3. Implanting plate elements in Code_Aster#

3.1. Description#

These elements (with names MEQ4GG4, MET3GG3) are based on plane QUAD4 and TRIA3 meshes. These elements are not exact at the nodes and you have to mesh with several elements to get the correct results.

3.2. Use and developments introduced#

These elements are used in the following way:

  • AFFE_MODELE (MODELISATION =”Q4GG”,…) for the triangle and the quadrangle.

  • AFFE_CARA_ELEM (COQUE =_F (EPAISSEUR =”EP”

ANGL_REP = (”\(\alpha\)” “” \(\beta\) “)

COEF_RIGI_DRZ = “CTOR”)

To perform post-processing (generalized efforts,…) in a coordinate system chosen by the user that is not the local coordinate system of the element, a reference direction d is given defined by two nautical angles in the global coordinate system. The projection of this reference direction onto the plane of the plate fixes a reference direction \(\mathit{X1}\). The normal to the plane fixes a second and the vector product of the two vectors defined above makes it possible to define the local trihedron in which the generalized efforts and the constraints will be expressed. The user must ensure that the chosen reference axis is not parallel to the normal of certain plate elements in the model. By default, this reference direction is the \(X\) axis of the global coordinate system for defining the mesh.

The value CTOR corresponds to the coefficient that the user can introduce for the treatment of stiffness and mass terms according to normal rotation at the plane of the plate. This coefficient must be small enough not to disturb the energy balance of the element and not too small for the stiffness and mass matrices to be reversible. A value of \({10}^{\mathrm{-}5}\) is set by default.

For a behavior:

  • Isotropic elastic homogeneous in thickness we use the keyword ELASdans DEFI_MATERIAU we use the keyword where we define the coefficients \(E\) Young’s modulus, \(\nu\) Poisson’s ratio, \(\rho\) the density:

ELAS =_F (E = young NU =nu, RHO =rho…)

  • Damageable elastoplastic of type GLRC_DAMAGE, this global reinforced concrete plate model is capable of representing its behavior up to the point of ruin. The characteristics of concrete and reinforcements are given in DEFI_GLRC.

DEFI_GLRC (RELATION = « GLRC_DAMAGE « , BETON = _F (MATER =…, EPAIS = … ),

NAPPE = _F (MATER =…, OMX =…))

AFFE_CHAR_MECA (

DDL_IMPO =_F (X =.. DY =.. DZ =.. DRX =.. DRY =.. DRZ =.. degree of freedom of the plate in the global coordinate system.

FORCE_COQUE =_F (FX =.. FY =.. FZ =.. MX =.. MY =.. MZ =..) These are the surface forces (membrane and flexure) on plate elements. These efforts can be given in the global frame or in the user frame defined by ANGL_REP.

FORCE_NODALE =_F (FX =.. FY =.. FZ =.. MX =.. MY =.. MZ =..) These are the shell forces in the global frame of reference.

3.3. Linear elasticity calculation#

The stiffness matrix and the mass matrix (options RIGI_MECA and MASS_MECA respectively) are numerically integrated. We do not check whether the mesh is flat or not. The calculation takes into account the fact that the terms corresponding to the plate degrees of freedom are expressed in the local coordinate system of the element. A transition matrix makes it possible to move from local degrees of freedom to global degrees of freedom.

The basic calculations currently available correspond to the options:

DEGE_ELNO: which gives the generalized deformations per element at the nodes based on the movements in the user coordinate system: EXX, EYY, EXY, KXX, KYY, KXY, GAX, GAY.

EFGE_ELNO: who gives the efforts (generalized constraints) per element to the nodes based on the displacements: NXX, NYY, NXY, MXX, MYY, MXY,, QX, QY.

SIEF_ELGA: which gives the efforts (generalized constraints) per element at the Gauss points from the displacements: NXX, NYY, NXY, MXX, MYY, MXY, QX, QY.

EPOT_ELEM: which gives the elastic deformation energy per element from the displacements.

ECIN_ELEM: which gives the kinetic energy per element.

Finally, we also calculate the option FORC_NODA for calculating the nodal forces for the CALC_CHAMP operator.

3.4. Nonlinear calculation#

Here too, the stiffness matrix is digitally integrated. We use the calculation option STAT_NON_LINE in which we define at the level of non-linear behavior the number of layers to be used for numerical integration.

STAT_NON_LINE (...

COMPORTEMENT =_F (RELATION =' GLRC_DAMAGE '

...)

For Q4GG modeling, the only laws of behavior used are global laws (since there is only one integration point in the thickness), connecting generalized deformations to generalized stresses.

The basic calculations currently available correspond to the options:

  • DEGE_ELNO which provides generalized element-wise deformations to the nodes in the user coordinate system based on the displacements.

  • SIGM_ELNO which makes it possible to obtain the stress field in the thickness per element at the nodes for all the sub-points (all the layers and all the positions: in the lower skin, in the middle and in the upper skin of the layer).

  • EFGE_ELNO which allows you to obtain the efforts (generalized constraints) per element at the nodes in the user frame of reference.

  • VARI_ELNO which calculates the field of internal variables and the constraints per element at the nodes for all layers, in the local coordinate system of the element.