*Heading
Mullins Effect, Compressible Hyperelasticity, Yeoh Model
Cyclic Uniaxial Tension, 3D element
User Subroutine required for this input file mmecdo3cut_user.f
** 
**
** 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=YEOH-MAT, controls=CONTR
1.,
*Hourglass Stiffness
0.5,,,,
*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
**
*Section Controls, hourglass=stiffness, name=CONTR
** 
** MATERIALS
** 
*Material, name=YEOH-MAT
*Hyperelastic, user, type=COMPRESSIBLE, properties=4
 1.326,   -0.326,   0.1319, 0.000725
*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=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
FACE1, 3, 3
FACE3, 2, 2
FACE6, 1, 1
TWO, 1, 1, 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