*Heading
Mullins effect, compressible Marlow model
3D element, cyclic uniaxial tension
Comparison of nominal stresses
** Job name: Job-1 Model name: mmecdo3cut_yeoh
**
** 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=C3D8RH
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=MARLOW
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=MARLOW
*HYPERELASTIC,MARLOW
*UNIAXIAL TEST DATA
  0.000000000000000,       0.000000000000000
  0.231494000000000,       0.030000000000000
  0.448560000000000,       0.060000000000000
  0.747177000000000,       0.105000000000000     
   1.13595000000000,       0.172500000000000     
   1.59760000000000,       0.273750000000000     
   2.08089000000000,       0.423750000000000     
   2.47973000000000,       0.573750000000000     
   3.03767000000000,       0.723750000000000     
   4.07610000000000,       0.873750000000000     
   5.99936000000000,        1.02375000000000     
   9.30106000000000,        1.17375000000000     
   14.5712000000000,        1.32375000000000     
   22.5031000000000,        1.47375000000000     
   33.9013000000000,        1.62375000000000     
   49.6884000000000,        1.77375000000000     
   70.9126000000000,        1.92375000000000     
   98.7549000000000,        2.07375000000000     
   134.537000000000,        2.22375000000000     
   179.726000000000,        2.37375000000000     
   235.948000000000,        2.52375000000000     
   304.986000000000,        2.67375000000000     
   388.797000000000,        2.82375000000000     
   489.510000000000,        2.97375000000000     
   509.043000000000,        3.00000000000000     
*VOLUMETRIC TEST DATA
  0.000000000000000,       1.00000000000000     
   82.7586206896552,       0.970000000000000     
   165.517241379310,       0.940000000000000     
   248.275862068965,       0.910000000000000     
   331.034482758621,       0.880000000000000     
   413.793103448276,       0.850000000000000     
   496.551724137931,       0.820000000000000     
   579.310344827586,       0.790000000000000     
   662.068965517241,       0.760000000000000     
   744.827586206897,       0.730000000000000     
   827.586206896552,       0.700000000000000     
*Mullins effect
1.1,100.0, 0.1
** ----------------------------------------------------------------
** 
** STEP: Step-1
** 
*Step, name=Step-1, nlgeom, inc=20
UNIAXIAL TENSION
*Static, direct
1., 20., 
** 
** BOUNDARY CONDITIONS
** 
*Boundary
FACE1, 3, 3
FACE3, 2, 2
FACE6, 1, 1
TWO, 1, 1, 2.
** 
** HISTORY OUTPUT
** 
***Output, history, frequency=1
*Output, history, frequency=10
*Element Output, elset=PART-1-1.ONE
SENER, S, DMENER
*Node Output, nset=TWO
U,RF,
*El Print, freq=999999
*Node Print, freq=999999
*End Step
** ----------------------------------------------------------------
** 
** STEP: Step-2
** 
*Step, name=Step-2, nlgeom
*Static, direct
1., 20., 
** 
** BOUNDARY CONDITIONS
** 
*Boundary, op=NEW
FACE1, 3, 3
FACE3, 2, 2
FACE6, 1, 1
TWO, 1, 1
*End Step
** ----------------------------------------------------------------
** 
** STEP: Step-3
** 
*Step, name=Step-3, nlgeom
*Static, direct
1., 20., 
** 
** BOUNDARY CONDITIONS
** 
*Boundary, op=NEW
FACE3, 2, 2
FACE6, 1, 1
TWO, 1, 1, 3.
FACE1, 3, 3
*End Step
** ----------------------------------------------------------------
** 
** STEP: Step-4
** 
*Step, name=Step-4, nlgeom
*Static, direct
1., 20., 
** 
** BOUNDARY CONDITIONS
** 
*Boundary, op=NEW
FACE1, 3, 3
FACE3, 2, 2
FACE6, 1, 1
TWO, 1, 1
** 
*End Step