Close this search box.

Material Model from Tension Force History


This article is part 3 in my series on how to use experimental uniaxial tension (cold drawing) data from specimens that undergo necking during the deformation. In the first article in the series I covered how you can use a material model to predict the force-displacement response, the onset of necking, and the natural draw ratio. In the second article I discussed why it is really difficult to extract (or calibrate) a material model from stress-strain data extracted from a single point in a tension specimen. In this article I will explain a better way to select and calibrate a material model from tension force data of a specimen that under goes necking. My study in this article is using Abaqus as the FE solver. Read on to learn how to convert force history to a material model!

Here are the other articles in this series:

Step 1: Create a FE Model of the Tension Test

Create a complete Abaqus FE model of the tension test. In this example I used a coarse mesh of C3D20 elements. Make sure that the material model is selected as linear elastic. The actual values of the elastic constants do not matter as this will be automatically replaced by MCalibration. Also make sure that you specify one history output for the reaction force and displacement to the top surface of the specimen. Also, make the bottom surface of the specimen fixed. Finally, make sure the simulated specimen is deformed with the same displacement history as your real experimental test. Here is the Abaqus step definition in my example.

					*Step, name=loadIt, nlgeom=YES, inc=999
0.01, 100., 1e-05, 1.5
*Controls, parameters=time incrementation
8, 16, 9, 50, 40, 30
*Boundary, 1, 1, 2, 2, 20., 3, 3
*Restart, write, frequency=0
*Output, field
*Node Output
*Element Output, directions=YES
*Output, history
*Node Output,
RF2, U2
*End Step
Mesh for material model from tension force history

Figure 1. FE mesh.

Step 2: Set Up the MCalibration Load Cases

I will use MCalibration to find a material model that matches the experimentally determined force-displacement results. I will specifically use a “Abaqus External Solver” load case, as shown in the figure below. Select the Load Experimental File button and select the experimental file containing time, displacement, and force columns. Then click on the Select Abaqus inp-file button and select the inp-file that was created in Step 1. Finally, select how many CPUs you want MCalibration should instruct Abaqus to use, the name of the linear elastic material model to replace, and the direction of the force and displacement.

MCalibration load case material model from tension force

Figure 2. MCalibration load case setup.

You should also set up any other load cases that you want to include in the material model calibration. In my example I added one Poisson’s ratio load case so I can have MCalibration find the bulk modulus of the material model.

Step 3: Select the Material Model in MCalibration

Just like in Part 2 of this study, I generated the “experimental data” using a FE simulation of the test specimen with a PolyUMod TNV material model that was calibrated to data for a polycarbonate. See the figure below. The goal in this study is really to see if I recover the real material model using the force-displacement data.

Figure 3. Material model selection.

To perform this study I selected the same TNV model structure, but I manually selected a starting point for the material parameter search based on a completely different set of parameters. I specifically used material parameters for UHMWPE, a material that does not undergo necking in uniaxial tension. Figure 4 shows the predictions from the initial guess of the material parameters.

Figure 4. Starting point for the material model calibration.

Step 4: Run the Material Parameter Optimization

To run the material model calibration just click Run Calibration in the toolbar. I manually stopped the calibration after MCalibration had tried 177 different material parameter combination. The results are shown in Figure 5, illustrating that the material model captures the “experimentally” observed force-displacement response accurately.

Figure 5. Screenshot of MCalibration after the calibration had been stopped.

Since I generated the “experimental” force-displacement data using a finite element simulation with a known material model, I can in this case also compare the predictions of the inversely calibrated material model to predictions from the real material model. Figure 7 shows that the material model that I generated in this article is in good agreemenbet with the original (real) experimental data for polycarbonate that I used to generated the force-displacement results form.

This shows that an inverse calibration approach using FE simulations can be used to accurately determine a material model for a material that undergoes significant necking!

Figure 6. Comparison between the real experimental data and predictions from the inversely calibrated material model.


More to explore

Leave a Comment