.. _sect-smm-cl: Constitutive Laws ----------------- In order to compute an element’s response to deformation, one needs to use an appropriate constitutive relationship. The constitutive law is used to compute the element’s stresses from the element’s strains. In the finite-element discretization, the constitutive formulation is applied to every quadrature point of each element. When the implicit formulation is used, the tangent matrix has to be computed. | The chosen materials for the simulation have to be specified in the mesh file or, as an alternative, they can be assigned using the at ``element_material`` vector. For every material assigned to the problem one has to specify the material characteristics (constitutive behavior and material properties) using the text input file (see :ref:`sect-io-material`). | In order to conveniently store values at each quadrature in a material point ``Akantu`` provides a special data structure, the at :cpp:class:`InternalField `. The internal fields are inheriting from the at :cpp:class:`ElementTypeMapArray `. Furthermore, it provides several functions for initialization, auto-resizing and auto removal of quadrature points. The constitutive law is precised within an input file. The dedicated material section is then read by :cpp:func:`initFull ` method of :cpp:class:`SolidMechanicsModel ` which initializes the different materials specified with the following convention .. code-block:: python material constitutive_law [ name = value rho = value ... ] where *constitutive_law* is the adopted constitutive law, followed by the material properties listed one by line in the bracket (*e.g.*, ``name`` and density :math:``rho``. Some constitutive laws can also have an *optional flavor*. For certain materials, it is possible to activate the large deformation strain and stress evaluations. Internally the strain measure becomes the right Cauchy–Green deformation tensor and the evaluated stress measure becomes the Piola-Kirchhoff stress tensor. This is activated by using: .. code-block:: python material constitutive_law [ finite_deformation = true # Activates the large deformation routines (bool) ... ] Sometimes it is also desired to generate random distributions of internal parameters. An example might be the critical stress at which the material fails. To generate such a field, in the text input file, a random quantity needs be added to the base value: All parameters are real numbers. For the uniform distribution, minimum and maximum values have to be specified. Random parameters are defined as a :math:`base` value to which we add a random number that follows the chosen distribution. The `Uniform `__ distribution is gives a random values between in :math:`[min, max)`. The `Weibull `__ distribution is characterized by the following cumulative distribution function: .. math:: F(x) = 1- e^{-\left({x/\lambda}\right)^m} which depends on :math:`m` and :math:`\lambda`, which are the shape parameter and the scale parameter. These random distributions are different each time the code is executed. In order to obtain always the same one, it possible to manually set the *seed* that is the number from which these pseudo-random distributions are created. This can be done by adding the following line to the input file *outside* the material parameters environments: .. code-block:: seed = 1.0 where the value 1.0 can be substituted with any number. Currently ``Akantu`` can reproduce always the same distribution when the seed is specified *only* in serial. The value of the *seed* can be also specified directly in the code (for instance in the main file) with the command: .. code-block:: RandGenerator::seed(1.0) The same command, with empty brackets, can be used to check the value of the *seed* used in the simulation. The following sections describe the constitutive models implemented in ``Akantu``. ----- Elastic ``````` The elastic law is a commonly used constitutive relationship that can be used for a wide range of engineering materials (*e.g.*, metals, concrete, rock, wood, glass, rubber, etc.) provided that the strains remain small (*i.e.*, small deformation and stress lower than yield strength). The elastic laws are often expressed as :math:`\boldsymbol{\sigma} = \boldsymbol{C}:\boldsymbol{\varepsilon}` with where :math:`\boldsymbol{\sigma}` is the Cauchy stress tensor, :math:`\boldsymbol{\varepsilon}` represents the infinitesimal strain tensor and :math:`\boldsymbol{C}` is the elastic modulus tensor. .. _sect-smm-linear-elastic-isotropic: Linear isotropic '''''''''''''''' Keyword: **elastic** Material description with input file: .. code-block:: python #input.dat material elastic [ name = steel rho = 7800 # density (Real) E = 2.1e11 # young's modulus (Real) nu = 0.3 # poisson's ratio (Real) Plane_stress = false # Plane stress simplification (only 2D problems) (bool) finite_deformation = false # activates the evaluation of strains with green's tensor (bool) ] Available energies Energies: - ``potential``: elastic potential energy ----- The linear isotropic elastic behavior is described by Hooke’s law, which states that the stress is linearly proportional to the applied strain (material behaves like an ideal spring), as illustrated in  :numref:`fig:smm:cl:el`. .. figure:: figures/cl/stress_strain_el.svg :alt: Elastic strain-stress curve :name: fig:smm:cl:el :width: 60.0% Stress-strain curve of elastic material and schematic representation of Hooke's law, denoted as a spring. The equation that relates the strains to the displacements is: point) from the displacements as follows: .. math:: \label{eqn:smm:strain_inf} \boldsymbol{\varepsilon} = \frac{1}{2} \left[ \nabla_0 \boldsymbol{u}+\nabla_0 \boldsymbol{u}^T \right] where :math:`\boldsymbol{\varepsilon}` represents the infinitesimal strain tensor, :math:`\nabla_{0}\boldsymbol{u}` the displacement gradient tensor according to the initial configuration. The constitutive equation for isotropic homogeneous media can be expressed as: .. math:: \label{eqn:smm:material:constitutive_elastic} \boldsymbol{\sigma } =\lambda\mathrm{tr}(\boldsymbol{\varepsilon})\boldsymbol{I}+2 \mu\boldsymbol{\varepsilon} where :math:`\boldsymbol{\sigma}` is the Cauchy stress tensor (:math:`\lambda` and :math:`\mu` are the the first and second Lame’s coefficients). In Voigt notation this correspond to .. math:: \begin{aligned} \left[\begin{array}{c} \sigma_{11}\\ \sigma_{22}\\ \sigma_{33}\\ \sigma_{23}\\ \sigma_{13}\\ \sigma_{12}\\ \end{array}\right] &= \frac{E}{(1+\nu)(1-2\nu)}\left[ \begin{array}{cccccc} 1-\nu & \nu & \nu & 0 & 0 & 0\\ \nu & 1-\nu & \nu & 0 & 0 & 0\\ \nu & \nu & 1-\nu & 0 & 0 & 0\\ 0 & 0 & 0 & \frac{1-2\nu}{2} & 0 & 0 \\ 0 & 0 & 0 & 0 & \frac{1-2\nu}{2} & 0 \\ 0 & 0 & 0 & 0 & 0 & \frac{1-2\nu}{2} \\ \end{array}\right] \left[\begin{array}{c} \varepsilon_{11}\\ \varepsilon_{22}\\ \varepsilon_{33}\\ 2\varepsilon_{23}\\ 2\varepsilon_{13}\\ 2\varepsilon_{12}\\ \end{array}\right]\end{aligned} This formulation is not sufficient to represent all elastic material behavior. Some materials have characteristic orientation that have to be taken into account. To represent this anisotropy a more general stress-strain law has to be used, as shown below. ----- .. _sect-smm-linear-elastic-anisotropic: Linear anisotropic '''''''''''''''''' Keyword: **elastic_anisotropic** Material description with input file: .. code-block:: python #input.dat material elastic_anisotropic [ name = aluminum rho = 1.6465129043044597 # density (Real) C11 = 105.092023 # Coefficient ij of material tensor C (Real) C12 = 59.4637759 # all the 36 values C13 = 59.4637759 # in Voigt notation can be entered C14 = 0 # zero coefficients can be omited C15 = 0 C16 = 0 C22 = 105.092023 C23 = 59.4637759 C24 = 0 C25 = 0 C26 = 0 C33 = 105.092023 C34 = 0 C35 = 0 C36 = 0 C44 = 30.6596356 C45 = 0 C46 = 0 C55 = 30.6596356 C56 = 0 C66 = 30.6596356 n1 = [-1, 1, 0] # Direction of first material axis (Vector) n2 = [ 1, 1, 1] # Direction of second material axis (Vector) n3 = [ 1, 1, -2] # Direction of thrid material axis (Vector) ] ---- We define the elastic modulus tensor as follows: .. math:: \begin{aligned} \left[\begin{array}{c} \sigma_{11}\\ \sigma_{22}\\ \sigma_{33}\\ \sigma_{23}\\ \sigma_{13}\\ \sigma_{12}\\ \end{array}\right] &= \left[ \begin{array}{cccccc} c_{11} & c_{12} & c_{13} & c_{14} & c_{15} & c_{16}\\ c_{21} & c_{22} & c_{23} & c_{24} & c_{25} & c_{26}\\ c_{31} & c_{32} & c_{33} & c_{34} & c_{35} & c_{36}\\ c_{41} & c_{42} & c_{43} & c_{44} & c_{45} & c_{46}\\ c_{51} & c_{52} & c_{53} & c_{54} & c_{55} & c_{56}\\ c_{61} & c_{62} & c_{63} & c_{64} & c_{65} & c_{66}\\ \end{array}\right] \left[\begin{array}{c} \varepsilon_{11}\\ \varepsilon_{22}\\ \varepsilon_{33}\\ 2\varepsilon_{23}\\ 2\varepsilon_{13}\\ 2\varepsilon_{12}\\ \end{array}\right]\end{aligned} To simplify the writing of input files the :math:`\boldsymbol{C}` tensor is expressed in the material basis. And this basis as to be given too. This basis :math:`\Omega_{{\mathrm{mat}}} = \{\boldsymbol{n_1}, \boldsymbol{n_2}, \boldsymbol{n_3}\}` is used to define the rotation :math:`R_{ij} = \boldsymbol{n_j} . \boldsymbol{e_i}`. And :math:`\boldsymbol{C}` can be rotated in the global basis :math:`\Omega = \{\boldsymbol{e_1}, \boldsymbol{e_2}, \boldsymbol{e_3}\}` as follow: .. math:: \begin{aligned} \boldsymbol{C}_{\Omega} &= \boldsymbol{R}_1 \boldsymbol{C}_{\Omega_{{\mathrm{mat}}}} \boldsymbol{R}_2\\ \boldsymbol{R}_1 &= \left[ \begin{array}{cccccc} R_{11} R_{11} & R_{12} R_{12} & R_{13} R_{13} & R_{12} R_{13} & R_{11} R_{13} & R_{11} R_{12}\\ R_{21} R_{21} & R_{22} R_{22} & R_{23} R_{23} & R_{22} R_{23} & R_{21} R_{23} & R_{21} R_{22}\\ R_{31} R_{31} & R_{32} R_{32} & R_{33} R_{33} & R_{32} R_{33} & R_{31} R_{33} & R_{31} R_{32}\\ R_{21} R_{31} & R_{22} R_{32} & R_{23} R_{33} & R_{22} R_{33} & R_{21} R_{33} & R_{21} R_{32}\\ R_{11} R_{31} & R_{12} R_{32} & R_{13} R_{33} & R_{12} R_{33} & R_{11} R_{33} & R_{11} R_{32}\\ R_{11} R_{21} & R_{12} R_{22} & R_{13} R_{23} & R_{12} R_{23} & R_{11} R_{23} & R_{11} R_{22}\\ \end{array}\right]\\ \boldsymbol{R}_2 &= \left[ \begin{array}{cccccc} R_{11} R_{11} & R_{21} R_{21} & R_{31} R_{31} & R_{21} R_{31} & R_{11} R_{31} & R_{11} R_{21}\\ R_{12} R_{12} & R_{22} R_{22} & R_{32} R_{32} & R_{22} R_{32} & R_{12} R_{32} & R_{12} R_{22}\\ R_{13} R_{13} & R_{23} R_{23} & R_{33} R_{33} & R_{23} R_{33} & R_{13} R_{33} & R_{13} R_{23}\\ R_{12} R_{13} & R_{22} R_{23} & R_{32} R_{33} & R_{22} R_{33} & R_{12} R_{33} & R_{12} R_{23}\\ R_{11} R_{13} & R_{21} R_{23} & R_{31} R_{33} & R_{21} R_{33} & R_{11} R_{33} & R_{11} R_{23}\\ R_{11} R_{12} & R_{21} R_{22} & R_{31} R_{32} & R_{21} R_{32} & R_{11} R_{32} & R_{11} R_{22}\\ \end{array}\right]\\\end{aligned} ----- .. _sect-smm-linear-elastic-orthotropic: Linear orthotropic '''''''''''''''''' Keyword: **elastic_orthotropic** Inherits from **elastic_anisotropic** Material description with input file: .. code-block:: python #input.dat material elastic_orthotropic [ name = test_mat_1 rho = 1 # density n1 = [-1, 1, 0] # Direction of first material axis (Vector) n2 = [ 1, 1, 1] # Direction of second material axis (Vector) n3 = [ 1, 1, -2] # Direction of thrid material axis (Vector) E1 = 1 # Young's modulus in direction n1 (Real) E2 = 2 # Young's modulus in direction n2 (Real) E3 = 3 # Young's modulus in direction n3 (Real) nu12 = 0.1 # Poisson's ratio 12 (Real) nu13 = 0.2 # Poisson's ratio 13 (Real) nu23 = 0.3 # Poisson's ratio 23 (Real) G12 = 0.5 # Shear modulus 12 (Real) G13 = 1 # Shear modulus 13 (Real) G23 = 2 # Shear modulus 23 (Real) ] ----- A particular case of anisotropy is when the material basis is orthogonal in which case the elastic modulus tensor can be simplified and rewritten in terms of 9 independents material parameters. .. math:: \begin{aligned} \left[\begin{array}{c} \sigma_{11}\\ \sigma_{22}\\ \sigma_{33}\\ \sigma_{23}\\ \sigma_{13}\\ \sigma_{12}\\ \end{array}\right] &= \left[ \begin{array}{cccccc} c_{11} & c_{12} & c_{13} & 0 & 0 & 0 \\ & c_{22} & c_{23} & 0 & 0 & 0 \\ & & c_{33} & 0 & 0 & 0 \\ & & & c_{44} & 0 & 0 \\ & \text{sym.} & & & c_{55} & 0 \\ & & & & & c_{66}\\ \end{array}\right] \left[\begin{array}{c} \varepsilon_{11}\\ \varepsilon_{22}\\ \varepsilon_{33}\\ 2\varepsilon_{23}\\ 2\varepsilon_{13}\\ 2\varepsilon_{12}\\ \end{array}\right]\end{aligned} .. math:: \begin{aligned} c_{11} &= E_1 (1 - \nu_{23}\nu_{32})\Gamma \qquad c_{22} = E_2 (1 - \nu_{13}\nu_{31})\Gamma \qquad c_{33} = E_3 (1 - \nu_{12}\nu_{21})\Gamma\\ c_{12} &= E_1 (\nu_{21} - \nu_{31}\nu_{23})\Gamma = E_2 (\nu_{12} - \nu_{32}\nu_{13})\Gamma\\ c_{13} &= E_1 (\nu_{31} - \nu_{21}\nu_{32})\Gamma = E_2 (\nu_{13} - \nu_{21}\nu_{23})\Gamma\\ c_{23} &= E_2 (\nu_{32} - \nu_{12}\nu_{31})\Gamma = E_3 (\nu_{23} - \nu_{21}\nu_{13})\Gamma\\ c_{44} &= \mu_{23} \qquad c_{55} = \mu_{13} \qquad c_{66} = \mu_{12} \\ \Gamma &= \frac{1}{1 - \nu_{12} \nu_{21} - \nu_{13} \nu_{31} - \nu_{32} \nu_{23} - 2 \nu_{21} \nu_{32} \nu_{13}}\end{aligned} The Poisson ratios follow the rule :math:`\nu_{ij} = \nu_{ji} E_i / E_j`. ----- .. _sect-smm-cl-neohookean: Neo-Hookean ''''''''''' Keyword: **neohookean** Inherits from **elastic** Material description with input file: .. code-block:: python #input.dat material neohookean [ name = material_name rho = 7800 # density (Real) E = 2.1e11 # young's modulus (Real) nu = 0.3 # poisson's ratio (Real) ] ----- The hyperelastic Neo-Hookean constitutive law results from an extension of the linear elastic relationship (Hooke’s Law) for large deformation. Thus, the model predicts nonlinear stress-strain behavior for bodies undergoing large deformations. .. figure:: figures/cl/stress_strain_neo.svg :alt: Neo-hookean Stress-strain curve. :name: fig:smm:cl:neo_hookean :width: 40.0% Neo-hookean Stress-strain curve. As illustrated in :numref:`fig:smm:cl:neo_hookean`, the behavior is initially linear and the mechanical behavior is very close to the corresponding linear elastic material. This constitutive relationship, which accounts for compressibility, is a modified version of the one proposed by Ronald Rivlin :cite:`Belytschko:2000`. The strain energy stored in the material is given by: .. math:: \label{eqn:smm:constitutive:neohookean_potential} \Psi(\boldsymbol{C}) = \frac{1}{2}\lambda_0\left(\ln J\right)^2-\mu_0\ln J+\frac{1}{2} \mu_0\left(\mathrm{tr}(\boldsymbol{C})-3\right) where :math:`\lambda_0` and :math:`\mu_0` are, respectively, Lamé’s first parameter and the shear modulus at the initial configuration. :math:`J` is the jacobian of the deformation gradient (:math:`\boldsymbol{F}=\nabla_{\!\!\boldsymbol{X}}\boldsymbol{x}`): :math:`J=\text{det}(\boldsymbol{F})`. Finally :math:`\boldsymbol{C}` is the right Cauchy-Green deformation tensor. Since this kind of material is used for large deformation problems, a finite deformation framework should be used. Therefore, the Cauchy stress (:math:`\boldsymbol{\sigma}`) should be computed through the second Piola-Kirchhoff stress tensor :math:`\boldsymbol{S}`: .. math:: \boldsymbol{\sigma } = \frac{1}{J}\boldsymbol{F}\boldsymbol{S}\boldsymbol{F}^T Finally the second Piola-Kirchhoff stress tensor is given by: .. math:: \boldsymbol{S} = 2\frac{\partial\Psi}{\partial\boldsymbol{C}} = \lambda_0\ln J \boldsymbol{C}^{-1}+\mu_0\left(\boldsymbol{I}-\boldsymbol{C}^{-1}\right) The parameters to indicate in the material file are the same as those for the elastic case: ``E`` (Young’s modulus), ``nu`` (Poisson’s ratio). ----- .. _sect-smm-cl-sls: Visco-Elasticity '''''''''''''''' Keyword: **sls_deviatoric** Inherits from **elastic** Material description with input file: .. code-block:: python #input.dat material sls_deviatoric [ name = material_name rho = 1000 # density (Real) E = 2.1e9 # young's modulus (Real) nu = 0.4 # poisson's ratio (Real) Eta = 1. # Viscosity (Real) Ev = 0.5 # Stiffness of viscous element (Real) Plane_stress = false # Plane stress simplification (bool, only 2D problems) ] Since this material inherits from :cpp:class:`MaterialElastic ` the parameter :math:`E` preceeds :math:`E_{\mathrm{inf}}`. So only :math:`E` and :math:`E_v` can be set, :math:`E_{\mathrm{inf}}` is deduced by :math:`E_{\mathrm{inf}} = E - E_{v}`. ----- Visco-elasticity is characterized by strain rate dependent behavior. Moreover, when such a material undergoes a deformation it dissipates energy. This dissipation results in a hysteresis loop in the stress-strain curve at every loading cycle (see :numref:`fig:smm:cl:visco-elastic:hyst`). In principle, it can be applied to many materials, since all materials exhibit a visco-elastic behavior if subjected to particular conditions (such as high temperatures). .. figure:: figures/cl/stress_strain_visco.svg :name: fig:smm:cl:visco-elastic:hyst :align: center :width: 40.0% Characteristic stress-strain behavior of a visco-elastic material with hysteresis loop .. figure:: figures/cl/visco_elastic_law.svg :name: fig:smm:cl:visco-elastic:model :align: center :width: 40.0% Schematic representation of the standard rheological linear solid visco-elastic model The standard rheological linear solid model (see Sections 10.2 and 10.3 of :cite:`simo92`) has been implemented in ``Akantu``. This model results from the combination of a spring mounted in parallel with a spring and a dashpot connected in series, as illustrated in :numref:`fig:smm:cl:visco-elastic:model`. The advantage of this model is that it allows to account for creep or stress relaxation. The equation that relates the stress to the strain is (in 1D): .. math:: \frac{d\varepsilon(t)}{dt} = \left ( E_{\mathrm{inf}} + E_{v} \right ) ^ {-1} \cdot \left [ \frac{d\sigma(t)}{dt} + \frac{E_{v}}{\eta}\sigma(t) - \frac{E_{\mathrm{inf}}E_V}{\eta}\varepsilon(t) \right ] where :math:`\eta` is the viscosity. The equilibrium condition is unique and is attained in the limit, as :math:`t \to \infty`. At this stage, the response is elastic and depends on the Young’s modulus :math:`E`. The mandatory parameters for the material file are the following: ``rho`` (density), ``E`` (Young’s modulus), ``nu`` (Poisson’s ratio), ``Plane_Stress`` (if set to zero plane strain, otherwise plane stress), ``eta`` (dashpot viscosity) and ``Ev`` (stiffness of the viscous element). Note that the current standard linear solid model is applied only on the deviatoric part of the strain tensor. The spheric part of the strain tensor affects the stress tensor like an linear elastic material. ----- .. _sect-smm-cl-maxwell: Maxwell Chain Visco-Elasticity '''''''''''''''''''''''''''''' Keyword: **viscoelastic_maxwell** Inherits from **elastic** Material description with input file: .. code-block:: python #input.dat material viscoelastic_maxwell [ name = material_name rho = 1000 # density (Real) Einf = 5.e9 # Infinite time Young's modulus (Real) nu = 0.4 # poisson's ratio (Real) Ev = [1.e9, 2.e9, 3.e9] # Maxwell elements' stiffness values (Vector) Eta = [1.e14, 2.e16, 3.e16] # Dashpot elements' viscosity values (Vector) Plane_stress = false # Plane stress simplification (bool, only 2D problems) ] ---- .. figure:: figures/cl/maxwell_chain.png :name: fig-smm-cl-visco-elastic-maxwell :align: center :width: 40.0% Schematic representation of the Maxwell chain A different visco-elastic rheological model available to users is the generalized Maxwell chain (see :cite:`de_borst_finiteelement_1994` and Section 46.7.4 of :cite:`diana_manual`). It consists of a series of sequential spring-dashpots (Maxwell elements) placed in parallel with one single spring (see :numref:`fig-smm-cl-visco-elastic-maxwell`). The relation between stresses and strain comes from .. math:: \sigma \left ( t \right ) = \int_{-\infty}^{t} E \left ( t, \tau \right ) \mathbf{D} \dot{\varepsilon} d\tau where :math:`E(t,\tau)` is the time-dependent relaxation function, :math:`\tau` is the loading age, and :math:`\mathbf{D}` is the dimensionless matrix relating a 3D deformation state to a 1D relaxation function. The relaxation function is expanded in the exponential series .. math:: :label: eqn-relaxation-function E \left ( t, \tau \right ) = E_{0} + \sum_{\alpha=1}^{n} E_{\alpha} e^{- \frac{t- \tau}{\lambda_{\alpha}}} where the relaxation time of each Maxwell element is defined as :math:`\lambda_{\alpha}=\eta_{\alpha} / E_{\alpha}` with :math:`\eta_{\alpha}` being the viscosity of a dash-pot. Assuming a constant strain rate within each time step, the analytical integration of the right-hand side of :eq:`eqn-relaxation-function` leads to the following form .. math:: \sigma \left ( t + \Delta t \right ) = E_{0} \mathbf{D} \varepsilon + \sum_{\alpha=1}^n \left ( \left ( 1 - e^{\frac{- \Delta t}{\lambda_{\alpha}}} \right ) \frac{E_{\alpha} \lambda_{\alpha}}{\Delta t} \mathbf{D} \delta \varepsilon + e^{\frac{-\Delta t}{\lambda_{\alpha}}} \sigma_{\alpha} \left ( t \right ) \right ) with :math:`\sigma_{\alpha}(t)` being the internal stress within each Maxwell element, defined as .. math:: \sigma_{\alpha} \left ( t \right ) = \mathbf{D} \int_0^t E_{\alpha} e^{\frac{-t- \tau}{\lambda_{\alpha}}} \dot{\varepsilon} d \tau The first term under the sum sign in above equation could be seen as the effective stiffness of a single Maxwell element multiplied by the matrix :math:`\mathbf{D}` and the strain increment :math:`\Delta \varepsilon`: .. math:: E_{\alpha}^{ef} = \left ( 1- e^{\frac{-Δt}{λ_α}} \right ) \frac{E_α λ_α}{Δt} Time increment :math:`Δt` controls the rate dependency of the effective stiffness. By limit analysis, we find the limiting values of the effective stiffness which are equal to :math:`E_0` for infinitely slow loading (:math:`Δt` tending to infinity) and :math:`E_0+ΣE_α` for infinitely fast (:math:`Δt` tending to 0). At the end of each converged time step, the internal stress :math:`σ_α(t)` is updated according to .. math:: σ_α \left ( t \right ) = σ_α \left ( t - Δt \right ) e^{\frac{-Δt}{λ_α}} + E_α^{ef} \mathbf{D} Δε The mandatory parameters for the material file are the following: ``rho`` (density), ``nu`` (Poisson’s ratio), ``Plane_Stress`` (if set to zero plane strain, otherwise plane stress), ``Einf`` (infinite time Young’s modulus), ``Ev`` (Maxwell elements' stiffness values stored in a vector), ``Eta`` (dashpots' viscosity values stored in a vector). The Maxwell model is applied on the entire strain tensor and does not distinguish between its deviatoric and hydrostatic components. Note that the time step has to be specified for the model using current material both for static and dynamic simulations: .. code-block:: c++ model.setTimeStep(time_step_value); .. _sect-smm-cl-plastic: Plastic ``````` Small-Deformation Plasticity '''''''''''''''''''''''''''' Keyword: **plastic_linear_isotropic_hardening** Inherits from **elastic** Material description with input file: .. code-block:: python #input.dat material plastic_linear_isotropic_hardening [ name = material_name rho = 1000 # density (Real) E = 2.1e9 # young's modulus (Real) nu = 0.4 # poisson's ratio (Real) h = 0.1 # Hardening modulus (Real) sigma_y = 1e6 # Yield stress (Real) ] Energies: - ``potential``: elastic part of the potential energy - ``plastic``: dissipated plastic energy (integrated over time) ----- The small-deformation plasticity is a simple plasticity material formulation which accounts for the additive decomposition of strain into elastic and plastic strain components. This formulation is applicable to infinitesimal deformation where the additive decomposition of the strain is a valid approximation. In this formulation, plastic strain is a shearing process where hydrostatic stress has no contribution to plasticity and consequently plasticity does not lead to volume change. :numref:`fig:smm:cl:Lin-strain-hard` shows the linear strain hardening elasto-plastic behavior according to the additive decomposition of strain into the elastic and plastic parts in infinitesimal deformation as .. math:: \boldsymbol{\varepsilon} &= \boldsymbol{\varepsilon}^e +\boldsymbol{\varepsilon}^p\\ \boldsymbol{\sigma} &= 2G(\boldsymbol{\varepsilon}^e) + \lambda \mathrm{tr}(\boldsymbol{\varepsilon}^e)\boldsymbol{I} .. figure:: figures/cl/isotropic_hardening_plasticity.svg :name: fig:smm:cl:Lin-strain-hard :align: center Stress-strain curve for the small-deformation plasticity with linear isotropic hardening. In this class, the von Mises yield criterion is used. In the von Mises yield criterion, the yield is independent of the hydrostatic stress. Other yielding criteria such as Tresca and Gurson can be easily implemented in this class as well. In the von Mises yield criterion, the hydrostatic stresses have no effect on the plasticity and consequently the yielding occurs when a critical elastic shear energy is achieved. .. math:: \label{eqn:smm:constitutive:von Mises} f = \sigma_{{\mathrm{eff}}} - \sigma_y = \left(\frac{3}{2} {\boldsymbol{\sigma}}^{{\mathrm{tr}}} : {\boldsymbol{\sigma}}^{{\mathrm{tr}}}\right)^\frac{1}{2}-\sigma_y (\boldsymbol{\varepsilon}^p) .. math:: \label{eqn:smm:constitutive:yielding} f < 0 \quad \textrm{Elastic deformation,} \qquad f = 0 \quad \textrm{Plastic deformation} where :math:`\sigma_y` is the yield strength of the material which can be function of plastic strain in case of hardening type of materials and :math:`{\boldsymbol{\sigma}}^{{\mathrm{tr}}}` is the deviatoric part of stress given by .. math:: \label{eqn:smm:constitutive:deviatoric stress} {\boldsymbol{\sigma}}^{{\mathrm{tr}}}=\boldsymbol{\sigma} - \frac{1}{3} \mathrm{tr}(\boldsymbol{\sigma}) \boldsymbol{I} After yielding :math:`(f = 0)`, the normality hypothesis of plasticity determines the direction of plastic flow which is normal to the tangent to the yielding surface at the load point. Then, the tensorial form of the plastic constitutive equation using the von Mises yielding criterion (see equation 4.34) may be written as .. math:: \label{eqn:smm:constitutive:plastic contitutive equation} \Delta {\boldsymbol{\varepsilon}}^p = \Delta p \frac {\partial{f}}{\partial{\boldsymbol{\sigma}}}=\frac{3}{2} \Delta p \frac{{\boldsymbol{\sigma}}^{{\mathrm{tr}}}}{\sigma_{{\mathrm{eff}}}} In these expressions, the direction of the plastic strain increment (or equivalently, plastic strain rate) is given by :math:`\frac{{\boldsymbol{\sigma}}^{{\mathrm{tr}}}}{\sigma_{{\mathrm{eff}}}}` while the magnitude is defined by the plastic multiplier :math:`\Delta p`. This can be obtained using the *consistency condition* which impose the requirement for the load point to remain on the yielding surface in the plastic regime. Here, we summarize the implementation procedures for the small-deformation plasticity with linear isotropic hardening: #. Compute the trial stress: .. math:: {\boldsymbol{\sigma}}^{{\mathrm{tr}}} = {\boldsymbol{\sigma}}_t + 2G\Delta \boldsymbol{\varepsilon} + \lambda \mathrm{tr}(\Delta \boldsymbol{\varepsilon})\boldsymbol{I} #. Check the Yielding criteria: .. math:: f = (\frac{3}{2} {\boldsymbol{\sigma}}^{{\mathrm{tr}}} : {\boldsymbol{\sigma}}^{{\mathrm{tr}}})^{1/2}-\sigma_y (\boldsymbol{\varepsilon}^p) #. Compute the Plastic multiplier: .. math:: \begin{aligned} d \Delta p &= \frac{\sigma^{tr}_{eff} - 3G \Delta P^{(k)}- \sigma_y^{(k)}}{3G + h}\\ \Delta p^{(k+1)} &= \Delta p^{(k)}+ d\Delta p\\ \sigma_y^{(k+1)} &= (\sigma_y)_t+ h\Delta p \end{aligned} #. Compute the plastic strain increment: .. math:: \Delta {\boldsymbol{\varepsilon}}^p = \frac{3}{2} \Delta p \frac{{\boldsymbol{\sigma}}^{{\mathrm{tr}}}}{\sigma_{{\mathrm{eff}}}} #. Compute the stress increment: .. math:: {\Delta \boldsymbol{\sigma}} = 2G(\Delta \boldsymbol{\varepsilon}-\Delta \boldsymbol{\varepsilon}^p) + \lambda \mathrm{tr}(\Delta \boldsymbol{\varepsilon}-\Delta \boldsymbol{\varepsilon}^p)\boldsymbol{I} #. Update the variables: .. math:: \begin{aligned} {\boldsymbol{\varepsilon^p}} &= {\boldsymbol{\varepsilon}}^p_t+{\Delta {\boldsymbol{\varepsilon}}^p}\\ {\boldsymbol{\sigma}} &= {\boldsymbol{\sigma}}_t+{\Delta \boldsymbol{\sigma}} \end{aligned} We use an implicit integration technique called *the radial return method* to obtain the plastic multiplier. This method has the advantage of being unconditionally stable, however, the accuracy remains dependent on the step size. The plastic parameters to indicate in the material file are: :math:`\sigma_y` (Yield stress) and ``h`` (Hardening modulus). In addition, the elastic parameters need to be defined as previously mentioned: ``E`` (Young’s modulus), ``nu`` (Poisson’s ratio). ----- Damage `````` In the simplified case of a linear elastic and brittle material, isotropic damage can be represented by a scalar variable :math:`d`, which varies from :math:`0` to :math:`1` for no damage to fully broken material respectively. The stress-strain relationship then becomes: .. math:: \boldsymbol{\sigma} = (1-d)\, \boldsymbol{C}:\boldsymbol{\varepsilon} where :math:`\boldsymbol{\sigma}`, :math:`\boldsymbol{\varepsilon}` are the Cauchy stress and strain tensors, and :math:`\boldsymbol{C}` is the elastic stiffness tensor. This formulation relies on the definition of an evolution law for the damage variable. In ``Akantu``, many possibilities exist and they are listed below. ---- .. _sect-smm-cl-damage-marigo: Marigo '''''' Keyword: **marigo** Inherits from **elastic** Material description with input file: .. code-block:: python #input.dat material marigo [ name = material_name rho = 1000 # density (Real) E = 2.1e9 # young's modulus (Real) nu = 0.4 # poisson's ratio (Real) Plane_stress = false # Plane stress simplification (bool, only 2D problems) Yd = 0.1 # Hardening modulus (Random) Sd = 1. # Damage energy (Real) ] Energies: - ``dissipated``: energy dissipated in damage ----- This damage evolution law is energy based as defined by Marigo :cite:`marigo81a`, :cite:`lemaitre96a`. It is an isotropic damage law. .. math:: \begin{aligned} Y &= \frac{1}{2}\boldsymbol{\varepsilon}:\boldsymbol{C}:\boldsymbol{\varepsilon}\\ F &= Y - Y_d - S d\\ d &= \left\{ \begin{array}{l l} \mathrm{min}\left(\frac{Y-Y_d}{S},\;1\right) & \mathrm{if}\; F > 0\\ \mathrm{unchanged} & \mathrm{otherwise} \end{array} \right.\end{aligned} In this formulation, :math:`Y` is the strain energy release rate, :math:`Y_d` the rupture criterion and :math:`S` the damage energy. The non-local version of this damage evolution law is constructed by averaging the energy :math:`Y`. .. _sect-smm-cl-damage-mazars: Mazars '''''' Keyword: **mazars** Inherits from **elastic** Material description with input file: .. code-block:: python #input.dat material mazars [ name = concrete rho = 3000 # density (Real) E = 32e9 # young's modulus (Real) nu = 0.2 # poisson's ratio (Real) K0 = 9.375e-5 # Damage threshold (Real) At = 1.15 # Parameter damage traction 1 (Real) Bt = 10000 # Parameter damage traction 2 (Real) Ac = 0.8 # Parameter damage compression 1 (Real) Bc = 1391.3 # Parameter damage compression 2 (Real) beta = 1.00 # Parameter for shear (Real) ] Energies: - ``dissipated``: energy dissipated in damage ----- This law introduced by Mazars :cite:`mazars84a` is a behavioral model to represent damage evolution in concrete. This model does not rely on the computation of the tangent stiffness, the damage is directly evaluated from the strain. The governing variable in this damage law is the equivalent strain :math:`\varepsilon_{{\mathrm{eq}}} = \sqrt{<\boldsymbol{\varepsilon}>_+:<\boldsymbol{\varepsilon}>_+}`, with :math:`<.>_+` the positive part of the tensor. This part is defined in the principal coordinates (I, II, III) as :math:`\varepsilon_{{\mathrm{eq}}} = \sqrt{<\boldsymbol{\varepsilon_I}>_+^2 + <\boldsymbol{\varepsilon_{II}}>_+^2 + <\boldsymbol{\varepsilon_{III}}>_+^2}`. The damage is defined as: .. math:: \begin{aligned} D &= \alpha_t^\beta D_t + (1-\alpha_t)^\beta D_c\\ D_t &= 1 - \frac{\kappa_0 (1- A_t)}{\varepsilon_{{\mathrm{eq}}}} - A_t \exp^{-B_t(\varepsilon_{{\mathrm{eq}}}-\kappa_0)}\\ D_c &= 1 - \frac{\kappa_0 (1- A_c)}{\varepsilon_{{\mathrm{eq}}}} - A_c \exp^{-B_c(\varepsilon_{{\mathrm{eq}}}-\kappa_0)}\\ \alpha_t &= \frac{\sum_{i=1}^3<\varepsilon_i>_+\varepsilon_{{\mathrm{nd}}\;i}}{\varepsilon_{{\mathrm{eq}}}^2}\end{aligned} With :math:`\kappa_0` the damage threshold, :math:`A_t` and :math:`B_t` the damage parameter in traction, :math:`A_c` and :math:`B_c` the damage parameter in compression, :math:`\beta` is the shear parameter. :math:`\alpha_t` is the coupling parameter between traction and compression, the :math:`\varepsilon_i` are the eigenstrain and the :math:`\varepsilon_{{\mathrm{nd}}\;i}` are the eigenvalues of the strain if the material were undamaged. The coefficients :math:`A` and :math:`B` are the post-peak asymptotic value and the decay shape parameters. .. _sect:smm:CLNL: Non-Local Constitutive Laws ``````````````````````````` Continuum damage modeling of quasi-brittle materials undergo significant softening after the onset of damage. This fast growth of damage causes a loss of ellipticity of partial differential equations of equilibrium. Therefore, the numerical simulation results won't be objective anymore, because the dissipated energy will depend on mesh size used in the simulation. One way to avoid this effect is the use of non-local damage formulations. In this approach a local quantity such as the strain is replaced by its non-local average, where the size of the domain, over which the quantitiy is averaged, depends on the underlying material microstructure. ``Akantu`` provides non-local versions of many constitutive laws for damage. Examples are for instance the material :ref:`sect-smm-cl-damage-mazars` and the material :ref:`sect-smm-cl-damage-marigo`, that can be used in a non-local context. In order to use the corresponding non-local formulation the user has to define the non-local material he wishes to use in the text input file: .. code-block:: none material constitutive_law_non_local [ name = material_name rho = $value$ ... ] where ``constitutive_law_non_local`` is the name of the non-local constitutive law, *e.g.* `marigo_non_local`. In addition to the material the non-local neighborhood, that should be used for the averaging process needs to be defined in the material file as well: .. code-block:: none non_local neighborhood_name weight_function_type [ radius = $value$ ... weight_function weight_parameter [ damage_limit = $value$ ... ] ] for the non-local averaging, *e.g.* ``base_wf``, followed by the properties of the non-local neighborhood, such as the radius, and the weight function parameters. It is important to notice that the non-local neighborhood must have the same name as the material to which the neighborhood belongs! The following two sections list the non-local constitutive laws and different type of weight functions available in ``Akantu``. \subsection{Non-local constitutive laws} Let us consider a body having a volume :math:`V` and a boundary :math:`\Gamma`. The stress-strain relation for a non-local damage model can be described as follows: .. _eq:non-local-const: .. math:: \vec{\sigma} = (1-\bar{d}) \vec{D}:\epsilon with :math:`\vec{D}` the elastic moduli tensor, :math:`\sigma` the stress tensor, :math:`\epsilon` the strain tensor and :math:`\bar{d}` the non-local damage variable. Note that this stres-strain relationship is similar to the relationship defined in Damage model except :math:`\bar{d}`. The non-local damage model can be extended to the damage constitutive laws: :ref:`sect-smm-cl-damage-marigo` and :ref:`sect-smm-cl-damage-mazars`. The non-local damage variable :math:`\bar{d}` is defined as follows: .. _eq:non-local-damage: .. math:: \bar{d}(\vec{x}) = \int_{V}W(\vec{x}, \vec{y}) d(\vec{y}) dV(\vec{y}) with :math:`W(\vec{x},\vec{y})` the weight function which averages local damage variables to describe the non-local interactions. A list of available weight functions and its functionalities in \akantu are explained in the next section. Non-local weight functions '''''''''''''''''''''''''' The available weight functions in ``Akantu`` are follows: - ``base_weight_function``: This weight function averages local damage variables by using a bell-shape function on spatial dimensions. - ``damaged_weight_function``: A linear-shape weight function is applied to average local damage variables. Its slope is determined by damage variables. For example, the damage variables for an element which is highly damaged are averaged over large spatial dimension (linear function including a small slope). - ``remove_damaged_weight_function``: This weight function averages damage values by using a bell-shape function as ``base_weight_function``, but excludes elements which are fully damaged. - ``remove_damaged_with_damage_rate_weight_function``: A bell-shape function is applied to average local damage variables for elements having small damage rates. - ``stress_based_weight_function``: Non local integral takes stress states, and use the states to construct weight function: an ellipsoid shape. Detailed explanations of this weight function are given in Giry et al. :cite:`giry13a`. ----- .. _sec-cohesive-laws: Cohesive Constitutive laws `````````````````````````` .. _ssect-smm-cl-coh-snozzi: Linear Irreversible Law ''''''''''''''''''''''' Keyword: **cohesive_linear** Material description with input file: .. code-block:: python #input.dat material cohesive_linear [ name = cohesive sigma_c = 0.1 # critical stress sigma_c (default: 0) G_c = 1e-2 # Mode I fracture energy beta = 0. # weighting parameter for sliding and normal opening (default: 0) penalty = 0. # stiffness in compression to prevent penetration (α in the text) kappa = 1. # ration between mode-I and mode-II fracture energy (Gc_II/Gc_I) contact_after_breaking = true # Activation of contact when the elements are fully damaged max_quad_stress_insertion = false # Insertion of cohesive element when stress is high # enough just on one quadrature point # if false the average stress on facet's quadrature points is used ] ----- .. figure:: figures/cl/linear_cohesive_law.svg :alt: Irreversible cohesive laws for explicit simulations. :name: fig:smm:coh:linear_cohesive_law :align: center :width: 60.0% Irreversible cohesive laws for explicit simulations. `Akantu` includes the Snozzi-Molinari :cite:`snozzi_cohesive_2013` linear irreversible cohesive law (see :numref:`fig:smm:coh:linear_cohesive_law`). It is an extension to the Camacho-Ortiz :cite:`camacho_computational_1996` cohesive law in order to make dissipated fracture energy path-dependent. The concept of free potential energy is dropped and a new independent parameter :math:`\kappa` is introduced: .. math:: \kappa = \frac{G_\mathrm{c, II}}{G_\mathrm{c, I}} where :math:`G_\mathrm{c, I}` and :math:`G_\mathrm{c, II}` are the necessary works of separation per unit area to open completely a cohesive zone under mode I and mode II, respectively. Their model yields to the following equation for cohesive tractions :math:`\vec{T}` in case of crack opening :math:`{\delta}`: .. math:: \vec{T} = \left( \frac{\beta^2}{\kappa} \Delta_\mathrm{t} \vec{t} + \Delta_\mathrm{n} \vec{n} \right) \frac{\sigma_\mathrm{c}}{\delta} \left( 1- \frac{\delta}{\delta_\mathrm{c}} \right) = \hat{\vec T}\, \frac{\sigma_\mathrm{c}}{\delta} \left( 1- \frac{\delta}{\delta_\mathrm{c}} \right) :label: eq-smm-coh-tractions where :math:`\sigma_\mathrm{c}` is the material strength along the fracture, :math:`\delta_\mathrm{c}` the critical effective displacement after which cohesive tractions are zero (complete decohesion), :math:`\Delta_\mathrm{t}` and :math:`\Delta_\mathrm{n}` are the tangential and normal components of the opening displacement vector :math:`\vec{\Delta}`, respectively. The parameter :math:`\beta` is a weight that indicates how big the tangential opening contribution is. The effective opening displacement is: .. math:: \delta = \sqrt{\frac{\beta^2}{\kappa^2} \Delta_\mathrm{t}^2 + \Delta_\mathrm{n}^2} In case of unloading or reloading :math:`\delta < \delta_\mathrm{max}`, tractions are calculated as: .. math:: \begin{eqnarray} T_\mathrm{n} &= \Delta_\mathrm{n}\, \frac{\sigma_\mathrm{c}}{\delta_\mathrm{max}} \left( 1- \frac{\delta_\mathrm{max}}{\delta_\mathrm{c}} \right) \\ T_\mathrm{t} &= \frac{\beta^2}{\kappa}\, \Delta_\mathrm{t}\, \frac{\sigma_\mathrm{c}}{\delta_\mathrm{max}} \left( 1- \frac{\delta_\mathrm{max}}{\delta_\mathrm{c}} \right) \end{eqnarray} so that they vary linearly between the origin and the maximum attained tractions. As shown in :numref:`fig:smm:coh:linear_cohesive_law`, in this law, the dissipated and reversible energies are: .. math:: \begin{eqnarray} E_\mathrm{diss} &= \frac{1}{2} \sigma_\mathrm{c}\, \delta_\mathrm{max}\\[1ex] E_\mathrm{rev} &= \frac{1}{2} T\, \delta \end{eqnarray} Moreover, a damage parameter :math:`D` can be defined as: .. math:: D = \min \left( \frac{\delta_\mathrm{max}}{\delta_\mathrm{c}},1 \right) which varies from 0 (undamaged condition) and 1 (fully damaged condition). This variable can only increase because damage is an irreversible process. A simple penalty contact model has been incorporated in the cohesive law so that normal tractions can be returned in case of compression: .. math:: T_\mathrm{n} = \alpha \Delta_\mathrm{n} \quad\text{if}\quad \Delta_\mathrm{n}\quad <\quad 0 where :math:`\alpha` is a stiffness parameter that defaults to zero. The relative contact energy is equivalent to reversible energy but in compression. The material name of the linear decreasing cohesive law is ``material_cohesive_linear`` and its parameters with their respective default values are: - ``sigma_c = 0`` - ``delta_c = 0`` - ``beta = 0`` - ``G_c = 0`` - ``kappa = 1`` - ``penalty = 0`` where ``G_c`` corresponds to :math:`G_\mathrm{c, I}`. A random number generator can be used to assign a random :math:`\sigma_\mathrm{c}` to each facet following a given distribution (see Section :ref:`sect-smm-cl`). Only one parameter between ``delta_c`` and ``G_c`` has to be specified. For random :math:`\sigma_\mathrm{c}` distributions, the chosen parameter of these two is kept fixed and the other one is varied. The bi-linear constitutive law works exactly the same way as the linear one, except for the additional parameter ``delta_0`` that by default is zero. Two examples for the extrinsic and intrinsic cohesive elements and also an example to assign different properties to inter-granular and trans-granular cohesive elements can be found in the folder ``examples/cohesive_element/``. ---- .. _ssect:smm:cl:coh-friction: Linear Cohesive Law with Friction ''''''''''''''''''''''''''''''''' Keyword: **cohesive_linear_friction** Material description with input file: .. code-block:: python #input.dat material cohesive_linear_friction [ name = interface beta = 1 # weighting parameter for sliding and normal opening (default: 0) G_c = 30e-3 # Mode I fracture energy penalty = 1.0e6 # stiffness in compression to prevent penetration (α in the text) sigma_c = 2.0 # critical stress sigma_c (default: 0) contact_after_breaking = true # Activation of contact when the elements are fully damaged mu = 0.5 # Maximum value of the friction coefficient penalty_for_friction = 5.0e3 # Penalty parameter for the friction behavior ] ----- This law represents a variation of the linear irreversible cohesive of the previous section, which adds friction. The friction behavior is approximated with an elasto-plastic law, which relates the friction force to the relative sliding between the two faces of the cohesive element. The slope of the elastic branch is called ``penalty_for_friction``, and is defined by the user, together with the friction coefficient, as a material property. The friction contribution evolves with the damage of the cohesive law: it is null when the damage is zero, and it becomes maximum when the damage is equal to one. This is done by defining a current value of the friction coefficient (mu) that increases linearly with the damage, up to the value of the friction coefficient defined by the user. The yielding plateau of the friction law is given by the product of the current friction coefficient and the local compression stress acting in the cohesive element. Such an approach is equivalent to a node-to-node contact friction. Its accuracy is acceptable only for small displacements. The material name of the linear cohesive law with friction is ``material_cohesive_linear_friction``. Its additional parameters with respect to those of the linear cohesive law without friction, with the respective default values, are: - ``mu = 0`` - ``penalty_for_friction = 0`` .. _ssect:smm:cl:coh-fatigue: Linear Cohesive Law with Fatigue '''''''''''''''''''''''''''''''' Keyword: **cohesive_linear_fatigue** Material description with input file: .. code-block:: python #input.dat material cohesive_linear_fatigue [ name = cohesive sigma_c = 1 # critical stress sigma_c (default: 0) beta = 1 # weighting parameter for sliding and normal opening (default: 0) delta_c = 1 # Critical displacement delta_f = 1 # delta_f (normalization of opening rate to alter reloading stiffness after fatigue) count_switches = true # Count the opening/closing switches per element ] ----- This law represents a variation of the linear irreversible cohesive law of the previous section, that removes the hypothesis of elastic unloading-reloading cycles. With this law, some energy is dissipated also during unloading and reloading with hysteresis. The implementation follows the work of :cite:`nguyen2001`. During the unloading-reloading cycle, the traction increment is computed as .. math:: \dot{T} = \begin{cases} K^- \, \dot{\delta} & \text{if $\dot{\delta} < 0$} \\ K^+ \, \dot{\delta} & \text{if $\dot{\delta} > 0$} \\ \end{cases} where :math:`\dot{\delta}` and :math:`\dot{T}` are respectively the effective opening displacement and the cohesive traction increments with respect to time, while :math:`K^-` and :math:`K^+` are respectively the unloading and reloading incremental stiffness. The unloading path is linear and results in an unloading stiffness .. math:: K^- = \frac{T_\mathrm{max}}{\delta_\mathrm{max}} where :math:`T_\mathrm{max}` and :math:`\delta_\mathrm{max}` are the maximum cohesive traction and the effective opening displacement reached during the precedent loading phase. The unloading stiffness remains constant during the unloading phase. On the other hand the reloading stiffness increment :math:`\dot{K}^+` is calculated as .. math:: \dot{K}^+ = \begin{cases} - K^+ \, \dot{\delta} / \delta_\mathrm{f} & \text{if $\dot{\delta} > 0$} \\ \left( K^+ - K^- \right) \, \dot{\delta} / \delta_\mathrm{f} & \text{if $\dot{\delta}$ < $0$} \end{cases} where :math:`\delta_\mathrm{f}` is a material parameter (refer to :cite:`vocialta15` for more details). During unloading the stiffness :math:`K^+` tends to :math:`K^-`, while during reloading :math:`K^+` gets decreased at every time step. If the cohesive traction during reloading exceeds the upper limit given by equation :eq:`eq-smm-coh-tractions`, it is recomputed following the behavior of the linear decreasing cohesive law for crack opening. .. _ssect:smm:cl:coh-exponential: Exponential Cohesive Law ''''''''''''''''''''''''' Keyword: **cohesive_exponential** Material description with input file: .. code-block:: python #input.dat material cohesive_exponential [ name = coh1 sigma_c = 1.5e6 # critical stress sigma_c (default: 0) beta = 1 # weighting parameter for sliding and normal opening (default: 0) delta_c = 1e-4 # Critical displacement exponential_penalty = true # Is contact penalty following the exponential law? contact_tangent = 1.0 # Ratio of contact tangent over the initial exponential tangent ] ----- Ortiz and Pandolfi proposed this cohesive law in 1999 :cite:`ortiz1999`. The traction-opening equation for this law is as follows: .. math:: T = e \sigma_c \frac{\delta}{\delta_c}e^{-\delta/ \delta_c} :label: eq:exponential_law This equation is plotted in :numref:`fig:smm:cl:ecl`. The term :math:`\partial{\vec{T}}/ \partial{\delta}` after the necessary derivation can expressed as .. math:: \frac{\partial{\vec{T}}} {\partial{\delta}} = \hat{\vec{T}} \otimes \frac {\partial{(T/\delta)}}{\partial{\delta}} \frac{\hat{\vec{T}}}{\delta}+ \frac{T}{\delta} \left[ \beta^2 \mat{I} + \left(1-\beta^2\right) \left(\vec{n} \otimes \vec{n}\right)\right] :label: eq:tangent_cohesive where .. math:: \frac{\partial{(T/ \delta)}}{\partial{\delta}} = \left\{\begin{array} {l l} -e \frac{\sigma_c}{\delta_c^2 }e^{-\delta / \delta_c} & \quad \text{if} \delta \geq \delta_{max}\\ 0 & \quad \text{if} \delta < \delta_{max}, \delta_n > 0 \end{array} \right. As regards the behavior in compression, two options are available: a contact penalty approach with stiffness following the formulation of the exponential law and a contact penalty approach with constant stiffness. In the second case, the stiffness is defined as a function of the tangent of the exponential law at the origin. .. figure:: figures/cl/cohesive_exponential.png :alt: Exponential cohesive law :name: fig:smm:cl:ecl :align: center Exponential cohesive law