We often use these models we call "unit cubes" for calibration purposes.  A "unit cube" is a single element with side-length of 1.   By having the side length of 1, then we can plot the U (displacement) variable as a stand-in for Engineering, or Nominal, strain.  Also, because the face areas are 1, the RF (reaction force) variable is a stand in for Engineering, or Nominal, stress.  

This use of unit cube models for calibration has been around for decades.  You will find an example of unit cube models in the Abaqus Benchmark Guide, in section  3.1.6 Rubber under uniaxial tension.   For rubber problems it is common to use 3 unit cubes, one for simple tension (ST), one for Planar Tension (PT), and one for Equibiaxial Tension (EB).  The attached zip file includes an Abaqus/CAE file and input file which contains these 3 unit cubes in a single file.  Each unit cube is a single C3D8H element.  We use an equation so that we can apply our load on a single node, and post-process the RF and U response for that single node.  An amplitude definition is used to load and unload several times to successive strain levels - in order to observe the Mullins effect.  The material model in this example is for a filled natural rubber and contains a Marlow model for Hyperelasticity, Mullins effect and Plasticity. If we plot the RF versus U for each unit cube we can see the Mullins effect clearly - these elements are excited in the Z, or 3 direction.  These files were prepared using 6.14-1 of Abaqus.

This image is a plot of the RF3 versus U3 for the uniaxial tension, or simple tension, unit cube.

Back to:  Sharing Abaqus test specimen models

Back to: Material Modeling and Calibration - An Overview and Curriculum