1. Static

1.1. Constraints

Cauchy’s postulate is that the contact forces exerted at one point by one part of a continuous medium on another only depend on the normal to the surface at this point delimiting the parts.

In accordance with this postulate, we call stress vector, for non-micropolar environments, \(\text{F}\left(\text{n}\right)\) the vector that characterizes the contact forces exerted through a surface element \(\mathit{dS}\) of normal \(\text{n}\) on a part of a continuous medium [bib 1] _.

We demonstrate [bib3] _, then, that the dependence at a fixed point of \(\text{F}\) on the normal \(\text{n}\) is linear and that there is a tensor called stress tensor \(\sigma\) such that:

\(\text{F}\left(\text{n}\right)=\sigma \text{n}\)

The unit of constraints in the international system is \(\text{N}\mathrm{.}{\text{m}}^{-2}\equiv \text{Pa}\).

For the entire structure, the « stress state » is characterized by a stress tensor field, which is more simply referred to as a stress field.

1.2. Effort

With regard to the structures of beams or shells, contrary to the case of the continuous medium, it should be noted that:

• only the normal \(\text{n}\) directions of cuts according to the space tangent to the manifold are possible,

• the characteristic quantities are obtained by integrating the quantities defined for continuous media into the section or thickness.

1.2.1. Case of the Discretes

Discretes are finite elements that may not have a physical dimension. They are represented by their stiffness matrix. The efforts are obtained by multiplying this matrix by the displacement vector:

\((\begin{array}{c}F\\ M\end{array})=\left[k\right]\text{.}(\begin{array}{c}D\\ R\end{array})\)

1.2.2. Case of beams

We call effort, the elements of reduction \(\left(F,M\right)\) in \(P\), the geometric center of inertia of the straight section \(\Sigma\), of the torsor resulting from the contact forces exerted on the section [bib2] _.

With the previous notations:

\(\begin{array}{ccc}F& ={\int }_{\Sigma }\text{F}(\tau )\text{ds}& (N)\\ {M}_{p}& ={\int }_{\Sigma }\text{PM}\wedge \text{F}(\tau )\text{ds}& (N\text{.}m)\end{array}\)

Force \(F\) breaks down into a normal force \(N\) and shear forces \(T\) in the plane of the section while the moment \(M\) at point \(P\) breaks down into a twisting moment and bending moments at point \(P\). The fuel assembly skeleton elements (R3.08.08) also carry the moments of grids \({M}_{g}\), with a formulation equivalent to \(M\).

For beams whose cross section is not considered to be rigid, these elements of reduction are not sufficient: for example, for beams taking into account the warping of the sections, one has to consider an additional quantity of force due to warping (the bimoment).

Multifibre beams (with 1D local behavior, connecting stresses to deformations, at a certain number of points in the section) and pipes (local behavior in plane stresses) provide both the elements of reduction of the beams but also a stress field for each fiber or sector.

1.2.3. Case of shells

Either a point \(P\) of a \(S\) surface medium of thickness \(h\), or an element of length \(\mathrm{dl}\) by \(S\), or \(n\) the normal orienting the shell at this point.

Let the elements of reduction \(\left(F,M\right)\) be at this point of a torsor resulting from the forces exerted through a surface element \(\mathrm{dS}=h\mathrm{dl}\) with a normal \(n\) tangent to \(S\) on a part of \(S\).

With the previous notations:

\(\begin{array}{ccc}F(P)& =\underset{-h/2}{\overset{+h/2}{\int }}\text{F}(\nu )\text{dh}& (N)\\ M(P)& =\underset{-h/2}{\overset{+h/2}{\int }}\text{PM}\wedge \text{F}(\nu )\text{dh}& (N\text{.}m)\end{array}\)

It is clear that \(M\) is in the tangential plane to \(S\) in \(P\).

Let \(N\left(P\right)\) be the projection of \(F\left(P\right)\) on the tangent plane to \(S\) in \(P\) and let, \(T(P)\) be its normal component to this tangent plane.

In the same way as for continuous media, it is shown that there are two symmetric tensors \(\text{N}\) and \(\text{M}\) and a vector \(Q\), defined in the tangential plane to \(S\), such as:

\(\begin{array}{}\text{F}=N\nu \\ T=Q\cdot \nu \\ \text{M}=\text{n}\wedge M\nu \end{array}\)

\((N,M,Q)\) are called the efforts at point \(P\):

• tensor \(N\) characterizes membrane forces,

• the \(M\) tensor the flexing moments,

• the \(Q\) vector: shear forces.

Notes:

• There are no universal conventions on the naming and signs of these tensors. In particular, the flexing moment tensor is sometimes taken with an inverse sign in the teaching and practice of French civil engineering engineers. Our convention is used in major finite element codes and allows for the same sign for a beam and a plate such as* \(\tau =\nu\).

• For non-linear materials, the law of behavior is evaluated at several points in the thickness but the equilibrium equations always relate to the force fields. It is not necessary to go back to the constraints to define the « stress state ».

Links with the constraint field

Under these conditions, let’s say a coordinate system whose third component is carried by \(\text{n}\), we have (\(\alpha ,\beta \mathrm{=}1\text{ou}2\)):

\(\begin{array}{ccc}{N}_{\alpha \beta }& \mathrm{=}{N}_{\beta \alpha }& \mathrm{=}\underset{\mathrm{-}h\mathrm{/}2}{\overset{+h\mathrm{/}2}{\mathrm{\int }}}{\sigma }_{\alpha \beta }\text{dh}\\ {M}_{\alpha \beta }& \mathrm{=}{M}_{\beta \alpha }& \mathrm{=}\underset{\mathrm{-}h\mathrm{/}2}{\overset{+h\mathrm{/}2}{\mathrm{\int }}}{x}_{3}{\sigma }_{\alpha \beta }\text{dh}\\ {Q}_{\alpha }& & \mathrm{=}\underset{\mathrm{-}h\mathrm{/}2}{\overset{+h\mathrm{/}2}{\mathrm{\int }}}{\sigma }_{\alpha 3}\text{dh}\end{array}\)

1.3. Nodal forces

We call equivalent nodal force or more simply nodal force, a vector \(F\) which is the representative of a linear form \(W\) (generally linked to an energy) acting on displacement fields \(u(x)\) discretized by finite elements.

The displacement fields \(u(x)\) are expressed from its nodal values that form a vector \(q\) and form functions \({\Phi }_{i}(x)\) by:

\(u\left(x\right)=\sum _{i}{q}_{i}{\mathrm{\Phi }}_{i}\left(x\right)\)

Under these conditions:

\(w\left(u\right)=\sum _{i}{q}_{i}{F}_{i}\)

Notes:

• The concept of knot here is very general and means, in fact, a carrier of degrees of freedom (whether Lagrange or Hermite).

• The concept of displacement is also very general and includes the concept of generalized displacement including translations and rotations.

1.4. Representation of fields

There are several ways to represent fields in a finite element modelling:

• for continuous fields throughout the domain, values at the nodes are used (CHAM_NO from Code_Aster)

\(u\left(x\right)=\sum _{i}{u}_{i}{\mathrm{\Phi }}_{i}\left(x\right)\)

we then speak of movements at the nodes, of constraints at the nodes or of forces at the nodes,

Note:

Stress or force fields are generally calculated at Gauss points, if they are represented continuously it is only for visualization purposes.

For the other fields, the values at certain characteristic points of the elements are used (Gauss points or nodes).

We then speak of constraints by elements at the nodes or forces by elements at the nodes, or even of constraints at Gauss points or forces at points of Gauss.

Note: axisymmetric models

For axisymmetric models, the axis of revolution is axis \(Y\) of the mesh. All the solid is meshed in \(X\ge 0\). The \(\mathit{Ox}\) axis therefore designates the radial direction. The components of the calculated fields will therefore be: \(X\) for the radial direction, \(Y\) for the axial direction, \(Z\) for the orthoradial (circumferential) direction.

1.5. Related quantities in Code_Aster

1.5.1. SIEF_R

The quantity SIEF_R represents the « stress state » of the structure, so it contains, at a minimum, the components:

• constraint fields for continuous environments (as a global reference frame):

  SIXX, SIYY, SIZZ, SIXY,, SIXZ, SIYZ

• beam and discrete force fields (in « user » coordinate system at the beam, at the discrete level):

  N, VY, VZ, MT, MFY, MFZ,, MGX, MGY, MGZ

• for beams with warping, you must add the bimoment (necessarily as a « user » coordinate system to the fiber):

  BX

• shell force fields (necessarily as a « user » reference point on the surface):

  NXX, NYY, NXY, MXX, MYY,,, MXY, QX, QY

In addition, it is sometimes convenient to be able to directly exploit the beam and discrete force fields in the global coordinate system:

FX, FY, FZ, MX, MX, MY, MZ

It is also interesting to represent the components of a stress field on the elements of beams or shells in the « user » coordinate system. To do this, the same components as in a global frame of reference will be used, although confusion is possible.

1.5.2. FORC_F and FORC_R

These quantities represent the forces applied to the structure on an interface.

For:

• a continuous medium is therefore a force vector,

• a beam, a force torsor,

• a shell, a force torsor.

This quantity must therefore have the following components:

• for a continuous environment:

  FX, FY, FZ

• more for beams and shells:

  MX, MY, MZ

1.5.3. DEPL_R

Given that,

• a field can only be attached to one quantity,

• that mixed finite element methods (mixing displacement-type unknowns and nodal forces-type unknowns) are not excluded,

• that the dualization of boundary conditions leads to the unknown being a vector containing Lagrange variables which are nodal forces in the sense specified above,

• that it is necessary to be able to perform any type of linear combination on nodal forces,

• that the numbering of the unknowns must be the same as that of the second members,

nodal forces (dual in the sense of the energy \(W\) of nodal movements) necessarily have the same components as the displacements, namely:

DX, DY, DZ, DRX, DRY,,, DRZ,,, DRGX, DRGY, DRGZ

plus, for beams with warping, the degree of freedom associated with the bimoment: GRX.

1.6. Calculation options

1.6.1. Calculation of the stress state

1.6.1.1. Field SIEF_ELGA

This is the field representing the stress state and allowing calculations to be carried out (geometric rigidity, nodal forces, etc.). It is expressed at Gauss points (and is possibly at sub-points for structural elements). The prefix for this field is SIEF, because depending on the element, it contains constraints or efforts.

(*) for plate and shell elements, the « user » coordinate system is the one defined from the user’s data (keyword ANGL_REP or VECTEUR in AFFE_CARA_ELEM/COQUE).

So these options calculate:

• the field of constraints for 2D and 3D continuous media elements, and elements with local behavior: COQUE_3D, plates, 1D shells (COQUE_AXIS, COQUE_D_PLAN, COQUE_C_PLAN), pipes, multifibre beams, at each « sub-point » of integration (layers in the thickness of the shells, fibers, angular sectors and position in the thickness for the pipes). The « user » coordinate system for plates and shells can be specific to each element.

• the force field for the beams (twister).

1.6.1.2. Field SIGM_ELGA

This is the field representative of the stress state at the Gauss points (or possibly at the sub-points for structural elements). The prefix for this field is SIGM because this field only contains constraints. It is an extraction of the constraints contained in field SIEF_ELGA.

1.6.2. Other representations of the stress state

1.6.2.1. Field SIEF_ELNO and SIEF_NOEU

These are fields representative of the stress state for exploitation purposes (printing or post-processing visualization) at the nodes per element (or possibly at the subpoints for structural elements) and at the nodes of the element. Depending on the elements, they contain constraints or efforts.

1.6.2.2. Field SIGM_ELNO and SIGM_NOEU

It is a field representative of the stress state for exploitation purposes (printing or post-processing visualization) at the nodes per element (or possibly sub-points for structural elements) and at the nodes of the element. The prefix for this field is SIGM because this field only contains constraints.

Notes:

• In this case, confusion is possible between the components in the user coordinate system and those in the global coordinate system that have the same name.

• The 6 components delivered in the local references by the beams and shells possibly contain null terms depending on the models used. For the most standard models:

  • three zero terms for beams,

  • two null terms for shells.

Thus, the stress field will be complete and, above all, it can be enriched whenever the modeling requires it (beam with shear, shell with pinch, etc…).

1.6.2.3. Field EFGE_ELGA, EFGE_ELNO, and EFGE_NOEU

These are fields containing the forces on the beam or shell elements for exploitation purposes (printing or post-processing visualization) at Gauss points, element-by-element nodes, and nodes.

1.6.3. Calculation of nodal forces and generalized reactions

The generalized nodal forces are calculated from the stress state, only one option is provided:

Calculation option	Symbolic concept name RESULTAT	Calculation performed	Massive elements (3D, 2D)	Beam, discrete elements	Shell
FORC_NODA	same	from field SIEF_ELGA	Forces	Forces	Forces and moments	Forces and moments

Nodal forces (dual in the sense of the energy \(W\) of nodal movements) have the same components as displacements, namely:

DX, DY, DZ, DRX, DRY, DRZ

Option REAC_NODA of the CALC_CHAMP operator makes a call to FORC_NODA and subtracts:

• static loading,

• loading, inertial and viscous forces in dynamics (in fact, the viscous contribution in dynamics is currently overlooked in CALC_CHAMP).

For massive elements, FORC_NODA in general have the dimension of a force. This is a field on mesh nodes where the value in a node is obtained from the constraints calculated on the elements competing with this node, so their values therefore vary when the mesh changes. In the absence of distributed loading, equilibrium imposes their nullity in an internal node, while they correspond to the reaction on the supports where a kinematic relationship is imposed (case of an imposed displacement).

In the case of shells, the components DX, DY and DZ give the FORC_NODA values (the dimensions of a force) in the global coordinate system of the mesh. These components are built with normal and sharp forces in the shell. The components DRX, DRY and DRZ give the FORC_NODA (moment dimensions) in the global coordinate system of the mesh, constructed with the bending moments in the shell.