*Heading
Mullins effect, compressible Yeoh model
3D element, cyclic uniaxial tension
Comparison of nominal stresses
** Job name: Job-1 Model name: x_mmecdo3cut_yeoh.inp
**
** PARTS
**
*Part, name=PART-1
*End Part
**
** ASSEMBLY
**
*Assembly, name=Assembly
**  
*Instance, name=PART-1-1, part=PART-1
*Node
      1,           0.,           0.,           0.
      2,           1.,           0.,           0.
      3,           1.,           1.,           0.
      4,           0.,           1.,           0.
      5,           0.,           0.,           1.
      6,           1.,           0.,           1.
      7,           1.,           1.,           1.
      8,           0.,           1.,           1.
*Element, type=C3D8R
1, 1, 2, 3, 4, 5, 6, 7, 8
*Elset, elset=ONE
 1,
** Region: (Section-1-ONE:ONE)
*Elset, elset=_I1, internal
 1,
** Section: Section-1-ONE
*Solid Section, elset=_I1, material=YEOH
1.,
*End Instance
*Nset, nset=ALL, instance=PART-1-1, generate
 1,  8,  1
*Nset, nset=FACE1, instance=PART-1-1, generate
 1,  4,  1
*Nset, nset=FACE2, instance=PART-1-1, generate
 5,  8,  1
*Nset, nset=FACE3, instance=PART-1-1
 1, 2, 5, 6
*Nset, nset=FACE4, instance=PART-1-1
 2, 3, 6, 7
*Nset, nset=FACE5, instance=PART-1-1
 3, 4, 7, 8
*Nset, nset=FACE6, instance=PART-1-1
 1, 4, 5, 8
*Nset, nset=SET, instance=PART-1-1
6,7,3
*NSET, NSET=TWO, instance=PART-1-1
2,
*EQUATION
** Since the S11 output is Cauchy or true stress, we need to
** determine the nominal stress for post-processing.
** Nodes 6,7,3 are tied to node 2 in dof 1 so that:
** Nominal stress (dof 1) = RF1 (@ node 2) / Original area
** (w/c is 1 x 1 = 1)
2
SET,1,1, PART-1-1.2,1,-1
*End Assembly
** 
** MATERIALS
** 
*Material, name=YEOH
*Hyperelastic, yeoh
 1.326,   -0.326,   0.1319, 0.000725,       0.,       0.
*Mullins effect
1.1,100.0, 0.1
*viscoelastic,time=prony
0.5,,3.
*Density
1.
** ----------------------------------------------------------------
** 
** STEP: Step-1
** 
*Step, name=Step-1
UNIAXIAL TENSION
*Dynamic, Explicit
,20., 
** 
** BOUNDARY CONDITIONS
** 
*Boundary
FACE1, 3, 3
FACE3, 2, 2
FACE6, 1, 1
*Boundary, type=VELOCITY
TWO, 1, 1, 0.1
** 
** HISTORY OUTPUT
** 
*Output, history, time interval=5
***Output, history
*energy output
allke, allse
*Element Output, elset=PART-1-1.ONE
SENER, S, DMENER
*Node Output, nset=TWO
U,RF,
*End Step
** ----------------------------------------------------------------
** 
** STEP: Step-2
** 
*Step, name=Step-2
*Dynamic, Explicit
,20.,
** 
** BOUNDARY CONDITIONS
** 
*Boundary, type=VELOCITY
TWO, 1, 1, -0.1
*End Step
** ----------------------------------------------------------------
** 
** STEP: Step-3
** 
*Step, name=Step-3
*Dynamic, Explicit
,20., 
** 
** BOUNDARY CONDITIONS
** 
*Boundary, type=VELOCITY
TWO, 1, 1, 0.15
*End Step
** ----------------------------------------------------------------
** 
** STEP: Step-4
** 
*Step, name=Step-4
*Dynamic, Explicit
,20., 
** 
** BOUNDARY CONDITIONS
** 
*Boundary, type=VELOCITY
TWO, 1, 1, -0.15
** 
*End Step