Sometimes it is important to not only predict the deformation response of a product when exposed to a mechanical load history, but also predict how the dissipated viscoplastic energy is converted to temperature changes in the material. That is, it is important to capture the fully coupled thermo-mechanical response of the product in its intended environment.
In the example presented here, I will show how to perform this type of FE analysis using Abaqus/Explicit and a temperature-dependent material model from the PolyUMod library. The first step setting up the analysis is to create a suitable material model. In this case I selected the Three Network (TN) model from the PolyUMod library. I used the default material parameters that are available in MCalibration, and which corresponds to a generic ultra high molecular weight polyethylene (UHMWPE) material tested at room temperature. The following figure shows the predicted stress-strain response at room temperature.
Note that all files that are used in this example can be downloaded using the link at the end of the post. To make the example more interesting I created a temperature-dependent TN model using the Multi-Temperature model framework. This model framework allows the material parameters of any PolyUMod material model to become fully temperature dependent. The first step to achieve this is to export the room temperature model from MCalibration into a separate txt-file using the Export Material model option in MCalibration, see the following image:
Here I need to select “PolyUMod External File”. In a real problem I would then repeat this step for each temperature of interest. Here, I will simply scale the predicted stress response by a factor of 0.8 to get an estimation of the stress-strain response at a temperature of 50°C. This is easy to do in MCalibration by selecting the menu option “Set or Scale Material Parameters”, and then specifying the 0.8 reduction factor.
Then export the re-scaled material model model to a different “PolyUMod External File”. The two exported material parameter files can now be combined into a single Multi-Temperature Model using the following option in MCalibration:
This new feature in MCalibration will ask for which material parameter files to combine, and the create a new multi-temperature model. An example of the stress-strain predictions from this model are shown in the following figure:
As you see, I used pure SI units in order to simplify the thermal property input (which we will specify later). We can now export this multi-temperature TN model into an Abaqus Python Script which can be directly read into Abaqus/CAE.
Once we have performed all these steps to setup the material model we can now switch over to Abaqus CAE to setup our coupled thermo-mechanical model. All of the Abaqus settings are selected as is normally done for an explicit thermo-mechanical model. There is only one, perhaps, tricky part, and that is to setup the material model within CAE. The following image shows the options that I selected.
Note that it is necessary to include “Inelastic Heat Fraction” in order to instruct Abaqus how much of the dissipated energy should be converted to heat. It is also necessary to specify the density, the specific heat, and the thermal conductivity. After that has been done the simulation is ready.
The following figure shows the final predicted temperature results. As expected, the temperature increase is the highest in the region with the largest energy dissipation.
All files that I used for this example can be downloaded from the following link.