Search

# How to Calibrate a Temperature-Dependent Ansys Hyperelastic Model

## Introduction

It is easy to calibrate an Ansys Hyperelastic model to experimental data at one temperature. In this article I will show how super easy it is to calibrate a temperature-dependent Ansys hyperelastic model

For more information about the temperature-dependent response of rubbers see my article “Why Does Rubber Have Odd Temperature Dependence?“.

## Experimental Data for an Unfilled Silicone Rubber

The following image shows experimental uniaxial tension data that I have for an unfilled silicone rubber. The tests were performed at 3 different temperatures: 20°C, 60°C, and 150°C. For this material the deformation resistance is due to entropy changes, so the stiffness increases with temperature. In fact, if you were to analyze the data in more detail you would find that for this material the stress is almost linearly dependent on the absolute temperature in Kelvin. We will not use that information in this example.

## Step 1: Calibrate a Hyperelastic Material Model to Each Temperature

Since the experimental stress-strain response is almost linear we can use a basic hyperelastic model, such as the Arruda-Boyce Eight-Chain model. I then used MCalibration to quickly calibrate the hyperelastic model to the data at each temperature. The following figures show the calibrated model results. As expected, the model predictions are in good agreement with the experimental data.

## Step 2: Combine the Models into a Temperature-Dependent Model

Each of the 3 material models is then exported to an Ansys dat-file. Here’s an example of what one of these files contain.

```				```
! MCalibration defined material model -- start
! Units: [length]=millimeter, [force]=Newton, [time]=seconds, [temperature]=Kelvin
! Material Model: Ansys-ArrudaBoyce
! Calibration file name: Calibrate_AB_T20.mcal
TB, HYPER, matid, 1, 2, BOYCE
TBDATA, 1, 0.248052141
TBDATA, 2, 1.21634503
MP, DENS, matid, 1e-09
! MCalibration defined material model -- end
```
```

The 3 files are then combined into one file using `TBTEMP` commands. Here is the final model. That is it! You can now use this model in Ansys WB as a command snippet.

```				```
TB, HYPER, matid, 1, 2, BOYCE
TBTEMP, 20.0
TBDATA, 1, 0.248052141
TBDATA, 2, 1.21634503
TBTEMP, 60.0
TBDATA, 1, 0.275389748
TBDATA, 2, 1.21416605
TBTEMP, 150.0
TBDATA, 1, 0.321847215
TBDATA, 2, 1.16325745

```
```

### How to Predict Stress Reduction After Yielding

Discussion of how to select and calibrate a material model that can predict stress reduction after yielding.

### How Important is the Bulk Modulus in FEA?

Investigation of how important the bulk modulus is in a FE simulation. Using MCalibration and Abaqus, I show that most of the time the bulk modulus has virtually no influence on the FE results.

### Basic FEA Theory – Part 5 – Solve For Displacements

Last article is in my series on basic FEA theory. In this article I put everything together to solve for the displacements.