Introduction
I recently calibrated a material model for an engineer at a well-known company. She needed a material model that can predict both the stress-strain response, and the residual strain after unloading. As I typically recommend, all experimental tests in this case were performed in uniaxial tension. The calibration went well and the model matched all data (including the residual strain) with high accuracy. To validate the material model it was then used to predict the response in a bending experiment that focused on the residual deformations. The validation results did not look very impressive. In this article I will try to explain why one needs to be particularly careful when predicting the residual deformations in bending.
Material Model
In this example I will use an Abaqus Parallel Rheological Framework (PRF) model consisting of 2 Yeoh hyperelastic networks, Bergstrom-Boyce flow, and isotropic hardening plasticity. I have no particular reason to use this model except that it is easy to use. There are many other viscoplastic material models that would give the same type of results. The following figures show the time-stress-strain response for a virtual load case in which the material is pulled in tension to an engineering strain of 10%, then unloaded to zero stress, and then held at zero stress for 1 hour.
FEA Model 1: Coarse Mesh
The left side of the validation part was held fixed, and a downward shear traction (force) was applied on the (right) tip surface of the part. The tip force magnitude was ramped up in 4 seconds, then gradually removed in another 4 seconds, the part was then left without any external loads for 1 hour. This FE model used 632 linear reduced integration hexahedral elements (Abaqus C3D8R).
The following figure show the max principal residual strain, and the vertical displacement of the tip of the part as a function of time.
FEA Model 2: Fine Mesh
I then created a second version of the model consisting of a finer mesh: 59,000 linear full integration hexahedral elements. All other settings were the same. The following image shows the predicted max principal strain after the final 1 hour hold time.
FEA Model 3: Fine Mesh (Quadratic Elements)
A third and final validation case was created using 15,520 full integration quadratic hexahedral elements (Abaqus C3D20). All other settings were the same. The following image shows the predicted max principal strain after the final 1 hour hold time.
Summary
The results from the three models give very different max principal strain values. The coarsest mesh gave a max principal strain of 0.45%, and the most refined mesh predicted 1.79%. That is 4X higher! Another way to compare the different models is consider the residual deformation the tip of the bar that bends. The following figure shows that the max displacement is not that different between the 3 models. The coarsest model only has a max error of about 14%. The final residual deformation is a very different story. The model with the coarse mesh predicts a final displacement that is 2.5X too small. That is a 60% error!
The lesson here is that it is very important to use a very refined mesh if you hope to accurately predict the residual strains or displacements in bending.
2 thoughts on “Why FEA Underpredicts Residual Strain in Bending”
Hei Jörgen,
Thanks for a nice blog (as usual 😉
But I’m a bit surprised why you are “surprised” that you need a finer mesh for this example. It is rather well known that for such bending cases — as FEM solves for displacements, but strain and stress are related to the first spatial derivative of displacement, hence you are taking the difference of very small numbers, and with our FPU limited precision — we get large errors quickly, if the mesh is not fine enough in these critical regions.
Furthermore, it’s clear that one does not need the fine mesh everywhere, it’s really very local to the bending region, and one could even get around with 3 elements in the beam width/depth direction. But then these comments are really usual 3D structural FEM calculation issues, and should be known by most FEM specialists, probably less by newcomers 🙂
Sincerely,
Ivar
Hello Ivar,
Good points! This article was motivated by a request from a FE manager at a large company. I know, of course, that determining the max stress / strain in bending requires quite a fine mesh since the max values occur at the surface, and most traditional elements do not have integration points at the surface of an element. From my perspective, the main reason for the article was to remind engineers that a fine mesh is needed also when predicting residual strain in bending (not just when determining the stresses & strains). Your point, however, is that a fine mesh is ALWAYS needed. It is hard to argue with that.
/Jorgen