uniform tension of a rubber specimen

In this page, a rubber specimen is modelled using solid elements and Mooney-Rivlin material.

Only a quarter of the specimen is modelled considering symmetry. The geometry can be seen as follows. The model can be downloaded. uniform-tension-of-a-rubber-specimen.zip

example one

Model Setup

The node and element information can be seen in node.supan and element.supan, the mesh is generated by ABAQUS, it is easy to adapt ABAQUS input file to be used here. C3D8 element with full integration and nonlinear geometry is used.

file node.supan
file element.supan

After loading nodes and elements, a MooneyRivlin material is defined with $C_1=80~\text{MPa}$, $C_2=20~\text{MPa}$ and $K=10^6~\text{MPa}$. This is a regularized version of Mooney-Rivlin model that allows a certain degree of dilatation. The $D_1$ parameter used in ABAQUS is the inverse of bulk modulus so that $D_1=0$ means fully incompressible. The displacement of magnitude of $10$ along $x$ axis is applied on the free end. A static step with an initial step size of $0.01$ is used. With fixed_step_size off, the algorithm automatically scale step size based on convergence performance.

material MooneyRivlin 1 1E6 80 20

To generate the node groups to be used to apply boundary conditions, here the generatebyplane command is used.

# all nodes on plane x=0
generatebyplane nodegroup 1 1. 0. 0. 0.
# all nodes on plane y=0
generatebyplane nodegroup 2 0. 1. 0. 0.
# all nodes on plane z=0
generatebyplane nodegroup 3 0. 0. 1. 0.
# all nodes on plane x=20
generatebyplane nodegroup 4 1. 0. 0. -20.

Now BCs and loads can be applied.

grouppenaltybc 1 1 1
grouppenaltybc 2 2 2
grouppenaltybc 3 3 3

groupdisplacement 1 0 10 1 4

Setup steps and perform the analysis.

step static 1
set fixed_step_size 0
set ini_step_size 1E-2
set symm_mat 0

converger AbsIncreDisp 1 1E-8 10 1

analyze

exit

Result

animation