4. Operands#
4.1. Keyword DEFINITION#
◊ DEFINITION
This keyword factor (not repeatable) is used to define the macro element.
4.1.1. Operand MODELE#
« Static substructuring » case:
Name of the model you want to condense. The matrices (and loads) that we condense are always calculated on the model as a whole. When you want to condense several subsets of the same mesh, you must therefore create several models on different mesh groups.
« Structural modification » case:
Name of the model given in the MODELE_CALCUL keyword of the PROJ_MESU_MODAL command associated with repgenedu keyword PROJ_MESU. This model serves as a support for the expansion of the measurement to the « external » nodes.
4.1.2. Operand CHAM_MATER#
The name of the material field associated with the model. This argument is useless if the model contains only discrete elements and static substructures. If not, it is mandatory.
4.1.3. Operand CARA_ELEM#
Name of the basic characteristics if the model includes beam, plate, or shell elements.
4.1.4. Operands CHAR_MACR_ELEM/INST#
This argument is used to define:
the thermal load which possibly modifies the characteristics of the material, when they depend on the temperature; the moment of thermal evolution will be specified if necessary (keyword INST),
the kinematic conditions applied to the**internal nodes* (cf. keyword EXTERIEUR) of the macro element.
During a calculation for which the characteristics of the material depend on the temperature, the temperature field to be used is specified here. The field used is the one corresponding to the instant inst of the thermal evolution referenced in the list of lchar loads (refer to the command CALC_MATR_ELEM (“RIGI_MECA”)) [U4.61.01].
Notes on kinematic conditions:
In static substructuring operators, « Dirichlet » kinematic conditions are always dualized, never eliminated.
In general, kinematic conditions will be applied on external nodes at the upper level of substructuring. So they won’t appear in the loads lchar.
On the other hand, the kinematic conditions that must be given before condensation (lchar) are those that can no longer be given after:
conditions involving internal nodes (imposed ddls or linear relationships) because these nodes will be eliminated,
the conditions defined from the **edges of the finite elements (FACE_IMPO)* * because these finite elements will no longer exist after condensation.
Note on the argument lchar:
The loads that appear in the list lchar, are those that allow the stiffness and mass matrices to be calculated:
possible temperature load modifying the characteristics of the material,
**kinematic conditions (dualization) .*
on the other hand, these charges do not play a role in the definition of loads (second members) .
For example, expansions due to the temperature field will only be taken into account in a load case if the load containing this temperature field is explicitly given in the definition of this load case (keywords CAS_CHARGEet * CHARGE). In the same way the **non-zero kinematic conditions must be given again in the definition of load cases.*
4.1.5. Operands NMAX_CAS/NMAX_CHAR#
One gives here a majorant of the number of load cases that the user will define on the macro element (see argument CAS_CHARGE). This number is taken by default to 10.
One gives here a plus of the number of load concepts that will be assigned to each load case (Cfargument CAS_CHARGE). This number is taken by default to 10.
4.1.6. Operand PROJ_MESU#
repgene refers to the name of the concept resulting from the PROJ_MESU_MODAL [U4.73.01] command, which made it possible to define the measurement and the projection base.
4.1.7. Operand MODE_MESURE#
One gives here the name of the concept containing the eigenmodes identified experimentally. These specific modes make it possible to build the modal model of the initial structure which will then be condensed to the « external » nodes.
4.2. Keyword EXTERIEUR#
♦ EXTERIEUR =
This factor keyword (not repeatable) is used to define all the « external » nodes where the matrices and the loads will be condensed (the other nodes will be called « internal »). This keyword must appear in the first call to command MACR_ELEM_STAT (you define the exterior of a macro element all at once).
Each external node carries the same degrees of freedom as the corresponding node in the mo model. A macro element is topologically (and geometrically) entirely defined by all of its external nodes.
4.2.1. Notes on defining the « exterior » of a macro element#
The exterior of a macro element is the set of « external » nodes that define the topology and geometry of the macro element,
each « external » node carries**all**the degrees of freedom that exist on that node in the underlying model. The macroelements produced by*Aster can only be used by gluing their external nodes together and therefore all the degrees of freedom they carry. Other calculation codes operate differently. For certain models (sliding, articulation,…), we will have to step back some nodes and to use, at the higher level of substructuration, linear relationships between the degrees of freedom of the external nodes of several macro-elements,
when defining the external nodes of a macroelement, if a node appears several times, it is only counted once,
for programming reasons, there must be both external nodes and internal nodes: none of the families can be empty.
4.2.2. Operand GROUP_NO#
List the names of the groups of nodes that we want to be « external ».
4.4. Keyword CAS_CHARGE.#
◊ CAS_CHARGE
This factor keyword makes it possible to define a set of load cases named (keyword NOM_CAS). These load cases can be applied to the higher level model (CALC_VECT_ELEM [U4.61.02]).
In general, we will try to apply nodal loads (FORCE_NODALE) to the upper level of substructuring.
On the other hand, all the loads defined on the finite elements must be applied before any condensation: (PESANTEUR, ROTATION,, FORCE_FACE,,, FORCE_CONTOUR, FORCE_INTERNE, FORCE_COQUE, FORCE_POUTRE, PRES_REP,…) since these finite elements will have « disappeared » after condensation.
Note that for a macro-element, there is no concept of outline, orientation, face,…
4.4.1. Operand NOM_CAS#
The condensed loading under the name nocas (between « quotes ») corresponds to the load defined by the arguments of CHARGE and INST to which are systematically added the loads with the name nocas that may be present on the lower-level substructures contained in the mo model.
4.4.2. Operand SUIV#
This keyword says whether the load case « follows » the macroelement in its geometric transformations: translation, rotation, (cf. operator DEFI_MAILLAGE [U4.23.01]). For example, loading due to rotation (centrifugal force), pressure (or thwarted expansion) is « follower » because its direction is linked to the position of the substructure. On the other hand, gravity is a loading that is « non-tracking » (its direction is absolute).
Attention:
Kinematic loads are always « follower » because they are taken into account in the stiffness matrix (dualization) and this matrix is « follower » by nature.
4.4.3. Operands CHARGE/INST#
◊ INST = GST,
The keywords CHARGE and INST have the same meaning as in the CALC_VECT_ELEM [U4.61.02] operator.