more realistic than linear: at a minimum, bilinear. That way the peaks will eliminate themselves, as they do in physical reality, generating microzones of plasticity.

February 20, 2023 at 6:49 amDario DenzlerSubscriber
Thanks for your reply. Make sense that with indefinitely small element, also my element stress will diverge. However, I have done many different simulations of press fits and it seems like we get "smoother" results if we look at elemental stress which makes it possilbe to kind of automate postprocessing. And if I get you right, elemental stresses are somewhat closer to reality as they are calculated directly from Gauss points.
For the nonlinear material, I will have a look at.

February 20, 2023 at 7:25 amClaudio PedrazziSubscriber
>>And if I get you right, elemental stresses are somewhat closer to reality as they are calculated directly from Gauss points.
I simply say that they are a more "basic" result of FEM. I try to formulate better:
In my understanding (but some ANSYS people could confirm this) the sequence of computation for a standard linear FEM based on K*u = F system of equation, where K= stiffness matrix, u=unknown nodal displacements, F= "forces", is the following:
1. First solve for u (nodal "displacements"). These are the real "unknowns" in the FEMmethod.
2. based on each element formulation, find the stress in the Gauss (integration) points in the elements. They are univoque (unique, unanbiguous).
3. optionally extrapolate the stress to the nodes (see ERESX). Since generally one node can belong to more than one element, they are not univoque, i.e. there is one stress for a given node for each element connected to it. Hence the optional extrapolation, the averaging and so on.

 You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 Saving & sharing of Working project files in .wbpz format
 Solver Pivot Warning in Beam Element Model
 Understanding Force Convergence Solution Output
 An Unknown error occurred during solution. Check the Solver Output…..
 What is the difference between bonded contact region and fixed joint
 whether have the difference between using contact and target bodies
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 User manual
 Colors and Mesh Display
 material damping and modal analysis

3778

2575

1825

1242

598
© 2023 Copyright ANSYS, Inc. All rights reserved.