Reference problem
=====================


Geometry
---------

According to the modeling :math:`\mathrm{2D}` (plane deformation) or :math:`\mathrm{3D}`, we consider respectively a square or a cube with a side of 0.05 :math:`\text{mm}` (see Figure. 1.1-1). Because of the symmetry, only a quarter of the geometry is shown.


.. image:: images/1000020100000357000001A14049437B8759E02C.png
    :width: 6.3374in
    :height: 3.0902in


.. _RefImage_1000020100000357000001A14049437B8759E02C.png:

**Figure** 1.1-a **: Geometries of a** square**(a) and a cube (b)**


Material properties
----------------------

Elasticity:


.. csv-table::

    ":math:`E=190000\text{MPa}` ", "Young's module"
    ":math:`\mathrm{\nu }=0.3` ", "Poisson's ratio"


Work hardening curve:

:math:`R(\mathrm{\kappa })=488.36+57.13(1-\mathrm{exp}(-8613\mathrm{\kappa }))+238.73(1-\mathrm{exp}(-10.39\mathrm{\kappa }))`

Ductile damage law GTN:


.. csv-table::

    ":math:`{q}_{1}=1.5` ", "Model parameter GTN"
    ":math:`{q}_{2}=1.07` ", "Model parameter GTN"
    ":math:`{f}_{0}=0.01` ", "Initial porosity"
    ":math:`{f}_{n}=0` ", "Germination Parameter"
    ":math:`{f}_{c}=0.05` ", "Coalescence porosity"
    ":math:`\mathrm{\delta }=3` ", "Coalescence coefficient related to coalescence"
    ":math:`c=2.22N` ", "Non-local parameter"
    ":math:`r=5000\mathit{MPa}` ", "Lagrange penalty parameter"


In particular, the non-local parameter :math:`c` and the penalty parameter :math:`r` are only used in the :math:`\mathit{GTN}` gradient law.

In DEFI_MATERIAU, the following information should be filled in:


.. csv-table::

    "**ELAS**", "**ECRO_** NL", "**GTN**", "**NON_LOCAL**"
    "E = 190000", "R0= 488.361123569", "Q1 = 1.5", "C_ GRAD_VARI = 2.22"
    "NU = 0.3", "R1 = 57.1333673502", "Q2 = 1.07"," PENA_LAGR =5000"
    "", "GAMMA_1 = 8613"," PORO_INIT = 0.01", ""
    "", "R2 = 238.731127339"," COAL_PORO = 0.05", ""
    "", "GAMMA_2 =10.386585592"," COAL_ACCE = 3", ""



Boundary conditions and loads
-------------------------------------

For modeling :math:`2D` (plane deformation), the horizontal displacements and the vertical displacements of all the nodes are controlled: :math:`{u}_{x}=(\mathrm{cosh}(t)-1)x+\mathrm{sinh}(t)y` and :math:`{u}_{y}=\mathrm{sinh}(t)x+(\mathrm{cosh}(t)-1)y` (see Figure 1.1-1 (a) for geometry). Here, :math:`t` refers to the moment of calculation.

For modeling :math:`3D`, the movements along the :math:`X` axis and the movements along the :math:`Y` axis of all the nodes are controlled: :math:`{u}_{x}=(\mathrm{cosh}(t)-1)x+\mathrm{sinh}(t)y` and :math:`{u}_{y}=\mathrm{sinh}(t)x+(\mathrm{cosh}(t)-1)y`, the movements along the :math:`Z` axis are blocked (see Figure 1.1-1 (b) for geometry).

Boundary conditions and loads are imposed in this way so that the problem in :math:`2D` and the problem in :math:`3D` are the same and homogeneous.

The load is imposed using 1000 identical time steps. The pseudo-calculation time is 1.