5. Implanting plate elements in Code_Aster#

5.1. Description#

These elements (with names MEDKTR3, MEDSTR3, MEDKQU4, MEDSQU4,,, MEDKTG3,, MEDKQG4, and MEQ4QU4) are based on plane TRIA3 and QUAD4 meshes. These elements are not exact at the nodes and you have to mesh with several elements to get the correct results.

5.2. Use and developments introduced#

These elements are used as follows:

AFFE_MODELE (MODELISATION = “DKT”.) for the triangle and quadrangle of type DKT
AFFE_MODELE (MODELISATION = “DST”.) for the triangle and quadrangle of type DST
AFFE_MODELE (MODELISATION = “DKTG”.) for the triangle and quadrangle of type DKTG
AFFE_MODELE (MODELISATION = “Q4G”.) for the Q4g quadrangle

Routine INI079 is used for the position of the Hammer and Gauss points on the surface of the plate and the corresponding weights.

AFFE_CARA_ELEM (COQUE =_F (EPAISSEUR =”EP”

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

COEF_RIGI_DRZ = “CTOR”)

To perform post-processing (constraints, 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.

ELAS =_F (E=young nu=nu ALPHA =alpha.. RHO =rho..)

for isotropic thermoelastic behavior that is homogeneous in thickness, the keyword ELAS is used in DEFI_MATERIAU where the coefficients \(E\) Young’s modulus, \(\nu\) Poisson’s ratio, \(\alpha\) thermal expansion coefficient and RHO the density are defined;

ELAS_ORTH (_FO) =_F (

e_L=ygl.. e_t=YGT.. G_LT=glt.. g_tz=GTZ.. NU_LT =Null..

ALPHA_L =alpha.. ALPHA_T =alpha..)

for orthotropic thermoelastic behavior whose axes of orthotropy are \(L\), \(T\) and \(z\) with isotropy of axis \(L\) (fibers in the \(L\) direction embedded by a matrix, for example) it is necessary to give the seven independent coefficients ygl, Young’s modulus longitudinal, longitudinal, ygt, Young’s modulus transverse, ygt, transversal Young’s modulus, glt, shear modulus in the plane \(\text{LT}\), gtz, shear modulus in plane \(\mathit{TZ}\) zero, Poisson’s ratio in plane \(\text{LT}\), and the alphal and alphat thermal expansion coefficients for longitudinal and transverse thermal expansion, respectively.

Orthotropic elastic behavior is only available associated with the keyword DEFI_COMPOSITE which allows you to define a multi-layer composite shell.

For a single orthotropic material, we will therefore use DEFI_COMPOSITE with a single layer. If you want to use ELAS_ORTH with transverse shear, you must necessarily use DST modeling. If we use models DKT, or DKTG, the transverse shear energy is not taken into account.

ELAS_COQUE (_FO) =F (

MEMB_L =C1111.. MEMB_LT =C1122.. MEMB_T =C2222.. MEMB_G_LT =C1212..

FLEX_L =D1111.. FLEX_LT =D1122.. FLEX_T =D2222.. FLEX_G_LT =D1212..

CISA_L =G11... CISA_T =G22... ALPHA =alpha.. RHO =rho..)

This behavior was added in DEFI_MATERIAU to take into account non-proportional stiffness matrices in membrane and in flexure, obtained by homogenization of a multilayer material. The coefficients of the stiffness matrices are then entered manually by the user into the user coordinate system defined by the keyword ANGL_REP. The thickness given in AFFE_CARA_ELEM is only used with the density defined by RHO. alpha is thermal expansion. If you want to use ELAS_COQUE with transverse shear, you must necessarily use DST modeling. If modeling DKT is used, transverse shear is not taken into account.

DEFI_COMPOSITE_F (COUCHE = EPAISSEUR: “EP”

MATER = “material”

ORIENTATION = (theta))

This keyword (cf. [R4.01.01] and [U4.42.03]) makes it possible to define a multilayer composite shell starting from the lower layer to the upper layer based on its characteristics layer by layer, thickness, type of the constituent material and orientation of the fibers in relation to a reference axis. The type of the constituent material is produced by the operator DEFI_MATERIAU under the keyword ELAS_ORTH. theta is the angle of the first direction of orthotropy (longitudinal direction or direction of the fibers) in the tangential plane to the element with respect to the first direction of the reference frame defined by ANGL_REP. By default theta is null, otherwise it must be provided in degrees and must be between \(–\mathrm{90º}\) and \(+\mathrm{90º}\).

AFFE_CHAR_MECA (DDL_IMPO =_F (

DX=.. 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 efforts in the global frame of reference.

5.3. 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 elementary calculations (CALC_CHAMP) currently available correspond to the options:

EPSI_ELNO and SIGM_ELNO which provide the deformations and stresses to the nodes in the user coordinate system of the lower skin, mid-thickness and upper plate skin element, the position being specified by the user. These values are stored as follows: 6 deformation or stress components:
EPXX EPYY EPZZ EPXY EPXZ EPYZ or SIXX SIYY SIZZ SIXY SIXZ SIYZ
DEGE_ELNO: which gives the deformations generalized by the element to the nodes based on the movements in the user coordinate system: EXX, EYY, EXY, KXX, KYY, KXY,, GAX,, GAY.
EFGE_ELNO: which gives the generalized efforts per element to the nodes based on the moves: NXX, NYY, NXY, MXX, MYY, MXY, QX, QY.
SIEF_ELGA: which gives the generalized efforts per element at the Gauss points based on the displacements: NXX, NYY, NXY, MXX, MYY, MXY, QX, QY.
EPOT_ELEM: which gives the elastic deformation energy per element based on 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.

5.4. Linear buckling calculation#

With option RIGI_MECA_GE activated in the element catalog, it is possible to perform a classical Euler buckling calculation after assembling the elastic and geometric stiffness matrices.

5.5. Calculation in plasticity or other non-linear behavior#

The stiffness matrix is also 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.

For DKT models, all the plane stress laws available in Code_Aster can be used.

For DST and Q4G models, only linear elasticity can be used.

For modeling DKTG, 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. In version 9.4, these laws are: GLRC_DM and GLRC_DAMAGE, as well as their coupling with elastoplastic laws in membranes (KIT_DDI).

The basic calculations currently available correspond to the options:

EPSI_ELNO which provides the elemental deformations to the nodes in the user coordinate system based on the movements, in lower skin, mid-thickness, and upper plate skin.
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 generalized efforts per element at the nodes in the user coordinate system.
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.