3. Example of use

This section provides a description of the main steps of a reinforcement calculation, for plane stress modeling.

For more examples, see the ssnp105 [V6.03.105] and ssnp106 [V6.03.105] test cases.

3.1. Before using the macro command

It is necessary to perform a linear elastic calculation with plane modeling (D_ PLAN, C_ PLAN).

All the elements are associated with the concrete material.

3.1.1. Mesh and model

MAIL = LIRE_MAILLAGE (FORMAT = 'ASTER',

INFO = 2,

UNITE = 20)

MAIL = DEFI_GROUP (reuse = MAIL,

CREA_GROUP_MA = _F (NOM = “everything”,

TOUT =” OUI “),

MAILLAGE = MAIL)

MODEL = AFFE_MODELE (AFFE = _F (GROUP_MA = “all”,

MODELISATION = (”C_ PLAN “,),

PHENOMENE = “MECANIQUE”),

MAILLAGE = MAIL)

3.1.2. Materials

Command CALC_BT finds a mesh composed of concrete rods and steel tie rods (the reinforcements). Both materials are defined here. However, for the basic calculation only the material concrete is used, the structure to be reinforced being considered homogeneous.

BETON = DEFI_MATERIAU (ELAS = _F (E = 30E9,

NAKED = 0.2)))


ACIER = DEFI_MATERIAU (ELAS = _F (

E = 210E9,

NAKED = 0.3)))


material = AFFE_MATERIAU (AFFE = _F (MATER = (BETON,),

TOUT = 'OUI'),

MODELE = MODEL)

3.1.3. Boundary conditions

Static boundary conditions are defined in the at the nodes structure.

These same boundary conditions will then be used in the calculation of connecting rods and tie rods.

bc = AFFE_CHAR_MECA (DDL_IMPO = (_F (GROUP_NO = ('SUP_1',),

LIAISON = 'ENCASTRE'),

_F (DY = 0.0,

GROUP_NO = ('SUP_2',)))),

FORCE_NODALE = (_F (FY = -300000.0,

GROUP_NO = 'LOAD_1'),

),

MODELE = MODEL)

3.1.4. Preliminary calculation

The aim here is to carry out the mechanical calculation that will provide the starting state for BT optimization, based on the loads and blockages defined previously.

At the moment, the only boundary conditions that can be applied are nodal forces and imposed degrees of freedom.

RESU = MECA_STATIQUE (CHAM_MATER = material,

EXCIT = _F (CHARGE = bc,

TYPE_CHARGE = 'FIXE_CSTE'),

MODELE = MODEL,

TITRE = 'SYSTEM')

3.2. Using the macro command

As already mentioned, in the keywords DDL_IMPO and FORCE_NODALE, the node groups and forces/displacements should be exactly the same as those used for the basic calculation.

Material BETON should be the same material used for the basic calculation. Material ACIER is used only in the body of the macro control.

STM_TOPO = CALC_BT (RESULTAT = RESU,

RESU_BT = CO ('RES_TOPO'),

INST = 1. ,

DDL_IMPO =( _F (GROUP_NO = 'SUP_1',

DX=0,

DY = 0),

_F (GROUP_NO = 'SUP_2',

DY = 0)

),

FORCE_NODALE =_F (

GROUP_NO = 'LOAD_1',

FY=-3000000.0

),

BETON = 'BETON',

ACIER = 'ACIER',

GROUP_MA_EXT = 'SKIN1',

GROUP_MA_INT = 'SKIN2',

SCHEMA = 'TOPO',

SIGMA_C = 350,000,

SIGMA_Y = 500000000,

PAS_X = 0.05,

PAS_Y = 0.05,

TOLE_BASE = 0.026,

NMAX_ITER = 200,

RESI_RELA_TOPO = 0.00001,

RESI_RELA_SECTION = 0.000001,

CRIT_SECTION = 0.5,

CRIT_ELIM = 0.5,

SECTION_MINI = 1e-6,

LONGUEUR_MAX = 7,

INIT_ALEA = 0,

)