I recently wrote an article about how to accurately perform a cold drawing (necking) FE simulation of thermoplastics like polycarbonate. In that study I selected a material model and then used a FE solver to determine the force-displacement response of a specimen that undergoes necking. In this study I will try to do the opposite, I will find a FE material model from tension with necking data. Before I started this study I thought that if you extract the uniaxial tensile stress and strain history of an integration point inside the specimen as a function of time, then that data could be used to accurately calibrate a material model. It turns out that this is certainly not easy to do. This article explains the challenges.
Note: This article is part 2 in my series on how to use experimental uniaxial tension (cold drawing) data from specimens that undergo necking during the deformation. Here are the other articles:
Strategy - FE Material Model from Tension with Necking
I performed the following steps: (1) I selected a suitable material model for polycarbonate, (2) I performed an Abaqus FE simulation of a dogbone-shaped specimen; (3) I then tried to determine the material model using only the FE simulation results from the tension simulation. The cool thing here is that I already know what the correct material model is, so I can easily evaluate the accuracy of different material model calibration strategies. As an alternative, I could have used DIC data from a tension experiment, and tried to determine the stress-strain response from that. That, however, would have been less interesting since I would not know what the correct material model was. The goal of this study is to examine if it is easy to determine a FE material model from tension with necking.
Figure 1. Is it possible to extract the correct stress-strain response from the FE simulation of the dogbone-shape specimen?
Results - Element in the Center of the Specimen
The FE simulation used quadratic elements (C3D20) with 27 integration points (3x3x3). Figure 2 shows the vertical strain in one element in the center (element 250). It is interesting to see the large difference between the different integration points, even though this element is relatively small.
Figure 2. Vertical strain history in all integration points in element 250.
To make the graphs easier to interpret, I have in the following only focused on the integration point at the element centroid. Figure 3a shows that the strain history at the element centroid is not that smooth. Figure 3b shows the extracted true stress-strain response at the element centroid. This stress-strain curve looks quite different than the actual stress-strain curve that was used to run the FE simulation. The actual stress-strain response of the material is shown in Figure 1.
Figure 3. Stress vs time, and stress vs strain predictions at the element centroid for FE material model from tension with necking.
The stress-strain response that was extracted from the element centroid looks very strange, and quite different from the actual response of the material model. To investigate this in more detail, I plotted in Figure 4 the strain rate history of the integration point. In that figure I also plotted the true Poisson’s ratio as function of time. The true vertical strain is initially linear with the applied displacement. Then as the neck starts to form, the reaction force goes down, so the axial strain also goes down. The strain is then almost constant while the neck propagates. The extracted Poisson’s ratio increases rapidly as the neck gets close to element 250. This increase is caused by the pressure that is introduced in the specimen from the neck.
Figure 4. Strain rate and Poisson’s ratio as a function of time.
Another interesting observation is that the two transverse strains are NOT the same in the FE simulation. As is shown in Figure 5, one of the transverse strains is almost 2X larger than the other. This difference has nothing to do the with material model (which is isotropic), but is simply caused by the specimen aspect ratio and the confinement from the boundary conditions.
Figure 5. Comparison between the different strain components at the element centroid.
The stress components at the element centroid are shown in Figure 6. This figure shows that although the vertical stress (S22) is dominating, the two transverse stresses are also quite large as the neck propagates through the element.
Figure 6. Stress components as a function of time.
If I use the real material model to predict the stress response using the extracted vertical strain history in the center element, then I get the stress-strain curve that is shown in Figure 7. It is surprising to see how different the two curves are. If the stress state in the tension specimen was uniaxial, then the two curves would have been the same. The fact that they are so different indicates that the multiaxial nature of the stress state cannot be ignored. This makes it quite challenging to recover the original material model using only axial stress-strain data from one integration point!
Figure 7. Comparison between extracted and predicted stress-strain behavior.
If I extract the stress-strain response of 4 other elements I get the results shown in Figure 8. I find it super interesting to see just how different the stress-strain curves are at those different locations within the gauge section. This suggests to me that one cannot accurately calibrate the stress-strain response to experimental DIC or FE data of a specimen that undergoes necking. This is simply due to the complicated stress state, which is not as close to uniaxial tension as I would have guessed. Virtual investigations using FE simulations can be quite useful!
Figure 8. Extracted stress-strain response from 5 different elements.
- The stress and strain state in a tension specimen is uniaxial before the neck has started to form, and after the neck has extended all the way through the gauge section.
- For intermediate strains, after the neck has started to propagate, the stress and strain state in the specimen is multiaxial.
- It is not easy to accurately calibrate a FE material model from tension with necking data using single point data, simply because the history of the complete stress and strain tensors are not known.
- A different and more accurate approach to calibrate a material model is to perform an inverse FE calibration of the actual specimen deformation. I will cover that in a separate article.