4. The main stages of a study#

In the general case, the main stages of a study are:

  • the preparation of the work, which is completed after reading the mesh,

  • modeling during which all the properties of finite elements and materials, boundary conditions and loads are defined and affected,

  • the calculation can then be carried out by executing global resolution methods [U4.5-], which may be based on commands for calculating and assembling matrices and vectors [U4.6-]

  • post-processing operations complementary to the calculation [U4.8-],

  • the operations for printing the results [U4.9-]

  • operations to exchange results with other software (graphic visualization for example) [U7.05-]

4.1. Start the study and acquire the mesh#

We will not return here to the possible fragmentation of the command file, which was presented in a previous paragraph.

The first executable command is:

The arguments in this command are only useful for maintenance operations or in the case of very large studies.

To read the mesh, coming from an external mesh software, one can operate in two ways:

convert the software file into a file in*Code_Aster format by a separate execution, which allows, possibly, to modify it by word processing and to keep it:

PRE_IDEAS () FIN ()

the normal study can then begin for example with:

my = LIRE_MAILLAGE ()

  • convert the file just before reading it:

PRE_IDEAS () my = LIRE_MAILLAGE ()

4.2. Assign modeling data to the mesh#

To build the modeling of a mechanical, thermal or acoustic problem, it is essential to assign to the topological entities of the mesh:

  • a finite element model,

  • the properties of materials (law of behavior and parameters of the law),

  • complementary geometric or mechanical characteristics,

  • boundary conditions or loads.

These assignments are obtained by various operators whose names are prefixed with « AFFE_ ». The syntax and operation of these operators use the facilities provided by the rules already mentioned above on the use of factor keywords.

4.2.1. Definition of a field of assignment#

To perform an assignment, it is essential to define an assignment domain by reference to the names of the topological entities defined in the mesh file. Five keywords can be used for this, depending on the operator specification:

  • refer to the whole mesh by

TOUT = “OUI”

  • assign to meshes by

MAILLE =( list of mesh names)

  • assign to mesh groups by

GROUP_MA =( list of mesh group names)

  • assign to nodes by

NOEUD = (list of node names)

  • assign to node groups by

GROUP_NO =( list of node group names)

4.2.2. Assign finite element type#

On the cells of the studied structure, which are at this stage only topological entities, it is essential to assign:

  • one or more phenomena to study: “MECANIQUE”, “THERMIQUE”, “ACOUSTIQUE”;

  • a finite element model compatible with the topological description of the mesh. This assignment induces an explicit list of degrees of freedom in each node and an interpolation law in the element.

To do this, we use the operator AFFE_MODELE [U4.41.01], which can be called several times on the same mesh. It uses the overload rule.

Note:

For a study with several phenomena treated (“MECANIQUE”, “ THERMIQUE “), it is essential to build a model for each phenomenon, by as many calls to AFFE_MODELE. On the other hand, for a given calculation (mechanical, thermal,…) one and only one model is needed.

To know the characteristics of the various finite elements available, refer to fascicles [U2-], and [U3-].

4.2.3. Assign material characteristics#

At this stage, it is necessary to assign material characteristics, and associated parameters, to each finite element of the model (except for discrete elements defined directly by a stiffness, mass and/or damping matrix). In other words, DEFI_MATERIAU is used to define a material and AFFE_MATERIAU is used to define a material field by combining the mesh. For a given calculation, one and only one material field is required.

You can also use the validated characteristics of the material catalog using the procedure INCLUDE_MATERIAU [U4.43.02].

A certain number of behavior models can be used: elastic, orthotropic elastic, thermal, acoustic, elastoplastic, elastoviscoplastic, damage. Note that it is possible to define several material characteristics for the same material: elastic and thermal, elasto-plastic, thermoplastic,…

4.2.4. Assign characteristics to items#

When using certain types of elements, for the “MECANIQUE” phenomenon, the geometric definition deduced from the mesh does not allow them to be completely described.

The missing characteristics must be assigned to the meshes:

for**shells*: the constant thickness on each mesh and a reference frame for the representation of the stress state,

for**beams, bars and pipes*: the characteristics of the cross section, and possibly the orientation of this section around the neutral fiber.

These operations are accessible by the operator AFFE_CARA_ELEM [U4.42.01]), which uses the overload rule to simplify the writing of the command.

Another possibility is offered by this operator: that of introducing, directly into the model, matrics of stiffness, mass or damping on POI1 meshes (or knots) or SEG2 meshes. These matrices correspond to the types of discrete finite elements with 3 or 6 degrees of freedom per node DIS_T or DIS_TR that must be assigned when calling the AFFE_MODELE operator.

4.2.5. Affect boundary conditions and loads#

In general, these operations are indispensable. They are carried out by several operators whose names are prefixed by AFFE_CHAR or CALC_CHAR. On the same model, it is possible to make several calls to these operators to define, as the study progresses, boundary conditions and/or loads.

The operators used differ with the phenomenon:

AFFE_CHAR_MECA real data only AFFE_CHAR_MECA_F function data “THERMIQUE” AFFE_CHAR_THER real data only AFFE_CHAR_THER_F function data “ACOUSTIQUE” AFFE_CHAR_ACOU real data only

In addition, it is possible to establish the seismic load to perform a relative motion response calculation with respect to the supports, using the CALC_CHAR_SEISME command.

Boundary and load conditions can be defined according to their nature:

  • at the knots,

  • on edge meshes (edge or face) or finite element support meshes, created in the mesh file. On these meshes the operator AFFE_MODELE has assigned the types of finite elements required.

For the detailed description of the operands of these operators and the rules for orienting the support cells (global coordinate system, local coordinate system or any coordinate system), refer to the documents [U4.44.01], [U4.44.02], and [], and [U4.44.04].

Boundary conditions can be treated in two ways:

by « elimination » of the imposed degrees of freedom (for linear mechanical models implementing only kinematic limit conditions (blocked degrees of freedom)* without a linear relationship. ** In this case, the boundary conditions will be defined by the command AFFE_CHAR_CINE.

  • by dualization [R3.03.01]. This method, thanks to its greater generality, makes it possible to deal with all types of boundary conditions (imposed degree of freedom, linear relationships between degrees of freedom,…); the method used leads to the addition of 2 multipliers of LAGRANGE for each imposed ddl or each linear relationship.

Each concept produced by calling these operators, of type AFFE_CHAR, corresponds to an inseparable system of boundary conditions and loads. In calculation commands, you can aggregate these concepts by providing a list of concepts of this type for operands CHARGE.

4.3. Perform calculations using global commands#

4.3.1. Analysis THERMIQUE#

To calculate the temperature field (s) corresponding to a linear or non-linear thermal analysis:

  • stationary (instant 0),

  • evolvable whose calculation times are specified by a list of reals defined in advance

The commands to use are:

  • THER_LINEAIRE for linear analysis [U4.54.01],

  • THER_NON_LINE for a non-linear analysis [U4.54.02],

  • THER_NON_LINE_MO for a steady-state mobile load problem [U4.54.03].

The calculations of the elementary and assembled matrices and vectors necessary for the implementation of the resolution methods are taken care of by these operators.

4.3.2. Analysis STATIQUE#

To calculate the mechanical evolution of a structure subject to a list of loads:

  • MECA_STATIQUE [U4.51.01]: linear behavior, with superposition of the effects of each load,

  • MACRO_ELAS_MULT [U4.51.02]: linear behavior, distinguishing the effects of each load,

  • STAT_NON_LINE [U4.51.03]: quasi-static evolution of a structure subjected to a history of loading in small or large transformations, made of a material whose behavior is linear or non-linear, with possible consideration of contact and friction.

If this mechanical calculation corresponds to a thermo-elasticity study, reference will be made to a instant of the thermal calculation already carried out. If the material has been defined with temperature-dependent characteristics, these are interpolated for the temperature corresponding to the requested calculation time.

For coupled thermohydromechanical problems, operator STAT_NON_LINE is used to simultaneously solve the 3 thermal, hydraulic and mechanical problems.

The calculations of the elementary and assembled matrices and vectors necessary for the implementation of the resolution methods are taken care of by these operators.

4.3.3. Analysis MODALE#

To calculate the eigenmodes and eigenvalues of the structure (corresponding to a vibration problem or a buckling problem).

CALC_MODES with OPTION among [“BANDE”, “CENTRE”, “”, “PLUS_”,” TOUT “] [U4.52.02]: calculation of eigenmodes by simultaneous iterations; eigenvalues and eigenvectors are real or complex;

  • CALC_MODES with OPTION among [“PROCHE”, “AJUSTE”, “”, “SEPARE”] [U4.52.02]: calculation of eigenmodes by inverse iterations; eigenvalues and eigenvectors are real or complex;

  • CALC_MODES with OPTION =” BANDE “and division of the band into several sub-bands [U4.52.02]: lightens the modal analysis by dividing the frequency interval into sub-intervals;

  • MODE_ITER_CYCL [U4.52.05]: calculation of the natural modes of a structure with cyclic repeatability from a base of real eigenmodes.

These operators first require the calculation of the matrices assembled with the command ASSEMBLAGE [U4.61.21] or ASSE_MATRICE [U4.61.22].

4.3.4. Analysis DYNAMIQUE#

To calculate the dynamic response, linear or non-linear, of the structure. Several operators are available. For example, we can cite:

DYNA_LINE [U4.53.05]: dynamic temporal response of a linear structure subjected to transient excitation, or in the frequency domain (harmonic), on a finite element basis or in generalized coordinates by modal recombination,

DYNA_VIBRA [U4.53.03]: dynamic temporal response of a linear structure subjected to transient excitation, or in frequency domain (harmonic), based on finite elements or in generalized coordinates by modal recombination. It can also deal with localized nonlinearities for modal-based transient response calculations.

These two operators can first calculate the calculation of the assembled matrices and vectors [U4.61-].

DYNA_NON_LINE [U4.53.01]: dynamic temporal response of a nonlinear structure subjected to transient excitation, which also calculates the assembled matrices and vectors.

4.4. The results#

The results produced by operators performing finite element calculations [U4.3-], [U4.4-] and [U4.5-] are of two main types:

  • or of the type cham_no or cham_elem (per node or per element) when it comes to operators producing only one field (for example RESOUDRE),

  • or of the RESULTAT type strictly speaking, which groups together sets of fields.

A field in a RESULTAT concept is identified:

  • by an access variable that can be:

  • a simple order number referring to the order in which the fields were arranged,

  • a parameter defined according to the type of concept RESULTAT:

  • frequency or mode number for a RESULTAT of the mode_meca type,

  • instant for a RESULTAT like evol_elas, temper, dyna_trans or evol_noli.

  • by a symbolic field name referring to the type of field: displacement, speed, state of constraint, generalized efforts,…

In addition to access variables, other parameters can be attached to a RESULTAT concept type.

The various fields are incorporated into a result concept:

  • either by the operator who created the concept, a global order (MECA_STATIQUE, STAT_NON_LINE,…) or a simple command (CALC_MODES, DYNA_LINE_TRAN,…),

  • or when executing a command that allows you to add a calculation option in the form of a field per element or a field at the nodes (CALC_CHAMP); we then explicitly say that we are enriching the concept:

4.5. Exploiting the results#

All the previous commands made it possible to build various concepts that can be used by calculation post-processing operators:

  • general post-processing operators (see fascicle [U4.81]), for example CALC_CHAMP, POST_ELEM, POST_RELEVE_T,

  • fracture mechanics operators (see fascicle [U4.82]), for example CALC_G,

  • metallurgy operator: CALC_META,

  • static mechanical post-treatment (see fascicle [U4.83]), for example POST_FATIGUE, POST_RCCM,

  • dynamic mechanical post-processing (see fascicle [U4.84]), for example POST_DYNA_ALEA, POST_DYNA_MODA_T.

  • extraction operators:

  • of a field in a result concept CREA_CHAMP [U4.72.04],

  • a generalized coordinate field for a dynamic calculation with a modal basis RECU_GENE [U4.71.03],

  • of a function of evolution of a component based on a result concept RECU_FONCTION [U4.32.03],

  • and the restoration of a dynamic response in the physical base REST_GENE_PHYS [U4.63.31],

  • an operator for post-processing functions or layers CALC_FONCTION that allows searches for peaks, extremes, linear combinations,… [U4.32.04].

Finally, two procedures IMPR_RESU [U4.91.01] and IMPR_FONCTION [U4.33.01] allow the printing and possibly the creation of files usable by other software packages, in particular for graphic visualization. In particular, we will remember the graphic visualization by PARAVIS, IDEAS,, GMSH, or GIBI regardless of the mesh tool used at the start.