4. Resolution#

4.1. Linear calculations: MECA_STATIQUE and other linear operators#

Linear calculations are performed in small deformations. Several linear resolution operators are available:

  • MECA_STATIQUE: solving a linear static mechanics problem [U4.51.01],

  • MACRO_ELAS_MULT: calculate linear static responses for different load cases or Fourier modes [U4.51.02],

  • CALC_MODES: calculation of eigenvalues and vectors by methods of subspaces or inverse iterations [U4.52.02],

  • MODE_ITER_CYCL: calculation of the natural modes of a cyclic symmetric structure [U4.52.05],

  • DYNA_LINE_TRAN: calculation of the transient dynamic response to any temporal excitation [U4.53.02].

By default, the only calculated fields are the displacement fields DEPL and the constraint fields SIEF_ELGA. Other fields are available through the OPTION operand (see the options available in paragraph [§5.2] on the use of CALC_CHAMP).

4.2. Nonlinear calculations: STAT_NON_LINE and DYNA_NON_LINE#

4.2.1. Behaviors and deformation hypotheses available#

The following information is taken from the documentation for using the STAT_NON_LINE operator: [U4.51.03].

STAT_NON_LINEDYNA_NON_LINE

TUYAU_3M **** TUYAU_6M **

COMPORTEMENT

RELATION

all behaviors available in C_ PLAN

DEFORMATION

PETIT

,

Incremental behavior relationships (keyword factor COMPORTEMENT) based on the hypothesis of small displacements and small deformations (keyword DEFORMATION = “PETIT”) are the only mechanical non-linear behavior relationships available for modeling TUYAU. These behavioral relationships relate deformation rates to stress rates. The nonlinear behaviors supported are those already existing in plane constraints defined in operators STAT_NON_LINE and DYNA_NON_LINE. In addition, with the De Borst method [R5.03.03], all 2D behaviors (D_ PLAN, AXIS) in small deformations can be used.

STAT_NON_LINE’s RESULTAT concept contains fields of constraints, displacement, and internal variables at integration points that are always calculated at gauss points:

  • SIEF_ELGA: Constraint tensor per element at the integration points in the element’s local coordinate system,

  • VARI_ELGA: Field of internal variables per element at the integration points in the local coordinate system of the element,

  • DEPL: travel fields.

In addition, a call to operator CALC_CHAMP allows access to other fields. In particular, it is possible to pass constraints and internal variables from Gauss points to nodes to form fields SIEF_ELNO and VARI_ELNO (see paragraph [§5.2]).

A field VARI_… can have several types of components. For example, the components of field VARI_ELNO are, for elements TUYAU:

\(K\) times: \((\mathrm{V1},\mathrm{V2},\dots \mathrm{..}\mathrm{Vn})\)

Where:

\(K\) is the total number of integration points \(K=(2\times \mathrm{NCOU}+1)\times (2\times \mathrm{NSEC}+1)\) \(N\) is the number of internal variables and depends on behavior.

4.2.2. Details on integration points#

For linear and non-linear calculations, numerical integration is carried out with a method of:

  • Gauss along the middle fiber.

The number of integration points is set to 3. For a mesh whose vertices are 1 and 2 and numbered from 1 to 2, the 3 gauss points are such that the first is close to 1, the second is at an equal distance from 1 and 2 and the third is closer to 2. It is therefore necessary to pay attention to the orientation of the cells when looking at the results at Gauss points 1 and 3. In fact, if you change the orientation of the cell and if you number it from 2 to 1, the first Gauss point is closer to 2.

  • Simpson in thickness and on circumference:

  • Thickness integration is a Simpson integration at 3 points per layer. The number of integration points per layer is fixed to 3, in the middle of the layer, in the upper skin and in the lower skin of the layer, the two end points being common with the neighboring layers.

  • The integration according to the circumference is a Simpson integration by sector, each sector being from angle \(2\pi /\mathrm{NSEC}\). \(\Phi\) is the angle between the generator and the center of the sector. The number of integration points per sector is set to 3, in the middle of the sector, in the upper (\(\Phi +2\pi /\mathrm{NSEC}\)) and lower (\(\Phi \mathrm{-}2\pi \mathrm{/}\mathit{NSEC}\)) parts of the sector, the two end points being common with the neighboring sectors.

The number of layers and the number of sectors must be defined by the user using the keywords: TUYAU_NCOU, TUYAU_NSEC and the AFFE_CARA_ELEM operator.

For example, with 3 layers and 16 sectors, the number of integration points per element is \((2\times \mathrm{NCOU}+1)\times (2\times \mathrm{NSEC}+1)\times \mathrm{NPG}\), which gives 693 integration points. For each gauss point along the length of the element, information on the layers is stored and for each layer on all sectors. If we want information at the Gauss point \(\mathrm{NG}\), on layer \(\mathrm{NC}\) level \(\mathrm{NCN}\) (\(\mathrm{NCN}=–1\) if lower, \(\mathrm{NCN}=0\) if middle, \(\mathrm{NCN}=+1\) if higher), on sector \(\mathrm{NS}\), level \(\mathrm{NSN}\) (\(\mathrm{NSN}=–1\) if lower, \(\mathrm{NSN}=0\) if lower, if middle, \(\mathrm{NSN}=+1\) if higher), then we look at the values we are looking for at the integration point:

\(\begin{array}{cc}\mathrm{NP}\text{=}& (\mathrm{NG}-1)\times (2\mathrm{NCOU}+1)\times (2\mathrm{NSEC}+1)\\ & +(2\times \mathrm{NC}+\mathrm{NCN}-1)\times (2\mathrm{NSEC}+1)+(2\times \mathrm{NS}+\mathrm{NSN})\end{array}\).

4.3. Dynamic calculations#

For dynamic calculations, no specificity due to finite element TUYAU exists.