Search

# Abaqus PRF Model – Network Parameters

## Abaqus PRF Model in MCalibration

This tutorial shows how Abaqus defines the network stiffnesses in the Parallel Rheological Framework (PRF) model, and how the MCalibration implementation of the PRF model is different.  Let’s just jump right in.

### Abaqus Implementation of the PRF Model

• Network 0 specifies the long-term equilibrium response
• The stiffness of network i is given by $$r_i$$ times the instantaneous response
• $$\sum r_i \le 1$$
• The stiffnesses of each network is specified using the command *Network Stiffness Ratio
• The constraint that the sum of r-values has to be less then one is the main reason MCalibration uses a different parameter definition. The Abaqus approach couples the parameters which makes the parameter optimization more difficult. The MCalibration approach has been designed to avoid this problem.

## MCalibration Implementation of the PRF Model

• Hyperelastic parameters give the response of the long-term equilibrium response
• Network i has a stiffness of $$S_i$$ times the equilibrium network

## How to Map the Material Parameters

The parameters shown in the table to the right can be converted from MCalibration to Abaqus style using the following equations:

• C10_abaqus = (1+S1+S2) * C10_mcal
• C20_abaqus = (1+S1+S2) * C20_mcal
• C30_abaqus = (1+S1+S2) * C30_mcal
• r1 = S1 / (1+S1+S2)
• r2 = S2 / (1+S1+S2)

Equivalent Abaqus inp-file parameters:

				
*Hyperelastic, Yeoh, Moduli=instantaneous
12, -0.12, 0.012, 0.001, 0, 0
*Viscoelastic, Nonlinear, NetworkId=1, SRatio=0.583333, Law=Power Law
6, 6, 0, 0, 1
*Viscoelastic, Nonlinear, NetworkId=2, SRatio=0.333333, Law=Power Law
12, 6, 0, 0, 1



Finally, remember that MCalibration performs these conversions automatically for you. The results presented here simply summarize how the conversions are performed.

### Plot Stress-Strain from Ansys Commands using MCalibration

Introduction In this article I will show how you can quickly convert any Ansys material model (in APDL format) into stress-strain predictions

### Can I Calibrate a Viscoplastic Material Model to a Single Tension Curve?

Sometimes it is possible to calibrate a viscoplastic material model to a single monotonic tension curve. This article has the details.

### How to Make Ansys find PolyUMod

Instructions for how to make sure Ansys Mechanical finds and uses a PolyUMod material model.