Abaqus Parallel Rheological Framework (PRF)

In this tutorial I will show how to first select a proper Abaqus Parallel Rheological Framework (PRF) model structure, and then demonstrate how to quickly and easily calibrate both a basic PRF model and a temperature-dependent PRF model.  

As will be shown below, there are certain PRF model elements and structures that should not be used!

When you use a PRF model in an Abaqus simulation you need to use one of the following:

Note that you cannot use a PRF model in a static analysis in Abaqus.

PRF Model Introduction

Let’s start with some of the basics:

  • The PRF model is a multi-network model where each network consists of one hyperelastic element and one flow element.
  • All networks have to have the same hyperelastic element type and the same flow element type.
  • All standard hyperelastic types in Abaqus are supported (I particularly like the Yeoh model).
  • The PRF model is a simplified version of the PolyUMod Parallel Network (PN) model, and has similar features to the PolyUMod TN and TNV models.
  • The PRF model networks can also include Mullins damage and pure plasticity. It is almost never necessary to use the plasticity option in the PRF model.
  • Use 2 networks when modeling rubber-like materials.
  • Use 3 networks when modeling thermoplastics.
  • It is almost never needed to use more than 3 networks.

Flow Element Components

The best flow element type for thermoplastics and thermosets is the Power-Law Strain Hardening model:

\(\dot{\varepsilon}^{cr} = \dot{\varepsilon}_0 \left( \left( \frac{\tilde{q}}{q_0+a\langle p\rangle} \right)^n \left[ (m+1) \varepsilon^{cr} \right]^m \right)^{1/(1+m)}. \)

Another available option is the Strain Hardening model:

\(\dot{\varepsilon}^{cr} = \left( A \tilde{q}^n \left[ (m+1) \varepsilon^{cr} \right]^m \right)^{1/(1+m)}.  \)

This flow model should not be used due to how the pre-factor A is defined. A third flow model is the Hyperbolic-sine model:

\( \dot{\varepsilon}^{cr} =A\left( sinh(B\tilde{q})\right)^n. \)

This model is also less useful since it does not contain any strain-dependence of the flow rate. The final flow model that is the Bergstrom-Boyce (BB) model. This model, of course, is really cool since it is based on work that I did during my PhD research at MIT.

\( \dot{\varepsilon}^{cr} = \dot{\varepsilon}_0 \left( \lambda^{cr} – 1 + E \right)^C \left[ \frac{\tilde{q}}{q_0} \right]^m. \)

This model is a good choice for rubber-like materials. In summary, use the Power-Law strain hardening model, or the Bergstrom-Boyce model.

Material Model Calibration

The PRF model can be quickly and accurately calibrated using MCalibration. As shown in our other tutorials, first read in the experimental data, then select the desired PRF model:

The run the calibration as normally done using MCalibration. Note that MCalibration has its own internal implementation of the listed PRF models. That makes the calibration very quick. Once the calibration has completed, you can export the calibrated material model to an Abaqus inp-file.

*Material, name=MCal_Mat
** Calibrated with MCalibration
** Units: [length]=millimeter, [force]=Newton, [time]=seconds, [temperature]=Kelvin
*Hyperelastic, Yeoh, Moduli=instantaneous
  1288.01,        0,        0,0.00016773,        0,        0
*Viscoelastic, Nonlinear, NetworkId=1, SRatio=0.789162, Law=Power Law
22.8048, 7.11344, -0.248253, 0.047694, 1
*Viscoelastic, Nonlinear, NetworkId=2, SRatio=0.20867, Law=Power Law
79.8319, 14.9972, -0.499959, 5.41635, 1

Calibrate a Temperature-Dependent PRF Model

To calibrate a temperature-dependent PRF model simply calibrate the same PRF model structure to each individual temperature. Then export the calibrated material models into individual inp-files (as shown above). You can then combine the individual calibrations into a temperature-dependent PRF model by opening a new MCalibration window, selecting the material model dialog box, and selecting “Temperature-Dependent PRF”. 

The software will then ask you for the already exported inp-files. MCalibration will then combine the models into one temperature-dependent model:

The final step is to specify the testing temperatures for the individual calibrations:

That is it! You can now export the combined model and use it in Abaqus. Life is good!

Share on facebook
Share on twitter
Share on linkedin

More to explore

Leave a Comment