1. Meshing and modeling#
The choice of finite elements has a direct influence on the solution. By choice, we mean the choice of the degree of the finite element approximation as well as the choice of a formulation. Since the degree of approximation is generally related to the degree of the meshes, the following paragraphs deal with the choice of the degree of the mesh and the choice of a finite element formulation, with a particular focus on incompressibility problems.
1.1. General information on the choice of the degree of mesh and the choice of finite elements#
In general, the use of a linear mesh is recommended in thermal engineering and the use of a quadratic mesh is recommended in mechanics. The CREA_MAILLAGE command (LINE_QUAD and QUAD_LINE) allows you to switch from a linear mesh to a quadratic mesh and vice versa, but does not allow you to generate quadratic elements with curved edges. Moreover, it is preferable to generate the quadratic elements directly with the mesh tool (the Salome-Meca mesh module for example). For fracture mechanics, the use of Barsoum elements at the bottom of a crack improves the quality of the result (order MODI_MAILLAGE/NOEUD_QUART).
The finite elements are selected in command AFFE_MODELE. In thermal, it is recommended to use lumped elements (_ DIAG). In mechanics, the finite elements classically used are iso-parametric elements (3D, D_ PLAN, C_ PLAN, AXIS). However, these elements are poorly suited to almost incompressible problems. The choice of a formulation that addresses this problem is the subject of the next paragraph.
For more details, see u2.01.10
1.2. Choosing a formulation to treat almost incompressible problems#
A problem is almost incompressible if the Poisson’s ratio is close to 0.5 (\(\nu >\mathrm{0,45}\)) or if the plastic deformation rate is high. This results in an oscillation of the stress trace. There are 6 formulations to deal with this problem in Code_Aster whose choice depends on the type of mesh, the deformation model and the quality/cost ratio calculation.
The possible formulations are:
in small deformations: _SI, _ INCO_UP, _, _ INCO_UPG, INCO_UPO
in large deformations: _ INCO_UP, _ INCO_UPG.
All formulations are compatible with 3D models, D_ PLAN and AXIS but under plane constraints (C_ PLAN) only the sub-integrated formulation (_SI) is possible.
The table below shows the compatibility between the almost incompressible formulation and the type of mesh (limited to the main 3D cells).
_IF |
_ INCO_UP |
_ |
_ INCO_UPG |
_ INCO_UPO |
|
HEXA20 |
X |
X |
X |
||
PENTA15 |
X |
X |
|||
PYRAM13 |
|||||
TETRA10 |
X |
X |
X |
||
HEXA8 |
X |
X |
|||
PENTA6 |
X |
||||
PYRAM5 |
X |
||||
TETRA4 |
X |
X |
X |
In the general case, it is therefore necessary to mix different formulations to cover all types of cells (for example, as no formulation manages PYRAM13 cells, it is also necessary to assign iso-parametric modeling).
In the case where small deformations are left, it is advisable to use a mixture of formulations (the mesh may include several types of mesh):
quality |
cost |
|
+++ |
+++ |
|
++ |
++ |
|
MODELISATION =( “3D”, “3D_SI”, “3D_ INCO_UPO “) |
For more details, see u2.01.10