7. Implanting shell elements in Code_Aster#

7.1. Description#

These elements (with names MEC3TR7H and MEC3QU9H) are based on curved TRIA7 and QUAD9 meshes. These elements are not exact at the nodes and you have to mesh with several elements to get the correct results.

7.2. Use and developments introduced#

These elements are used as follows:

MA = CREA_MAILLAGE (MAILLAGE: MAILINI

MODI_MAILLE: (OPTION: 'QUAD8_9'

TOUT: 'OUI')...)

We use a MODI_MAILLE mesh modification routine to go from 8-node quadrangles to 9-node quadrangles or from 6-node triangle elements to 7-node triangle elements.

AFFE_MODELE (MODELISATION: 'COQUE_3D'...) for the triangle and the quadrangle

Routine INI080 is used for the position of Hammer and Gauss points on the surface of the shell and the corresponding weights.

AFFE_CARA_ELEM (COQUE :( EPAISSEUR :'EP'

ANGL_REP: (:math:`\alpha`, :math:`\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, the direction \(\mathit{X1}\) of the user coordinate system is defined as the projection of a reference direction \(\underline{d}\) onto the surface \(\omega\) of the element. This reference direction \(\underline{d}\) is chosen by the user who defines it by two nautical angles in the global coordinate system. The normal \(N\) on the surface of the element fixes the second direction at the point of observation in question. The vector product of the two vectors defined above \(\mathit{Y1}\mathrm{=}N\mathrm{\wedge }\mathit{X1}\) makes it possible to define the local trihedron in which the generalized efforts representing the state of constraints will be expressed. The user must ensure that the chosen reference axis is not parallel to the normal of certain shell elements. By default, the reference direction \(\underline{d}\) is the \(X\) axis of the global coordinate system for defining the mesh.

The value CTOR corresponds to the coefficient that the user can enter for the treatment of stiffness and mass terms according to normal rotation at the surface of the shell. 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—5 is set by default.

ELAS: (e:YOUNG NU: :math:`\nu` ALPHA: :math:`\alpha`.. RHO: :math:`\rho`..)

For a thermo-elastic isotropic behavior that is homogeneous in thickness, the keyword ELAS is used in DEFI_MATERIAU where we define the coefficients \(E\), Young’s modulus, \(\nu\) Poisson’s ratio, \(\alpha\) thermal expansion coefficient, thermal expansion coefficient and RHO the density.

AFFE_CHAR_MECA (DDL_IMPO: (

EX:.. OF:.. DZ:.. DRX:.. DRY:.. DRZ:.. DDL case in the global coordinate system.

FORCE_COQUE: (FX:.. FY:.. FZ:.. MX:.. MY:.. MY:..). These are the surface forces on shell elements. These efforts can be given in the global frame or in the user frame defined by ANGL_REP.

FORCE_NODALE: (FX:.. FY:.. FZ:.. MX:.. MY:.. MY:..). These are shell efforts in the global benchmark.

7.3. Linear elasticity calculation#

The stiffness matrix and the mass matrix (options RIGI_MECA and MASS_MECA respectively) are numerically integrated into the TE0401 and TE0406, respectively. The calculation takes into account the fact that the terms corresponding to the degrees of freedom of shell rotation 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 shell skin element. These values are stored as follows: 6 deformation or stress components,

  • EPXX EPYY EPZZ EPXY EPXZ EPYZ or SIXX SIYY SIZZ SIXY SIXZ SIYZ,

  • 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 constraints per element at the Gauss points in the element’s local coordinate system based on the displacements: SIXX, SIYY, SIZZ, SIXY, SIXZ, SIYZ.

  • EPOT_ELEM: which gives the elastic deformation energy per element based on the displacements.

  • ECIN_ELEM: which gives the kinetic energy per element.

Finally, TE0416 also calculates option FORC_NODA for calculating nodal forces for operator CALC_CHAMP.

7.4. Plasticity calculation#

The stiffness matrix is also integrated numerically, by layers, in TE0414. 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. All the plane stress laws available in the*Code_Aster* can be used.

STAT_NON_LINE (...

COMPORTEMENT: (RELATION: ''

COQUE_NCOU: 'NOMBRE FROM COUCHES')

...)

The basic calculations currently available correspond to the options:

  • EPSI_ELNO which provides element-wise deformations to the nodes in the user coordinate system based on displacements, in lower skin, mid-thickness, and upper shell skin.

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

  • 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.