*Heading
Mullins Effect, Compressible Arruda-Boyce Model, 2D Element
with Viscoelasticity, Cyclic Uniaxial Tension
** Job name: Job-1 Model name: mmecdo2cut_arruda.inp
**
** PARTS
**
*Part, name=PART-1
*End Part
**
** ASSEMBLY
**
*Assembly, name=Assembly
**  
*Instance, name=PART-1-1, part=PART-1
*Node
      1,           0.,           0.
      2,           0.,           1.
      3,           1.,           0.
      4,           1.,           1.
*Element, type=CPE4RH
1, 1, 3, 4, 2
*Elset, elset=ONE
 1,
** Region: (Section-1-ONE:ONE)
*Elset, elset=_I1, internal
 1,
** Section: Section-1-ONE
*Solid Section, elset=_I1, material=TREL
1.,
*End Instance
*Nset, nset=ALL, instance=PART-1-1, generate
 1,  4,  1
*Nset, nset=BOT, instance=PART-1-1
 1, 3
*Nset, nset=LEFT, instance=PART-1-1
 1, 2
*Nset, nset=RIGHT, instance=PART-1-1
 3, 4
*Nset, nset=TOP, instance=PART-1-1
 2, 4
*Nset, nset=SET, instance=PART-1-1
3
*Nset, nset=FOUR, instance=PART-1-1
4
*EQUATION
** Since the S11 output is Cauchy or true stress, we need to
** determine the nominal stress for post-processing.
** Node 3 is tied to node 4 in dof 1 so that:
** Nominal stress (dof 1) = RF1 (@ node 4) / Original area
** (w/c is 1 x 1 = 1)
2
SET,1,1, FOUR,1,-1
*End Assembly
** 
** MATERIALS
** 
*Material, name=TREL
*Hyperelastic, arruda-boyce
200.,    5., 0.001
*Mullins effect
1.1,100., 0.1
*viscoelastic,time=prony
0.5,,10.0
** ----------------------------------------------------------------
** 
** STEP: Step-1
** 
*Step, name=Step-1, nlgeom, inc=20
UNIAXIAL TENSION
*visco
1., 20., 
** 
** BOUNDARY CONDITIONS
** 
*Boundary
FOUR, 1, 1, 2.
BOT, 2, 2
LEFT, 1, 1
**
** HISTORY OUTPUT
** 
*Output, history, frequency=10
***Output, history, frequency=1
*Element Output, elset=PART-1-1.ONE
SENER, S, DMENER
*Node Output, nset=FOUR
U,RF
*El Print, freq=999999
*Node Print, freq=999999
*End Step
** ----------------------------------------------------------------
** 
** STEP: Step-2
** 
*Step, name=Step-2, nlgeom
*visco
1., 20., 
** 
** BOUNDARY CONDITIONS
** 
*Boundary, op=NEW
FOUR, 1, 1, 0.
BOT, 2, 2
LEFT, 1, 1
** 
*End Step
** ----------------------------------------------------------------
** 
** STEP: Step-3
** 
*Step, name=Step-3, nlgeom
*visco,CETOL=0.1
1., 20., 
** 
** BOUNDARY CONDITIONS
** 
*Boundary, op=NEW
FOUR, 1, 1, 3.
BOT, 2, 2
LEFT, 1, 1
** 
*End Step
** ----------------------------------------------------------------
** 
** STEP: Step-4
** 
*Step, name=Step-4, nlgeom
*visco
1., 20., 
** 
** BOUNDARY CONDITIONS
** 
*Boundary, op=NEW
FOUR, 1, 1, 0.
BOT, 2, 2
LEFT, 1, 1
*End Step