I use plastic behaviour for a material in abaqus:
YS plastic strain
8MPa 0
8MPa 1
8MPa 100
And Abaqus seems to ignore the elastic limit, the von Mises stress happily rises above 8MPa. But it does not happen when the mesh is linear with ticked reduced integration. Why is this and how do I fix this bug?
Maciej Gierulski The issue you are facing is not a bug, but a known issue with ABAQUS. When you use a plastic material model with a linear mesh, ABAQUS will extrapolate the stress values from the integration points to the nodes. This extrapolation can sometimes lead to stress values that exceed the elastic limit. To fix this issue, you can use a quadratic mesh. Quadratic meshes are more accurate than linear meshes, and they are less likely to produce stress values that exceed the elastic limit. You can also use reduced integration elements. Reduced integration elements use a lower order integration rule, which reduces the accuracy of the stress calculations. However, this also reduces the likelihood of stress values exceeding the elastic limit.
In your case, since the issue does not happen when the mesh is linear with ticked reduced integration, it is likely that the problem is caused by the extrapolation of the stress values. You can try using a quadratic mesh or reduced integration elements to fix the issue.
Here are some additional tips for avoiding this issue:
- Use a fine mesh. A finer mesh will produce more accurate stress calculations, which will make it less likely that stress values will exceed the elastic limit.
- Use a material model with a smooth yield curve. A smooth yield curve will make it less likely that stress values will exceed the elastic limit in a localized region.
- Use a stabilization scheme. A stabilization scheme can help to prevent stress values from exceeding the elastic limit.
Finally, I'd like to ask, "Have you confirmed the consistency of your input unit system?"
I hope it helps ! To get further guidance, please reach out to me on WhatsApp at https://wa.me/+923440907874, as I don't frequently check my ResearchGate profile.
Engr. Tufail What I'm seeing is the exact opposite: linear mesh with reduced integration works fine, disabling reduced integration or switching to quadratic introduces the problem. I tried refining the mesh and the problem got worse, anyway my model is too large to refine it indefinitely. I'm not sure how to use smooth yield curve or a stabilisation scheme.
Maciej Gierulski Since the behavior you're describing is somewhat counterintuitive, it may require a more detailed examination of your specific model and setup to pinpoint the exact cause of the issue. If you're experiencing the opposite behavior where a linear mesh with reduced integration works fine while disabling reduced integration or switching to a quadratic mesh introduces the problem of stress values exceeding the elastic limit, that is indeed unexpected. Units you are using are not consistent or perhaps the mesh is not the representative of what you are expecting the output from. Regarding the smooth yield curve for a stabalisation scheme, creating a smooth yield curve for a material model in ABAQUS is crucial for accurate finite element simulations. It involves several key steps, starting with the selection of an appropriate material model that supports a smooth yield behavior. Defining the elastic properties, such as Young's Modulus and Poisson's ratio, sets the foundation for the material's behavior before plastic deformation occurs. The choice of a yield function, such as the von Mises or Tresca criterion, determines when plasticity initiates, and it should be continuous to avoid abrupt transitions. Defining the yield stress and hardening behavior ensures that the material's response to stress remains smooth and realistic during plastic deformation. If you have experimental data, fitting it to the chosen material model helps create a curve that closely matches observed behavior (Abaqus offers this option). Here is an additional example of how to do it, " https://www.youtube.com/watch?v=AtXTdUJKq1U&ab_channel=NitikornResearchPartner ". Good luck!
Do not use nodal stress. Your finding has to be based on element stress which is nothing but gauss point stress and does not get extrapolated.
Venkateswarlu Gattineni indeed, when I use the probe tool set for elements i only get results within the yield limit. but why does abaqus display those wrong values on the visualisation for quadratic mesh or no reduced integration? and why does it display the right values for linear mesh with reduced integration?
Maciej Gierulski Linear elements with reduced integration use uniform distribution of stress components, therefore nodal values of Mises stress coincide with its correct value at integration point (centroid). Elements with full integration use element shape functions for extrapolation of stress components from integration points (wher Mises stresses are correct) to nodes, therefore nodal Mises values can somewhat exceed yield limit. That's the price for visualization.
- Badges
- Science topic
- Similar topics
- Physical Sciences
- Atomic, Molecular and Optical Physics
- Atoms