Advanced material modeling for rubbery materials with permanent set.
For many years you could not combine permanent set (plasticity) material behavior with hyperelasticity in Abaqus. This became especially desirable with the advent of TPEs (Thermo Plastic Elastomers) which are a block copolymer blend combining a traditional elastomer (e.g. EPDM) with a traditional plastic (e.g. a rigid styrene). This newer class of materials exhibits the high elongation of elastomers along with the plasticity or permanent set one sees in rigid plastics.
The use of *ELASTIC together with *PLASTIC in Abaqus is based on an additive decomposition of the total strain into an elastic strain and plastic strain. This additive decomposition of strain is not appropriate at large strains. At large strains one needs to use a multiplicative decomposition of the deformation gradient, often given the shorthand "Fe*Fp", or simply "FeFp", since F is the symbol used for the deformation gradient.
See the attached paper with the filename 2007_ECCMR_PermanentSet.pdf for more detailed theoretical information and references.
This work was implemented in Abaqus version 6.7EF in the fall of 2007. So, beginning with version 6.7EF you can define a material that includes *HYPERELASTIC, *PLASTIC and even *MULLIINS EFFECT. Along with the implementation in the solvers, there was a test data parsing tool developed as a plug-in for A/CAE. This plug-in tool is documented in the ClientCare Knowledgebase article QA00000008645. More details of the way the test data is partitioned and transformed is made available in article QA00000041611. The pdf document attached to QA00000041611 is also attached to this post. In version 6.12 of Abaqus this plug-in test data parsing tool was moved into A/CAE as part of the "calibration" functionality.
This post is intended to give some reference background for the "FeFp", or Hyperelasticity with Permanent Set material model, and more importantly, provide a demonstration of the use of the plug-in tool for calibration of a material model from test data. For the demonstration, please first browse through the attached PowerPoint presentation (PDF format) named Material Modeling FeFp Plugin. Then play the attached MP4 video for a tutorial demonstration of the A/CAE plug-in. The files required for you to repeat the demonstration on your own are (attached to this post):
EPDM_cae.zip (this is the .cae model file)
st_EPDM.zip (this is the .inp model file; the "st" stands for simple tension and it is a unit cube model)
EPDM_uniaxial_csv.zip (this is the uniaxial test data for an EPDM rubber)
These files come from the KB article QA00000008645 and are re-posted here for your convenience. Remember that this demonstration is based on using Abaqus version 6.11.
There is also a KB article, QA00000041611, titled "Understanding the intermediate configuration when partitioning test data into *HYPERELASTIC and *PLASTIC subsets". This article helps you understand that this tool partitions the test data, but also transforms the test data.
Question: I am using the "Hyperelasticity with Permanent Set" material calibration tool in Abaqus/CAE. After I calibrate my uniaxial test data and perform a simple uniaxial stress analysis, I see that the stress-strain response computed by Abaqus does not match the data given in the corresponding *UNIAXIAL TEST DATA keyword option. Why is this?
Answer: When the "Hyperelasticity with Permanent Set" material calibration behavior is used, the test data you supply is automatically partitioned into a corresponding set of *HYPERELASTIC and *PLASTIC definitions. The resulting *HYPERELASTIC definition is given with respect to an intermediate, unloaded, stress-free configuration that exists after unloading.
The pdf document from QA00000041611 is also posted here for convenience.
The zip file for the plug-in (Abaqus 6.14 version) is also attached to this post.
Back to: Material Modeling and Calibration - An Overview and Curriculum
