3. Operands#

MACRO_ELAS_MULT is a macro command that calls elementary operators that can temporarily create concepts on a global basis, so it is possible that the file associated with the latter contains records marked destroyed that are superfluous. To reduce the final size of the file, when you want to keep it, you can use the FIN procedure and the RETASSAGE =” OUI “keyword in the command set.

3.1. Operands MODELE/CHAM_MATER/CARA_ELEM#

Arguments for calculating the stiffness matrix (and the second members) are provided.

♦ MODELE = me,

Name of the model whose elements are the subject of mechanical calculation.

◊ CHAM_MATER = chmat,

Material field name.

◊ CARA_ELEM = character,

Name of the characteristics of the structural elements (beam, shell, discrete,…) if they are used in the model.

3.2. Operand NUME_DDL#

◊ NUME_DDL = naked,

A keyword used to name the numbering for later use or to use existing numbering. If no name is provided, a dial is created temporarily for each call to MACRO_ELAS_MULT.

3.3. Operands CHAR_MECA_GLOBAL/LIAISON_DISCRET#

♦/CHAR_MECA_GLOBAL = lchmg,

Key word defining the mechanical boundary conditions for the blocking of the structure.

These conditions are the same for all load cases. They are defined by AFFE_CHAR_MECA or AFFE_CHAR_MECA_F [U4.44.01].

/LIAISON_DISCRET = “OUI”,

This key word is simply used to say that there are no mechanical or kinematic conditions for blocking the structure.

3.4. Keyword CAS_CHARGE#

Keyword factor used to define a load case.

For each occurrence of the factor keyword, we build a second member (unless we use VECT_ASSE (in which case the second member is already assembled)) and we solve the linear system.

3.4.1. Operand NOM_CAS#

♦ NOM_CAS = my case,

Character string, used as an access variable to the result data structure.

Note:

Each case is named by the user and the concept of order number does not exist.

3.4.2. Operands MODE_FOURIER/TYPE_MODE#

◊ MODE_FOURIER = fashion,

Positive or zero integer indicating the harmonic of FOURIER on which the elementary stiffness matrix and the elementary vector are calculated.

◊ TYPE_MODE = type,

The harmonic type will be symmetric (“SYME”), or antisymmetric (“ANTI”) or symmetric and antisymmetric (“TOUS”) (see Fourier user manual [U2.01.07]).

3.4.3. Operands CHAR_MECA/VECT_ASSE#

◊ CHAR_MECA = lcharm,

List of char_meca concepts produced by AFFE_CHAR_MECA [U4.44.01] or AFFE_CHAR_MECA_F [U4.44.01] based on the mo model.

Note to define a « thermal expansion only » load case:

  • taking into account thermal expansion in a load case is systematic if the material field « contains » temperature (AFFE_VARC/NOM_VARC =” TEMP “).

  • for this load to be the only one taken into account, lcharm must contain a « zero » mechanical load (for example a zero nodal force on a node).

◊ VECT_ASSE = check,

Cham_no_depl_r concept representing the second member of the linear system to be solved.

3.4.4. Operands OPTION#

◊ OPTION =/'SANS',

/”SIEF_ELGA”, [DEFAUT]

By default the MACRO_ELAS_MULT command calculates the stresses at Gauss points (or generalized forces for structural elements).

The other post-processing options will be calculated afterwards by the CALC_CHAMP [U4.81.04] command.

If the user indicates OPTION = “SANS”, these constraints will not be calculated and the resulting data structure will be smaller.

3.4.5. Operand SOUS_TITRE#

♦ SOUS_TITRE = subtitle,

Subtitle that we want to give to the result displacement field.

3.5. Keyword SOLVEUR [U4.50.01]#

This keyword makes it possible to choose the method of solving linear systems. Recall that, in the case of the multiple load case, only one factorization is done for each call to MACRO_ELAS_MULT and one resolution for each load case.

3.6. Operand TITRE#

See [U4.03.01].