Many applications involving materials like polymers or rubber filled-elastomers demonstrate hyperelastic-finite plastic behavior. The Abaqus Unified FEA suite from SIMULIA currently provides many material models to represent real-world material behavior. However, the existing inelastic models are applicable only where the elastic portion is small and usually linear elastic.
The FeFp model is the first step towards a generalized material model for finite (large strain) elastic-plastic materials. It follows a multiplicative decomposition of the elastic and plastic deformations. Analysts who want to use a material model with a nonlinear elastic finite strain behavior and nonlinear plastic hardening will find the FeFp model useful. A parallel elastic network is included for purposes of modeling a reinforcing phase in the material. The current implementation can be used with solid, axisymmetric and plane strain elements. Rate and temperature dependence are planned for future versions.
Usage
The FeFp model is implemented by way of Abaqus VUMAT and UMAT user subroutines. Material model setup is straightforward and does not involve extensive calibration. It can be invoked by either providing material constants or uniaxial test data. The elastic regime needs to be identified appropriately by the user since this data will be used to calculate the elastic and plastic behaviors after yield and during unloading. All test data can be conveniently entered in engineering stress-strain terms.
To define the material model in terms of material constants, as few as 6 parameters are necessary (4 material constants, and 2 flags). In its simplest form, the FeFp model uses two constants to represent the neo-Hookean hyperelastic model in the elastic regime and two other constants for the plastic hardening. The FeFp model also comes with a parallel elastic network whose behavior can be either neo-Hookean or general uniaxial test data. Both the FeFp network and the elastic network contribute a portion of their stress to the overall stress based on user's specified proportion factor. This network is incorporated in the constitutive model to simulate cases where there are elastic inclusions in the overall inelastic matrix. This elastic network can easily be activated or deactivated by a parameter passed into the VUMAT.
In addition to being able to handle simple elastic-plastic behavior represented by the aforementioned 4 material constants, the FeFp network can also model general nonlinear elastic and plastic behaviors. This behavior can be defined in terms of material test data supplied via a separate text file that incorporates the following keywords:
*TOTAL UNIAXIAL TEST DATA
Provide the complete engineering stress-strain response with data pairs
*ELASTIC UNIAXIAL DATA
Provide the elastic regime data in terms of engineering stress-strain data pairs
*VOLUMETRIC TEST DATA (optional)
Provide compressibility data (pressure vs. volume)
Among these specified data, the *TOTAL UNIAXIAL TEST DATA can be data directly from the test. More attention should be given when providing data under *ELASTIC UNIAXIAL DATA since it is used to calculate the onset of the plasticity and the post yielding elastic behavior. In its simplest form, the *ELASTIC UNIAXAL DATA can be specified to be the same as the *TOTAL UNIAXIAL TEST DATA up to the yield point. The *VOLUMETRIC TEST DATA is optional. If it is not used the material is assumed incompressible.
Compression Example
Below is a uniaxial compression simulation using sample compression data from a general polymeric material. As shown, the FeFp material model is able to capture the test data very accurately, even under significant compression. The specification of this FeFp material model was accomplished using the compression test data with the *TOTAL UNIAXIAL TEST DATA keyword and the *ELASTIC UNIAXAL DATA keyword.
Comparison of Compressive Uniaxial Test Data with FeFp Material Model Response
Additional Information
Visit the Abaqus Process Automation Portal. Registration to the portal is free, and you will find over 50 scripts, plug-ins and other helpful additions to Abaqus.
>> Learn more
Extensions for Abaqus are made available "as is" and without warranty. Support may be available for some extensions for a fee.
>>
Contact your local support office
This extension for Abaqus was developed by the SIMULIA Central region office. Contact their office for more specfic information on this extension.
>> Contact SIMULIA Central
Finite Elasto-Plasticity 