5. Additional calculations and post-treatments#

5.1. Elementary matrix calculations: operator CALC_MATR_ELEM#

The operator CALC_MATR_ELEM (documentation [U4.61.01]) makes it possible to calculate elementary matrices assembled by the command ASSE_MATRICE (documentation [U4.61.22]).

The only matrices that can be calculated with pipe elements are the stiffness and mass matrices of the elements of the model:

These elementary matrix calculations are for example used to determine the natural frequencies of a thick cylindrical ring, in test case SDLS109G.

5.2. Element-based calculations: operator CALC_CHAMP#

The operator CALC_CHAMP (documentation [U4.81.04]) calculates fields to elements:

stresses, deformations, internal variables at the nodes;
equivalent values (not available for modeling TUYAU).

The post-treatment options for pipe components are presented below. For structures modelled by pipe elements, it is particularly important to know how the stress results are presented: the approach adopted in the*Code_Aster* consists in observing the stresses in a particular coordinate system linked to the element whose reference axis was defined in paragraph [§3.2.2]. This approach seems to be the most physical because, for a cylindrical structure, the constraints that are easiest to interpret are not the constraints in the Cartesian coordinate system but the constraints in cylindrical coordinates. In addition, this approach allows for greater flexibility of use.

CALC_CHAMP	TUYAU_3M	TUYAU_6M	Remarks
“SIEF_ELGA”
“SIEF_ELNO”
“SIGM_ELGA”
“SIGM_ELNO”
“EFGE_ELGA”
“EFGE_ELNO”
“EPSI_ELGA”
“EPSI_ELNO”
“VARI_ELNO”

SIEF_ELGA: calculation of the stresses per element at the points of integration of the element based on the displacements (Use only in elasticity), in the local coordinate system of the element.
SIEF_ELNO: calculation of the stresses per element at the nodes of the element from the constraints at the Gauss points, in the local coordinate system of the element.
SIGM_ELGA: calculation of the constraints per element at the integration points of the element from SIEF_ELGA in the local coordinate system of the element.
SIGM_ELNO: calculation of the constraints per element at the nodes of the element from SIGM_ELNO, in the local coordinate system of the element.
EFGE_ELGA: calculation of the generalized forces per element at Gauss points from the displacements, by integration starting from SIEF_ELGA, in the local coordinate system of the element.
EFGE_ELNO: calculation of the generalized forces per element at the nodes from the linear displacements and calculated by integration from SIEF_ELGA in non-linear mode, in the local coordinate system of the element.
EPSI_ELGA: calculation of the deformations per element at the points of integration of the element from the displacements, in the coordinate system local to the element (small deformations).
EPSI_ELNO: calculation of the deformations per element at the nodes of the element from the deformations at the points of Gauss, in the coordinate system local to the element (small deformations).
VARI_ELNO: calculation of the field of internal variables per element at the nodes using Gauss points, for all layers (in the SUP/MOY/INF thickness) and for all sectors in the element’s local coordinate system.

A single constraint tensor (or a single set of internal variables) is then obtained per node of each element, which allows graphical analysis (evolution of a component,…).

5.3. Node calculations: operator CALC_CHAMP#

The operator CALC_CHAMP (documentation [U4.81.04]) performs the calculation of the fields at the nodes by average and the calculation of the forces and reactions:

fields at the nodes: constraints, deformations, internal variables, equivalent values;
Option name: replace _ ELNO_ with _ NOEU_
Fields at nodes can be calculated by CALC_CHAMP

SIEF_NOEU, VARI_NOEU

forces and reactions:
based on the constraints, the balance: FORC_NODA (calculation of nodal forces based on the constraints at the integration points, element by element),
then by removing the load applied: REAC_NODA (calculation of the nodal forces of reaction to the nodes, based on the constraints at the integration points, element by element):

REAC_NODA = FORC_NODA - loads applied,

useful for load verification and for calculating results, moments, etc.

5.4. Quantity calculations on all or part of the structure: operator POST_ELEM#

The operator POST_ELEM (documentation [U4.81.22]) allows quantities to be calculated on all or part of the structure. The quantities calculated correspond to particular calculation options of the affected modeling.

		TUYAU_3M	TUYAU_6M	Remarks
“MASS_INER”

For TUYAU models, the only option currently available is the calculation, on each element, of the mass, inertia and the position of the center of gravity (option “MASS_INER”).

5.5. Quantity field component values: operator POST_RELEVE_T#

For TUYAU models, the POST_RELEVE_T operator (documentation [U4.81.21]) can be used to, on a line, extract values (for example SIEF_ELNO). The product concept is a table type.

Important note:

If you come from an interface with a mesher (PRE_GIBI, * PRE_IDEAS, , PRE_GMSH), the nodes of a groupno are arranged in numerical order. The nodes must be reordered along the stripping line. The solution is to use the operator DEFI_GROUP with the option NOEU_ORDO. This option allows you to create a GROUP_NOordonné containing the nodes of a set of meshes made up of segments (SEG2, SEG3ou * SEG4) .

An example of component extraction is given in test case SSNL503 (see description in paragraph [§6.2]):

TAB_DRZ = POST_RELEVE_T (ACTION =_F (

GROUP_NO = “D”,

INTITULE = “TB_DRZ”,

RESULTAT = RESUL,

NOM_CHAM = “DEPL”,

NOM_CMP = “DRZ”,

TOUT_ORDRE = “OUI”,

OPERATION = “EXTRACTION”

)

)

The purpose of this syntax is:

to extract:	OPERATION = “EXTRACTION”
on line (the group of nodes) D:	GROUP_NO = “D”
the DRZdu displacement component:	NOM_CHAM = “DEPL”, NOM_CMP = “DRZ”,
for all calculation times:	TOUT_ORDRE = “OUI”