4. Keyword COMPORTEMENT#

This key word factor helps to define behavioral relationships.

Most laws of behavior (especially in plasticity) are written incrementally, because the history of the material influences its behavior; if this is not the case we are dealing with elastic behaviors, linear or not. In the same calculation, it is possible to have certain parts of the structure obeying incremental behaviors, and other parts obeying various elastic behaviors.

It is the behavior that determines (through its catalog) the type of integration used. For example, behaviors CABLE, ELAS_HYPER, ELAS_POUTRE_GR, ELAS_VMIS_LINE,,,, ELAS_VMIS_TRAC, ELAS_VMIS_PUIS are integrated elastically (non-linearly) and not incrementally. As for ELAS behavior, both types of integration are possible

For the precise meaning of these different relationships, refer to the various Reference documentation as well as to the documentation in DEFI_MATERIAU [U4.43.01].

4.1. Modeling of plane stresses using the Borst method#

Some behavior models have not been developed under plane constraints. In this case, we automatically use the De Borst algorithm [R5.03.03] which allows the hypothesis of plane constraints to be taken into account at the level of the equilibrium algorithm (unlike behavior models developed explicitly in plane constraints, which take this hypothesis at the level of integration of laws of behavior). It is therefore also possible to assign any nonlinear law to structural elements DKT, COQUE_3D and TUYAU ). Again, it is necessary to use only the tangent matrix.

Likewise, for cases using a mono-dimensional constraint state (POU_D_EM, POU_D_TGM,,,, GRILLE,,, GRILLE_MEMBRANE, BARRE), in order to be able to use behaviors that have not been developed specifically in 1D, we automatically use a method similar to that of De Borst to integrate the behaviors available in 3D into 1D [R5.03.09].

The De Borst method is not available either for metallurgical behaviors or with DEFORMATION = “SIMO_MIEHE”.

When using MFront, De Borst mode is triggered automatically if the law has not been written in plane constraints. If MFront is used in « prototype » mode (keyword RELATION =” MFRONT “), it is up to the user to choose the operating mode (native plane constraints in MFront or by De Borst algorithm).

4.2. Local and non-local modeling#

In the case of softening behaviors, the response of a local behavior model with damage is dependent on the mesh. To overcome this difficulty, some models can be used non-locally. Any model written in non-local language results in the introduction of an additional material characteristic, the characteristic length. For some models, it is defined under the keyword factor NON_LOCAL of the DEFI_MATERIAU operator.

The response of non-local modeling is more independent of the mesh. There are three types of non-local laws, which can be activated in AFFE_MODELE by the MODELISATION keyword:

“3D_GRAD_VARI”, “D_PLAN_GRAD_VARI”, or “AXIS_GRAD_VARI”. These are non-local laws where the gradient of the internal variables of the local model intervenes (confer [R5.04.01]).
“3D_GVNO”, “D_PLAN_GVNO”, or “AXIS_GVNO”. Like the previous type, they are non-local laws where the damage gradient intervenes. The treatment of damage is now nodal, as the degree of freedom of the global system and no longer as an internal variable of the local model (confer [R5.04.04]).
“D_PLAN_2DG”, “D_PLAN_DIL” in addition to the model to be regularized (confer [R5.04.03]). It is a model regularized by a micro-structural approach where either the deformation field or the volume deformation intervenes.

4.3. Behavioral laws and control variables#

As a reminder, the model may include one or more control variables (temperature, drying, drying, irradiation, metallurgical phase, etc.), whose field is assigned to the mesh cells via the keyword AFFE_VARC of the AFFE_MATERIAU command (cf. [U4.43.03]).

A control variable can impact material properties, which are then a function of them.

In some cases, they can also generate deformation. This is the case of the following control variables: the temperature “TEMP”, the drying “SECH” (we then speak of desiccation shrinkage deformation), the hydration “HYDR” (endogenous shrinkage deformation) and the anelastic deformations” EPSAXX “,” EPSAYY “,” “,” “,”, “EPSAZZ EPSAXY EPSAXZ EPSAXZ “. These deformations are often called « thermal deformations » for a misnomer.

Depending on the way in which the law of behavior was developed, these deformations due to the control variables are taken into account using a generic mechanism. For other laws, they are taken into account in a specific way.

Currently, the generic code_aster mechanism covers the following scope:

calculation and consideration of thermal deformation with a thermal expansion coefficient ALPHA isotropic/anisotropic/transverse isotropic, and differentiable according to the metallurgical phase in the isotropic case;
calculation and consideration of desiccation shrinkage and endogenous shrinkage in the case where the material parameters controlling them, K_DESSIC and B_ENDOGE, are isotropic;
taking into account anelastic deformations.

This generic mechanism is only available for deformation measurements of the small deformation type (all but “SIMO_MIEHE”, i.e. “PETIT”, “PETIT_REAC”, “GDEF_LOG”, “GREEN_LAGRANGE” and in principle “GROT_GDEP” cf. § 4.6 — however it is not available for the latter kinematics). For example, this means that a control variable such as temperature cannot be used at the same time as a “SIMO_MIEHE” or “GROT_GDEP” kinematics with the generic mechanism.

Note that laws such as MFront and UMAT follow the generic mechanism.

4.4. Operand RELATION#

4.4.1. Elastic models#

Unless otherwise specified, all models may include temperature dependence. Moreover, they are all integrated purely implicitly.

4.4.1.1. Behaviors ELAS, ELAS_ISTR, ELAS_ORTH, and ELAS_GLRC#

« Linear » elastic behavior relationship, that is, the relationship between the deformations and the stresses under consideration is linear. Under certain conditions this relationship becomes incremental: it then makes it possible to take into account initial movements and constraints; behavior ELAS is therefore by default non-incremental, except in the following cases:

if there is an initial state (ETAT_INIT, SIGM_INIT)
if DEFORMATION = PETIT_REAC
if the order is CALCUL.

If necessary, if these exceptions are not enough we can force an incremental elastic behavior using VMIS_ISOT_LINE for example, with a high elastic limit. Likewise, you can force hyperelasticity by taking ELAS_VMIS_LINE, with a high elastic limit.

The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the following keywords:

ELAS (_FO), as far as isotropic elasticity is concerned,
ELAS_ISTR (_FO), with respect to transverse isotropic elasticity,
ELAS_ORTH (_FO), with respect to orthotropic elasticity.
ELAS_GLRC (_FO), with respect to the elasticity of the plate elements DKTG and Q 4GG.

The material parameters defined in ELAS are used for a certain number of behaviors, and also for calculating the elastic stiffness matrix (PREDICTION =” ELASTIQUE “or MATRICE =” ELASTIQUE” under the keyword NEWTON cf [U4.51.03]).

Supported models: 3D, 2D, CONT_PLAN, DISCRET,,,,, INCO_UPG,,,,,,,,,, INCO_UP, POU_*, ,, *, Q CONT_1D CONT_1D PMF SHB CABLE CABLE_POULIE COQUE_3D DKTG 4GG.
Number of internal variables: 1
Meaning: \(\mathit{V1}\): empty so it’s always zero

4.4.1.2. Behavior ELAS_HYPER#

A « nonlinear » hyperelastic behavior relationship, that is, the relationship between stresses is the derivative of a hyper-elastic potential with respect to Green deformations. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ELAS_HYPER. This relationship is only supported in HPP and in Green-Lagrange kinematics (DEFORMATION =” PETIT “or” GREEN_LAGRANGE “).

Supported models: 3D, D_PLAN
Example: see test SSNV187
Reference documentation: R5.03.19

Note: this behavior cannot take into account thermal deformations.

4.4.1.3. Behavior ELAS_HYPER_VISC#

« Non-linear » visco-hyperelastic behavior relationship. The hyper-elastic part is defined by the deformation potential of Signorin (same as ELAS_HYPER). Viscous flow is taken into account by adding a Prony series of order n to the second Piola Kirchoff tensor. PK2. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ELAS_HYPER. This relationship is only supported in HPP and in Green-Lagrange kinematics (DEFORMATION =” PETIT “or” GREEN_LAGRANGE “).

Supported models: 3D, D_PLAN
Example: see test SSNV518 and SSNV519
Reference documentation: R5.03.19

4.4.1.4. Behavior ELAS_VMIS_LINE#

VonMises’s « nonlinear » elastic behavior relationship (Hencky’s law) with linear isotropic work hardening. The necessary data for the material field are provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ECRO_LINE and ELAS (see [R7.02.03] for more details of its use in fracture mechanics).

Supported models: 3D, 2D, C_PLAN
Example: see test SSNP110
Reference documentation: R5.03.20

Note: this behavior is unusable with a state of non-zero initial constraints. It should therefore not be used as a second time.

4.4.1.5. Behavior ELAS_VMIS_TRAC#

VonMises’s « nonlinear » elastic behavior relationship (Hencky’s law) with nonlinear isotropic work hardening defined by a tensile curve. The necessary data for the material field are provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords TRACTION and ELAS (see [R7.02.03] for more details of its use in fracture mechanics).

Supported models: 3D, 2D and C_PLAN
Example: see test SSNV108
Reference documentation: R5.03.20

Note: this behavior is unusable with a state of non-zero initial constraints. It should therefore not be used as a second time.

4.4.1.6. Behavior ELAS_VMIS_PUIS#

VonMises’s « nonlinear » elastic behavior relationship (Hencky’s law) with nonlinear isotropic work hardening defined by a power function. The parameters are provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ECRO_PUIS and ELAS.

Supported models: 3D, 2D
Example: see test COMP001I
Reference documentation: R5.03.20

Note: this behavior is unusable with a state of non-zero initial constraints. It should therefore not be used as a second time.

4.4.1.7. Behavior ELAS_POUTRE_GR#

Elastic behavior relationship for beams with large displacements and large rotations (DEFORMATION =” GROT_GDEP “is mandatory). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword ELAS or ELAS_FO (Cf. [R5.03.40] for more details).

Supported models: POU_D_T_GD
Internal variables (not of interest to the user, but necessary for operation): 3
Example: see test SSNL103

4.4.1.8. Behavior CABLE#

Elastic behavior relationship adapted to cables (DEFORMATION =” GROT_GDEP “mandatory): the Young’s modulus of the cable may be different in compression and in tension (in particular it may be zero in compression). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword CABLE (confer [R3.08.02] for more details).

Supported models: CABLE
Example: see test HSNL100

4.4.1.9. Behavior ELAS_MEMBRANE_SV#

Hyper-elastic Saint Venant Kirchhoff behavior relationship adapted to membranes (DEFORMATION =” GROT_GDEP “mandatory, confer [R3.08.07] for more details). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword ELAS. This relationship cannot include a temperature dependence.

Supported models: MEMBRANE
Example: see test SSNS115

4.4.1.10. Behavior ELAS_MEMBRANE_NH#

Neo-hookean hyper-elastic behavior relationship adapted to membranes (DEFORMATION = “GROT_GDEP” mandatory, confer [R3.08.07] for more details). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword ELAS. This relationship cannot include a temperature dependence.

Supported models: MEMBRANE
Example: see test SSNS115

4.4.1.11. Behavior CZM_ELAS_MIX#

Elastic cohesive behavior relationship, cf. [R7.02.11], modeling the opening and elastic sliding of an interface. This law can be used with the finite interface element based on a mixed formulation in augmented Lagrangian (see [R3.06.13]) and makes it possible to introduce a cohesive force through the interface in open and sliding mode. This law can in particular be used to verify the data of a study before moving on to an interface damage model (cracking). The required data is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword CZM_ELAS. It is also possible to choose to apply perfect adhesion conditions in the normal and/or tangential direction (the corresponding rigidities are then of no effect, perfect adherence corresponding to infinite stiffness). Finally, it is also possible to adopt unilateral behavior in the normal direction: contact when closing, elasticity when opening. In this last configuration, the model becomes non-linear.

Supported models: all INTERFACE models (see U3.13.14).
Number of internal variables (for post-processing purposes): 3

V1: normal movement jump, V2: tangential jump in the first direction, V3: tangential jump in the second direction (zero in 2D).

Examples: see test SSLV01.

4.4.2. Elastoplastic models#

4.4.2.1. Behavior VMIS_ISOT_TRAC#

Relationship of the elastoplasticity behavior of VonMises to nonlinear isotropic work hardening. The curve \((\sigma ,\varepsilon )\) in simple traction is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword TRACTION (Cf. [R5.03.02] for more details). It is possible to define several traction curves depending on the temperature. You must also enter the keyword ELAS (_FO) in the DEFI_MATERIAU operator. In the case where a traction curve is provided, the YOUNG module used for the behavior relationship is the one calculated from the first point of the traction curve, the one used for the calculation of the elastic matrix (see keyword NEWTON [U4.51.03]) is the one given in ELAS (_FO). Example: see test FORMA03.

Local models supported: 3D, 2D, INCO_UPG, 2D,,, INCO_UP,, C_PLAN, CONT_1D, CONT_1D (PMF), SHB. Large SIMO_MIEHE deformations are available for this behavior.
Number of internal variables: 2
\(\mathrm{V1}\): cumulative plastic deformation,
\(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, 1 for plastic).

Example: test SSNV501, SSNV156.

4.4.2.2. Behavior VMIS_ISOT_PUIS#

Relationship of the elastoplasticity behavior of VonMises to nonlinear isotropic work hardening defined by a power function. The parameters are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword ECRO_PUIS (confer [R5.03.02] for more details). You must also enter the keyword ELAS (_FO) in the DEFI_MATERIAU operator.

Supported models: 3D, 2D, C_PLAN, CONT_1D, INCO.
Number of internal variables: 2
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, 1 for plastic).
Large SIMO_MIEHE deformations are available for this behavior.

Example: see test COMP002.

4.4.2.3. Behavior VMIS_ISOT_LINE#

Relationship of the elastoplasticity behavior of VonMises to linear isotropic work hardening. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01] under the keywords ECRO_LINE (_FO) and ELAS (_FO) (Cf. [R5.03.02]).

Local models supported: 3D, 2D, C_PLAN, 2D,,, CONT_1D,, CONT_1D (PMF), INCO_UPG, INCO_UP.
Number of internal variables: 2
Meaning (except modeling BARRE): \(\mathrm{V1}\):: cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, 1 for plastic).

Example: see test SSNP156.

Large SIMO_MIEHE deformations are available for this behavior.

Supports method IMPL_EX; in this case, the variable \(\mathrm{V2}\) represents the cumulative plastic deformation increment divided by the time increment (i.e. an approximation of \(\dot{p}\)

4.4.2.4. Behavior VMIS_ISOT_NL#

Relationship of the elastoplasticity behavior of VonMises to nonlinear isotropic work hardening (combination of an affine term, two exponential terms and a power term). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01] under the keywords ECRO_NL (_FO) and ELAS (_FO) (Cf. [R5.03.33]).

Local and GRAD_VARI models supported: 3D, D_PLAN, AXIS
Number of internal variables: 8
Meaning: \(V1\): work-hardening variable (generally cumulative plastic deformation), \(V2\): plasticity indicator (see Note 1) (0 for elastic, 1 for plastic with regular flow, 2 for plastic with singular flow), \(V3\) to \(V8\): components of plastic deformation.

Example: see test SSNV263.

The large GDEF_LOGsont deformations available for this behavior.

Compatible with models GRAD_VARI and GRAD_INCO.

4.4.2.5. Behavior VMIS_JOHN_COOK#

Von Mises elastoplasticity behavior relationship with nonlinear isotropic work hardening defined by the Johnson-Cook law. The parameters are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword ECRO_COOK (Cf. [R5.03.02] for more details). You must also enter the keyword ELAS (_FO) in the DEFI_MATERIAU operator.

Supported models: 3D, 2D, C_PLAN,, CONT_1D, INCO_UPG, INCO_UP.
Number of internal variables: 5
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic), \(\mathrm{V3}\): anelastic deformation increment, \(\mathit{V4}\): time increment,: time increment, \(\mathit{V5}\): mechanical dissipation speed.

Example: see test COMP002.

4.4.2.6. Behavior VMIS_CINE_LINE#

Relationship of elasto-plasticity behavior of VonMises to linear kinematic work hardening. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ECRO_LINE (_FO) and ELAS (_FO) (confer [R5.03.02] for more details).

Supported models: 3D, INCO_UPG, INCO_UP,,, C_PLAN, D_PLAN, 1D (PMF)
Number of internal variables: 8.

◦ \(\mathrm{V1}\) to \(\mathit{V6}\): 6 components of the kinematic work hardening tensor \(X\),

◦ \(\mathrm{V7}\): plasticity indicator (see Note 1) (0 for elastic, 1 for plastic).

◦ \(V8\): equivalent plastic deformation.

Number of internal variables for models BARRE, PMF: 2
Example: see test SSNP14.
For models BARRE and PMF, the behavior is then 1D: 2 internal variables are sufficient: \(\mathit{V1}\) represents the sole component of the recall tensor, and \(V2\) the plasticity indicator (see Note 1); the 5 others are zero.

4.4.2.7. Behavior VMIS_ECMI_TRAC#

Relationship of the elastoplasticity behavior of VonMises to combined work hardening, linear kinematics and isotropic nonlinear (Cf. [R5.03.16] for more details). Isotropic work hardening is given by a \((\sigma ,\varepsilon )\) traction curve or possibly by several curves if these depend on the temperature. The characteristics of the material are provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords PRAGER (_FO) (for kinematic work hardening), TRACTION (for isotropic work hardening) and ELAS (_FO).

Meaning: \(\mathrm{V1}\) to \(\mathrm{V6}\): 6 components of the kinematic work hardening tensor \(X\), \(\mathrm{V7}\): plasticity indicator (see Note 1) (0 for elastic, 1 for plastic).
Number of internal variables: 8
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, V2: plasticity indicator (see Note 1) (0 for elastic, 1 for plastic), \(\mathrm{V3}\) to \(\mathrm{V8}\): 6 components of the kinematic work hardening tensor \(\alpha\).
Example: see test SSNP102.

4.4.2.8. Behavior VMIS_ECMI_LINE#

Relationship of the elastoplasticity behavior of vonMises to combined work hardening, linear kinematics and linear isotropic (confer [R5.03.16] for more details). The characteristics of the material are provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords PRAGER (_FO) (for kinematic work hardening), ECRO_LINE (_FO) (for isotropic work hardening) and ELAS (_FO).

Supported models: 3D, 2D, INCO_UPG, INCO_UP,,,, C_PLAN, CONT_1D (by DE BORST), CONT_1D (PMF).
Number of internal variables: 8
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, 1 for plastic), \(\mathrm{V3}\) to \(\mathrm{V8}\): 6 components of the kinematic work hardening tensor \(\alpha\).
Example: see test SSNP102

4.4.2.9. Behavior VMIS_CIN1_CHAB#

Behavioral relationship that accounts for the cyclic behavior of the material in elasto-plasticity with a nonlinear kinematic work hardening tensor, a nonlinear isotropic work hardening, a work hardening effect on the recall tensor variable. All the constants of the material may possibly depend on the temperature. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CIN1_CHAB (_F0), ELAS (_FO) (confer [R5.03.04] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D (by DE BORST).
Number of internal variables: 8
\(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic), \(\mathrm{V3}\) to \(\mathrm{V8}\): 6 components of the kinematic work hardening tensor \(\alpha\).

4.4.2.10. Behavior VMIS_CIN2_CHAB#

Behavioral relationship that accounts for the cyclic behavior of the material in elastoplasticity with 2 nonlinear kinematic work hardening tensors, a nonlinear isotropic work hardening, a work hardening effect on the recall tensor variable. All the constants of the material may possibly depend on the temperature. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CIN2_CHAB (_F0), ELAS (_FO) (confer [R5.03.04] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D (by DE BORST).
Number of internal variables: 14
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic), \(\mathrm{V3}\) to \(\mathrm{V8}\): 6 components of the 1st tensor of the kinematic variable \({\alpha }_{1}\), \(\mathrm{V9}\) to \(\mathrm{V14}\): 6 components of the 2nd tensor of the kinematic variable, to: 6 components of the 2nd tensor of the kinematic variable \({\alpha }_{2}\).
Example: see test SSNV101A

4.4.2.11. Behavior VMIS_CIN2_MEMO#

J.L.Chaboche elastoplastic behavior relationship with 2 kinematic variables that accounts for the cyclic behavior in elastoplasticity with 2 nonlinear kinematic work hardening tensors, a nonlinear isotropic work hardening, a work hardening effect on the recall tensor variables and a memory effect of the greatest work hardening. All the constants of the material may possibly depend on the temperature. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CIN2_CHAB (_F0), ELAS (_FO), MEMO_ECRO (_FO) (Cf. [R5.03.04] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D (by DE BORST).
Number of internal variables: 28
Meaning: \(\mathit{V1}\): cumulative plastic deformation, \(\mathit{V2}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic), \(\mathit{V3}\) to \(\mathit{V8}\): 6 components of the 1st tensor of the kinematic variable \({\alpha }_{1}\), \(\mathit{V9}\) to \(\mathit{V14}\): 6 components of the 2nd tensor of the kinematic variable, to: 6 components of the 2nd tensor of the kinematic variable \({\alpha }_{2}`**, ** :math:\)mathit{V15}`: Work hardening function \(R(p)\), \(\mathit{V16}\): variable relating to the work hardening memory \(q\), \(\mathit{V17}\) to \(\mathit{V22}\): 6 components of the tensor relating to the work hardening memory \(\xi\), \(\mathit{V23}\) to \(\mathit{V28}\): 6 components of the tensor deformation plastic.
Example: see test SSND105, COMP002H

4.4.2.12. Behavior VMIS_CIN2_NRAD#

Chaboche elastoplastic behavior relationship with 2 kinematic variables that accounts for the cyclic behavior in elastoplasticity with 2 nonlinear kinematic work hardening tensors, a nonlinear isotropic work hardening, a work hardening effect on the recall tensor variables, and a non-proportionality effect of loading. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CIN2_CHAB (_F0), ELAS (_FO), CIN2_NRAD (confer [R5.03.04] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D (by DE BORST).
Number of internal variables: 14
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic), \(\mathrm{V3}\) to \(\mathrm{V8}\): 6 components of the 1st tensor of the kinematic variable \({\alpha }_{1}\), \(\mathrm{V9}\) to \(\mathrm{V14}\): 6 components of the 2nd tensor of the kinematic variable, to: 6 components of the 2nd tensor of the kinematic variable :math:`{alpha }_{2}`**, **
Example: see test SSND105D

4.4.2.13. Behavior VMIS_MEMO_NRAD#

Relationship of elastoplastic Chaboche behavior to 2 kinematic variables that accounts for the cyclic behavior in elastoplasticity with 2 nonlinear kinematic work hardening tensors, a nonlinear isotropic work hardening, a work hardening effect on the recall tensor variables, and an effect of non-proportionality of loading and a memory effect of greater work hardening. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CIN2_CHAB (_F0), ELAS (_FO), MEMO_ECRO (_FO), CIN2_NRAD (Cf. [R5.03.04] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D (by DE BORST).
Number of internal variables: 28
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic), \(\mathrm{V3}\) to \(\mathrm{V8}\): 6 components of the 1st tensor of the kinematic variable \({\alpha }_{1}\), \(\mathrm{V9}\) to \(\mathrm{V14}\): 6 components of the 2nd tensor of the kinematic variable, to: 6 components of the 2nd tensor of the kinematic variable \({\alpha }_{2}`**, ** :math:\)mathrm{V15}`: Work hardening function \(R(p)\), \(\mathrm{V16}\): variable relating to the work hardening memory \(q\), \(\mathrm{V17}\) to \(\mathrm{V22}\): 6 components of the tensor relating to the work hardening memory \(\xi\), \(\mathrm{V23}\) to \(\mathrm{V28}\): 6 components of the tensor deformation plastic.
Example: see test SSND115

4.4.2.14. Behavior DIS_CHOC#

Isothermal contact and shock model with Coulomb friction based on a discrete element with 1 or 2 knots, treated by penalization. The parameters characterizing the shock and the friction are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword DIS_CONTACT [R5.03.17].

Supported models: 3D_DIS, 2D_DIS
Number of internal variables: 8

The internal variables describe the behavior in the tangential plane defined by the local directions \(y\) and \(z\), which are defined in relation to the normal shock direction \(x\).

◦ \(V1\): next move \({y}_{\mathit{local}}\) (differential node displacement if \(\mathit{SEG}2\)).

◦ \(V2\): next move \({z}_{\mathit{local}}\) (differential node displacement if \(\mathit{SEG}2\)).

◦ \(V3\): next speed \({y}_{\mathit{local}}\) (differential speed of knots if \(\mathit{SEG}2\)).

◦ \(V4\): next speed \({z}_{\mathit{local}}\) (differential speed of knots if \(\mathit{SEG}2\)).

◦ \(V5\): force following \({y}_{\mathit{local}}\).

◦ \(V6\): force following \({z}_{\mathit{local}}\).

◦ \(V7\): if the friction threshold is reached \(\text{=}1\) otherwise \(\text{=}0\)

◦ \(V8\): game between nodes following \({x}_{\mathit{local}}\).

4.4.2.15. Behavior CHOC_ELAS_TRAC#

Isothermal contact model with a non-linear elastic shock based on a discrete element with 2 knots. The parameters characterizing shock and friction are provided in operator DEFI_MATERIAU [U4.43.01], under the keyword DIS_CHOC_ELAS [R5.03.17].

Supported models: DIS_T
Number of internal variables: 1
Meaning: \(\mathrm{V1}\): empty (so 0). The behavior is elastic, non-linear.

4.4.2.16. Behavior DIS_CONTACT#

Isothermal contact and shock model with Coulomb friction based on a discrete element with 1 or 2 knots. Behaviour DIS_CONTACT reflects contact with shock and friction between two structures, via two types of relationships:

the unilateral contact relationship which expresses the non-interpenetrability between solid bodies,
the friction relationship that governs the variation of tangential forces in contact. For the present developments, a simple relationship will be retained: Coulomb’s law of friction.

The parameters characterizing the shock and the friction are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword DIS_CONTACT [R5.03.17].

Supported models: 3D_DIS.
Number of internal variables: 9

◦ \(V1\): component of the tangent force along the local axis \(y\): \({F}_{\mathit{cy}}\)

◦ \(V2\): component of the tangent force along the local axis \(z\): \({F}_{\mathit{cz}}\)

◦ \(V3\): displacement due to sliding in the tangential plane along the local \(y\) axis.

◦ \(V4\): displacement due to sliding in the tangential plane along the local \(z\) axis.

◦ \(V5\): speed along the local \(x\) axis.

◦ \(V6\): speed along the local \(y\) axis.

◦ \(V7\): speed along the local \(z\) axis.

◦ \(V8\): management of the initial interpenetration of the discrete.

◦ \(V9\): initial contact management.

4.4.2.17. Behavior DIS_ECRO_TRAC#

Behavior DIS_ECRO_TRAC is a non-linear behavior, making it possible to schematize the behavior of a uniaxial device, along the local axis \(x\) or in the tangential plane \(\mathit{yz}\) of discrete elements to two nodes (mesh SEG2) or of discrete elements to one node (mesh POI1).

The non-linear behavior is given by a \(F=\mathit{fonction}(\mathrm{\Delta }U)\) curve:

for a SEG2, \(\mathrm{\Delta }U\) represents the relative displacement of the two nodes in the element’s local coordinate system;
for a POI1, \(\mathrm{\Delta }U\) represents the absolute movement of the node in the local coordinate system of the element;
for a SEG2ou a POI1, \(F\) represents the effort expressed in the local coordinate system of the element.

The only data needed is the function describing the non-linear behavior. This function must meet the following criteria:

it is a function in the sense of code_aster defined with the operator DEFI_FONCTION;
the interpolations on the abscissa and ordinate axes are linear;
the name of the abscissa when defining the function is DX or DTAN;
extensions to the left and right of the function are excluded;
the function must be defined by at least three points in the case of isotropic work hardening or by exactly three points in the case of kinematic work hardening;
the first point is \((\mathrm{0.0,}0.0)\) and must be provided in the function definition;
the function must be strictly increasing;
the derivative of the function must be less than or equal to its derivative at point \((\mathrm{0.0,0}.0)\).

Behavior DIS_ECRO_TRAC has 17 internal variables:

	Variable name
V1	FORCEX	Force along the local x axis of the element.
V2	FORCEY	Force along the local y axis of the element.
V3	FORCEZ	Force along the element’s local z-axis.
V4	DEPLX	Move along the local x axis of the element.
V5	DEPLY	Move along the local y axis of the element.
V6	DEPLZ	Move along the element’s local z-axis.
V7	DISSTHER	Dissipation.
V8	PCUM	Plastic indicator.
V9	DEPLPX	Anelastic displacement along the local x axis of the element.
V10	DEPLPY	Anelastic displacement along the local y axis of the element.
V11	DEPLPZ	Anelastic displacement along the local z-axis of the element.
V12	FORCXX	Kinematic work hardening along the local x axis of the element.
V13	FORCXY	Kinematic work hardening along the local y axis of the element.
V14	FORCXZ	Kinematic work hardening along the local z axis of the element.
V15	RAIDEX	Tangent stiffness of the discrete along the local x axis of the element.
V16	RAIDEY	Tangent stiffness of the discrete along the local y axis of the element.
V17	RAIDEZ	Tangent stiffness of the discrete along the local z axis of the element.

4.4.2.18. Behavior ARME#

Isothermal elastoplastic behavior relationship for line armaments. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword ARME [R5.03.17].

Supported models: 3D_DIS
Number of internal variables: 1
Meaning: \(\mathrm{V1}\): maximum value reached of the quantity in absolute value \((\mathrm{uy}–\mathrm{ule})\) where \(\mathrm{uy}\) is the displacement in the local direction \(y\) of the mesh SEG2 and \(\mathrm{ule}\) the limiting displacement of the elastic domain.
Example: see test SSNL101.

4.4.2.19. Behavior RELAX_ACIER#

Behavioral relationship allowing to model the relaxation of prestress cables, available for bar-type models.

To take into account the influence of temperature on relaxation, all the coefficients of the law can be functions of temperature.

The data required for the material is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword RELAX_ACIER [R5.03.9].

Supported models: 1D
Number of internal variables: 2

◦ \(\mathit{V1}\): the cumulative anelastic deformation: \({\mathrm{\epsilon }}^{\mathit{an}}\).

◦ \(\mathit{V2}\): memorizing the stiffness tangent to the behavior.

Examples: see tests SSNL143 [a, b, c].

4.4.2.20. Behavior ASSE_CORN#

Isothermal elastoplastic behavior relationship for bolted connections of tower angles. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword ASSE_CORN [R5.03.32].

Supported models: 3D_DIS
Number of internal variables: 7
Example: see test SSNL102.

4.4.2.21. Behaviour DIS_GOUJ2E_PLAS#

Model to represent the local behavior of a threaded assembly stud thread (discrete element). The behavior is elastic everywhere except along the local \(Y\) axis. In this direction, it is a Von Mises isothermal elastoplasticity law with nonlinear isotropic work hardening (see [R5.03.17] for more details). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords TRACTION (for the local direction \(Y\)) and ELAS. The curve entered in TRACTION actually represents the shear force-displacement jump curve \(Y\) of a local calculation of a fillet and ELAS defines the stiffness assigned to the discrete for the other directions (in fact \(X\) local)).

Supported models: 2D_DIS_T
Number of internal variables: 2
Meaning: \(\mathrm{V1}\): cumulative plastic displacement, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 if elastic, 1 if plastic).
Example: see test ZZZZ120

4.4.2.22. Behaviour DIS_GOUJ2E_ELAS#

Model to represent the local elastic behavior of a threaded assembly stud thread (discrete element). The behavior is elastic everywhere (see [R5.03.17] for more details). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword ELAS.

Supported models: 2D_DIS_T
Number of internal variables: 1
Meaning: \(V1\): empty (so 0).

4.4.2.23. Behaviour VMIS_ASYM_LINE#

Relationship of uniaxial isothermal behavior of Von Mises elastoplasticity to isotropic work hardening with different elasticity limits in tension and compression. This asymmetric model of member elements makes it possible to model the interaction between a buried pipe or cable and the ground. The necessary data for the material field are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword ECRO_ASYM_LINE (Cf. [R5.03.09] for more details).

Modeling supported: BARRE
Number of internal variables: 4
Meaning: \(\mathrm{V1}\): cumulative plastic deformation under tension, \(\mathrm{V2}\): plasticity indicator (see Note 1) in traction, \(\mathrm{V3}\): cumulative plastic deformation under compression, \(\mathrm{V4}\): plasticity indicator (see Note 1) in compression.
Example: see test SSNL112.

4.4.2.24. Behaviour DIS_ECRO_CINE#

Model with non-linear kinematic work hardening based on a discrete element with 1 or 2 knots, defined independently on each degree of freedom (forces, moments), of the type \(F={K}_{e}(U-{U}_{\mathrm{an}})\). The parameters characterizing the elastic limit \({F}_{y}\), the ductile plate \({F}_{u}\), the kinematic work-hardening constant \({k}_{x}\), and the power \(n\) defining the curvilinear part of the traction curve, are provided in the DEFI_MATERIAU [U4.43.01] operator, under the keyword DIS_ECRO_CINE, under the keyword, see also [R5.03.17]; in addition, the elastic stiffness \({K}_{e}\) is given via the affe_cara_elem command [U4.42.01].

Supported models: DIS_T, DIS_TR,, 2D_DIS_T, 2D_DIS_TR.
Number of internal variables: 3.
Meaning: \(\mathrm{V1}\): anelastic displacement \({U}_{\mathrm{an}}\), \(\mathrm{V2}\): kinematic work hardening variable \(\tilde{\alpha }\), \(\mathrm{V3}\): energy dissipated.
Example: see test SSND102 [V6.08.102].

4.4.2.25. Behaviour DIS_BILI_ELAS#

Behavior DIS_BILI_ELAS is used to model bilinear elastic behavior in translation. The law of behavior was designed to be used with all discrete elements.

The behavior is characterized by 2 slopes and by an effort that defines the slope break. For each degree of freedom considered, the behavior of the discrete is either elastic or elastic-bilinear. If in one of the directions the bilinear behavior is not defined, the behavior in this direction is then elastic and the values given in the AFFE_CARA_ELEM command are taken. Law DIS_BILI_ELAS only concerns the degrees of translation, so this implies that the behavior is elastic for the degrees of freedom of rotation that exist for this discrete. For each direction, the 3 characteristics (KDEB, KFIN, FPRE) are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword DIS_BILI_ELAS, see also [R5.03.17]; they are necessarily given in the local coordinate system of the element, so it is necessary in the command AFFE_CARA_ELEM under the keyword factor DISCRET to specify REPERE =” LOCAL “. The quantities KDEB and KFIN are functions that depend on temperature and can be defined as a function, sheet, or formula. The local coordinate system is defined in the standard way in the AFFE_CARA_ELEM command under the ORIENTATION factor keyword.

There is one internal variable per degree of translational freedom. It can take 3 values:

◦ \(V1=0\), discretion has never been sought in this direction.

◦ \(V1=1\), we are in the case where \(\mathrm{\mid }F\mathrm{\mid }\mathrm{\le }\text{FPREC}\)

◦ \(V1=2\), we are in the case where \(\mid F\mid >\text{FPREC}\)

4.4.2.26. Behaviour VMIS_CINE_GC#

Von Mises elastoplasticity behavior relationship with linear kinematic work hardening written in 1D and in CONT_PLAN, based on ECRO_LINE. The characteristics of the material are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword ecro_line (for linear work hardening).

The supported models are 1D and C_PLAN, the number of internal variables is 12 (confer [R5.03.02] « Integrating Von Mises elastoplastic behavior relationships », for more details).

◦ \(V1\): Boundary constraint criterion,

◦ \(V2\) :Deformation limit criterion,

◦ \(V3\) :Equivalent deformation,

◦ \(V4\): Plastic indicator,

◦ \(V5\) :non-recoverable dissipation,

◦ \(V6\) :thermodynamic dissipation.

◦ \(V7\) to \(V12\): Components of the work hardening tensor.

4.4.2.27. Behaviour DASHPOT#

Behavioral relationship for discrete elements DIS_T linking, at each calculation time \({t}_{i}\), the nodal force \(F({t}_{i})\) to the displacement increment \({\mathrm{\Delta }}_{x}({t}_{i})\) in the following way: \(F({t}_{i})=K{\mathrm{\Delta }}_{x}({t}_{i})\) where \(K\) is a stiffness parameter provided by the user via the command affe_cara_elem [U4.42.01] (CARA =” K_T_D_L “or “ K_T_D_N “).

Supported models: DIS_T.
Number of internal variables: 0.
Reference material: [R5.03.17].
Example: see ssnd119a test [V6.08.119].

4.4.2.28. Behaviors CHOC_ENDO and CHOC_ENDO_PENA#

These behaviors are dedicated to discrete elements such as K_T_D_L. They make it possible to model shocks taking into account:

a threshold function, which limits the shock force during loading depending on the displacement,
damage to the shock absorbers during loading,
the evolution of the « gap », due to repeated shocks,
variable depreciation during the calculation.

The material that allows the characteristics to be given is DIS_CHOC_ENDO.

The description of the behaviors can be found in the documentation [R5.03.17] « Behavioral relationships of discrete elements ».

4.4.3. Elasto-viscoplastic models#

Unless otherwise specified, all models may include temperature dependence. For each model, it is specified whether the integration is implicit or semi-implicit.

4.4.3.1. Behaviour VISC_ISOT_LINE#

Relationship of visco-elastoplastic behavior in large deformations (formulation SIMO_MIEHE only). The plastic model is VMIS_ISOT_LINE, i.e. with linear isotropic work hardening. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01] under the keywords ECRO_LINE (_FO), ELAS (_FO).

The law of viscosity is a hyperbolic sine law (confer [R5.03.21]. The viscous parameters should be entered under the keyword VISC_SINH in the DEFI_MATERIAU operator.

Supported models: 3D, 2D, INCO_UPG and INCO_UP
Integration: implicit
Number of internal variables: 3
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, 1 for plastic).

Example: see test SSNL129D

4.4.3.2. Behaviour VISC_ISOT_NL#

Relationship of visco-elastoplastic behavior in small and large deformations (formulation GDEF_LOG). The plastic model is VMIS_ISOT_NL, i.e. with non-linear isotropic work hardening. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01] under the keywords ECRO_NL (_FO), ELAS (_FO).

The law of viscosity is Norton’s law (confer [R5.03.33]. The viscous parameters should be entered under the keyword NORTON in the DEFI_MATERIAU operator.

Local and GRAD_VARI models supported: 3D, D_PLAN, AXIS
Number of internal variables: 8
Meaning: \(V1\): work-hardening variable (generally cumulative plastic deformation), \(V2\): plasticity indicator (see Note 1) (0 for elastic, 1 for plastic with regular flow, 2 for plastic with singular flow), \(V3\) to \(V8\): components of plastic deformation.
The large GDEF_LOGsont deformations available for this behavior.
Compatible with models GRAD_VARI and GRAD_INCO.

Example: see test SSNV264

4.4.3.3. Behaviour VISC_ISOT_TRAC#

Relationship of visco-elastoplastic behavior in large deformations (formulation SIMO_MIEHE only). The plastic model is VMIS_ISOT_TRAC, i.e. with non-linear isotropic work hardening. The curve \((\sigma ,\varepsilon )\) in simple traction is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword TRACTION (confer [R5.03.02] for more details). It is possible to define several traction curves depending on the temperature. You must also enter the ELAS (_FO) keyword in the DEFI_MATERIAU operator.

The law of viscosity is a hyperbolic sine law (confer [R5.03.21]. The viscous parameters should be entered under the keyword VISC_SINH in the DEFI_MATERIAU operator.

Supported models: 3D, 2D, CONT_1D (PMF), INCO_UPG and INCO_UP
Integration: implicit
Number of internal variables: 3
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, 1 for plastic),
Example: see test SSNL129A

4.4.3.4. Behaviour LEMAITRE#

Lemaitre nonlinear visco-plastic behavior relationship (without threshold). A particular case of this relationship (by cancelling the UN_SUR_M parameter) gives a relationship of NORTON. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords LEMAITRE (_FO) and ELAS (_FO) (confer [R5.03.08] for more details). The correspondence of the internal variables allows chaining with a calculation using elasto-plastic behavior with isotropic work hardening (“VMIS_ISOT_LINE” or “VMIS_ISOT_TRAC”). The integration of this model is carried out by a semi-implicit (PARM_THETA =0.5) or implicit (PARM_THETA =1) method.

Supported models: 3D, 2D, C_PLAN (by DE BORST), INCO_UPG, INCO_UP, CONT_1D (by DE BORST)
Number of internal variables: 2
Meaning: \(\mathit{V1}\): cumulative plastic deformation, \(\mathit{V2}\): empty so it is always equal to 0.
Example: see test SSNA104

4.4.3.5. Behaviour NORTON#

Norton visco-plastic behavior relationship (without threshold). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords LEMAITRE (_FO) and ELAS (_FO) (with UN_SUR_M =0). The integration of this model is carried out by a theta method with ALGO_INTE =” NEWTON_PERT “(PARM_THETA) or by an explicit method (ALGO_INTE = RUNGE_KUTTA)

Supported models: 3D, 2D, C_PLAN (by DE BORST), INCO_UPG, INCO_UP, CONT_1D (by DE BORST)
Number of internal variables: 7
Meaning: \(\mathrm{V1}\) to \(\mathit{V6}\): 6 components of plastic deformation, \(\mathit{V7}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic).
Example: see tests SSNP02E, SSNP02D

4.4.3.6. Behaviour DIS_VISC#

Behavior DIS_VISC is an extended non-linear viscoelastic rheological behavior, of the ZENER type, making it possible to schematize the behavior of a uniaxial damper, applicable to the local degree of freedom \(\mathit{dx}\) of discrete elements at two nodes (mesh SEG2) or and discrete elements at one node (mesh) or and of discrete elements at one node (mesh POI1), in the case of a connection with a non-meshed fixed frame (see static examples and dynamics in test case SSND101). The arrangement of the linear elastic components makes it possible to take into account a wide range of environmental situations of the damping part of the device and its attachments.

The speed is estimated via the displacement increment (and not by the diagram). The parameters characterizing the model are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword DIS_VISC, see also [R5.03.17]. The elastic stiffness \({K}_{e}\), which is used for the prediction phase of the nonlinear algorithm, is given via the affe_cara_elem [U4.42.01] command.

Supported models: DIS_T, DIS_TR,, 2D_DIS_T, 2D_DIS_TR.
Number of internal variables: 4.

◦ \(\mathrm{V1}\): FORCE: contains the effort \(\sigma\) at every moment in the rheological model.

◦ \(\mathrm{V2}\): UVISQ: viscous displacement of the shock absorber \({\epsilon }_{v}\)

◦ \(\mathit{V3}\): UVISQ: contains the energy dissipated updated at each moment: \(\mathrm{V2}=-\sum F\mathrm{.}\Delta U\)

◦ \(\mathit{V4}\): RAIDEUR: stiffness tangent to behavior \(\mathit{dF}/\mathit{dU}\)

Example: see test SSND101 [V6.08.101].

4.4.3.7. Behaviour VISC_CIN1_CHAB#

Chaboche behavior relationship (reports on the cyclic behavior of the material) in elasto-viscoplasticity with a nonlinear kinematic work hardening tensor, a nonlinear isotropic work hardening, a work hardening effect on the recall tensor variable and taking into account the viscosity. All the constants of the material may possibly depend on the temperature. The required material field data is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CIN1_CHAB (_F0), ELAS (_FO) (see [R5.03.04] for more details) and LEMAITRE for viscosity. The integration is completely implicit.

Supported models: 3D, 2D, C_PLAN (by DE BORST), INCO_UPG, INCO_UP, CONT_1D (by DE BORST)
Number of internal variables: 8
Meaning: \(\mathrm{V1}\): cumulative visco-plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic), V3 to V8:6 components of the kinematic work-hardening tensor \(\alpha\).
Example: see test HSNV124

4.4.3.8. Behaviour VISC_CIN2_CHAB#

Chaboche behavior relationship (reports on the cyclic behavior of the material) in elasto-viscoplasticity with 2 non-linear kinematic work hardening tensors, a nonlinear isotropic work hardening, a work hardening effect on the recall tensor variable and taking into account the viscosity. All the constants of the material may possibly depend on the temperature. The required material field data is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CIN2_CHAB (_F0), ELAS (_FO) (see [R5.03.04] for more details) and LEMAITRE for viscosity. The integration is completely implicit.

Supported models: 3D, 2D, C_PLAN (by DE BORST]), INCO_UPG, INCO_UP, CONT_1D (by DE BORST)
Number of internal variables: 14
Meaning: \(\mathrm{V1}\): cumulative visco-plastic deformation, \(\mathit{V2}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic), \(\mathrm{V3}\) to \(\mathrm{V8}\): 6 components of the 1st tensor of the kinematic variable \({\alpha }_{1}\), \(\mathrm{V9}\) to \(\mathrm{V14}\): 6 components of the 2nd tensor of the kinematic variable, to: 6 components of the 2nd tensor of the kinematic variable \({\alpha }_{2}\).
Example: see test HSNV124

4.4.3.9. Behaviour VISC_CIN2_MEMO#

Relationship of elastoviscoplastic behavior of Chaboche to 2 kinematic variables that accounts for the cyclic behavior in elasto-viscoplasticity with 2 nonlinear kinematic work hardening tensors, a nonlinear isotropic work hardening, a work hardening effect on the recall tensor variables and a memory effect of the greatest work hardening. All the constants of the material may possibly depend on the temperature. The necessary data for the material field are provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CIN2_CHAB (_F0), ELAS (_FO), MEMO_ECRO (_FO), LEMAITRE for viscosity. The integration is completely implicit. (see [R5.03.04] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D (by DE BORST).
Number of internal variables: 28
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic), \(\mathrm{V3}\) to \(\mathrm{V8}\): 6 components of the 1st tensor of the kinematic variable \({\alpha }_{1}\), \(\mathrm{V9}\) to \(\mathrm{V14}\): 6 components of the 2nd tensor of the kinematic variable, to: 6 components of the 2nd tensor of the kinematic variable \({\alpha }_{2}`**, ** :math:\)mathrm{V15}`: Work hardening function \(R(p)\), \(\mathrm{V16}\): variable relating to the work hardening memory \(q\), \(\mathrm{V17}\) to \(\mathrm{V22}\): 6 components of the tensor relating to the work hardening memory \(\xi\), \(\mathrm{V23}\) to \(\mathrm{V28}\): 6 components of the tensor deformation plastic.
Example: see test SSND105, COMP002H, SSNV118

4.4.3.10. Behavior VISC_CIN2_NRAD#

Relationship of elastoviscoplastic behavior of Chaboche to 2 kinematic variables that accounts for the cyclic behavior in elasto-viscoplasticity with 2 nonlinear kinematic work hardening tensors, a nonlinear isotropic work hardening, a work hardening effect on the recall tensor variables, and a non-proportionality effect of loading. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CIN2_CHAB (_F0), ELAS (_FO), CIN2_NRAD (confer [R5.03.04] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D (by DE BORST).
Number of internal variables: 14
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic), \(\mathrm{V3}\) to \(\mathrm{V8}\): 6 components of the 1st tensor of the kinematic variable \({\alpha }_{1}\), \(\mathrm{V9}\) to \(\mathrm{V14}\): 6 components of the 2nd tensor of the kinematic variable, to: 6 components of the 2nd tensor of the kinematic variable :math:`{alpha }_{2}`**, **
Example: see test SSND105D

4.4.3.11. Behavior VISC_MEMO_NRAD#

Relationship of elastoplastic Chaboche behavior to 2 kinematic variables that accounts for the cyclic behavior in elasto-viscoplasticity with 2 nonlinear kinematic work hardening tensors, a nonlinear isotropic work hardening, a work hardening effect on the recall tensor variables, and an effect of non-proportionality of the loading and a memory effect of the greatest work hardening. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CIN2_CHAB (_F0), ELAS (_FO), MEMO_ECRO (_FO), CIN2_NRAD (confer [R5.03.04] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D (by DE BORST).
Number of internal variables: 28
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1) (0 for elastic, number of internal iterations for plastic), \(\mathrm{V3}\) to \(\mathrm{V8}\): 6 components of the 1st tensor of the kinematic variable \({\alpha }_{1}\), \(\mathrm{V9}\) to \(\mathrm{V14}\): 6 components of the 2nd tensor of the kinematic variable, to: 6 components of the 2nd tensor of the kinematic variable \({\alpha }_{2}`**, ** :math:\)mathrm{V15}`: Work hardening function \(R(p)\), \(\mathrm{V16}\): variable relating to the work hardening memory \(q\), \(\mathrm{V17}\) to \(\mathrm{V22}\): 6 components of the tensor relating to the work hardening memory \(\xi\), \(\mathrm{V23}\) to \(\mathrm{V28}\): 6 components of the tensor deformation plastic.
Example: see test SSND115

4.4.3.12. Behavior VISCOCHAB#

Relationship of elastoviscoplastic behavior of Chaboche to 2 kinematic variables that accounts for the cyclic behavior in elastoplasticity with 2 non-linear kinematic work hardening tensors, a nonlinear isotropic work hardening, a work hardening effect on the recall tensor variables, a memory effect of the greatest hardening, and restoration effects. All the constants of the material may possibly depend on the temperature. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords VISCOCHAB (_F0), ELAS (_FO). The integration is either implicit or explicit (RUNGE_KUTTA) (Cf. [R5.03.12] for more details).

Supported models: 3D, 2D, CONT_1D (by DE BORST).
Number of internal variables: 28
Meaning: \(\mathrm{V1}\) to \(\mathrm{V12}\): 12 components of the 2 kinematic tensors \({X}_{1}\), \({X}_{2}`**; **** :math:\)mathrm{V13}`: cumulative plastic deformation, \(\mathrm{V14}\): Work hardening function \(R(p)\), \(\mathrm{V15}\): variable relating to the work hardening memory \(q\), variable relating to the work hardening memory, variable relating to the work hardening memory, variable relating to the work hardening memory, variable relating to the work hardening memory \(q\), \(\mathrm{V16}\) to \(\mathrm{V21}\): 6 components of the tensor relating to the work hardening memory \(\xi\), \(\mathrm{V22}\): plasticity indicator (see Note 1) (0 for elastic, 1 for plastic), \(\mathrm{V23}\) to \(\mathrm{V28}\): 6 components of the plastic deformation tensor (only in the explicit case).
Example: see test HSNV125D, COMP002I, SSNV118

4.4.3.13. Behavior NORTON_HOFF#

Relationship of viscosity behavior independent of temperature, to be used for the calculation of limit loads of structures, at a threshold of VON MISES. The only material parameter is the elastic limit to be entered in the operator DEFI_MATERIAU [U4.43.01] under the keyword ECRO_LINE (confer [R7.07.01] and [R5.03.12] for more details). For the calculation of the limit load, there is a specific keyword under PILOTAGE for this model (see keyword PILOTAGE: “ANA_LIM” from STAT_NON_LINE [U4.51.03]). It is strongly recommended to use linear search (see keyword RECH_LINEAIRE of STAT_NON_LINE [U4.51.03]). Indeed, the calculation of the limit load requires a lot of linear search iterations (of the order of 50) and Newton iterations (of the order of 50).

Modeling supported: INCO_UPG
Number of internal variables: 1
Meaning: \(\mathrm{V1}\): empty so it’s 0.
Example: see test SSNV124

4.4.3.14. Behavior VISC_TAHERI#

Behavioral (visco) -plastic relationship modeling the response of materials under cyclic plastic loading, and in particular making it possible to represent ratchet effects. The required material field data are provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords TAHERI (_FO) for the description of work hardening, LEMAITRE (_FO) for viscosity and ELAS (_FO) (confer [R5.03.05] for more details). In the absence of LEMAITRE, the law is purely elasto-plastic.

Supported models: 3D, 2D, C_PLAN (by DE BORST), INCO_UPG, INCO_UP, CONT_1D (by DE BORST).
Number of internal variables: 9
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): peak stress, \(\mathrm{V3}\) to \(\mathrm{V8}\): 6 components of the plastic deformation tensor at the last discharge, \(\mathrm{V9}\): charge/discharge indicator (0 for elastic discharge, 1 if conventional plastic charge, 1 if conventional plastic charge, 2 if plastic charge with two surfaces, 3 if pseudo-discharge).
Example: see tests SSNV102 (without viscosity) and SSNV170 (with viscosity).

4.4.3.15. Behavior KICHENIN_NL#

Behavioral relationship that superimposes an elastoplastic branch on a viscoelastic branch in small and large deformations (formulation GDEF_LOG). The elastoplastic branch corresponds to a VonMises threshold behavior and linear kinematic work hardening; the viscoelastic branch corresponds to a Maxwell model whose shock absorber is non-linear and follows a Norton law without threshold and follows a Norton law without threshold [R5.03.36]. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01] under the keywords KICHENIN_NL (_FO) and ELAS (_FO).

Important note: under the keyword factor ELAS, we define a Young’s modulus E and a Poisson’s ratio NU (as well as a thermal expansion coefficient ALPHA if applicable). They characterize*only* the elastoplastic branch, those relating to the viscoelastic branch being defined under the keyword KICHENIN_NL (E_VISC and NU_VISC). In particular, the instantaneous apparent stiffness of the model is not limited to the value E defined under ELASmais also includes the value E_VISC.

Supported models: 3D, D_PLAN, AXIS
Number of internal variables: 14
Meaning: \(\mathrm{V1}\): cumulative plastic deformation (classically affected by a factor of 2/3 in the root), \(V2\) to \(V7\): components of plastic deformation, \(V8\): cumulative viscous deformation (also affected by a factor 2/3 in the root), \(V9\) to \(V14\): components of viscous deformation.
The large GDEF_LOGsont deformations available for this behavior.

Examples: see test SSNV267et SSNV268.

4.4.4. Crystalline behaviors#

♦ COMPOR = comp [compor]

The details of crystalline behaviors are provided via the compor concept, from DEFI_COMPOR.

4.4.4.1. Behavior MONOCRISTAL#

This model makes it possible to describe the behavior of a single crystal whose behavior relationships are provided via the compor concept.

The number of internal variables is a function of the choices made in DEFI_COMPOR:

The first six are the 6 components of visco-plastic deformation: \({E}_{\mathrm{ij}}^{\mathrm{vp}}\):

\({E}^{\mathit{vp}}\mathrm{=}\mathrm{\sum }_{t}(\Delta {E}^{\mathit{vp}})\) with \(\Delta {E}^{\mathit{vp}}\mathrm{=}\mathrm{\sum }_{s}{\mu }_{s}\Delta {\gamma }_{s}\)

\({V}_{1}\mathrm{=}{E}_{\mathit{xx}}^{\mathit{vp}}\), \({V}_{2}={E}_{\mathrm{yy}}^{\mathrm{vp}}\), \({V}_{3}={E}_{\mathrm{zz}}^{\mathrm{vp}}\), \({V}_{4}=\sqrt{(2)}{E}_{\mathrm{xy}}^{\mathrm{vp}}\),, \({V}_{5}=\sqrt{(2)}{E}_{\mathrm{xz}}^{\mathrm{vp}}\), \({V}_{6}=\sqrt{(2)}{E}_{\mathrm{yz}}^{\mathrm{vp}}\)

\({V}_{7}\), \({V}_{8}\), \({V}_{9}\) are the values of \({\alpha }_{1}\) \({\gamma }_{1}\) \({p}_{1}\) for the glide system \(s\mathrm{=}1\)

\({V}_{10}\), \({V}_{11}\), \({V}_{12}\) correspond to system \(s\mathrm{=}2\), and so on, where:

\({\alpha }_{s}\) represents the kinematic variable of the \(s\) system in the case of phenomenological models, and the dislocation density in a model derived from DD;
\({\gamma }_{s}\) represents the plastic sliding of the \(s\) system
\({p}_{1}\) represents the cumulative plastic slippage of the \(s\) system

Taking into account irradiation:

in case DD_CC_IRRA, \({n}_{\mathrm{irra}}=12\) internal variables must be added: \({V}_{6+{\mathrm{3n}}_{s}+1}\) to \({V}_{6+{\mathrm{3n}}_{s}+12}\) contain for each sliding system the density of dislocations linked to irradiation \({\rho }_{s}^{\mathrm{irr}}\)
in case DD_CFC_IRRA, \({n}_{\mathrm{irra}}=24\) internal variables must be added: \({V}_{6+{\mathrm{3n}}_{s}+1}\) to \({V}_{6+{\mathrm{3n}}_{s}+12}\) contain for each sliding system \({\rho }_{s}^{\mathrm{loops}}\) \({V}_{6+{\mathrm{3n}}_{s}+13}\) to \({V}_{6+{\mathrm{3n}}_{s}+24}\) contain for each sliding system \({\phi }_{s}^{\mathrm{voids}}\)

The cissions for each sliding system are then stored: \({\tau }_{1}\),… \({\tau }_{{n}_{s}}\)

In the case where we take into account the rotation of the crystal lattice, we must add \({n}_{\mathrm{rota}}=16\) internal variables:

\({V}_{6+{\mathrm{3n}}_{s}+1}\) to \({V}_{6+{\mathrm{3n}}_{s}+9}\) are the 9 components of the rotation matrix \(Q\),
\({V}_{6+{\mathrm{3n}}_{s}+10}\) to \({V}_{6+{\mathrm{3n}}_{s}+12}\) are the 3 components of \(\Delta {\omega }^{p}\),
\({V}_{6+{\mathrm{3n}}_{s}+13}\) to \({V}_{6+{\mathrm{3n}}_{s}+15}\) are the 3 components of \(\Delta {\omega }^{e}\),
\({V}_{6+{\mathrm{3n}}_{s}+16}\) represents \(\Theta\)

The antepenultimate internal variable is the cleavage constraint: \(\underset{s}{\text{max}}(\Sigma \text{.}n)\mathrm{:}n\)

The penultimate internal variable contains the global cumulative plastic deformation, defined by:

\({V}_{p-1}=\sum \Delta {E}_{\mathrm{eq}}^{\mathrm{vp}}\) with \(\Delta {E}_{\mathit{eq}}^{\mathit{vp}}\mathrm{=}\sqrt{\frac{2}{3}(\Delta {\mathrm{E}}^{\mathit{vp}}\mathrm{:}\Delta {\mathrm{E}}^{\mathit{vp}})}\)

The last internal variable, \(\mathit{Vp}\), (\(p=6+{\mathrm{3n}}_{s}+{n}_{\mathrm{rota}}+3\), \({n}_{s}\) being the total number of sliding systems) is an indicator of plasticity (see Note 1) (threshold exceeded in at least one sliding system at the current time step). If it is zero, there was no increase in internal variables at the current moment. Otherwise, it contains the number of local Newton iterations (for an implicit resolution) that were required to obtain convergence.

For more details see [R5.03.11].

Supported models: 3D, 2D, C_PLAN (by DE BORST).
Example: see test SSNV194

4.4.4.2. Behavior POLYCRISTAL#

This model makes it possible to describe the behavior of a polycrystal whose behavior relationships are provided via the compor concept, from DEFI_COMPOR.

The number of internal variables is \(p\mathrm{=}7+\mathrm{6m}+\mathrm{\sum }_{g\mathrm{=}\mathrm{1,}m}({\mathrm{3n}}_{s}(g))+\mathrm{6m}+1\), \(m\) being the number of phases and \({n}_{s}(g)\) being the number of phase sliding systems (\(g\)).

The first six internal variables are the components of macroscopic viscoplastic deformation \({E}^{\mathit{vp}}\):

\({V}_{1}={E}_{\mathrm{xx}}^{\mathrm{vp}}\), \({V}_{2}={E}_{\mathrm{yy}}^{\mathrm{vp}}\), \({V}_{3}={E}_{\mathrm{zz}}^{\mathrm{vp}}\), \({V}_{4}=\sqrt{(2)}{E}_{\mathrm{xy}}^{\mathrm{vp}}\),, \({V}_{5}=\sqrt{(2)}{E}_{\mathrm{xz}}^{\mathrm{vp}}\), \({V}_{6}=\sqrt{(2)}{E}_{\mathrm{yz}}^{\mathrm{vp}}\);

the seventh is the macroscopic cumulative equivalent viscoplastic deformation \(P\):

\({V}_{7}=\sum \Delta {E}_{\mathrm{eq}}^{\mathrm{vp}}\) with \(\Delta {E}_{\mathit{eq}}^{\mathit{vp}}\mathrm{=}\sqrt{\frac{2}{3}(\Delta {\mathrm{E}}^{\mathit{vp}}\mathrm{:}\Delta {\mathrm{E}}^{\mathit{vp}})}\);

then, for each phase, we find the 6 components of the viscoplastic deformations or of the \(\beta\) tensor of the phase: \({\left\{{\varepsilon }_{\mathrm{xx}}^{\mathrm{vp}}(g),{\varepsilon }_{\mathrm{yy}}^{\mathrm{vp}}(g),{\varepsilon }_{\mathrm{zz}}^{\mathrm{vp}}(g),\sqrt{(2)}{\varepsilon }_{\mathrm{xy}}^{\mathrm{vp}}(g),\sqrt{(2)}{\varepsilon }_{\mathrm{xz}}^{\mathrm{vp}}(g),\sqrt{(2)}{\varepsilon }_{\mathrm{yz}}^{\mathrm{vp}}(g)\right\}}_{g=\mathrm{1,}m}\);
then, for each phase:
- for each phase sliding system, we find the values of \({\alpha }_{s}\) \({\gamma }_{s}\) \({p}_{s}\);
- in the case where the behavior takes into account irradiation (currently MONO_DD_CC_IRRA), \(12\) internal variables must then be added: the dislocation densities due to irradiation.
then, for each phase, we find the 6 components of the phase constraints: \({\left\{{\sigma }_{\mathit{xx}}(g),{\sigma }_{\mathit{yy}}(g),{\sigma }_{\mathit{zz}}(g),\sqrt{(2)}{\sigma }_{\mathit{xy}}(g),\sqrt{(2)}{\sigma }_{\mathit{xz}}(g),\sqrt{(2)}{\sigma }_{\mathit{yz}}(g)\right\}}_{g\mathrm{=}\mathrm{1,}m}\);
the last internal variable is an indicator of plasticity (see Note 1) (threshold exceeded in at least one sliding system at the current time step).

For more details see [R5.03.11].

Supported models: 3D
Example: see test SSNV171

4.4.5. Behaviors specific to fuel rods and metals under irradiation#

4.4.5.1. Behavior VISC_IRRA_LOG#

Law of axial creep under irradiation of fuel assemblies. It makes it possible to model primary and secondary creep, parameterized by neutron fluence (cf. [R5.03.09]) The parameters are provided in the DEFI_MATERIAU [U4.43.01] operator, under the keywords VISC_IRRA_LOG. The fluence field is defined by the AFFE_VARC keyword from the AFFE_MATERIAU command.

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D, CONT_1D (PMF).
Number of internal variables: 2. \(\mathit{V1}\): cumulative equivalent visco-plastic deformation, \(\mathit{V2}\): memorization of the irradiation history (fluence).
Example: see test SSNV113

4.4.5.2. Behavior GRAN_IRRA_LOG#

Relationship of creep and enlargement behavior under irradiation for fuel assemblies, similar to law VISC_IRRA_LOG for viscoplastic deformation, and also integrating a deformation of enlargement under irradiation (cf. [R5.03.09]). The fluence field is defined by the AFFE_VARC keyword from the AFFE_MATERIAU command. Behavior characteristics are provided in the DEFI_MATERIAU [U4.43.01] operator, under the GRAN_IRRA_LOG keyword. Since the magnification only takes place in one direction, it is necessary in 3D and 2D cases to give the direction of the magnification by the operand ANGL_REP of the keyword MASSIF of the of the operator AFFE_CARA_ELEM.

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D, CONT_1D (PMF).
Number of internal variables: 3. \(\mathit{V1}\): cumulative equivalent visco-plastic deformation, \(\mathit{V2}\): memorization of the irradiation history (fluence), \(\mathit{V3}\): enlargement deformation.
Example: see test SSNL128

4.4.5.3. Behavior LEMAITRE_IRRA#

Relationship between creep and growth behavior under irradiation for fuel assemblies. The fluence field is defined by the AFFE_VARC keyword from the AFFE_MATERIAU command. Behavior characteristics are provided in the DEFI_MATERIAU [U4.43.01] operator, under the LEMAITRE_IRRA keyword. Since the magnification only takes place in one direction, it is necessary in 3D and 2D cases to give the direction of the magnification by the operand ANGL_REP of the keyword MASSIF of the of the operator AFFE_CARA_ELEM. The integration diagram is implicit or semi-implicit, but it is recommended to use a semi-implicit integration, i.e. PARM_THETA = 0.5.

Supported models: 3D, 2D, C_PLAN (by DE BORST).
Number of internal variables: 3. \(\mathit{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): zero, \(\mathit{V3}\): enlargement deformation.
Example: see test SSNL121.

4.4.5.4. Behavior LEMA_SEUIL#

Relationship of viscoplastic behavior with threshold under irradiation for fuel assemblies (cf. [R5.03.08]). The fluence field is defined by the AFFE_VARC keyword from the AFFE_MATERIAU command. The characteristics of the magnification are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword LEMA_SEUIL. The integration of the model is achieved by a semi-implicit or implicit method.

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D (by DE BORST).
Number of internal variables: 2
\(\mathrm{V1}\): cumulative plastic deformation,
\(\mathrm{V2}\): represents the current threshold
Example: see test SSNA104

4.4.5.5. Behavior IRRAD3M#

Relationship of elasto-plastic behavior under irradiation of 304 and 316 stainless steels, materials of which the internal structures of nuclear reactor vessels are made. The fluence field is defined by the AFFE_VARC keyword from the AFFE_MATERIAU command. The model takes into account plasticity, creep under irradiation, swelling under neutron flow. The characteristics are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword IRRAD3M. The integration of the model is carried out by an implicit time schema (cf. [R5.03.13]).

Supported models: 3D, 2D, C_PLAN (by DE BORST)
Number of internal variables: 5
\(\mathrm{V1}\): cumulative equivalent plastic deformation,
\(\mathrm{V2}\): threshold for irradiation creep
\(\mathrm{V3}\): equivalent irradiation plastic deformation
\(\mathrm{V4}\): swelling
\(\mathrm{V5}\): plasticity indicator (see Note 1)
Example: see test SSNA118

4.4.5.6. Behavior DIS_GRICRA#

Behavior DIS_GRICRA makes it possible to model the connections between grids and rods in fuel assemblies. It is based on discrete 2-node elements, with 6 ddls per node (translation+rotation). The law of behavior on each subsystem (sliding -axial friction, rotation in the plane, and rotation out of plane) is of the plasticity type with positive work-hardening in the tangential to the discrete directions to model the sliding, and of the unilateral elastic type in the direction of the discrete to model the contact. The parameters of DIS_GRICRA, characterizing contact and friction, are directly stiffness in rotation and thresholds in rotation (critical angle type). These parameters are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword DIS_GRICRA. Unlike the other discretes, the stiffness characteristics of AFFE_CARA_ELEM are not taken into account. The discrete stiffness matrix should therefore be taken to be zero in AFFE_CARA_ELEM. Stiffness is only derived from the parameters in DEFI_MATERIAU.

The unilateral contact takes place in the direction \(X\) given by the SEG2 mesh of the discrete element, and the sliding takes place in the \(Y\) direction given by the key word ORIENTATION of AFFE_CARA_ELEM (confer [R5.03.17] for more details). The tangent matrix is symmetric.

Supported models: DIS_TR
Number of internal variables: 6
\(\mathrm{V1}\): cumulative plastic displacement
\(\mathrm{V2}\): touch/friction indicator (1 if sliding, 0 if not sliding)
\(\mathrm{V3}\): rotating detachment indicator
\(\mathrm{V4}\): plastic angle (sliding)
\(\mathrm{V5}\): cumulative plastic angle
\(\mathit{V6}\): memorizing the irradiation history (fluence)
Example: see test SSNL131

4.4.6. Mechanical models with the effects of metallurgical transformations#

The following behavioral relationships apply to a material that undergoes metallurgical phase changes (confer [R4.04.02] for more detail). Mechanical calculations taking metallurgy into account are based on a calculation of the evolution of metallurgical phases (see order CALC_META [U4.85.01]).

4.4.6.1. Behaviors in kit type META_ * except META_LEMA_ANI#

Two types of material can be activated by the keyword RELATION_KIT, either ACIER, which includes at most five different metallurgical phases, or ZIRC, which includes at most three different metallurgical phases.

In addition, the name of the behavioral relationship is of the form META_x_yy_zzz, with the following possibilities

The meaning of the letters defined above is as follows:

P	=	plastic behavior
V	=	viscoplastic behavior
IL	=	linear isotropic work hardening
INL	=	isotropic non-linear work hardening
CL	=	linear kinematic work hardening
PT	=	transformation plasticity
RE	=	metallurgical work hardening restoration


Examples:

COMPORTEMENT = (RELATION = 'META_P_INL'
RELATION_KIT = 'ZIRC')

COMPORTEMENT = (RELATION = 'META_V_CL_PT_RE'
RELATION_KIT = 'ACIER')

See also the tests: HSNV101, HSNV1202, HSNV103,, HSNV104,, HSNV105, HTNA100.

Note:: for all metallurgical laws, plane stresses are impossible even with the DE BORST method.

The material data required for the mechanical calculation must be defined for each metallurgical phase present in the material. They are provided in operator DEFI_MATERIAU [U4.43.01]:

		Behaviour type	DEFI_MATERIAU keywords
P	=	elastoplastic behavior	ELAS_META (_FO) followed by work hardening…
V	=	viscoplastic behavior	META_VISC_FO and elastoplastic data
IL	=	linear isotropic work hardening	ELAS_META (_FO) and META_ECRO_LINE
INL	=	isotropic non-linear work hardening	ELAS_META (_FO) and META_TRACTION (*)
CL	=	linear kinematic work hardening	ELAS_META (_FO) and META_ECRO_LINE
PT	=	transformation plasticity	META_PT
RE	=	metallurgical work hardening restoration	META_RE

Note: Attention, under META_TRACTION, you must enter not the stress-deformation curve but the isotropic work hardening curve as a function of the cumulative plastic deformation

Number of internal variables and meaning

Information on internal variables is grouped here because their number varies according to the type of work hardening (isotropic or kinematic), the type of material (ACIER or ZIRC), and the type of deformations (PETIT, PETIT_REAC, GROT_GDEP or SIMO_MIEHE).

The phases of steel are as follows:

Phase	Type	Name
Ferrite	Cold	FERRITE
Perlite	Cold	PERLITE
Bainite	Cold	BAINITE
Martensite	Cold	MARTENSITE
Austenite	Warm	AUSTENITE

The phases of zircaloy are as follows:

Phase	Type	Name
Alpha	Cold	ZIRCALPH
Alpha+Beta	Cold	ZIRCALBE
Beta	Hot	ZIRCBETA


The internal variables depend on the type of deformation and the type of work hardening:

Déformation	Isotropic work hardening		Kinematic work hardening
Déformation	Isotropic work hardening		Kinematic work hardening
	ACIER	ZIRC	ACIER	ZIRC
PETIT, PETIT_REAC, and GROT_GDEP	\(\mathrm{V1}\) to \(mathrm{V5}\): variables related to isotropic work hardening for the 5 phases	\(\mathrm{V1}\) to \(mathrm{V3}\): variables related to isotropic work hardening for the 3 phases	\(\mathrm{V1}\) to \(mathrm{V30}\): variables related to kinematic work hardening:math:alpha`for the 5 phases	\(\mathrm{V1}\) to \(mathrm{V18}\): variables related to kinematic work hardening:math:alpha`for the 3 phases
	\(\mathrm{V6}\): medium isotropic work hardening	\(\mathrm{V4}\): medium isotropic work hardening	\(\mathrm{V31}\) to \(mathrm{V36}\): medium kinematic work hardening \(X\)	\(\mathrm{V19}\) to \(mathrm{V24}\): medium kinematic work hardening \(X\)
	\(\mathrm{V7}\): plasticity indicator (0 if elastic, 1 if plastic)	\(\mathrm{V5}\): plasticity indicator (0 if elastic, 1 if plastic)	\(\mathrm{V37}\): plasticity indicator (see Note 1) (0 if elastic, 1 if plastic)	\(\mathrm{V25}\): plasticity indicator (see Note 1) (0 if elastic, 1 if plastic)
SIMO_MIEHE	\(\mathrm{V8}\): trace of elastic deformations divided by 3 used in large deformations	\(\mathrm{V6}\): trace of elastic deformations divided by 3 used in large deformations	Does not exist	Does not exist

4.4.2

The first line of the table gives the classical internal variables of plasticity (see §), by phase. They are therefore also named by phase. For example, for isotropic work hardening of a steel alloy, we have: FERRITE # EPSPEQ, #, PERLITE # EPSPEQ, BAINITE # EPSPEQ, MARTENSITE # EPSPEQ and AUSTENITE # EPSPEQ.

The following lines are global quantities. For example, we apply the law of mixtures to the internal variables by phase.

4.4.6.2. Behavior META_LEMA_ANI#

META_LEMA_ANI is an anisotropic law of viscoplastic behavior taking into account metallurgy, for Zirconium only [R4.04.04] and [R4.04.05] (and the HSNV134 and HSNV135 tests).

The characteristics are:

consideration of the three metallurgical phases of Zircaloy.
Lemaitre type viscosity, without threshold
anisotropy with Hill criterion

Supported models are: 3D, 2D, INCO.

The material coefficients are defined in operator DEFI_MATERIAU under “META_LEMA_ANI”.

The internal variables of model META_LEMA_ANI are:

\(V1\to \mathit{VN}\): N symmetric tensor components of elastic deformations

\(\mathit{VN}+1\): p: cumulative viscous deformation

\(\mathit{VN}+2\): Zb: beta phase proportion

\(\mathit{VN}+3\): epsther: thermal deformation

\(\mathit{VN}+4\): seq: equivalent Hill stress

\(\mathit{VN}+5,+6,+7\): sv1, sv2, sv3: viscous stress of the \(\alpha\) pure, \(\alpha \beta\) and \(\beta\) phases respectively

\(\mathit{VN}+8\): pch: phase change indicator (0 or 1)

\(\mathit{VN}+9\): tdeq moment at which the temperature is TDEQ (see [R4.04.04]) (initialized to 0 at the start of the calculation)

\(\mathit{VN}+10\): tfeq moment at which the temperature is TFEQ (see [R4.04.04]) (initialized to 0 at the start of the calculation)

4.4.6.3. MetaSteel Behavior EPIL_PT#

The MetaSteel EPIL_PTest law is specific to ACIER alloys (five metallurgical phases) that undergo metallurgical phase changes. This law is characterized by linear isotropic work hardening and makes it possible to take into account transformation plasticity.

All the material parameters are entered in the keyword MetaSteel factor EPIL_PT (_FO) of the DEFI_MATERIAU command.

The internal variables depend on the type of modeling, 2D or 3D:

Modeling type
2D	3D
\(V1\) to \(V4\): components of the elastic deformation tensor	\(V1\) to \(V6\): components of the elastic deformation tensor
\(V5\) to \(V9\): variables related to isotropic work hardening for the 5 phases	\(V7\) to \(V11\): variables related to isotropic work hardening for the 5 phases
\(V10\): medium isotropic work hardening	\(V12\): medium isotropic work hardening
\(V11\): plasticity indicator (0 if elastic, 1 if plastic)	\(V13\): plasticity indicator (0 if elastic, 1 if plastic)

Supported models are 3D, AXIS and D_PLAN. These models can be used with the keywords DEFORMATION =” PETIT “,” PETIT_REAC “or” GROT_GDEP “.

The implementation of the MetaSteel EPIL_PT law is illustrated in the mfron06 test case.

4.4.7. Local and non-local damage patterns#

4.4.7.1. Behaviors ROUSSELIER, ROUSS_PRet ROUSS_VISC#

Note:

The following three models “ ROUSSELIER “(elastoplastic model), “ ROUSS_PR” (elastoplastic model) and “ ROUSS_VISC “(elastoviscoplastic model) are three different versions of the Rousselier model. This model is an elasto (visco) plastic behavior relationship that makes it possible to account for the growth of cavities and to describe ductile failure in steels. Apart from the plastic/viscous side, the essential difference lies in the way in which large deformations are treated. For the model “ ROUSSELIER “it is a typical formulation Simo_Miehe (DEFORMATION: “SIMO_MIEHE”) and for the other two a typical formulation “ PETIT_REAC “(DEFORMATION:” PETIT_REAC “). On various examples treated in plasticity, it was found that the model “ ROUSS_PR “needs a lot more Newton iterations to converge compared to the model “ ROUSSELIER “ .

It should also be noted that these three models treat broken material differently. In the models “ ROUSS_PR “and “ ROUSS_VISC “, when the porosity reaches a limit porosity, the material is considered to be broken. The behavior is then replaced by an imposed fall in constraints. To activate this modeling of the broken material, it is then necessary to enter in the operator DEFI_MATERIAU [:external:ref:`U4.43.01 <U4.43.01>`], under the key word ROUSSELIER (_FO), the two coefficients* “ PORO_LIMI “and “ D_SIGM_EPSI_NORM “in the operator * []. For “ ROUSSELIER “, we don’t do anything particular because the stress naturally tends to zero when the porosity tends to one. The two previous parameters can be filled in but have no impact on the model.

“ ROUSSELIER “

Elastoplastic behavior relationship. It makes it possible to account for the growth of cavities and to describe ductile rupture. This model is used exclusively with the keyword DEFORMATION = “SIMO_MIEHE”). The necessary data for the material field are provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ROUSSELIER (_FO) and ELAS (_FO) (Cf. [R5.03.06] for more details). To facilitate the integration of this model, it is advisable to systematically use the global redistribution of the time step (see STAT_NON_LINE [U4.51.03], keyword INCREMENT). This model is not developed under plane stress. Moreover, with the SIMO_MIEHE keyword, you cannot use plane constraints using the DE BORST method.

Local models supported: 3D, 2D, INCO_UPG (if DEFORMATION =” PETIT “or” SIMO_MIEHE “)

Number of internal variables: 9
Meaning: \(\mathrm{V1}\): cumulative plastic deformation, \(\mathrm{V2}\): porosity value,: porosity value, \(\mathit{V3}\): plasticity indicator (see Note 1) (0 if elastic, 1 if plastic with regular solution, 2 if plastic with a singular solution). \(V4\) to \(V9\): 6 components of an Eulerian tensor in large deformations of elastic deformations,
Example: see test SSNV147.

Non-local modeling supported: use INCO models with internal length

Number of internal variables: 12
Meaning:
\(V1\): cumulative plastic deformation,
\(V2\) to \(V4\): cumulative plastic deformation gradient along the \(x,y,z\) axes, respectively,
V5: porosity,
\(V6\) to \(V11\): elastic deformations used for SIMO_MIEHE,
\(V12\): plasticity indicator (see Note 1) (0 if elastic, 1 if plastic and regular solution, 2 if plastic and singular solution).
Example: see test SSNP122

“ ROUSS_PR “

Elastoplastic behavior relationship. It makes it possible to account for the growth of cavities and to describe ductile rupture. This model is used exclusively with the keywords DEFORMATION: “PETIT_REAC” or “PETIT”, (preferably use the “PETIT_REAC” modeling because it is a large deformation model). The necessary data for the material field are provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ROUSSELIER (_FO) and ELAS (_FO) (Cf. [R5.03.06] for more details). It is also possible to take into account the nucleation of cavities. It is then necessary to enter the parameter AN (keyword not activated for the model ROUSSELIER and ROUSS_VISC) under ROUSSELIER (_FO). To facilitate the integration of this model, it is recommended to use the local automatic redistribution of the time step (keyword ITER_INTE_PAS).

Supported models: 3D, 2D, C_PLAN (by DE BORST), INCO_UPG, INCO_UP.
Number of internal variables: 5
Meaning: \(V1\): cumulative plastic deformation, \(V2\): porosity value,: porosity value, \(V3\): dissipation indicator, \(V4\) = stored energy, \(V5\) = plasticity indicator (see Note 1)
Example: test SSNV103

“ ROUSS_VISC “

Elasto-visco-plastic behavior relationship. It makes it possible to account for the growth of cavities and to describe ductile rupture. This model is used exclusively with the keywords DEFORMATION =” PETIT_REAC “or” PETIT “, (take the” PETIT_REAC “model because it is a large deformation model). The necessary data for the material field are provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords VISC_SINH, ROUSSELIER (_FO) and ELAS (_FO) (Cf. [R5.03.06] for more details). To facilitate the integration of this model, it is recommended to use the automatic local redistribution of the time step (keyword ITER_INTE_PAS). For the integration of this law, a \(\mathrm{\theta }\) -method is available and it is recommended to use a semi-implicit integration, i.e.: PARM_THETA = 0.5

Supported models: 3D, 2D, C_PLAN (by DE BORST), INCO.
Number of internal variables: 5
Meaning: \(V1\): cumulative plastic deformation, \(V2\): porosity value,: porosity value, \(V3\): dissipation indicator, \(V4\) = stored energy, \(V5\) = plasticity indicator (see Note 1)
Example: test SSNP117.

4.4.7.2. Behaviors GTN and VISC_GTN#

The law of behavior entitled “GTN” or “VISC_GTN” for its viscoplastic version, named after its authors Gurson, Tvergaard and Needleman, is an elasto-visco-plastic model that accounts for the ductile damage of metals by describing the phases of germination, growth and coalescence of cavities.

By nature, this model is based on a kinematics of large deformations, restricted to “GDEF_LOG”.

In addition to the local version of the model, a formulation with a cumulative plastic deformation gradient (”*_ GRAD_VARI “modeling) is also available to control the location of deformations, which is inherent in damage models. Finally, isochoric plastic deformations are generally observed over a large load range; the resulting incompressibility problems may require the use of mixed finite elements displacement—pressure—swelling (models “*_ INCO_UPG “”local or “*_ GRAD_INCO “”non-local).

The data that characterizes the material is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ELAS, ECRO_NL, GTN, and NON_LOCAL. This model is not developed in plane constraints, the latter not being compatible theoretically with the pronounced gradients that result from the location of the deformations.

There are 25 internal variables, plus the archiving of T constraints specific to “GDEF_LOG”. Their meaning is as follows:

\(V1\): work hardening variable
\(\mathrm{V2}\): total porosity
\(\mathit{V3}\): plasticity indicator (0 = elastic, 1 = regular plastic, 2 = peak regime)
\(\mathit{V4}\) to \(\mathit{V9}\): components of plastic deformation
\(V10\): cumulative plastic deformation
\(V11\): porosity resulting from germination
\(V12\): total damage (combination of germination, growth and coalescence)
\(V13\): damage speed
\(V14\) to \(V19\): components of**T** constraints
\(V20\): damage extrapolated for the plasticity calculation, before correction
\(V21\): Difference between extrapolated and corrected damage, measured in terms of stresses (distance between the thresholds corresponding to each of these damage values)
\(V22\): Contribution of work hardening to stresses
\(V23\): Contribution of viscosity to stresses
\(V24\): Contribution of non-local interactions to constraints
\(V25\): free component available to the user/developer in post-processing

We can refer to test cases SSNV250à SSNV257 as well as SSNV265et SSNV266 for examples of use.

4.4.7.3. Behavior HAYHURST#

Hayhurst elasto-viscoplastic model, to describe the behavior of austenitic steels, with scalar damage in hyperbolic sine, a function of the maximum principal stress or the stress trace, isotropic work hardening and a viscous law in hyperbolic sine.

This model is used with the keywords DEFORMATION = PETIT or PETIT_REAC. or GDEF_LOG. The required data is defined in DEFI_MATERIAU under the keywords HAYHURST and ELAS.

Supported models: 3D, 2D, INCO_UPG, INCO_UP.
Number of internal variables: 12
Meaning: \(\mathrm{V1}\) to \(\mathrm{V6}\): 6 components of viscoplastic deformation, \(\mathrm{V7}\): cumulative plastic deformation,: cumulative plastic deformation, \(\mathrm{V8}\) and \(\mathrm{V9}\): work-hardening variables \({H}_{1}\) and \({H}_{2}\), \(\mathit{V10}\): variable \(\phi\), \(\mathit{V11}\): damage, \(\mathit{V12}\): indicator.
Example: test SSNV261

4.4.7.4. Behavior VENDOCHAB#

Viscoplastic model coupled with Lemaitre-Chaboche isotropic damage [R5.03.15]. This model is used with the keywords DEFORMATION = PETIT or PETIT_REAC. The required data is defined in DEFI_MATERIAU under the keywords VENDOCHAB (_FO), LEMAITRE (_FO), and ELAS (_FO).

Supported models: 3D, 2D, INCO_UPG, INCO_UP.
Number of internal variables: 9
Meaning: \(\mathit{V1}\) to \(\mathit{V6}\): viscoplastic deformation, \(\mathit{V7}\): cumulative plastic deformation,: cumulative plastic deformation, \(\mathit{V8}\): isotropic work hardening, \(\mathit{V9}\): damage.
Example: test SSNV183

4.4.7.5. Behavior VISC_ENDO_LEMA#

Viscoplastic model coupled with Lemaitre-Chaboche isotropic damage, corresponding to a simplified version of model VENDOCHAB in the case where the coefficients ALPHA_D and BETA_D are zero and K_D = R_D. cf. [R5.03.15]. This model is used with the keywords DEFORMATION = PETIT or PETIT_REAC. The required data is defined in DEFI_MATERIAU under the keywords VISC_ENDO (_FO), LEMAITRE (_FO), and ELAS (_FO).

Supported models: 3D, 2D, INCO_UPG, INCO_UP.
Number of internal variables: 9
Meaning: \(\mathrm{V1}\) to \(\mathrm{V6}\): viscoplastic deformation, \(\mathrm{V7}\): cumulative plastic deformation,: cumulative plastic deformation, \(\mathrm{V8}\): isotropic work hardening, \(\mathrm{V9}\): damage.
Example: test SSND108

4.4.7.6. Behavior CZM_EXP_REG#

Cohesive behavior relationship (Cohesive Zone Model EXPonentielle REGularisée) (Cf. [R7.02.11] for more details) modeling the opening of a crack. This law can be used with the linear finite element of the joint type (Cf. [R3.06.09] for more detail) or with its THM version (cf. [R7.02.15]) and makes it possible to introduce a cohesive force between the lips of the crack. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword RUPT_FRAG. The use of this model often requires the presence of control by PRED_ELAS (cf. [U4.51.03]).

Modeling supported: PLAN_JOINT, AXIS_JOINT, 3D_JOINT,,, AXIS_JHMS, PLAN_JHMS.
Number of internal variables: 9
Meaning: \(\mathrm{V1}\): threshold corresponding to the largest displacement jump (in norm) ever reached, \(\mathrm{V2}\): dissipation indicator (0: no, 1: yes), \(\mathrm{V3}\) damage indicator (0: healthy, 1: damaged), \(\mathrm{V4}\): indicator of the percentage of energy dissipated (in norm) ever reached,: indicator of the percentage of energy dissipated,: indicator of the percentage of energy dissipated, \(\mathrm{V5}\): value of the energy dissipated, \(\mathrm{V7}\) to \(\mathrm{V9}\): values of the jump , (V9=0 in 2D)
Example: see test SSNP118, SSNP133, SSNV199

4.4.7.7. Behavior CZM_LIN_REG#

Cohesive behavior relationship (Cohesive Zone Model LINéaire REGularisée) (Cf. [R7.02.11] for more details) modeling the opening of a crack. The advantage of such a law, compared to CZM_EXP_REG, is to be able to represent a real breakthrough. The latter is visible thanks to the internal variable \(\mathrm{V3}\) (\(\mathrm{V3}=2\) corresponds to a totally broken element). This law can be used with the linear finite element of the joint type (Cf. [R3.06.09] for more detail) or with its THM version (cf. [R7.02.15]) and makes it possible to introduce a cohesive force between the lips of the crack. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword RUPT_FRAG. The use of this model often requires the presence of control by PRED_ELAS (see [U4.51.03]).

Modeling supported: PLAN_JOINT, AXIS_JOINT, 3D_JOINT,,, AXIS_JHMS, PLAN_JHMS.
Number of internal variables: 9
Meaning: \(\mathrm{V1}\): threshold corresponding to the largest displacement jump (in norm) ever reached, \(\mathrm{V2}\): dissipation indicator (0: no, 1: yes), V3 damage indicator (0: healthy, 1: damaged, 2: broken), \(\mathrm{V4}\): indicator of the percentage of energy dissipated (in norm) ever reached,: indicator of the percentage of energy dissipated,: indicator of the percentage of energy dissipated, \(\mathrm{V5}\): value of the energy dissipated, \(\mathrm{V7}\) to \(\mathrm{V9}\): values of the jump, (V9=0 in 2D)
Example: see test SSNP118, SSNV199

4.4.7.8. Behavior CZM_OUV_MIX#

Cohesive behavior relationship (Cohesive Zone Model OUVerture MIXte) (Cf. [R7.02.11]) modeling the opening and propagation of a crack. This law can be used with the finite interface element based on an augmented Lagrangian mixed formulation (see [R3.06.13]) and makes it possible to introduce a cohesive force between the lips of the crack in open mode only. This law is used when symmetry conditions are imposed on the interface element. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword RUPT_FRAG. The use of this model requires the presence of control by PRED_ELAS (cf. [U4.51.03]).
Modeling supported: all INTERFACE models (see U3.13.14).
Number of internal variables: 9

\(V1\): jump threshold (highest norm reached),

\(V2\): indicator of the regime of the law = -1: Contact, 0: Initial or current adherence, 1: Damage, 2: Fracture, 3: Return to zero with zero stress.

\(V3\): damage indicator 0 if material is healthy, 1 if material is damaged, 2 if material is broken.

\(V4\): percentage of energy dissipated,

\(V5\): value of the energy dissipated,

\(V6\): current residual energy value: zero for this law (valid for CZM_xxx_REG).

\(V7\): normal jump, \(V8\): tangential jump, \(V9\): tangential jump (null in 2D).

Examples: see tests SSNP118 and SSNV199.

4.4.7.9. Behavior CZM_EXP_MIX#

Cohesive behavior relationship (Cohesive Zone Model EXPonentielle MIXte) (Cf. [R7.02.11]) modeling the opening and propagation of a crack. This law can be used with the finite interface element based on an augmented Lagrangian mixed formulation (see [R3.06.13]) and makes it possible to introduce a cohesive force between the lips of the crack in opening mode in an exponential form. It is suitable for modeling semi-fragile materials such as concrete. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword RUPT_FRAG. The use of this model may sometimes require using steering techniques by PRED_ELAS to facilitate convergence (cf. [U4.51.03]).

Modeling supported: all INTERFACE models (see U3.13.14).
Number of internal variables: 9

\(\mathit{V1}\): jump threshold (highest norm reached),

\(\mathit{V2}\): indicator of the regime of the law = -1: Contact, 0: Initial or current adherence, 1: Damage, 2: Fracture, 3: Return to zero with zero stress.

\(\mathit{V3}\): damage indicator 0 if material is healthy, 1 if material is damaged, 2 if material is broken.

\(\mathit{V4}\): percentage of energy dissipated,

\(\mathit{V5}\): value of the energy dissipated,

\(\mathit{V6}\): current residual energy value: zero for this law (valid for CZM_xxx_REG).

\(\mathit{V7}\): normal jump, \(\mathit{V8}\): tangential jump, \(\mathit{V9}\): tangential jump (null in 2D).

Examples: see tests SSNP118 and SSNP166.

4.4.7.10. Behavior CZM_EXP_MIX#

Modeling supported: all INTERFACE models (see U3.13.14).
Number of internal variables: 9

\(\mathit{V1}\): jump threshold (highest norm reached),

\(\mathit{V2}\): indicator of the regime of the law = -1: Contact, 0: Initial or current adherence, 1: Damage, 2: Fracture, 3: Return to zero with zero stress.

\(\mathit{V3}\): damage indicator 0 if material is healthy, 1 if material is damaged, 2 if material is broken.

\(\mathit{V4}\): percentage of energy dissipated,

\(\mathit{V5}\): value of the energy dissipated,

\(\mathit{V6}\): current residual energy value: zero for this law (valid for CZM_xxx_REG).

\(\mathit{V7}\): normal jump, \(\mathit{V8}\): tangential jump, \(\mathit{V9}\): tangential jump (null in 2D).

Examples: see tests SSNP118 and SSNP166.

4.4.7.11. Behavior CZM_TAC_MIX#

Cohesive behavior relationship (Cohesive Zone Model TAlon -Curnier MIXte) (see [R7.02.11]) modeling the opening and propagation of a crack. This law can be used with the finite interface element based on a mixed augmented Lagrangian formulation (see [R3.06.13]) and makes it possible to introduce a cohesive force between the lips of the crack in the three rupture modes with an irreversibility of the Talon-Curnier type. Attention, this law cannot be used when symmetry conditions are imposed on the interface element. In this case you should use CZM_OUV_MIX.

The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword RUPT_FRAG. The use of this model requires the presence of control by PRED_ELAS (cf. [U4.51.03]).

Modeling supported: all INTERFACE models (see U3.13.14).
Number of internal variables: 9

\(\mathit{V1}\): jump threshold (highest norm reached),

\(\mathit{V2}\): indicator of the regime of the law = -1: Contact (only for CZM_OUV_MIX), 0: Initial or current adherence, 1: Damage, 2: Rupture, 3: Return to zero at zero stress.

\(\mathit{V3}\): damage indicator 0 if material is healthy, 1 if material is damaged, 2 if material is broken.

\(\mathit{V4}\): percentage of energy dissipated,

\(\mathit{V5}\): value of the energy dissipated,

\(\mathit{V6}\): current residual energy value: zero for this law (valid for CZM_xxx_REG).

\(\mathit{V7}\): normal jump, \(\mathit{V8}\): tangential jump, \(\mathit{V9}\): tangential jump (null in 2D).

Examples: see tests SSNP118, SSNA115, SSNV199.

4.4.7.12. Behavior CZM_TRA_MIX#

Cohesive behavior relationship (Cohesive Zone Model TRApèze MIXte) (see [R7.02.11]) modeling the opening and propagation of a ductile fracture. This law can be used with the finite interface element based on an augmented Lagrangian mixed formulation (see [R3.06.13]) and makes it possible to introduce a cohesive force between the lips of the crack only in opening mode. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword RUPT_DUCT.

Modeling supported: all INTERFACE models (see U3.13.14).
Number of internal variables: 9

\(\mathrm{V1}\): jump threshold, allows you to take into account the irreversibility of the cracking, see its definition in the previous parts (specific to each law).

\(\mathrm{V2}\): indicator of the regime of the law \(\mathrm{V2}=-1\): Contact, \(\mathrm{V2}=0\): initial or current adherence,: initial or current adherence, \(\mathrm{V2}=1\): dissipation, \(\mathrm{V2}=2\): final break, \(\mathrm{V2}=3\): plateau.

\(\mathrm{V3}\): damage indicator \(\mathrm{V3}=0\) if material is healthy, \(\mathrm{V3}=1\) if material is damaged, \(\mathrm{V3}=2\) if material is broken.

\(\mathrm{V4}\): percentage of energy dissipated.

\(\mathrm{V5}=\mathrm{V4}\times {G}_{c}\): value of the energy dissipated.

\(\mathrm{V6}\): current residual energy value: zero for this law (valid for CZM_xxx_REG).

\(\mathrm{V7}={\delta }_{n}\): normal jump, \(\mathrm{V8}={\delta }_{t}\): tangential jump, \(\mathrm{V9}={\delta }_{\tau }\) tangential jump (null in 2D).

Examples: see tests SSNP151, SSNA120.

4.4.7.13. Behavior CZM_FAT_MIX#

Cohesive behavior relationship for fatigue (see [R7.02.11]). This law can be used with the finite interface element based on an augmented Lagrangian mixed formulation (see [R3.06.13]). The aim is to simulate the propagation of fatigue cracks in 2D or 3D (mode I only) with the possibility of considering a non-linear surrounding material in order to model (among other things) the delay effect associated with overload. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword RUPT_FRAG. The use of this model requires the presence of control by PRED_ELAS (cf. [U4.51.03]).

Modeling supported: all INTERFACE models (see U3.13.14).
Number of internal variables: 9
Example: see tests SSNP118, SSNP139

4.4.7.14. Behavior CZM_LAB_MIX#

Cohesive behavior relationship (Cohesive Zone Model Steel-Concrete Link MIXte) (cf. [R7.02.11]) modeling the behavior of a steel-concrete interface. This law can be used with finite interface elements based on a mixed formulation of the augmented Lagrangian type (cf. [R3.06.13]) and makes it possible to model the sliding of steel with respect to concrete.

The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword CZM_LAB_MIX.

Supported models: all INTERFACE models (see U3.13.14).
Number of internal variables: 5

\(V1\): jump threshold (highest norm reached),

\(V2\): law regime indicator = 0: Initial or current adherence, 1: Damage, 2: Fracture, 3: Return to zero at zero stress.

\(V3\): normal jump, \(V4\): tangential jump, \(V5\): tangential jump (null in 2D).

Example: see test SSNS110.

4.4.7.15. Behavior CZM_TURON#

Cohesive behavior relationship CZM_TURON allowing to model the damage of a cracking interface with a coupling between the responses according to the different stress modes (N opening mode and tangent modes T1 and T2). In fact, this law makes it possible to consider different properties in pure normal and tangent modes (joint anisotropy). It is described in detail in the documentation [R7.02.21].

This law is typically used in the context of modeling glued joints made of composite material in wind turbine blades.

The law is supported by finite joint elements whose degrees of freedom are the jumps in movement when passing the interface (see R3.06.13).

The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword RUPT_TURON.

Supported models: JOINT models: PLAN_JOINT, AXIS_JOINT, 3D_JOINT.
Examples: see ssnv110.
Number of internal variables: 16
V1: PLUS GRANDE NORME DU SAUT É QUIVALENT TOTAL
V2: VARIABLE SEUIL
V3: VARIABLE FROM ENDOMMAGEMENT
V4: INDICATEUR OF DISSIPATION (0: SI REGIME LIN, 1: SI REGIME DISS)
V5: INDICATEUR FROM ENDOMMAGEMENT (0: SAIN, 1: ENDOMMAGE, 2: CASSE)
V6 TO V8: VALEURS FROM SAUT DANS TO REPERE LOCAL
V9: VALEUR FROM SAUT EQUIVALENT TOTAL
V10: VALEUR FROM SAUT EQUIVALENT TANGENTIEL
V11: POURCENTAGE FROM ENERGIE DISSIPEE
V12: VALEUR FROM ENERGIE DISSIPEE
V13: TAUX FROM MIXITE BETA TO T+ (CALCULE PAR LES SAUTS)
V14: TAUX FROM MIXITE B TO T+ (CALCULE PAR LES TAUX FROM RESTITUTION D’ENERGIE)
V15: SEUIL FROM INITIATION FROM ENDOMMAGEMENT TO MODE MIXTE TO T+
V16: SEUIL FROM PROPAGATION FROM FISSURE TO MODE MIXTE TO T+

4.4.7.16. Behavior RUPT_FRAG#

Non-local behavioral relationship based on the formulation of J.J. Marigo and G. Francfort of fracture mechanics by J.J. Marigo and G. Francfort (no equivalent in a local version). This model describes the appearance and propagation of cracks in an elastic material (cf. [R7.02.11]). The characteristics of the material are defined in the operator DEFI_MATERIAU [U4.43.01] under the keywords ELAS, RUPT_FRAG and NON_LOCAL.

Non-local modeling supported: GRAD_VARI.
Number of internal variables: 4
Meaning: \(\mathrm{V1}\): damage value, \(\mathrm{V2}\) to \(\mathrm{V4}\): 3 components of the damage gradient.
Example: see test SSNA101.

4.4.7.17. Behavior RANKINE#

Behavioral relationship used for simplified modeling of joints in concrete dams [R7.01.39]. This is a criterion for perfect plasticity in traction involving the components of the main stresses: \({\mathrm{\sigma }}_{i=\mathrm{1,2,3}}\le {\mathrm{\sigma }}_{t}\). When a main constraint reaches threshold value \({\mathrm{\sigma }}_{t}\), the joint opens in that direction. It should be noted that the plastic deformation thus created is not reversible, the model therefore does not make it possible to represent the re-closure of the joint and is only valid on a monotonous loading path. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword RANKINE.

Modeling supported: D_PLAN, C_PLAN,, AXIS, 3D.
Number of internal variables: 9
Example: see tests SSNV515, SSNV516

4.4.7.18. Behavior JOINT_MECA_RUPT#

Relationship of contact, elastic behavior with tensile strength and rupture (Cf. [R7.01.25]). This law can be used with linear and quadratic joint finite elements. Hydromechanical modeling is only possible for quadratic joints (Cf. [R3.06.09] for more details). The normal behavior is of the cohesive type, while the tangential behavior is always linear with stiffness depending on the normal opening of the joint. The hydrostatic pressure due to the presence of liquid in the joint is taken into account; hydromechanical coupling is also possible. The procedure for injecting concrete under pressure (claving), which is specific to the construction of dams, is also implemented. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword JOINT_MECA_RUPT.

Modeling supported: PLAN_JOINT, AXIS_JOINT, 3D_JOINT,,, PLAN_JOINT_HYME, 3D_JOINT_HYME.
Number of internal variables: 18
Example: see tests SSNP162, SSNP142, SSNP143

4.4.7.19. Behavior JOINT_MECA_FROT#

An elastoplastic version of the Mohr-Coulomb law of friction (confer [R7.01.25]). This law can be used with linear and quadratic joint finite elements. Hydromechanical modeling is only possible for quadratic joints (Cf. [R3.06.09] for more details).. Only the tangential part of the displacement is broken down into two components - plastic and elastic. The flow is normal for this tangential part. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword JOINT_MECA_FROT.

Modeling supported: PLAN_JOINT, AXIS_JOINT, 3D_JOINT,,, PLAN_JOINT_HYME, 3D_JOINT_HYME.
Number of internal variables: 18
Example: see tests SSNP162d /e/f/j /k/l, SSNP142c /d/g/h

4.4.7.20. Behavior JOINT_MECA_ENDO#

Law JOINT_MECA_ENDO is a unified behavior model for joints (main application for dams) [R7.01.25]. The latter makes it possible to model both the rupture and the friction between the lips of the joints. The surrounding material has pure mechanical behavior. Friction is managed by the internal plasticity variable and failure by the damage variable. The coupling takes place through the term kinematic work hardening. The law is written in the generalized standard formalism, it admits a hydro-mechanical coupling similar to that of the previous laws JOINT_MECA_FROT and JOINT_MECA_RUPT. The cleaving and sawing procedures are not activated.

Modeling supported: PLAN_JOINT, AXIS_JOINT, 3D_JOINT,,, PLAN_JOINT_HYME, 3D_JOINT_HYME.
Number of internal variables: 20
Example: see tests SSNP164a /b/c/d/e/f

4.4.7.21. Behavior ENDO_HETEROGENE#

Law ENDO_HETEROGENE is an isotropic damage model representing the formation and propagation of cracks based on a distribution of micro-defects given by a Weibull model. The presence of cracks in the structure is modelled by lines of broken elements (\(d\mathrm{=}1\)). Element breakage can be caused either by the initiation of a new crack or by propagation (see [R7.01.29] for more details). It is therefore a model with two thresholds. This law is adapted to heterogeneous materials such as argillite for example.

The characteristics of the material are defined in the operator DEFI_MATERIAU [U4.43.01] under the keywords ENDO_HETEROGENE, ELAS and NON_LOCAL.

Non-local modeling supported: D_PLAN_GRAD_SIGM

Number of internal variables for modeling D_PLAN_GRAD_SIGM: 12
Meaning:
\(\mathrm{V1}\): damage value \(d\),
\(\mathrm{V2}\): healthy element (0), pointed (1), broken by priming (2), broken by propagation (3)
\(\mathrm{V3}\): rupture stress by priming,
\(\mathrm{V4}\): breaking stress by propagation,
\(\mathrm{V5}\): number of the element pointed to number 1,
\(\mathrm{V6}\): number of the element pointed to number 2 (when priming),
\(\mathrm{V7}\): breaking Newton’s iteration,
\(\mathrm{V8}\): current Newton’s iteration,
\(\mathrm{V9}\): coordinate \(X\) of the crack point after rupture by propagation,
\(\mathrm{V10}\): coordinate \(Y\) of the crack point after rupture by propagation,
\(\mathrm{V11}\): coordinate \(X\) of the crack point 2 during priming,
\(\mathrm{V12}\): coordinate \(Y\) of the crack point 2 during priming,
Example: see ssnop147 and ssnp148 test

4.4.7.22. Behavior FONDATION#

Law FONDATION describes the nonlinear elastoplastic behavior of a rectangular surface foundation subjected to static or seismic three-dimensional stress. This law of behavior is affected on 3D discrete elements composed of a single translation and rotation node (DIS_TR) affected by a diagonal stiffness matrix (K_TR_D_N) by means of the relationship FONDATION called by the nonlinear problem solving operators STAT_NON_LINE [R5.03.01] or DYNA_NON_LINE [R5.05.05].

The key word used to define material characteristics in DEFI_MATERIAU is FONDA_SUPERFI.

The law represents both the sliding mechanism, the mechanism of loss of bearing capacity as well as the mechanism of detachment from the foundation. Before using one of the mechanisms mentioned above, all loading directions have linear elastic behavior described by classical stiffness characteristics.

Modeling supported: DIS_TR.
Number of internal variables: 21
Examples: See test cases SSNL201 and SSNL202.
Reference documentation: R5.03.31.

4.4.8. Behaviors specific to the modeling of concrete and reinforced concrete#

4.4.8.1. Behavior ENDO_ISOT_BETON#

Fragile elastic behavior relationship. It is a local modeling with scalar damage and negative linear isotropic work hardening that distinguishes the tensile and compressive behavior of concrete (see [R7.01.04] for more details). The characteristics of the material are defined in the operator DEFI_MATERIAU [U4.43.01] under the keywords BETON_ECRO_LINE and ELAS.

Local models supported: 3D, 2D, C_PLAN (by DE BORST), INCO_UPG, INCO_UP, CONT_1D (by DE BORST)

Number of internal variables: 2
Meaning: \(\mathrm{V1}\): damage value, \(\mathrm{V2}\): damage indicator (0 for elastic regime (zero damage), 1 if damaged, 2 if broken (damage equal to 1)).
Example: see test SSNV149.

4.4.8.2. Behavior ENDO_FISS_EXP#

Non-local quasifragile behavior relationship intended for modeling concrete cracking at the scale of the individual crack. The model introduces a characteristic damage threshold for concrete, restores some of the stiffness in the directions of compression stresses and tends towards a cohesive law when the internal length (the non-local scale) tends to zero (see [R5.03.28] for more details). The characteristics of concrete are ideally defined in the operator DEFI_MATER_GC [U4.42.07] in terms of engineer quantities or, otherwise, in the operator DEFI_MATERIAU [U4.43.01] (keywords factors ENDO_FISS_EXP, ELAS and NON_LOCAL) to fill in the values of the internal parameters of the law.

Local modeling not supported.

Non-local modeling supported: GRAD_VARI

Number of internal variables: 9
Meaning: V1 = damage value, V2 = damage indicator (0 for elastic regime (zero damage), 1 if damaged, 2 if broken (damage equal to 1)) V3 = residual stiffness, V4 to V9 = mechanical deformation at the end of the time step (used in case of recovery with mesh adaptation)
Example: see tests SSNL125, SSNP168,, SSNV234, SSNA119

4.4.8.3. Behavior ENDO_LOCA_EXP#

A local quasifragile behavior relationship intended for modeling concrete cracking at the scale of homogeneous cracked areas, see [R4.01.42]. The model introduces a characteristic damage threshold for concrete and restores some of the stiffness in the directions of compression stresses. It provides a homogeneous response approximately identical to the averaged localized response of the ENDO_FISS_EXP model under confined uniaxial stress. The characteristics of concrete are ideally defined in the operator DEFI_MATER_GC [U4.42.07] in terms of engineer quantities or, otherwise, in the operator DEFI_MATERIAU [U4.43.01] (keywords factors ENDO_LOCA_EXP, ELAS) to fill in the values of the internal parameters of the law.

Supported models: 3D, D_PLAN, AXIS. Modeling C_PLAN is not available natively; it is only provided by the DE BORST feature.

Number of internal variables: 5

V1 = damage value
V2 = damage indicator (0 for elastic regime, 1 if damaged, 2 if broken)
V3 = damage expressed in terms of residual stiffness
V4 = elastic deformation energy volume density
V5 = volume density of energy consumed by the damage mechanism

Examples: see tests SSNV261A, SSNV147K, SSNV147L

4.4.8.4. Behavior ENDO_SCALAIRE#

Fragile elastic behavior relationship. It is a non-local modeling with scalar damage and negative work-hardening that distinguishes between tensile and compressive behavior with respect to the load surface (see [R5.03.25] for more details). The characteristics of the material are defined in the operator DEFI_MATERIAU [U4.43.01] under the keywords ENDO_SCALAIRE, NON_LOCAL and ELAS.

Local modeling not supported.

Non-local modeling supported: GRAD_VARI

Number of internal variables: 3
Meaning: \(\mathit{V1}\): damage value, \(\mathit{V2}\): damage indicator (0 for elastic regime (zero damage), 1 if damaged, 2 if broken (damage equal to 1)) \(\mathit{V3}\): residual stiffness
Example: see tests SSNL125, SSNP146,, SSNV223, SSNA119

4.4.8.5. Behavior ENDO_CARRE#

Fragile elastic behavior relationship. This is a non-local modeling with quadratic regularized damage and negative isotropic work hardening, which distinguishes between compression and tensile behavior (see [R5.03.26] for more details). The characteristics of the material are defined in the operator DEFI_MATERIAU [U4.43.01] under the keywords ECRO_LINE, NON_LOCAL and ELAS.

Local modeling not supported.

Non-local modeling supported: GVNO

Number of internal variables: 2
Meaning: \(\mathrm{V1}\): damage value, \(\mathrm{V2}\): damage indicator (0 for elastic regime (zero damage), 1 if damaged

Example: see tests SSNP307, SSNA119, SSNV220

4.4.8.6. Behaviour ENDO_ORTH_BETON#

Relationship of anisotropic behavior of concrete with damage [R7.01.09]. This is a local modeling of damage taking into account the closure of cracks. The characteristics of the materials are defined in the operator DEFI_MATERIAU under the keywords ELAS and ENDO_ORTH_BETON.

Local models supported: 3D, 2D, C_PLAN (by DE BORST), INCO, CONT_1D (by DE BORST)

Number of internal variables: 7
Meaning: \(\mathrm{V1}\) to \(\mathrm{V6}\): tensile damage tensor
\(\mathrm{V7}\): compression damage
Example: see test SSNV176

4.4.8.7. Behaviour MAZARS#

Fragile elastic behavior relationship. It makes it possible to account for the softening of concrete and distinguishes between tensile and compressive damage. A single scalar damage variable is used (see [R7.01.08] for more details). The characteristics of the material are defined in the operator DEFI_MATERIAU [U4.43.01] under the keywords MAZARS and ELAS (_FO). In the case of thermal loading, the material coefficients depend on the maximum temperature reached at the Gauss point in question. In addition, the assumed linear thermal expansion does not contribute to the evolution of damage (same for desiccation shrinkage and endogenous shrinkage).

Local models supported: 3D, 2D, C_PLAN, INCO, CONT_1D (by DE BORST)

Number of internal variables: 4
Meaning: \(\mathit{V1}\): damage value, \(\mathit{V2}\): damage indicator (0 if not damaged, 1 if damaged), \(\mathit{V3}\): maximum temperature reached at the Gauss point in question, \(\mathit{V4}\): deformation equivalent to the Mazars meaning.
Example: see test SSNP113

4.4.8.8. Behaviour MAZARS_UNIL#

Fragile elastic behavior relationship. It makes it possible to account for the softening of concrete and distinguishes between tensile and compression damage using 2 variables (confer [R5.03.09] for more details). The characteristics of the material are defined in the operator DEFI_MATERIAU [U4.43.01] under the keywords MAZARS and ELAS.

MAZARS_UNIL corresponds to the one-sided writing of the Mazars model (Mu model).

Supported models: 1D, C_PLAN, 3D. Internal variables: 8 (confer [R5.03.09] for more details).

◦ \(\mathrm{V1}\): Criteria under constraint,

◦ \(\mathrm{V2}\) :Deformation criterion,

◦ \(\mathrm{V3}\): Damage,

◦ \(\mathrm{V4}\) :Equivalent tensile deformation,

◦ \(\mathit{V5}\) :Equivalent compression deformation,

◦ \(\mathit{V6}\) :Tri-axial ratio.

◦ \(\mathit{V7}\) :Maximum temperature reached in the material,

◦ \(\mathit{V8}\) :non-recoverable dissipation.

4.4.8.9. Behaviour ENDO_PORO_BETON#

ENDO_PORO_BETON is the concrete damage model developed within LMDC (Materials and Construction Sustainability Laboratory) in collaboration with the EDF Hydraulic Engineering Center. This damage module takes into account the asymmetry of concrete behavior (traction-compression), residual deformations and crack closure. In tension, the damage is described by an orthotropic tensor and in compression, the damage is described by an isotropic tensor. This module can also be coupled with module FLUA_PORO_BETON through the use FLUA_ENDO_PORO to take into account creep phenomena and also with the model RGI_BETON. Note that RGI_BETON is a set of three modules to take into account delayed deformations of concrete with FLUA_PORO_BETON, concrete damage with ENDO_PORO_BETON and internal swelling reactions (alkali-reaction and internal sulphatic) with RGI_BETON. To use it, it is necessary to fill in the material parameters in DEFI_MATERIAU: ENDO_PORO_BETON. [U4.43.01]

Supported models: 3D, 2D
Number of internal variables: 108
Meaning: see [R7.01.30]
Example: see test SSNV238 and SSNV239

4.4.8.10. Behaviour BETON_DOUBLE_DP#

A three-dimensional behavior relationship used to describe the nonlinear behavior of concrete. It includes a Drücker-Prager criterion in tension and a Drücker-Prager criterion in compression, decoupled. Both criteria can have softening work hardening. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords BETON_DOUBLE_DP and ELAS (_FO) (confer [R7.01.03] for more details). To facilitate the integration of this model, you can use the automatic local redistribution of the time step (see keyword ITER_INTE_PAS).

Supported models: 3D, D_PLAN and AXIS
Number of internal variables: 4
Meaning: \(\mathrm{V1}\): cumulative plastic deformation under compression, \(\mathrm{V2}\): cumulative plastic deformation under tension,: cumulative plastic deformation under tension, \(\mathrm{V3}\): maximum temperature reached at the Gauss point in question, \(\mathrm{V4}\): plasticity indicator (see Note 1).
Example: see test SSNV143.

4.4.8.11. Behaviour GRILLE_ISOT_LINE#

Isothermal behavior relationship of uniaxial Von Mises elastoplasticity with linear isotropic work hardening used for the modeling of reinforced concrete reinforcements. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ELAS and ECRO_LINE (refer to document [R5.03.09] for more detail).

Supported models: GRILLE
Number of internal variables: 4
Meaning: \(\mathrm{V1}\): cumulative plastic deformation in the longitudinal direction, \(\mathrm{V2}\): plasticity indicator (see Note 1).
Example: see test SSNS100

4.4.8.12. Behaviour GRILLE_CINE_LINE#

Isothermal behavior relationship of uniaxial Von Mises elastoplasticity with linear kinematic work hardening used for the modeling of reinforced concrete reinforcements. The necessary data for the material field are provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ELAS and ECRO_LINE (see document [R5.03.09] for more detail).

Supported models: GRILLE
Number of internal variables: 4
Meaning: \(\mathrm{V1}\): kinematic work hardening in the longitudinal direction, \(\mathrm{V2}\): plasticity indicator (see Note 1), \(\mathrm{V3}\): unused.
Example: see test SSNS100

4.4.8.13. Behaviour GRILLE_PINTO_MEN#

Pinto-Menegotto elastoplastic uniaxial isothermal behavior relationship for the modeling of reinforced concrete reinforcements under cyclic loading. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword PINTO_MENEGOTTO (enter document [R5.03.09] for more detail).

Supported models: GRILLE
Number of internal variables: 16
Meaning: cf. document [R5.03.09]
Example: see test SSNS100

4.4.8.14. Behaviour PINTO_MENEGOTTO#

Elastoplastic uniaxial isothermal behavior relationship modeling the response of steel reinforcements in reinforced concrete under cyclic loading. The necessary data for the material field are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword PINTO_MENEGOTTO (see document [R5.03.09] for more detail).

Supported models: CONT_1D
Number of internal variables: 8
Meaning: cf. document [R5.03.09]
Example: see test SSNS10

4.4.8.15. Behaviour GLRC_DAMAGE#

This law of behavior replaces an old version, GLRC. It is a global model of a reinforced concrete plate capable of representing its behavior up to the point of ruin. Unlike local models where each component of the material is modeled separately, in global models, the law of behavior is written directly in terms of constraints and generalized deformations. The phenomena taken into account are elastoplasticity coupled between membrane and flexural effects (compared to flexural elastoplasticity only in GLRC) and flexural damage. Coupled membrane/flexure damage is treated with GLRC_DM, which, on the other hand, completely neglects elastoplasticity. Material characteristics are defined in DEFI_MATERIAU (U4.43.01) under the GLRC_DAMAGE keyword. For details on the formulation of the model see [R7.01.31].

Attention, this law of behavior should not be used in non-linear analysis.

This law of behavior is mainly used for the chaining of calculations between Code_Aster and Europlexus.

Supported models: DKTG, Q 4GG
Number of internal variables. 19
Meaning: \(\mathrm{V1}\) to \(\mathrm{V3}\): plastic membrane extension, \(\mathrm{V4}\) to \(\mathrm{V6}\): plastic curvatures, V7: plastic dissipation, \(\mathrm{V8}\) to \(\mathrm{V9}\): damage variables for positive and negative bending respectively, \(\mathrm{V10}\): damage dissipation, to: \(\mathrm{V11}\) \(\mathrm{V13}\) orthotropy angles, \(\mathrm{V14}\) to \(\mathrm{V19}\): components of the kinematic work hardening tensor (3 for membrane forces, 3 for flexing moments).
Example: see tests SSNS104, SDNS108

4.4.8.16. Behaviour GLRC_DM#

This global model makes it possible to represent the damage of a reinforced concrete plate under moderate stresses. Unlike local models where each component of the material is modeled separately, in global models, the law of behavior is written directly in terms of constraints and generalized deformations. Modeling to breakage is not recommended, since plasticization phenomena are not taken into account, but are taken into account in GLRC_DAMAGE. In contrast, modeling the coupling of damage between membrane and flexure effects in GLRC_DM is taken into account, which is not the case in GLRC_DAMAGE. Material characteristics are defined in DEFI_MATERIAU [U4.43.01] under the key words GLRC_DM. For details on the formulation of the model see [R7.01.32].

Supported modeling: DKTG.

Number of internal variables: 18
\(\mathrm{V1}\) (ENDOFL +) to \(\mathrm{V2}\) (ENDOFL -): damage variables for positive and negative bending respectively
\(\mathrm{V3}\): INDIEND1: damage indicator corresponding to \(\mathrm{V1}\) (0 for elastic regime and 1 if the damage speed is not zero)
\(\mathrm{V4}\): INDIEND2: damage indicator corresponding to \(\mathrm{V2}\) (0 for elastic regime and 1 if the damage speed is not zero)
\(\mathrm{V5}\): ADOUTRAC: relative weakening of membrane stiffness under tension
\(\mathrm{V6}\): ADOUCOMP: relative weakening of membrane stiffness under compression
\(V7\): ADOUFLEX: relative weakening of stiffness during bending
\(V8\): ACIXELS: ratio between the deformation of the steel in the X direction (maximum between the lower and upper sheet) and the deformation EPSI_ELS
\(V9\): ACIXELU: ratio between the deformation of the steel in the X direction (maximum between the lower and upper sheet) and the deformation EPSI_ELU
\(V10\): ACIYELS: ratio between the deformation of the steel in the Y direction (maximum between the lower and upper sheet) and the deformation EPSI_ELS
\(V11\): ACIYELU: ratio between the deformation of the steel in the Y direction (maximum between the lower and upper sheet) and the deformation EPSI_ELU
\(V12\): BETSUP: ratio between the lowest main deformation (in compression) of the concrete on the upper side and the limiting deformation of the concrete in compression EPSI_C.
\(V13\): BETINF: ratio between the lowest main deformation (in compression) of concrete on the lower side and the limiting deformation of concrete in compression EPSI_C.
\(V14\): TRAMAX: maximum temporal deformation under traction
\(V15\): COMMAX: maximum temporal deformation in compression
\(V16\): FLEMAX: maximum temporal deformation during bending
\(V17\): ERRCOM: error expressed as a percentage between the areas of the curve under theoretical compression (defined by EPSI_C and FCJ) and the approximate curve (NYC, GAMMA_C) between 0 and COMMAX
\(V18\): ERRFLE: Error expressed as a percentage between the areas of the curve in theoretical bending (calculation of reinforced concrete section) and the approximate curve (MFY, GAMMA_F) between 0 and FLEMAX

Example: see test SSNS106.

4.4.8.17. Behaviour JONC_ENDO_PLAS#

Behavior JONC_ENDO_PLAS is a non-linear rheological behavior, of an elastic type, then damaging and finally integrating a plastic regime (irreversible deformations in rotation), making it possible to model a flexural junction between a wall and a floor or a raft, in reinforced concrete, in reinforced concrete, in out-of-plane bending, cf. [U2.02.03], applicable to the local degree of freedom of relative rotation \(\theta\) along the local axis \(\mathit{Oz}\), discrete elements in translation/rotation with two nodes (mesh SEG2), (see examples in the SSND114 test case).

The parameters characterizing the model are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword JONC_ENDO_PLAS, see also [R5.03.17]. The elastic stiffness \({K}_{e}\), which is used for the prediction phase of the nonlinear algorithm, is given via the affe_cara_elem [U4.42.01] command.

Supported models: DIS_TR.
Number of internal variables: 9.

\(V\mathrm{1 }\): differential rotation \({\theta }_{2}-{\theta }_{1}\) on the discrete element, along the local axis \(\mathrm{Oz}\), named ROTATOTA.

\(V\mathrm{2 }\): plastic rotation \({\theta }^{p}\) (along the local axis \(\mathrm{Oz}\)), named ROTAPLAS,

\(V\mathrm{3 }\): intermediate variable of rotation in positive flexure \({\theta }^{\text{+}}\), named ROTAPLUS,

\(V\mathrm{4 }\): intermediate variable of rotation in negative flexure \({\theta }^{\text{-}}\), named ROTAMOIN,

\(V\mathrm{5 }\): return moment variable associated with kinematic work hardening \(X={K}_{p}\mathrm{.}\alpha\), named XCIN_MZZ,

\(V6\): instantaneous dissipation \({D}_{\mathrm{diss}}\) (plastic damage and work-hardening mechanisms), called DISSTOTA,

\(V7\): internal damage variable \({D}^{\text{+}}\) in the lower wall (positive flexure), named ENDOPLUS,

\(V8\): internal damage variable \({D}^{\text{-}}\) in the upper wall (negative flexure), named ENDOMOIN,

\(V9\): variable for initializing damage thresholds (activated at the first time step), named INISEUIL.

Example: see test SSND114 [V6.08.114].

4.4.8.18. Behaviour DHRC#

This global model, formulated in generalized deformations and forces, makes it possible to represent the damage to a reinforced concrete plate as well as the steel/concrete slip resulting from the damage, for moderate cyclic stresses. Unlike local models where each component of the material is modeled separately, in global models, the law of behavior is written directly in terms of constraints and generalized deformations. Modeling to breakage is not recommended, since plasticization phenomena are not taken into account, but are taken into account in GLRC_DAMAGE. In contrast, modeling the coupling of damage between membrane and flexure effects in DHRC is taken into account, which is not the case in GLRC_DAMAGE. Compared to model GLRC_DM, model DHRC also makes it possible to represent: the steel/concrete sliding and the associated energy dissipation, the anisotropic elastic coupling in flexion-membrane resulting from any asymmetry between the lower and upper layers of steel. The characteristics of the material are to be provided in DEFI_MATERIAU [U4.43.01] under the keywords DHRC, based on prior homogenization calculations. For details on the formulation of the model see [R7.01.36].

Supported modeling: DKTG.

Number of internal variables: 9
\(\mathit{V1}\) to \(\mathit{V2}\): damage variables for positive and negative flexure respectively,
\(\mathit{V3}\) to \(\mathit{V6}\): steel/concrete slip variables: directions \(x\) and \(y\) (in local coordinate system) for steels in the upper layer then the same for steels in the lower layer,
\(\mathit{V7}\) to \(\mathit{V9}\): internal energy dissipation due to damage, internal energy dissipation due to slippage, and total dissipation (sum of the previous two).

Example: see test SSNS106.

4.4.8.19. Behaviour CORR_ACIER#

Damaging elastoplastic model for which the plastic deformation at break depends on the corrosion rate (cf. [R7.01.20]). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ELAS and CORR_ACIER.

Models: 3D, 2D, CONT_1D, CONT_1D (PMF)
3 internal variables:
\(\mathrm{V1}\): cumulative plastic deformation
\(\mathrm{V2}\): damage coefficient
\(\mathrm{V3}\): plasticity indicator (see Note 1)
Example: see test SSNL127.

4.4.8.20. Behaviour BETON_REGLE_PR#

Non-linear elastic concrete behavior relationship (developed by the company NECS) called « rectangular parabola ». The characteristics of the material are defined in the operator DEFI_MATERIAU [U4.43.01] under the keyword BETON_REGLE_PRet ELAS.

Law BETON_REGLE_PR is a concrete law similar to regulatory concrete laws (hence its name) that has the following summary characteristics:

it is a 2D law and more exactly 2 times 1D: in the natural deformation coordinate system, we write a 1D stress-deformation law;
the 1D law on each specific direction of deformation is as follows:
in traction, linear up to a peak, linear softening up to 0;
in compression, a power law up to a plateau (hence PR: parabola-rectangle).
Modelings: C_PLAN, D_PLAN

Example: see test SSNP129 or SSNS114

The equations for the model are described in [R7.01.27].

4.4.8.21. Behaviour JOINT_BA#

2D local behavioral relationship describing the phenomenon of the steel-concrete bond for reinforced concrete structures. It makes it possible to account for the influence of the bond in the redistribution of stresses in the concrete body as well as the prediction of cracks and their spacing. Available for monotonic and cyclic loading, it takes into account the effects of crack friction, and confinement. A single scalar damage variable is used (see [R7.01.21] for more details). The characteristics of the material are defined in the operator DEFI_MATERIAU [U4.43.01] under the keywords JOINT_BA and ELAS.

Supported models: PLAN_JOINT and AXIS_JOINT.
Number of internal variables: 6
Meaning: \(\mathrm{V1}\): damage value in the normal direction, \(\mathrm{V2}\): damage value in the tangential direction,: damage value in the tangential direction, \(\mathrm{V3}\): scalar variable of isotropic work hardening for damage in mode 2,: scalar variable of isotropic work hardening for damage in mode 2, \(\mathrm{V5}\): cumulative sliding deformation due to crack friction, \(\mathrm{V4}\) \(\mathrm{V6}\): value of kinematic work hardening by friction of cracks.
Example: see test SSNP126

4.4.8.22. Behavior BETON_GRANGER#

Behavioral relationship for modeling concrete creep. The required data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword BETON_GRANGER (see [R7.01.01] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D (by DE BORST), CONT_1D (PMF)
Number of internal variables: 55
Meaning: see [R7.01.01]
Example: see test SSNP116

4.4.8.23. Behavior BETON_GRANGER_V#

Behavioral relationship for modeling concrete creep taking into account the phenomenon of aging. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword V_BETON_GRANGER (confer [R7.01.01] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST), CONT_1D (by DE BORST)
Number of internal variables: 55
Meaning: see [R7.01.01]
Example: see test YYYY117

4.4.8.24. Behavior BETON_UMLV#

Behavioral relationship for modeling concrete creep taking into account the distinction between volume creep and deviatoric creep in order to account for phenomena in cases of multiaxial creep. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword BETON_UMLV (confer [R7.01.06] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST),
Number of internal variables: 21
Meaning: see [R7.01.06]
Example: see test SSNV163

4.4.8.25. Behavior BETON_RAG#

Behavioral relationship for modeling structures affected by the alkali-granulate reaction. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword BETON_RAG (confer [R7.01.26] for more details).

Supported models: 3D, AXIS, D_PLAN
Number of internal variables: 33
Meaning: see [R7.01.26]

4.4.8.26. Behavior BETON_BURGER#

Behavioral relationship for modeling concrete creep taking into account the distinction between volume creep and deviatoric creep in order to account for phenomena in cases of multiaxial creep. Taking into account the thermo-activation of creep deformations via an Arrhenius law. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword BETON_BURGER (confer [R7.01.35] for more details).

Supported models: 3D, 2D, C_PLAN (by DE BORST),
Number of internal variables: 33
Meaning: see [R7.01.35]
Example: see tests SSNV163, SSNV174,, SSNV180,, SSNV181 and SSNV235

4.4.8.27. Behavior FLUA_PORO_BETON#

FLUA_PORO_BETON is the concrete creep model developed within LMDC (Materials and Construction Sustainability Laboratory) in collaboration with the EDF Hydraulic Engineering Center. This creep module takes into account all delayed deformations (shrinkage, desiccation creep and clean creep) using poromechanical modeling and a BURGER diagram. This module belongs to model RGI_BETON. Note that RGI_BETON is a set of three modules to take into account delayed deformations of concrete with FLUA_PORO_BETON, concrete damage with ENDO_PORO_BETON and internal swelling reactions (alkali-reaction and internal sulphatic) with RGI_BETON. To use it, it is necessary to fill in material parameters FLUA_PORO_BETON in DEFI_MATERIAU.

Supported models: 3D, 2D
Number of internal variables: 108
Reference documentation: R7.01.30
Example: see tests SSNV235 and SSNV236

4.4.8.28. Behavior RGI_BETON#

RGI_BETONest the concrete swelling reaction model (alkali-reaction and internal sulphatic) developed at LMDC (Construction Materials and Sustainability Laboratory) in collaboration with the EDF Hydraulic Engineering Center. This module belongs to model RGI_BETON. Note that RGI_BETON is a set of three modules to take into account delayed deformations of concrete with FLUA_PORO_BETON, damage to concrete with ENDO_PORO_BETON and internal swelling reactions with RGI_BETON. To use it, it is necessary to fill in material parameters RGI_BETON in DEFI_MATERIAU.

Supported models: 3D, 2D
Number of internal variables: 108
Reference documentation: R7.01.30

4.4.8.29. Behavior RGI_BETON_BA#

RGI_BETON_BAest an extension of RGI_BETON allowing to model a reinforced concrete matrix without differentiating the mesh of the two materials. The behaviors of the two materials are evaluated independently and then homogenized and coupled in order to deduce the response of reinforced concrete. This extension is also developed within the LMDC (Materials and Construction Sustainability Laboratory) in collaboration with the EDF Hydraulic Engineering Center. To use it, it is necessary to fill in material parameters RGI_BETON_BA in DEFI_MATERIAU.

Supported models: 3D, 2D
Number of internal variables: 158
Reference documentation: R7.01.30 and R7.01.45

4.4.9. Mechanical behaviors for geo-materials#

Mechanical models for geo-materials (soils, rocks) can for the most part be used in mechanical models alone or in THM models, via the keywords KIT_HM, KIT_HHM, KIT_THM, KIT_THHM.

4.4.9.1. Behavior GONF_ELAS#

Behavioral relationship used to describe the behavior of « swelling clay » materials (bentonite). It is a non-linear elastic model relating net stress (\(\mathrm{contrainte}-\mathrm{Pgaz}\)) to swelling pressure, which in turn depends on suction (or capillary pressure). This model is developed for unsaturated HH models.

Supported models: HHM, THHM.
Number of internal variables: 0
Example: see the tests reproducing the swelling of a clay cell that is gradually saturated: plan (wtnp119a, b, c, d), axi (wtna110a, b, c, d) and 3D (wtnv136a, b, c, d) and 3D (wtnv136a, b, c, d)

4.4.9.2. Behavior MOHR_COULOMB#

Elastoplastic behavior relationship for calculations in soil mechanics. This is the simplest model used to represent, as a first approximation, the breaking behavior of a ground under monotonic loading. This model is a multi-criteria model characterized by the intersection of 6 planes in the space of the deviators of the main constraints (see [R7.01.28] for more details). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords MOHR_COULOMB and ELAS.

Supported models: 3D, 2D, THM.
Number of internal variables: 3
Meaning: \(\mathrm{V1}\): volume plastic deformation, \(\mathrm{V2}\): norm of deviatory deformations, \(\mathrm{V3}\): indicator of activation of plasticity (1) or not (0).
Example: see tests SSNV232, SSNV233,, SSNP104, WTNV142

4.4.9.3. Behavior CJS#

Elastoplastic behavior relationship for calculations in soil mechanics. This model is a multi-criteria model that includes a nonlinear elastic mechanism, an isotropic plastic mechanism, and a deviatory plastic mechanism (see [R7.01.13] for more details). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CJS and ELAS. To facilitate the integration of this model, you can use the automatic local redistribution of the time step (see keyword ITER_INTE_PAS).

Supported models: 3D, 2D, CONT_PLAN (by DE BORST), CONT_1D (by DE BORST), THM.
Number of internal variables: 16 in 3D and 14 in 2D
Meaning: \(\mathrm{V1}\): isotropic threshold, \(\mathrm{V2}\): angle of the deviatory threshold, \(\mathrm{V3}\) to \(\mathrm{V8}\) (V3 to V6 in 2D): 6 (4 in 2D) components of the kinematic work hardening tensor, \(\mathrm{V9}\) (\(\mathrm{V7}\) in 2D): distance normalized to the deviatory threshold, \(\mathrm{V10}\) (\(\mathrm{V8}\) in 2D): relationship between the deviatory threshold and the threshold critical deviatoric, \(\mathrm{V11}\) (\(\mathrm{V9}\) in 2D): distance normalized to the isotropic threshold, \(\mathrm{V12}\) (\(\mathrm{V10}\) in 2D): number of internal iterations, \(\mathrm{V13}\) (\(\mathrm{V11}\) in 2D): value of the local test to stop the iterative process, \(\mathrm{V14}\) (\(\mathrm{V12}\) in 2D): number of local redivisions of the time step, \(\mathrm{V15}\) (\(\mathrm{V13}\) in 2D): sign of the product contracted from the deviatoric stress by the deviatoric plastic deformation, \(\mathrm{V16}\) (\(\mathrm{V14}\) in 2D): indicator (0 if elastic, 1 if elastoplastic with isotropic plastic mechanism, 2 if elastoplastic with isotropic plastic mechanism, 2 if elastoplastic with deviatory plastic mechanism, 2 if elastoplastic with isotropic and deviatory plastic mechanisms).
Example: see tests SSNV135, SSNV136,, SSNV154, WTNV100

4.4.9.4. Behavior LAIGLE#

Behavioral relationship for rock modeling using the Lagle model. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword LAIGLE (Cf. document [R7.01.15] for more details). To facilitate the integration of this model, you can use the automatic local redistribution of the time step (keyword ITER_INTE_PAS).

Supported models: 3D, 2D, THM
Number of internal variables: 4
Meaning: \(\mathrm{V1}\): cumulative plastic deviatory deformation, \(\mathrm{V2}\): cumulative plastic volume deformation, \(\mathrm{V3}\) rock behavior domains, \(\mathrm{V4}\): condition indicator.
Example: see test SSNV158, WTNV101

4.4.9.5. Behavior LETK#

Behavioral relationship for the elastoviscoplastic modeling of rocks according to the Lagle and Kleine model. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword LETK (Cf. document [R7.01.24] for more details). Since the tangent operator is not validated, it is possible to use the disturbance matrix under the keyword TYPE_MATR_TANG. The operator relating to elastic prediction is that of nonlinear elasticity specific to the law.

Supported models: 3D, 2D, THM
Number of internal variables: 7
Meaning: \(\mathrm{V1}\): elastoplastic work hardening variable, \(\mathrm{V2}\): plastic deviatoric deformation,: plastic deviatory deformation,: plastic deviatory strain,: deviatory viscoplastic strain, \(\mathrm{V5}\): indicator of contraction (0) or of expansion (1),: indicator of plastic deformation,: indicator of plastic deformation (cf. \(\mathrm{V3}\) \(\mathrm{V4}\) \(\mathrm{V6}\) \(\mathrm{V7}\) Note 1)
Example: see tests SSNV206A, WTNV135A

4.4.9.6. Behavior HOEK_BROWN#

Modified Hoek and Brown behavior relationship for modeling rock behavior [R7.01.18] for pure mechanics. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword HOEK_BROWNP. To facilitate the integration of this model, it is possible to use the local automatic redistribution of the time step (see keyword ITER_INTE_PAS).

Supported models: 3D, 2D, C_PLAN
Number of internal variables: 3
Meaning: see [R7.01.18]
Example: see test SSNV184

4.4.9.7. Behavior HOEK_BROWN_EFF#

Modified Hoek and Brown behavior relationship for modeling rock behavior [R7.01.18] in THM. The coupling is formulated into effective constraints. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword HOEK_BROWNP. To facilitate the integration of this model, it is possible to use the local automatic redistribution of the time step (see keyword ITER_INTE_PAS).

Supported models: THM
Number of internal variables: 3
Meaning: see [R7.01.18]
Example: see test WTNV128

4.4.9.8. Behavior HOEK_BROWN_TOT#

Modified Hoek and Brown behavior relationship for modeling rock behavior [R7.01.18] in THM. The coupling is formulated in total constraints. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword HOEK_BROWNP. To facilitate the integration of this model, it is possible to use the local automatic redistribution of the time step (see keyword ITER_INTE_PAS).

Supported models: THM
Number of internal variables: 3
Meaning: see [R7.01.18]
Example: see test WTNV129

4.4.9.9. Behavior CAM_CLAY#

Elastoplastic behavior relationship for calculations in normally consolidated soil mechanics (Cf. [R7.01.14] for more details). The elastic part is non-linear. The plastic part may be hardening or softening. The data required for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords CAM_CLAY and ELAS.

If model CAM_CLAY is used with modeling THM, the keyword PORO entered under CAM_CLAY and under THM_INIT must be the same.

Modeling supported: 3D, 2D and THM
Number of internal variables: 2
Meaning: \(\mathrm{V1}\): volume plastic deformation, \(\mathrm{V2}\): plasticity indicator (see Note 1).
Example: see tests SSNV160, WTNV122

4.4.9.10. Behavior BARCELONE#

Relationship describing the elastoplastic mechanical behavior of unsaturated soils coupled with hydraulic behavior (Cf. [R7.01.14] for more details). This model is reduced to the Cam-Clay model in the saturated case. Two criteria are involved: a mechanical plasticity criterion (that of Cam-Clay) and a water criterion controlled by suction (or capillary pressure). This model should be used in KIT_HHM or KIT_THHM relationships. The data required for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords BARCELONE, CAM_CLAY and ELAS.

Modeling supported: THM
Number of internal variables: 5
Meaning: \(\mathrm{V1}\): \(p\) critical (1/2 consolidation pressure), \(\mathrm{V2}\): plasticity indicator (see Note 1) mechanical, \(\mathrm{V3}\): water threshold, \(\mathrm{V4}\): water irreversibility indicator, \(\mathrm{V5}\): \(\mathrm{Ps}\) (cohesion).
Example: see test WTNV123

4.4.9.11. Behavior DRUCK_PRAGER#

Associated Drucker-Prager type behavior relationship for soil mechanics (see [R7.01.16] for more details). The characteristics of the material are defined in the operator DEFI_MATERIAU [U4.43.01] under the keywords DRUCK_PRAGER and ELAS (_FO). However, it is assumed that the thermal expansion coefficient is constant. Work hardening can be linear or parabolic.

Modeling supported: THM, 3D, 2D
Number of internal variables: 3
\(\mathrm{V1}\): cumulative plastic deviatory deformation, \(\mathrm{V2}\): cumulative plastic volume deformation, V3 status indicator.
Example: see tests SSNV168, WTNA101

4.4.9.12. Behavior DRUCK_PRAG_N_A#

Drucker-Prager type behavior relationship not associated for soil mechanics (see [R7.01.16] for more details). The characteristics of the material are defined in the operator DEFI_MATERIAU [U4.43.01] under the keywords DRUCK_PRAGER and ELAS (_FO). However, it is assumed that the thermal expansion coefficient is constant. Work hardening can be linear, parabolic, or exponential.

Modeling supported: THM, 3D, 2D
Number of internal variables: 9
\(\mathrm{V1}\): cumulative plastic deviatory deformation, \(\mathrm{V2}\): cumulative plastic volume deformation, \(V3\) status indicator. From \(V4\) to \(V9\), anelastic deformations.
Example: see test SSND104, SSNV168, WTNA101.

4.4.9.13. Behavior VISC_DRUC_PRAG#

Behavioral relationship for elasto-visco-plastic modeling of rocks. Elastoplasticity is of the Drucker-Prager type and the creep is a Perzyna power law. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword VISC_DRUC_PRAG (Cf. document [R7.01.22] for more details).

Modeling supported: 3D and THM
Supported models: 3D, 2D, THM
Number of internal variables: 4
Meaning: \(\mathrm{V1}\): viscoplastic work hardening variable, \(\mathrm{V2}\): plasticity indicator (see Note 1), \(\mathrm{V3}\): work-hardening level, \(\mathrm{V4}\): number of local iterations
Example: see tests SSNV211A, WTNV137A, WTNV138A

4.4.9.14. Behavior HUJEUX#

Cyclic elastoplastic behavior relationship for soil mechanics (granular geomaterials: sandy clays, normally consolidated or over-consolidated, gravel…). This model is a multi-criteria model that includes a non-linear elastic mechanism, three deviatory plastic mechanisms and an isotropic plastic mechanism (Cf. [R7.01.23] for more details). The data required for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords HUJEUX and ELAS. To facilitate the integration of this model, you can use the automatic local redistribution of the time step (keyword ITER_INTE_PAS).

Modeling supported: 3D and THM
Open integration schemes: “NEWTON”, “NEWTON_PERT”, “”, “”, “NEWTON_RELI”, “SEMI_EXPLICITE”, “BASCULE_EXPLICIT”, “SPECIFIQUE”
Number of internal variables: 50
Meaning: \(V1\) to \(V3\): strain hardening factors of monotonic deviatory mechanisms, \(V4\): strain hardening factor of the monotonic isotropic mechanism, \(V5\) to \(V7\): work hardening factors of cyclic deviatory mechanisms, \(V8\): strain hardening factor of the cyclic isotropic mechanism,: strain hardening factor of the cyclic isotropic mechanism, \(V9\) to \(V22\): history variables related to cyclic mechanisms, \(V23\): cumulative plastic volume deformation, \(V24\) to \(V31\): indicators of the state of monotonic and cyclic mechanisms, \(V32\): Hill criterion. “INDETAC3”, “HIS34”, “”, “,” HIS35 “,” “,” “,” XHYZ1 XHYZ2 THYZ1 “,” THYZ2 “,” “,” RHYZ “,” XHXZ1 “,” “,” “,” “,” “,” “,” “,” “,” “,” “,” XHXZ2 “,” “,” THXZ1 “THXZ2 RHXZ XHXY1 XHXY2 THXY1 THXY2 RHYZ
Example: see tests SSNV197, SSNV204, SSNV205,, WTNV132, WTNV133, WTNV134.

4.4.9.15. Behavior JOINT_BANDIS#

Nonlinear elastic behavior relationship for hydraulic seals in rock mechanics. In the direction normal to the joint, there is a hyperbolic relationship between the effective stress and the opening of the joint. In the tangential direction, we have linear elastic behavior. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword JOINT_BANDIS (enter document [R7.02.15] for more details).

Modeling supported: PLAN_JHMS, AXIS_JHMS
Number of internal variables: 1
Meaning: \(\mathrm{V1}\): longitudinal permeability of the crack
Example: see tests WTNP125, WTNP126.

4.4.9.16. Behavior LKR#

Behavioral relationship for thermo-elasto (visco) plastic modeling of rocks. The necessary data for the material field are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword LKR (cf. document [R7.01.40] for more details). Since the tangent operator is not complete, it is possible to use the disturbance matrix under the keyword TYPE_MATR_TANG. The operator relating to elastic prediction is that of nonlinear elasticity specific to the law.

Supported models: 3D, 2D, THM
Number of internal variables: 12
Meaning: \(V1\): work-hardening variable of the plastic mechanism, \(V2\): equivalent plastic deformation,: equivalent plastic deformation variable,: equivalent plastic deformation variable,: equivalent plastic deformation variable,: contraction (0) or expansion (1) indicator,: equivalent plastic deformation variable, \(V3\): viscoplasticity indicator, \(V4\): equivalent viscoplastic deformation indicator, \(V5\): indicator of contraction (0) or expansion (1),: indicator of dilatance (1), \(V6\): indicator of viscoplasticity, \(V7\): indicator of plasticity, \(V8\): volume mechanical elastic deformation, \(V9\): volume thermal elastic deformation,: volume thermal elastic deformation, \(V10\): volume plastic deformation, \(V11\): volume viscoplastic deformation, \(V12\): domain
Example: see tests SSNV206, WTNV135.

4.4.9.17. Iwan behavior#

Multicriteria elasto-plastic law of behavior in soil mechanics adapted for cyclic deviatoric behavior, written under MFront. Iwan’s law of behavior [R7.01.38] makes it possible to reproduce shear modulus degradation curves. The data required for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword “Iwan”.

Supported models: 3D
Open integration schemes: “NEWTON”, “NEWTON_PERT”,
Number of internal variables: 103
Meaning: \(V1\) to \(V6\): terms of the elastic strain tensor, \(V7\) to \(V18\): scalar plastic multipliers of the load surfaces, \(V19\) to \(V91\): terms of the kinematic strain tensors, \(V92\) to \(V103\): values of the load surface
Example: see tests MFRON02, COMP012,, SSNV205, SSNV207.

4.4.9.18. Mohr-Coulombas behavior#

Law of elastoplastic behavior in soil mechanics (granular geo-materials) adapted for monotonic loads, written under MFront *. This elastoplastic behavior law with a smoothed Mohr-Coulomb load surface [R7.01.43] makes it possible, for example, to analyze the load-bearing capacity of a geotechnical structure. The proposed smoothing of the Mohr-Coulomb criterion, compared to the law of origin [R7.01.28], aims to increase the robustness of the implicit numerical integration. The data required for the material field, as well as the smoothing parameters, are provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword “Mohrcoulombas”.

Supported models: “3D”, “AXIS”, “”, “D_PLAN”; “THM”
Open integration schemes: “NEWTON”,
Number of internal variables: 10 in 3D, 8 in 2D;
Meaning: \(V1\) to \(V6\) in 3D; \(V1\) to \(V4\) in 2D: components of the elastic deformation tensor, \(V7\) in 3D (\(V5\) in 2D): equivalent plastic deformation \({\Vert {\epsilon }^{p}\Vert }_{\mathit{VM}}\), \(V8\) in 3D (\(V6\) in 2D): volume plastic deformation \(\text{tr}{\epsilon }^{p}\) , \(V9\) in 3D (\(V7\) in 2D): density of mechanical energy dissipated \(D(t)={\int }_{0}^{t}\mathrm{\sigma }\mathrm{:}{d\mathrm{\epsilon }}^{p}\), \(V10\) in 3D (\(V8\) in 2D): indicator of activation of plasticity (1) or not (0).
Example: see test cases SSNV232, SSNV233,,, WTNV142, COMP012, SSNP104.

4.4.9.19. Behavior NLH_CSRM#

The law of behavior NLH_CSRM makes it possible to model the elasto-visco-plastic behavior of coherent geomaterials. It will eventually replace laws LETK and LKR.

The scope of use of model NLH_CSRMest for the time being limited to isotropic mechanical behavior. Taking into account structural anisotropy and the dependence of work hardenings on temperature — effective in the latest version of model LKR — will be the subject of future renderings; as will the dependence of the criteria on the third invariant of the stress deflector (Lode angle).

The NLH_CSRM model is part of the thermodynamic framework of generalized standard materials with two irreversible mechanisms,

Plastic mechanism — irreversible instantaneous behavior: hardening and/or softening workings, contracting or expanding volume behavior, influence of the average stress on the fragile nature of the compression response,…;
Viscoplastic mechanism — irreversible delayed behavior (Perzyna type): primary, secondary, and tertiary creep (ruin).

A coupling between these two mechanisms makes it possible — among other things — to represent the dependence of the maximum resistance of certain geomaterials on the stress rate.

This law was implicitly integrated via the MFront tool. Its reference documentation bears the key R7.01.46. The parameters to be entered in the operator DEFI_MATERIAU are 13 in number: 2 elastic parameters, 11 for the plastic and viscoplastic mechanisms. YoungModulus and Poisson Ratio should be entered in the keywords factor ELASet NLH_CSRM.

Supported models: “3D”, “AXIS”, “”, “D_PLAN”, “THM”, “THHM”,…
Integration diagrams: “NEWTON” implicit,
Number of internal variables: 24 in 3D, 18 in 2D
Example: see test cases SSNV206, WTNV135,, COMP012, COMP001.

4.4.9.20. Behavior MCC#

Behavioral model MCC makes it possible to qualitatively represent the phenomenology of granular soils under monotonic loads, taking into account the effects of dilatance/contraction, softening/hardening, as well as the critical state. It updates the formulation and the numerical resolution method of law CAM_CLAY [R7.01.14], while remaining faithful to the elements of phenomenology predicted by the law, in order, ultimately, to replace it. Model MCC is a generalized standard. Behavioral equations are solved using an implicit direct time integration method in MFront. The reference documentation for model MCC has the key [R7.01.48]. The parameters to be entered in the operator DEFI_MATERIAU under the keyword MCC are seven in number: three parameters define isotropic non-linear elasticity, three parameters characterize the initial elasticity domain, and a last one controls kinematic-isotropic work hardening combined with volume plastic deformation. In the keyword ELAS, we enter the Young’s modulus and the Poisson’s ratio derived from the initial compressibility and shear modules of the MCC model.

Supported models: “3D”, “AXIS”, “”, “D_PLAN”, “THM”, “THHM”…
Integration diagrams: “NEWTON” implicit
Number of internal variables: 12 in 3D, 10 in 2D
Example: see test cases SSNV160, SSNV202,, COMP012, WTNV122

4.4.9.21. Behavior CSSM#

Behavioral model CSSM (« Critical State Soil Model ») is a combination of two models aimed at representing the monotonic and cyclical drained behavior of soils, respectively. The first component is based on the modified Cam-Clay model, which describes the phenomena of dilatance or contraction as well as confinement effects under monotonic and drained loads. The second component is an Iwan multi-mechanism model, designed to represent the cyclical nonlinear behavior of soils at low levels of deformation. The model adheres to the framework of generalized standard materials. Behavioral equations are solved using an implicit direct time integration method, implemented in MFront. The reference documentation for model CSSM has the key [R7.01.49]. The behavior model CSSM includes a total of eleven parameters to be entered in the DEFI_MATERIAU operator: two to describe the reversible (elastic) behavior, five for the irreversible behavior related to the modified Cam-Clay component, and three for the irreversible behavior associated with the Iwan component. A final parameter weighs the contributions of the two components on the shear behavior of model CSSM. In the keyword ELAS, we fill in the Young’s modulus and the Poisson’s ratio derived from the compressibility and shear modules of the model.

Supported models: “3D”, “AXIS”, “”, “D_PLAN”, “THM”, “THHM”…
Integration diagrams: “NEWTON” implicit
Number of internal variables: 71 in 3D, 49 in 2D
Example: see test cases SSNV160, SSNV205,,, SSNV207, COMP012, WTNV122

4.4.9.22. Behavior VMIS_ISOT_CUVE#

Law of elastoplastic behavior for irradiated tank steel, based on multiscale modeling of the plasticity of materials with a cubic-centered structure. The law is monotonic with non-linear isotropic work hardening, written under MFront. The input parameters are the experimental characteristics of the microstructure [R4.04.06]. If microstructural data is not known, the law makes it possible to reproduce traction curves at any temperature and any deformation rate from a single tension curve at a given temperature and deformation rate. The parameters of the law with their meanings (including typical values for the base metal) are entered in the operator DEFI_MATERIAU [U4.43.01], under the keyword “VMIS_ISOT_CUVE”.

Supported models: “3D”, “AXIS”, “D_PLAN”
Open integration schemes: “NEWTON_PERT”
Number of internal variables: 9 in 3D, 7 in 2D
Meaning:: \(V1\) to \(V6\) in 3D; \(V1\) to \(V4\) in 2D: components of the elastic deformation tensor, \(V7\) in 3D; \(V5\) in 2D: equivalent cumulative plastic deformation (EquivalentPlasti), \(V8\) in 3D; \(V6\) in 3D; in 2D: equivalent cumulative plastic deformation (EPSPEQ), \(V9\) in 3D; \(V7\) in 2D: indicator of activation of plasticity (1) or not (0)
Example: see test cases MFRON07, SSNA128

4.4.10. Behaviors integrated by external software#

It is important to note that the use of these laws of behavior in their own way implies specific validation for the study under consideration, because we place ourselves outside the field qualified of code_aster.

4.4.10.1. Tag UMAT#

♦ NB_VARI = nbvar

Umat is a Fortran routine format familiar to users of Abaqus code, used to integrate their own laws of behavior.

The dynamic library containing the Umat routine must be prepared before the calculation is run. To do this, the user has an easy way to compile this library using the as_run --make_shared utility (cf. [U1.04.00]).

The coupling between Umat and code_aster is reflected in the command file as follows:

at the level of COMPORTEMENT, the keyword RELATION =” UMAT “;
still under COMPORTEMENT, the NB_VARI keyword allows you to specify the number of internal variables of the behavior, and of course the usual keywords GROUP_MA, DEFORMATION;
we indicate the path to the library under the keyword LIBRAIRIE and the name of the symbol (name of the routine contained in the library) under the keyword NOM_ROUTINE;
the hypothesis of plane constraints is taken into account by méthode de De Borst;
keywords related to local integration (RESI_INTE, ITER_INTE_MAXI,,, ALGO_INTE, PARM_THETA) are not used.

The required data for the material field is provided in operator DEFI_MATERIAU, under the keyword UMAT/UMAT_FO.

The current limitations of the interface between code_aster and Umat are:

energy output (for the moment, they are not recovered by**code_aster**);
at the same time no thermo-mechanical coupling for the moment.

For more details on the use of Umat in code_aster, refer to dedicated notice d’utilisation.

Supported models: 3D, AXIS, D_PLAN.
Example: see tests umat001, umat002.

4.4.10.2. Tag MFRONT#

< https://thelfer.github.io/tfel/web/index.html>` #dnt_bgneijpdeolbkhilpiafkaljopoflgjo`_ is a code generator that makes it easy to write and integrate laws of behavior. It is developed by the CEA Cadarache as part of the PLEIADES platform.

The dynamic library containing routine MFront must be prepared before the calculation is run. To do this, the user will use the CREA_LIB_MFRONT command.

The coupling between MFront and code_aster is reflected in the command file as follows:

at the level of COMPORTEMENT, the keyword RELATION =” MFRONT “;
still under COMPORTEMENT, the usual keywords GROUP_MA, DEFORMATION (you can use in particular large deformations with “GDEF_LOG” and “GREEN_LAGRANGE”);
the behavior to be used is indicated under the COMPOR_MFRONT keyword, from CREA_LIB_MFRONT;
the hypothesis of plane constraints is taken into account by méthode de De Borst;
the RESI_INTE, ITER_INTE_MAXI keywords are transmitted to law MFront;
the keywords ALGO_INTE, PARM_THETA are not used.
option SYME_MATR_TANG allows you to say whether the behavior matrix will be symmetric (by default) or not.

The required data for the material field is provided in operator DEFI_MATERIAU, under the keyword MFRONT/MFRONT_FO.

If file MFront allows it, checks can be made on the values of the material parameters. The behavior when the limits are exceeded is controlled by the VERI_BORNE keyword which is set to “ARRET” by default. The other possible choices (for behavior in prototype mode) are “MESSAGE” (printing the message without interrupting the calculation) and “SANS” (the error is ignored).

For more information on the use of MFront in code_aster, refer to the dedicated notice d’utilisation.

Supported models: 3D, AXIS, D_PLAN.
Example: see tests mfron01, mfron02,, mfron03,, mfron05, mfron06.

4.4.11. Behaviour for multifibre beams#

4.4.11.1. Behavior MULTIFIBRE#

When the modeling includes elements of multifibre beams, it is necessary to indicate the meshes and groups of cells concerned by this modeling, in order to point to the right behavior: keyword RELATION =” MULTIFIBRE “under COMPORTEMENT.

The definition of the material is done using the commands: DEFI_COMPOR and AFFE_MATERIAU.

COMPF = DEFI_COMPOR (

GEOM_FIBRE =GF, MATER_SECT = BETON,

MULTIFIBRE = (

_F (GROUP_FIBRE =” SACI “, MATER = ACIER, RELATION =” VMIS_CINE_GC”),

_F (GROUP_FIBRE =” SBET “, MATER = BETON, RELATION =” MAZARS”),

CHMAT = AFFE_MATERIAU (

MAILLAGE =MY,

AFFE =_F (GROUP_MA = “POUTRE”, MATER = (ACIER, BETON,),),),

AFFE_COMPOR =_F (GROUP_MA = “POUTRE”, COMPOR = COMPF)

4.5. Operand RELATION_KIT under COMPORTEMENT#

For behaviors specific to concrete and porous media, RELATION_KIT makes it possible to couple several behaviors. For mechanical behaviors with the effects of metallurgical transformations, RELATION_KIT allows you to choose the type of material treated (ACIER or ZIRCALOY). Finally, to model cables that rub in their sheath (elements CABLE_GAINE), RELATION_KIT makes it possible to define the law of cable behavior and the law of friction of the cable in its sheath.

4.5.1. KIT associated with metallurgical behavior#

/'ACIER'

/'ZIRC'

Allows you to choose for all metallurgical behavior laws (META_xxx) to treat a steel-type or Zircaloy material. The material type ACIER comprises at most 5 different metallurgical phases, the material ZIRC comprises at most 3 different metallurgical phases.

Examples:

COMPORTEMENT = (RELATION = 'META_P_INL'
RELATION_KIT = 'ZIRC')

COMPORTEMENT = (RELATION = 'META_V_CL_PT_RE'
RELATION_KIT = 'ACIER')

4.5.2. KIT associated with the behavior of concrete: “KIT_DDI”#

Allows you to add two anelastic deformation terms defined by certain laws of behavior already existing in COMPORTEMENT (Cf. [R5.03.60] for more details). A concrete creep model with elastoplastic or damaging behavior can be assembled. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords ELAS (_FO) (the two laws must have the same modulus YOUNG) and those corresponding to the two models chosen.

Under the assumption that creep is a phenomenon that evolves more slowly than plasticity, the tangent matrix of the complete model is assimilated to that of plasticity. This choice will therefore require adapting the calculation increments to the times characteristic of the phenomena modelled in order not to handicap the calculation in terms of the number of iterations. In this case, the local convergence parameters (RESI_INTE and ITER_INTE_MAXI under the keyword CONVERGENCE) are the same for the integration of the two models.

With creep models:

“BETON_GRANGER”
“BETON_GRANGER_V”

The following behavioral models may be associated:

“BETON_DOUBLE_DP”
“VMIS_ISOT_TRAC”
“VMIS_ISOT_PUIS”
“VMIS_ISOT_LINE”
“ROUSS_PR”
“BETON_DOUBLE_DP”

With the creep model

“BETON_UMLV”

The following behavioral models may be associated:

“ENDO_ISOT_BETON”,
“MAZARS”

Supported models: 3D, 2D, CONT_PLAN (by DE BORST or ANALYTIQUE) depending on each model.

The internal variables of each law are accumulated in the table of internal variables, and returned law by law.

Example:

COMPORTEMENT = _F (RELATION = 'KIT_DDI'
RELATION_KIT = ('BETON_UMLV_FP', 'MAZARS'))

4.5.3. KIT associated with the behavior of porous media (thermo-hydro-mechanical models)#

For more details on thermo-hydro-mechanical models and behavior models, you can consult the documents [R7.01.10] and [R7.01.11], as well as the user manual [U2.04.05].

4.5.3.1. Keyword RELATION#

Relationships KIT_XXXX allow two to four equilibrium equations to be solved simultaneously. The equations considered depend on the suffix XXXX with the following rule:

M refers to the mechanical balance equation,
T denotes the thermal equilibrium equation,
H refers to a hydraulic balance equation.
V refers to the presence of a phase in vapor form (in addition to the liquid)

The associated thermo-hydro-mechanical problems are treated in a totally coupled manner.

A single letter H means that the porous medium is saturated (a single pressure variable \(p\)), for example either with gas, or liquid, or with a liquid/gas mixture (whose gas pressure is constant).

Two letters H mean that the porous medium is unsaturated (two pressure variables \(p\)), for example a liquid/vapor/gas mixture.

The presence of the two letters HV means that the porous medium is saturated by a component (in practice water), but that this component can be in liquid or vapor form. There is then only one conservation equation for this component, so only one degree of freedom pressure, but there is a liquid flow and a vapor flow.

The table below summarizes which kit each model corresponds to:

KIT_HM	D_PLAN_HM, D_PLAN_HMS, D_PLAN_HMD, AXIS_HM,,,, AXIS_HMS,, AXIS_HMD, 3D_HM, 3D_HMS, 3D_HMD
KIT_THM	D_PLAN_THM, D_PLAN_THMS, D_PLAN_THMD, AXIS_THM,,,, AXIS_THMS,, AXIS_THMD, 3D_THM, 3D_THMS, 3D_THMD
KIT_HHM	D_PLAN_HHM, D_PLAN_HHMS, D_PLAN_HHMD, AXIS_HHM,,,, AXIS_HHMS,, AXIS_HHMD, 3D_HHM, 3D_HHMS, 3D_HHMD
KIT_THH	D_PLAN_THHD, D_PLAN_THHS, AXIS_THHD,, AXIS_THHS,, 3D_THHD, 3D_THHS,
KIT_HH	D_PLAN_HHS, D_PLAN_HHD, AXIS_HHS,, AXIS_HHD,, 3D_HHS, 3D_HHD,
KIT_THV	D_PLAN_THVD, AXIS_THVD, 3D_THVD
KIT_THHM	D_PLAN_THHMS, D_PLAN_THHMD, AXIS_THHMS,, AXIS_THHMD,,, 3D_THHM, 3D_THHMS, 3D_THHMD
KIT_HH2	3D_HH2S 3D_HH2D 3D_HH2SUDA AXIS_HH2D AXIS_HH2S D_PLAN_HH2D D_PLAN_HH2S D_PLAN_HH2SUDA
KIT_THH2	D_PLAN_THH2D, AXIS_THH2D, 3D_THH2D,, D_PLAN_THH2S,, AXIS_THH2S, 3D_THH2S
KIT_HH2M	D_PLAN_HH2M, D_PLAN_HH2MS, D_PLAN_HH2MD, AXIS_HH2M,,,, AXIS_HH2MS,, AXIS_HH2MD, 3D_HH2M, 3D_HH2MS, 3D_HH2MD
KIT_THH2M	D_PLAN_THH2MD, AXIS_THH2MD, 3D_THH2MD D_PLAN_THH2MS, AXIS_THH2MS, 3D_THH2MS, D_PLAN_HH2M_SI

4.5.3.2. Keyword RELATION_KIT#

For each phenomenon modelled, we must specify in RELATION_KIT:

the model of mechanical behavior of the skeleton,
the behavior of liquids/gases,
hydraulic law.
HYDR_UTIL (if the mechanical behavior is without damage): Means that no material data has been entered « hard ». Concretely, in the saturated case, it will be necessary to define the following 6 curves point by point (by DEFI_FONCTION):
saturation as a function of capillary pressure,
the derivative of this curve,
the relative permeability of the liquid as a function of saturation,
its derivative.
the relative permeability to the gas as a function of saturation,
its derivative.
HYDR_VGM (if the mechanical behavior is without damage). Here and only for the liquid/gas coupling laws” LIQU_GAZ “,” LIQU_AD_GAZ “,” “,” “,” “,” LIQU_AD_GAZ “and” LIQU_VAPE_GAZ_VAPE “, the saturation and permeability curves relating to water and gas and their derivatives are defined by the Mualem Van-Genuchten model. The user must then fill in the parameters of this law \((n,\mathit{Pr},\mathit{Sr})\). The Mualem Van-Genuchten model is as follows:

\({k}_{r}^{w}=\sqrt{{S}_{\mathrm{we}}}{(1-{(1-{S}_{\mathrm{we}}^{1/m})}^{m})}^{2}\), \({k}_{r}^{\mathrm{gz}}=\sqrt{1-{S}_{\mathrm{we}}}{(1-{S}_{\mathrm{we}}^{1/m})}^{\mathrm{2m}}\)

and

\({S}_{\mathrm{we}}=\frac{1}{{(1+{(\frac{{P}_{c}}{{P}_{r}})}^{n})}^{m}}\) where \({S}_{\mathrm{we}}=\frac{{S}_{w}-{S}_{\mathrm{wr}}}{1-{S}_{\mathrm{wr}}-{S}_{\mathrm{gr}}}\) and \(m=1-\frac{1}{n}\)

HYDR_VGC (if the mechanical behavior is without damage). Exactly the same as HYDR_VGM except for the gas permeability law, which is a cubic law:

\({k}_{r}^{\mathrm{gz}}={(1-{S}_{w})}^{3}\)

HYDR_TABBAL (if the mechanical behavior is without damage). Only for the liquid/gas coupling laws” LIQU_VAPE_GAZ “,” LIQU_AD_GAZ “,” LIQU_AD_GAZ_VAPE “,” LIQU_GAZ “, “LIQU_GAZ”, “LIQU_GAZ_ATM”. The user must then fill in the parameters of this law:math: (t (mathit {HR}), {A} _ {0}, {S} _ {mathit {BJH}}}, {mathrm {omega}}} _ {mathrm {omega}}} _ {omega}} _ {omega}} _ {s} _ {s} _ {s}}right) |} _ {mu}) [voir [U2.04.05])) `[]) as well as, as in the HYDR_UTIL case, the saturation curves, derived from the saturation, the relative permeabilities and their derivatives.
HYDR_ENDO (if “MAZARS” or “ENDO_ISOT_BETON” is used) under RELATION_KIT (this keyword allows you to enter the saturation curve and its derivative as a function of capillary pressure as well as the relative permeability and its derivative as a function of saturation.

4.5.3.3. Mechanical behaviors of the skeleton (if there is mechanical modeling M)#

“ELAS”
“GONF_ELAS”
“MOHR_COULOMB”
“CJS”
“CAM_CLAY”
“BARCELONE”
“LAIGLE”
“DRUCK_PRAGER”
“DRUCK_PRAG_N_A”
“HOEK_BROWN_EFF”
“HOEK_BROWN_TOT”
“MAZARS”
“ENDO_ISO_BETON”
“HUJEUX”
“JOINT_BANDIS”
“Iwan”
“MohrCoulombas”
“MCC”
“CSSM”

4.5.3.4. Behaviors of liquids/gases#

'LIQU_SATU'

Behavioral law for a porous medium saturated by a single liquid (confer [R7.01.11] for more details). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword THM_LIQ.

'LIQU_GAZ'

Behavioral law for an unsaturated porous liquid/gas medium without phase change (confer [R7.01.11] for more details). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords THM_LIQ and THM_GAZ.

'GAZ'

Law of behavior of an ideal gas, that is, verifying the relationship \(P/\rho =\mathrm{RT}/\mathrm{Mv}\) where \(P\) is the pressure, \(\rho\) the density, \(\mathrm{Mv}\) the molar mass, \(R\) the Boltzman constant and \(T\) the temperature (confer [R7.01.11] for more details). For saturated medium only. The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keyword THM_GAZ.

'LIQU_GAZ_ATM'

Behavioral law for a porous medium unsaturated with a liquid and gas at atmospheric pressure (confer [R7.01.11] for more details). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords THM_LIQU.

'LIQU_VAPE_GAZ'

Behavioral law for an unsaturated porous water/vapor/dry air medium with phase change (confer [R7.01.11] for more details). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords THM_LIQ, THM_VAPE and THM_GAZ.

'LIQU_AD_GAZ_VAPE'

Behavioral law for an unsaturated porous water/vapor/dry air/dissolved air medium with phase change (confer [R7.01.11] for more details).

The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords THM_LIQ, THM_VAPE, THM_GAZ and THM_AIR_DISS.

'LIQU_AD_GAZE'

Behavioral law for an unsaturated porous water/dry air/dissolved air medium with phase change (confer [R7.01.11] for more details). So this is a vaporous version of the complete law below

The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords THM_LIQ, THM_GAZ and THM_AIR_DISS.

'LIQU_VAPE'

Behavioral law for a porous medium saturated by a component present in liquid or vapor form. with phase change (confer [R7.01.11] for more details). The necessary data for the material field is provided in the operator DEFI_MATERIAU [U4.43.01], under the keywords THM_LIQ and THM_VAPE

4.5.3.5. Hydraulic law#

“HYDR_UTIL” (if the mechanical behavior is without damage): Means that no material data has been entered « hard ». Concretely, in the saturated case, it will be necessary to define the following 6 curves point by point (by DEFI_FONCTION):

saturation as a function of capillary pressure,
the derivative of this curve,
the relative permeability of the liquid as a function of saturation,
its derivative.
the relative permeability to the gas as a function of saturation,
its derivative.

“HYDR_VGM” (if the mechanical behavior is without damage). Here and only for the liquid/gas coupling laws” LIQU_GAZ “,” LIQU_AD_GAZ_VAPE “,” “,” “,” “,” LIQU_AD_GAZ “and” LIQU_VAPE_GAZ “, the saturation and permeability curves relating to water and gas and their derivatives are defined by the Mualem Van-Genuchten model. The user must then fill in the parameters of this law \((n,\mathrm{Pr},\mathrm{Sr})\). The Mualem Van-Genuchten model is as follows:

\({k}_{r}^{\mathrm{gz}}=\sqrt{1-{S}_{\mathrm{we}}}{(1-{S}_{\mathrm{we}}^{1/m})}^{\mathrm{2m}}\) and \({S}_{\mathrm{we}}=\frac{1}{{(1+{(\frac{{P}_{c}}{{P}_{r}})}^{n})}^{m}}\)

where

\({S}_{\mathrm{we}}=\frac{{S}_{w}-{S}_{\mathrm{wr}}}{1-{S}_{\mathrm{wr}}-{S}_{\mathrm{gr}}}\) and \(m=1-\frac{1}{n}\).

“HYDR_VGC” (if the mechanical behavior is without damage). Here and only for the liquid/gas coupling laws” LIQU_GAZ “,” LIQU_AD_GAZ_VAPE “,” “,” “,” “,” LIQU_AD_GAZ “and” LIQU_VAPE_GAZ “, the saturation and permeability curves relating to water and their derivatives are defined by the Mualem Van-Genuchten model (see above). The relative permeability to gas is defined by a cubic law:

\({k}_{r}^{\mathrm{gz}}={(1-{S}_{w})}^{3}\)

The user must then fill in the parameters of this law \((n,\mathrm{Pr},\mathrm{Sr})\).

“HYDR_ENDO” (if “MAZARS” or “ENDO_ISOT_BETON” is used) under RELATION_KIT (this keyword makes it possible to enter the saturation curve and its derivative as a function of capillary pressure as well as the relative permeability and its derivative as a function of saturation.

4.5.3.6. Possible combinations#

Depending on the value of the keyword RELATION =” KIT_XXXX “chosen, not all behaviors are legal in RELATION_KIT (for example, if you choose an unsaturated porous medium, you cannot affect an ideal gas-type behavior). All possible combinations are summarized here.

For relationship KIT_HM and KIT_THM:

('ELAS' 'GAZ' '' HYDR_UTIL ')

('MOHR_COULOMB' 'GAZ' '' HYDR_UTIL ')

('CJS' 'GAZ' '' HYDR_UTIL ')

('HUJEUX' 'GAZ' '' HYDR_UTIL ')

('LAIGLE' 'GAZ' '' HYDR_UTIL ')

('CAM_CLAY' 'GAZ' '' HYDR_UTIL ')

('JOINT_BANDIS' 'GAZ' '' HYDR_UTIL ')

('MAZARS' 'GAZ' '' HYDR_ENDO ')

('ENDO_ISOT_BETON' 'GAZ' '' HYDR_ENDO ')

('ELAS' 'LIQU_SATU' '' HYDR_UTIL ')

('MOHR_COULOMB' 'LIQU_SATU' '' HYDR_UTIL ')

('CJS' 'LIQU_SATU' '' HYDR_UTIL ')

('HUJEUX' 'LIQU_SATU' '' HYDR_UTIL ')

('LAIGLE' 'LIQU_SATU' '' HYDR_UTIL ')

('CAM_CLAY' 'LIQU_SATU' '' HYDR_UTIL ')

('JOINT_BANDIS' 'LIQU_SATU' '' HYDR_UTIL ')

('MAZARS' 'LIQU_SATU' '' HYDR_ENDO ')

('ENDO_ISOT_BETON' 'LIQU_SATU' '' HYDR_ENDO ')

('ELAS' 'LIQU_GAZ_ATM' '' HYDR_UTIL ')

('MOHR_COULOMB' 'LIQU_GAZ_ATM' '' HYDR_UTIL ')

('CJS' 'LIQU_GAZ_ATM' '' HYDR_UTIL ')

('HUJEUX' 'LIQU_GAZ_ATM' '' HYDR_UTIL ')

('LAIGLE' 'LIQU_GAZ_ATM' '' HYDR_UTIL ')

('CAM_CLAY' 'LIQU_GAZ_ATM' '' HYDR_UTIL ')

('MAZARS' 'LIQU_GAZ_ATM' '' HYDR_ENDO ')

('ENDO_ISOT_BETON' 'LIQU_GAZ_ATM' '' HYDR_ENDO ')

For relationship KIT_HHMet KIT_THHM:

('ELAS' 'LIQU_GAZ' '' HYDR_UTIL ')

('GONF_ELAS' 'LIQU_GAZ' '' HYDR_UTIL ')

('MOHR_COULOMB' 'LIQU_GAZ' '' HYDR_UTIL ')

('CJS' 'LIQU_GAZ' '' HYDR_UTIL ')

('HUJEUX' 'LIQU_GAZ' '' HYDR_UTIL ')

('LAIGLE' 'LIQU_GAZ' '' HYDR_UTIL ')

('CAM_CLAY' 'LIQU_GAZ' '' HYDR_UTIL ')

('BARCELONE' 'LIQU_GAZ' '' HYDR_UTIL ')

('ELAS' 'LIQU_GAZ' '' HYDR_VGM ')

('GONF_ELAS' 'LIQU_GAZ' '' HYDR_VGM ')

('CJS' 'LIQU_GAZ' '' HYDR_VGM ')

('LAIGLE' 'LIQU_GAZ' '' HYDR_VGM ')

('CAM_CLAY' 'LIQU_GAZ' '' HYDR_VGM")

('BARCELONE' 'LIQU_GAZ' '' HYDR_VGM ')

('MAZARS' 'LIQU_GAZ' '' HYDR_ENDO ')

('ENDO_ISOT_BETON' 'LIQU_GAZ' '' HYDR_ENDO ')

('ELAS' 'LIQU_VAPE_GAZ' '' HYDR_UTIL ')

('GONF_ELAS' 'LIQU_VAPE_GAZ' '' HYDR_UTIL ')

('MOHR_COULOMB' 'LIQU_VAPE_GAZ' '' HYDR_UTIL ')

('CJS' 'LIQU_VAPE_GAZ' '' HYDR_UTIL ')

('HUJEUX' 'LIQU_VAPE_GAZ' '' HYDR_UTIL ')

('LAIGLE' 'LIQU_VAPE_GAZ' '' HYDR_UTIL ')

('CAM_CLAY' 'LIQU_VAPE_GAZ' '' HYDR_UTIL ')

('BARCELONE' 'LIQU_VAPE_GAZ' '' HYDR_UTIL ')

('ELAS' 'LIQU_VAPE_GAZ' '' HYDR_VGM ')

('GONF_ELAS' 'LIQU_VAPE_GAZ' '' HYDR_VGM ')

('CJS' 'LIQU_VAPE_GAZ' '' HYDR_VGM ')

('LAIGLE' 'LIQU_VAPE_GAZ' '' HYDR_VGM ')

('CAM_CLAY' 'LIQU_VAPE_GAZ' '' HYDR_VGM ')

('BARCELONE' 'LIQU_VAPE_GAZ' '' HYDR_VGM ')

('MAZARS' 'LIQU_VAPE_GAZ' '' HYDR_ENDO ')

('ENDO_ISOT_BETON' 'LIQU_VAPE_GAZ' '' HYDR_ENDO ')

('ELAS' 'LIQU_AD_GAZ_VAPE' '' HYDR_UTIL ')

('GONF_ELAS' 'LIQU_AD_GAZ_VAPE' '' HYDR_UTIL ')

('MOHR_COULOMB' 'LIQU_AD_GAZ_VAPE' '' HYDR_UTIL ')

('CJS' 'LIQU_AD_GAZ_VAPE' '' HYDR_UTIL ')

('HUJEUX' 'LIQU_AD_GAZ_VAPE' '' HYDR_UTIL ')

('LAIGLE' 'LIQU_AD_GAZ_VAPE' '' HYDR_UTIL ')

('CAM_CLAY' 'LIQU_AD_GAZ_VAPE' '' HYDR_UTIL ')

('BARCELONE' 'LIQU_AD_GAZ_VAPE' 'HYDR_UTIL') ('ELAS' '' LIQU_AD_GAZ_VAPE '' HYDR_VGM ')

('GONF_ELAS' 'LIQU_AD_GAZ_VAPE' '' HYDR_VGM ')

('CJS' 'LIQU_AD_GAZ_VAPE' '' HYDR_VGM ')

('LAIGLE' 'LIQU_AD_GAZ_VAPE' '' HYDR_VGM ')

('CAM_CLAY' 'LIQU_AD_GAZ_VAPE' '' HYDR_VGM ')

('BARCELONE' 'LIQU_AD_GAZ_VAPE' '' HYDR_VGM ')

('MAZARS' 'LIQU_AD_GAZ_VAPE' '' HYDR_ENDO ')

('ENDO_ISOT_BETON' 'LIQU_AD_GAZ_VAPE' '' HYDR_ENDO ')

('ELAS' 'LIQU_AD_GAZ' '' HYDR_UTIL ')

('GONF_ELAS' 'LIQU_AD_GAZ' '' HYDR_UTIL ')

('MOHR_COULOMB' 'LIQU_AD_GAZ' '' HYDR_UTIL ')

('CJS' 'LIQU_AD_GAZ' '' HYDR_UTIL ')

('HUJEUX' 'LIQU_AD_GAZ' '' HYDR_UTIL ')

('LAIGLE' 'LIQU_AD_GAZ' '' HYDR_UTIL ')

('CAM_CLAY' 'LIQU_AD_GAZ' '' HYDR_UTIL ')

('BARCELONE' 'LIQU_AD_GAZ' '' HYDR_UTIL ')

('ELAS' 'LIQU_AD_GAZ' '' HYDR_VGM ')

('GONF_ELAS' 'LIQU_AD_GAZ' '' HYDR_VGM ')

('CJS' 'LIQU_AD_GAZ' '' HYDR_VGM ')

('LAIGLE' 'LIQU_AD_GAZ' '' HYDR_VGM ')

('CAM_CLAY' 'LIQU_AD_GAZ' '' HYDR_VGM ')

('BARCELONE' 'LIQU_AD_GAZ' '' HYDR_VGM ')

('MAZARS' 'LIQU_AD_GAZ' '' HYDR_ENDO ')

('ENDO_ISOT_BETON' 'LIQU_AD_GAZ' '' HYDR_ENDO ')

For relationship KIT_THH and KIT_HH:

('LIQU_GAZ' 'HYDR_UTIL')

('LIQU_VAPE_GAZ' 'HYDR_UTIL')

('LIQU_AD_GAZ_VAPE' 'HYDR_UTIL')

('LIQU_AD_GAZ' 'HYDR_UTIL')

('LIQU_GAZ' 'HYDR_VGM')

('LIQU_VAPE_GAZ' 'HYDR_VGM')

('LIQU_AD_GAZ_VAPE' 'HYDR_VGM')

For relationship KIT_THV:

('LIQU_VAPE' 'HYDR_UTIL')

Note:

In case of convergence problems it can be very useful to activate the linear search as shown in the example given at the top of this section. However, linear research does not systematically improve convergence, so it should be handled with care.

Example:

COMPORTEMENT =_F (
    RELATION = 'KIT_THM',
    RELATION_KIT = ('LIQU_SATU', 'CJS', 'HYDR_UTIL'))

In this example, we treat a thermo-hydro-mechanical problem for a saturated porous medium in a coupled manner, LIQU_SATU as liquid behavior, CJS as mechanical behavior.

Other examples are available, either in the document [U2.04.05], or in the set of tests WTNAxxx, WTNLxxx, WTNPxxx, WTNVxxx.

4.5.4. KIT associated with the modeling of friction cables: KIT_CG#

To model friction or slippery cables, it is necessary to be able to specify both the behavior to be assigned to the cable and the law of friction behavior of the cable in its sheath. To do this, the RELATION keyword is given the value “KIT_CG”. In the keyword RELATION_KIT, you must enter the law of behavior of the cable (all those accepted by the BARRE modeling) and then the law of friction behavior which is always CABLE_GAINE_FROT.

For more details on the law of friction, you can consult the reference documentation for elements CABLE_GAINE [R3.08.10].

Example:

COMPORTEMENT = _F (RELATION = 'KIT_CG',
RELATION_KIT = ('ELAS', 'CABLE_GAINE_FROT'))

4.6. Operand DEFORMATION#

◊ DEFORMATION

This keyword makes it possible to define the hypotheses used for the calculation of deformations: by default, we consider small displacements and small deformations.

4.6.1. Deformation model PETIT#

The deformations used in the behavior relationship are the linearized deformations:

\({\mathrm{\epsilon }}_{\mathit{ij}}=\frac{1}{2}({u}_{i,j}+{u}_{j,i})\)

This means that we remain on the Small Perturbations Hypothesis: small displacements, small rotations, small deformations (less than about 5%)

4.6.2. Deformation model GREEN_LAGRANGE#

This kinematics links the Green-Lagrange strain tensor \(\mathrm{E}\) to the second stress Piola Kirchhoff (PK2) \(\mathrm{S}\):

\(\mathrm{E}=\frac{1}{2}({\mathrm{F}}^{T}\mathrm{F}-\mathit{Id})\)

\(\mathrm{\sigma }=\frac{1}{\mathit{det}(\mathrm{F})}(\mathrm{F}\mathrm{S}{\mathrm{F}}^{\mathrm{T}})\)

where \(\mathrm{F}\) refers to the transformation gradient (\({F}_{\mathit{ij}}={\mathrm{\delta }}_{\mathit{ij}}+{u}_{i,j}\)) and \(\mathrm{\sigma }\) the Cauchy constraint. We can refer to [R5.03.20].

Notes:

This kinematics is in particular adapted to the treatment of large deformations of hyperelastic materials (such as ELAS_HYPER).
This kinematics is not compatible with plane constraints.

4.6.3. Deformation model GROT_GDEP#

This kinematic formulation makes it possible to treat large rotations and large displacements, but while remaining in small deformations in the case of the following models:

to deal with large rotations and small deformations for all incremental behavior laws under COMPORTEMENT equipped with COQUE_3D models. It is a total Lagrangian formulation, allowing to calculate the exact configuration for large rotations [R3,07,05].

Attention:

It is strongly discouraged to use linear search for COQUE_3Davec the option GROT_GDEP (sometimes convergence is impossible and if we converge, the calculation needs more Newton iterations) .

to deal with large displacements and rotations and small deformations for plate and shell elements: models DKT (only in linear elasticity), DKTG (only with the behaviors GLRC_*) and SHB.
to treat large displacements and rotations and small deformations for models POU_D_TGM and POU_D_EM (multifibre beams) (formerly REAC_GEOM). The hypothesis is that the geometry is updated at each iteration and geometric rigidity is added to the material stiffness to form the tangent stiffness. For large rotations, instead of using a complex « exact » approach as for POU_D_T_GD and COQUE_3D, moderate rotations (of the second order) are allowed. This type of deformation calculation makes it possible to deal effectively with problems with multifibre beams with non-linear behavior, in moderate rotations [R3.08.09].

4.6.4. Deformation model PETIT_REAC#

The deformation increments used for the incremental behavior relationship are the linearized deformations of the displacement increment in the updated geometry. That is, if \(X,u,\Delta u\) respectively denote the position, displacement, and displacement increment calculated at a given iteration of a hardware point [R5.03.24].

\(\Delta {\epsilon }_{\mathrm{ij}}=\frac{1}{2}(\frac{\partial \Delta {u}_{i}}{\partial {(X+u)}_{j}}+\frac{\partial \Delta {u}_{j}}{\partial {(X+u)}_{i}})\)

The balance is therefore resolved on the current geometry but the behavior remains written under the hypothesis of small deformations. Consequently, the use of PETIT_REAC is therefore not appropriate for large rotations but it is suitable for large deformations, under certain conditions [10]:

very small increments,
very small rotations (which implies a loading that is almost radial)
small elastic deformations compared to plastic deformations,
isotropic behavior.

Apart from these hypotheses, this approximation can give very poor results. It is therefore necessary to verify the convergence of the results in relation to discretization.

Attention:

It is not recommended to use this option with structural elements COQUE, , COQUE_1Det POU (an alarm message appears in the.mess file) .

4.6.5. Deformation model SIMO_MIEHE#

It is an incrementally objective formulation in large deformations of the laws of behavior based on a Von Mises criterion with isotropic work hardening. The elastic stress-strain relationship is hyperelastic. All the information on the \(F\) transformation gradient is taken into account, both the rotation and the deformations:

\({F}_{\mathrm{ij}}={\delta }_{\mathrm{ij}}+\frac{\partial {u}_{i}}{\partial {x}_{j}}\)

This makes it possible to perform calculations in large plastic deformations, with the behavioral relationships” VMIS_ISOT_LINE “,” VMIS_ISOT_TRAC “,” ROUSSELIER “and all the behaviors, with isotropic hardening only, associated with a material undergoing metallurgical phase changes (relationships META_X_IL_XXX_XXX and META_X_INL_XXX_XXX,).

This formulation automatically adds 6 internal variables to the chosen behavior, storing at the end the 6 components of the \(\frac{1}{2}({I}_{d}-{b}^{e})\) tensor (cf. [R5.03.21]).

Attention:

This option is only valid for models 3D, 3D, 2D, INCO_UPG (no plane constraint with the DE BORST method). For more information on the formulation of large plastic deformations according to SIMO and MIEHE, we can refer to [R5.03.21].

In large “SIMO_MIEHE” deformations, tangent matrices are not symmetric except for the (hyper) -elastic case. Until version 7.4, the matrix was systematically symmetrized. From now on, it is the non-symmetric matrix that is**provided. If he wishes, the user can nevertheless ask to symmetrize it under the keyword SOLVEUR = _F (SYME = “OUI”). Attention: SYME = “OUI” is not the default. Resolutions will therefore take longer with this new version if nothing has been done with regard to the command file. On the other hand, the non-symmetric tangent matrix will allow better convergence.

4.6.6. Deformation model GDEF_LOG#

It is a formulation in large deformations using a logarithmic deformation measure, resulting from an approach due to Miehe, Apel, Lambrecht. It makes it possible to use the following incremental elastoplastic or visco-plastic behavior laws (cf. [R5.03.24]):

VMIS_ISOT_ , VMIS_JOHN_COOK, VMIS_CINE_LINE, VMIS_ECMI_, VMIS_CIN *_,*_ CHAB, VMIS_CIN2_MEMO, VISC_CIN *_ CHAB, VISC_CIN2_MEMO, purpose. LEMAITRE

This formulation is only valid for 3D, 2D models. It allows for an incrementally objective integration of laws of behavior such as models SIMO_MIEHE and GEDF_HYPO_ELAS. However, like all hypoelastic laws, these laws of behavior are, from a decreasing point of view, limited to slight elastic deformations. To save computation time, a specific tensor is stored in 6 additional internal variables. The tensor in question, \(T\) is the stress tensor expressed in logarithmic space. Because it is stored in the internal variables, this means that the user wishing to use formalism GDEF_LOG with an initial constraint field (ETAT_INIT) must refer to docs [U4.51.03] and [V6.03.159] (test case ssnap159b).

4.6.7. Deformation models for MFront#

Only large deformation models GDEF_LOG can be used with MFront behaviors (RELATION =” MFRONT “).

code_aster’s GDEF_LOG models are necessarily based on a law written in small deformations.

4.7. Operands TOUT/GROUP_MA/MAILLE#

/TOUT = 'OUI'
/| GROUP_MA = lgrma
     | MESH = lma

Specify the meshes on which the incremental behavior relationship is used.

Note:

If you don’t explicitly specify the behavior on some elements of the model, code_aster will select RELATION =” ELAS “and DEFORMATION =” PETIT” by default on these elements. An informational message is printed in the message file. You will get an explicit alarm if you don’t assign any model elements in an instance of COMPORTEMENT .

4.8. Operands RESI_CPLAN_RELA, RESI_CPLAN_MAXI, ITER_CPLAN_MAXI#

The DE BORST method allows you to add the plane stress condition to all COMPORTEMENT models (for more details see the [R5.03.03] documentation). The hypothesis of plane constraints is verified at convergence.

◊ RESI_CPLAN_RELA =/1.E-6, [DEFAUT]

/\({\mathrm{\epsilon }}_{\mathit{rela}}\)

/RESI_CPLAN_MAXI =/\({\mathrm{\epsilon }}_{\mathit{abso}}\)

In some cases, convergence is achieved for Newton’s algorithm, but not for the verification of the state of plane constraints, which leads to additional iterations, or even an excessive re-division of the time step. These keywords make it possible to dissociate the precision relating to the integration of the law of behavior from that used to test the hypothesis of plane constraints. For this verification, two criteria are possible:

be a relative criterion: :math: left| {mathrm {sigma}} _ {mathit {zz}}right|<Vertmathrm {sigma}Vertleft|times {times {mathrm {sigma}}} _ {mathit {rela}}}
be an absolute criterion: :math: left| {mathrm {sigma}} _ {mathit {zz}}right|< {mathrm {epsilon}}} _ {mathit {abso}}

◊ ITER_CPLAN_MAXI =/10 [DEFAUT]
                           /iter_cplan_maxi

This keyword allows you to specify the number of iterations left to the DE BORST algorithm within each iteration of the algorithm for solving balance equations (nested diagrams). If this number of iterations is reached, no error is triggered but the global convergence cannot be pronounced and additional iterations of solving the balance equations are activated, even if the equilibrium equations are well solved.

4.9. Operand RIGI_GEOM#

◊ RIGI_GEOM =/'DEFAUT' [DEFAUT]
                        /'OUI'

The argument RIGI_GEOM is used to activate the balance calculation on the deformed configuration of the structure, only for POU_D_TGM multi-fiber beams.

4.10. Operand PARM_THETA#

◊ PARM_THETA =/1. [DEFAUT]
                        /theta [R]

For the laws of behavior LEMAITRE, ROUSS_VISC, GTN, and VISC_GTN, the argument theta is used to integrate the law of behavior.

For LEMAITRE, ROUSS_VISC, it can take values 0.5 (semi-implicit) or 1 (implicit).

For GTN and VISC_GTN, any value between 0 and 1 is allowed; the value of 0.5 is recommended, which seems to lead to the best precision.

4.11. Operands RESI_INTE, ITER_INTE_MAXI#

◊ RESI_INTE =/resinted,
                       /1.e-6 (by default),

◊ ITER_INTE_MAXI => dyed,
                            /20 (by default),

In some behavioral relationships, a non-linear equation or a non-linear system must be solved locally (at each Gauss point). These operands (residue and maximum number of so-called internal iterations) are used to test the convergence of this iterative resolution algorithm. They are useless in case ALGO_INTE =” ANALYTIQUE “,” SPECIFIQUE “, or” SANS_OBJET “. For more details, refer to the reference documentation for each behavior.

For example, the optional keyword RESI_INTE can be used for couplage avec MFront. In MFront, the implicit and explicit integrators use variables that are deformations (or of the same order of magnitude as the deformations). The value of RESI_INTE is passed to the convergence parameter used by MFront (parameter epsilon), so it is an absolute parameter. In this case, its default value is the same as that defined in file MFront (directive « @Epsilon » set to 1.0e-8 by default). Similarly, the maximum number of iterations value in file MFront (directive « @MaximumNumberOfIterations » or « @IterMax » although obsolete set to 100 by default) is only overloaded if the ITER_INTE_MAXI keyword is present on the Aster side.

4.12. Operand RESI_RADI_RELA#

◊ RESI_RADI_RELA = Tolrad

Measuring the error \(\mathrm{\eta }\) due to discretization in time, directly re related to the rotation from normal to the load surface. We calculate the angle between \({n}^{\text{-}}\), the normal to the plasticity criterion at the beginning of the time step (instant t-), and \({n}^{\text{+}}\), the normal to the plasticity criterion calculated at the end of the step of

time as follows: :math: `mathrm {eta} =frac {1} {2}left|left|left|mathrm {eta} =frac {Delta}

nright|right|=frac {1} {2} {2}left|left| {n} ^ {text {+}} - {n} ^ {text {-}}right|right|right|=left|m athrm {sin} (frac {mathrm {alpha}} {2})right|`. This provides a measure of the error (equal used to calculate component ERR_RADI of option DERA_ELGA of CALC_CHAMP) . The time step is cut up (via DEFI_LIST_INST) if \(\mathrm{\eta }>\mathrm{tolrad}\). This criterion is operational for Von Mises elastoplastic behaviors with isotropic, linear and mixed kinematics work hardening: VMIS_ISOT_LINE, VMIS_ISOT_TRAC, VMIS_ISOT_PUIS, VMIS_CINE_LINE, VMIS_ECMI_LINE, VMIS_ECMI_TRAC, and for the elasto-visco-plastic behaviors of Chaboche: VMIS_CIN1_CHAB, VMIS_CIN2_CHAB, VMIS_CIN2_MEMO, VISC_CIN1_CHAB, VISC_CIN2_CHAB, VISC_CIN2_MEMO.

4.13. Operand ITER_INTE_PAS#

◊ ITER_INTE_PAS =/0 [DEFAUT]
                        /itepas

Allows the time step to be redivided locally to facilitate the integration of the local behavioral relationship (at each integration point). If itepas equals: math: 0, :math: 0, :math: 1, or:math: -1 there is no redistribution. If itepas is positive, the time step is systematically divided locally into small itepas of time before integrating the behavioral relationship. If itepas is negative, the redistribution into | itepas| small time steps is only performed in case of local non-convergence.

Attention: this keyword is only possible with DEFORMATION =” PETIT “, DEFORMATION =” PETIT_REAC” and DEFORMATION =” GROT_GDEP “. It cannot be used in large deformations.

4.14. Operand ALGO_INTE#

◊ ALGO_INTE = /' ANALYTIQUE '
                    # methods for solving scalar equations
                    /' SECANTE '
                    /' DEKKER '
                    /' NEWTON_1D '
                    /' BRENT '
                    # methods for solving systems of equations
                    /' NEWTON '
                    /' NEWTON_RELI '
                    /' NEWTON_PERT '
                    /' RUNGE_KUTTA '
                    # specific resolution methods (no parameters)
                    /' SPECIFIQUE '
                    /' SANS_OBJET '

Allows you to specify the type of integration diagram to solve the equation or the system of nonlinear equations formed by the equations constituting the models of behavior with internal variables: A resolution method by default is provided for each behavior. However, it is possible to change the resolution method by default for a number of behaviors. For example:

the VISC_ENDO_LEMA model can be integrated either with SECANTE or with BRENT,
the VENDOCHAB model can be integrated with either NEWTON or RUNGE_KUTTA.
the MONOCRISTAL model can be integrated either with NEWTON, or with NEWTON_RELI, with NEWTON_PERT, or with RUNGE_KUTTA.

4.15. Operand TYPE_MATR_TANG#

For relationships other than “RGI_BETON”, “FLUA_PORO_BETON”, “”, “FLUA_ENDO_PORO”, and “RGI_BETON_BA”:

◊ TYPE_MATR_TANG = /' PERTURBATION ',
                        /' VERIFICATION ',
◊ VALE_PERT_RELA =/1.E-5, [DEFAUT]
                        /perturb, [R]

This keyword allows the verification of the tangent matrix for a given behavior. It is mainly aimed at developers of behavioral laws, and its use should be reserved for models with very few elements. In the absence of this keyword, the tangent matrix is calculated in a conventional manner. (These keywords are used in conjunction with REAC_ITER =1).

TYPE_MATR_TANG= »DISTURBANCE » allows you to use the tangent matrix calculated by disturbance instead of the tangent matrix calculated by the behavior. The value of the disturbance is given by perturb. In order for this to work independently of the units, the disturbance is calculated relative to the max norm of the increase in displacement on the element: :math: mathrm {delta} U=mathit {delta} U=mathit {perturb}=mathit {perturb}\ timesmathit {max} | {U} _ {i} |. This is only possible for 2D and 3D continuous media models, in pure mechanics, with only degrees of freedom of movement.
TYPE_MATR_TANG = » VERIFICATION « concerns developers who want to check an elementary tangent matrix (on a small problem: one element is enough: only the last matrices are kept). The disturbance matrix is stored, as well as the coherent tangent matrix, which makes it possible to compare them. In addition, the veri_matr_tang Python module allows this comparison easily, as well as the symmetry test of the matrix. See tests COMP001, COMP002.

For the relationships” RGI_BETON “,” FLUA_PORO_BETON “,” “,” FLUA_ENDO_PORO “, and” RGI_BETON_BA “:

◊ TYPE_MATR_TANG = /' MATR_ELAS ', [DEFAUT]
                        /' MATR_ENDO ',

For these 4 laws, this keyword allows you to choose the type of matrix used between the elastic matrix “MATR_ELAS” and the discharge matrix “MATR_ENDO”.

4.16. Operand POST_ITER#

◊ POST_ITER = /' CRIT_RUPT ',

Definition of an action to be performed in post-processing Newton iterations, at each time step.

In case CRIT_RUPT, this is a criterion for failure under critical stress. If the greatest mean principal stress in an element exceeds a given threshold sigc, the Young’s modulus is divided at the next time step by the coefficient coef. These two coefficients are defined under the CRIT_RUPT keyword of the DEFI_MATERIAU [U4.43.01] operator.

This criterion is available for behavior laws VISCOCHAB, VMIS_ISOT_TRAC (_ LINE), VISC_ISOT_TRAC (_ LINE), and validated by the SSNV226A, B, C tests.

4.17. Operand POST_INCR#

◊ POST_INCR = /' REST_ECRO ',

Definition of an action to be performed in post-processing each time step of a thermomechanical calculation.

In case REST_ECRO, post-treatment consists in modifying the internal variables in order to take into account the phenomenon of work-hardening restoration. The cumulative plastic deformation is modified using the REST_ECRO parameters of the DEFI_MATERIAU operator [U4.43.01].

This criterion is available for behavior laws VMIS_ISOT_TRAC (_ LINE), VMIS_ECMI_LINE,),, VMIS_CIN1_CHAB, and VMIS_CIN2_CHAB, and for 3D models, AXIS, D_PLAN, and C_PLAN.

4.18. Operand REGU_VISC#

◊ REGU_VISC = /' NON ', [DEFAUT]
                    /' OUI '

This keyword makes it possible to activate the addition of a viscous constraint to the real constraints resulting from the law of behavior. This viscous regularization can make it possible to control possible material instabilities, at the cost of energy dissipation by viscosity. It follows a Maxwell model whose characteristic stiffness and time are specified in the command DEFI_MATERIAU [U4.43.01] under the keyword factor VISC_ELAS. The model in question is described in the documentation [R5.03.34]. This viscous regularization is only activated for certain laws of behavior: ENDO_FISS_EXP, ENDO_ISOT_BETON,,, ENDO_LOCA_EXP, GTN, ROUSS_VISC, VISC_GTN, VMIS_ISOT_LINE and VMIS_ISOT_NL.