Solid Mechanics Model

The solid mechanics model is a specific implementation of the Model interface dedicated to handle the equations of motion or equations of equilibrium. The model is created for a given mesh. It will create its own FEEngine object to compute the interpolation, gradient, integration and assembly operations. A SolidMechanicsModel object can simply be created like this:

SolidMechanicsModel model(mesh);

where mesh is the mesh for which the equations are to be solved. A second parameter called spatial_dimension can be added after mesh if the spatial dimension of the problem is different than that of the mesh.

This model contains at least the following six Arrays:


contains a Boolean value for each degree of freedom specifying whether that degree is blocked or not. A Dirichlet boundary condition can be prescribed by setting the blocked_dofs value of a degree of freedom to true. A Neumann boundary condition can be applied by setting the blocked_dofs value of a degree of freedom to false. The displacement, velocity and acceleration are computed for all degrees of freedom for which the blocked_dofs value is set to false. For the remaining degrees of freedom, the imposed values (zero by default after initialization) are kept.


contains the displacements of all degrees of freedom. It can be either a computed displacement for free degrees of freedom or an imposed displacement in case of blocked ones (\(\vec{u}\) in the following).


contains the velocities of all degrees of freedom. As displacement, it contains computed or imposed velocities depending on the nature of the degrees of freedom (\(\dot{\vec{u}}\) in the following).


contains the accelerations of all degrees of freedom. As displacement, it contains computed or imposed accelerations depending on the nature of the degrees of freedom (\(\ddot{\vec{u}}\) in the following).


contains the external forces applied on the nodes (\(\vec{f}_{\st{ext}}\) in the following).


contains the internal forces on the nodes (\(\vec{f}_{\mathrm{int}}\) in the following).

Some examples to help to understand how to use this model will be presented in the next sections.

Model Setup

Setting Initial Conditions

For a unique solution of the equations of motion, initial displacements and velocities for all degrees of freedom must be specified:

\[\begin{split}\vec{u}(t=0) & = \vec{u}_0\\ \dot{\vec u}(t=0) & = \vec{v}_0\end{split}\]

The solid mechanics model can be initialized as follows:


This function initializes the internal arrays and sets them to zero. Initial displacements and velocities that are not equal to zero can be prescribed by running a loop over the total number of nodes. Here, the initial displacement in \(x\)-direction and the initial velocity in \(y\)-direction for all nodes is set to \(0.1\) and \(1\), respectively:

auto & disp = model.getDisplacement();
auto & velo = model.getVelocity();

for (UInt node = 0; node < mesh.getNbNodes(); ++node) {
    disp(node, 0) = 0.1;
    velo(node, 1) = 1.;

Setting Boundary Conditions

This section explains how to impose Dirichlet or Neumann boundary conditions. A Dirichlet boundary condition specifies the values that the displacement needs to take for every point \(x\) at the boundary (\(\Gamma_u\)) of the problem domain (fig:smm:boundaries):

\[\vec{u} = \bar{\vec u} \quad \forall \vec{x}\in \Gamma_{u}\]

A Neumann boundary condition imposes the value of the gradient of the solution at the boundary \(\Gamma_t\) of the problem domain (fig:smm:boundaries):

\[\vec{t} = \mat{\sigma} \vec{n} = \bar{\vec t} \quad \forall \vec{x}\in \Gamma_{t}\]

Fig. 7 Problem domain \(\Omega\) with boundary in three dimensions. The Dirchelet and the Neumann regions of the boundary are denoted with \(\Gamma_u\) and \(\Gamma_t\), respecitvely.

Different ways of imposing these boundary conditions exist. A basic way is to loop over nodes or elements at the boundary and apply local values. A more advanced method consists of using the notion of the boundary of the mesh. In the following both ways are presented.

Starting with the basic approach, as mentioned, the Dirichlet boundary conditions can be applied by looping over the nodes and assigning the required values. Fig. 8 shows a beam with a fixed support on the left side. On the right end of the beam, a load is applied. At the fixed support, the displacement has a given value. For this example, the displacements in both the \(x\) and the \(y\)-direction are set to zero. Implementing this displacement boundary condition is similar to the implementation of initial displacement conditions described above. However, in order to impose a displacement boundary condition for all time steps, the corresponding nodes need to be marked as boundary nodes using the function blocked. While, in order to impose a load on the right side, the nodes are not marked. The detail codes are shown as follows

auto & blocked = model.getBlockedDOFs();
const auto & pos = mesh.getNodes();

UInt nb_nodes = mesh.getNbNodes();

for (UInt node = 0; node < nb_nodes; ++node) {
  if(Math::are_float_equal(pos(node, _x), 0)) {
    blocked(node, _x) = true; // block dof in x-direction
    blocked(node, _y) = true; // block dof in y-direction
    disp(node, _x) = 0.; // fixed displacement in x-direction
    disp(node, _y) = 0.; // fixed displacement in y-direction
  } else if (Math::are_float_equal(pos(node, _y), 0)) {
    blocked(node, _x) = false; // unblock dof in x-direction
    forces(node, _x) = 10.;    // force in x-direction

Fig. 8 Beam with fixed support and load.

For the more advanced approach, one needs the notion of a boundary in the mesh. Therefore, the boundary should be created before boundary condition functors can be applied. Generally the boundary can be specified from the mesh file or the geometry. For the first case, the function createGroupsFromMeshData is called. This function can read any types of mesh data which are provided in the mesh file. If the mesh file is created with Gmsh, the function takes one input strings which is either tag_0, tag_1 or physical_names. The first two tags are assigned by Gmsh to each element which shows the physical group that they belong to. In Gmsh, it is also possible to consider strings for different groups of elements. These elements can be separated by giving a string physical_names to the function createGroupsFromMeshData


Boundary conditions support can also be created from the geometry by calling createBoundaryGroupFromGeometry. This function gathers all the elements on the boundary of the geometry.

To apply the required boundary conditions, the function applyBC needs to be called on a SolidMechanicsModel. This function gets a Dirichlet or Neumann functor and a string which specifies the desired boundary on which the boundary conditions is to be applied. The functors specify the type of conditions to apply. Three built-in functors for Dirichlet exist: FlagOnly, FixedValue and IncrementValue. The functor FlagOnly is used if a point is fixed in a given direction. Therefore, the input parameter to this functor is only the fixed direction. The FixedValue functor is used when a displacement value is applied in a fixed direction. The IncrementValue applies an increment to the displacement in a given direction. The following code shows the utilization of three functors for the top, bottom and side surface of the mesh which were already defined in the Gmsh

model.applyBC(BC::Dirichlet::FixedValue(13.0, _y), "Top");
model.applyBC(BC::Dirichlet::FlagOnly(_x), "Bottom");
model.applyBC(BC::Dirichlet::IncrementValue(13.0, _x), "Side");

To apply a Neumann boundary condition, the applied traction or stress should be specified before. In case of specifying the traction on the surface, the functor FromTraction of Neumann boundary conditions is called. Otherwise, the functor FromStress should be called which gets the stress tensor as an input parameter

Vector<Real> surface_traction{0., 0., 1.};
auto surface_stress(3, 3) = Matrix<Real>::eye(3);

model.applyBC(BC::Neumann::FromTraction(surface_traction), "Bottom");
model.applyBC(BC::Neumann::FromStress(surface_stress), "Top");

If the boundary conditions need to be removed during the simulation, a functor is called from the Neumann boundary condition to free those boundary conditions from the desired boundary

model.applyBC(BC::Neumann::FreeBoundary(), "Side");

User specified functors can also be implemented. A full example for setting both initial and boundary conditions can be found in examples/ The problem solved in this example is shown in fig-smm-bc_and_id. It consists of a plate that is fixed with movable supports on the left and bottom side. On the right side, a traction, which increases linearly with the number of time steps, is applied. The initial displacement and velocity in \(x\)-direction at all free nodes is zero and two respectively.


Fig. 9 Plate on movable supports.

As it is mentioned in Section ref{sect:common:groups}, node and element groups can be used to assign the boundary conditions. A generic example is given below with a Dirichlet boundary condition:

// create a node group
NodeGroup & node_group = mesh.createNodeGroup("nodes_fix");

/* fill the node group with the nodes you want */

// create an element group using the existing node group

// boundary condition can be applied using the element group name
model.applyBC(BC::Dirichlet::FixedValue(0.0, _x), "el_fix");

Material Selector

If the user wants to assign different materials to different finite elements groups in Akantu, a material selector has to be used. By default, Akantu assigns the first valid material in the material file to all elements present in the model (regular continuum materials are assigned to the regular elements and cohesive materials are assigned to cohesive elements or element facets).

To assign different materials to specific elements, mesh data information such as tag information or specified physical names can be used. MeshDataMaterialSelector class uses this information to assign different materials. With the proper physical name or tag name and index, different materials can be assigned as demonstrated in the examples below:

auto mat_selector =

In this example the physical names specified in a GMSH geometry file will by used to match the material names in the input file.

Another example would be to use the first (tag_0) or the second (tag_1) tag associated to each elements in the mesh:

auto mat_selector = std::make_shared<MeshDataMaterialSelector<UInt>>(
    "tag_1", model, first_index);

where first_index (default is 1) is the value of tag_1 that will be associated to the first material in the material input file. The following values of the tag will be associated with the following materials.

There are four different material selectors pre-defined in Akantu. MaterialSelector and DefaultMaterialSelector is used to assign a material to regular elements by default. For the regular elements, as in the example above, MeshDataMaterialSelector can be used to assign different materials to different elements.

Apart from the Akantu’s default material selectors, users can always develop their own classes in the main code to tackle various multi-material assignment situations.

Static Analysis

The SolidMechanicsModel class can handle different analysis methods, the first one being presented is the static case. In this case, the equation to solve is

(3)\[\mat{K} \vec{u} = \vec{f}_{\mathrm{ext}}\]

where \(\mat{K}\) is the global stiffness matrix, \(\vec{u}\) the displacement vector and \(\vec{f}_{\st{ext}}\) the vector of external forces applied to the system.

To solve such a problem, the static solver of the SolidMechanicsModel object is used. First, a model has to be created and initialized. To create the model, a mesh (which can be read from a file) is needed, as explained in Section~ref{sect:common:mesh}. Once an instance of a SolidMechanicsModel is obtained, the easiest way to initialize it is to use the initFull method by giving the SolidMechanicsModelOptions. These options specify the type of analysis to be performed and whether the materials should be initialized with initMaterials or not

SolidMechanicsModel model(mesh);
model.initFull(_analysis_method = _static);

Here, a static analysis is chosen by passing the argument _static to the method. By default, the Boolean for no initialization of the materials is set to false, so that they are initialized during the initFull. The method initFull also initializes all appropriate vectors to zero. Once the model is created and initialized, the boundary conditions can be set as explained in Section Setting Boundary Conditions. Boundary conditions will prescribe the external forces for some free degrees of freedom \(\vec{f}_{\st{ext}}\) and displacements for some others. At this point of the analysis, the function solveStep can be called

auto & solver = model.getNonLinearSolver();
solver.set("max_iterations", 1);
solver.set("threshold", 1e-4);
solver.set("convergence_type", SolveConvergenceCriteria::_residual);


This function is templated by the solving method and the convergence criterion and takes two arguments: the tolerance and the maximum number of iterations (100 by default), which are \(10^{-4}\) and \(1\) for this example. The modified Newton-Raphson method is chosen to solve the system. In this method, the equilibrium equation (Eq. 3) is modified in order to apply a Newton-Raphson convergence algorithm:

\[\begin{split}\mat{K}^{i+1}\delta\vec{u}^{i+1} &= \vec{r} \\ &= \vec{f}_{\st{ext}} -\vec{f}_{\st{int}}\\ &= \vec{f}_{\st{ext}} - \mat{K}^{i} \vec{u}^{i}\\ \vec{u}^{i+1} &= \vec{u}^{i} + \delta\vec{u}^{i+1}~,\end{split}\]

where \(\delta\vec{u}\) is the increment of displacement to be added from one iteration to the other, and \(i\) is the Newton-Raphson iteration counter. By invoking the solveStep method in the first step, the global stiffness matrix \(\mat{K}\) from (Eq. 3) is automatically assembled. A Newton-Raphson iteration is subsequently started, \(\mat{K}\) is updated according to the displacement computed at the previous iteration and one loops until the forces are balanced (SolveConvergenceCriteria::_residual), i.e. \(||\vec{r}|| <\) threshold. One can also iterate until the increment of displacement is zero (SolveConvergenceCriteria::_solution) which also means that the equilibrium is found. For a linear elastic problem, the solution is obtained in one iteration and therefore the maximum number of iterations can be set to one. But for a non-linear case, one needs to iterate as long as the norm of the residual exceeds the tolerance threshold and therefore the maximum number of iterations has to be higher, e.g. \(100\)

solver.set("max_iterations", 100);

At the end of the analysis, the final solution is stored in the displacement vector. A full example of how to solve a static problem is presented in the code examples/static/ This example is composed of a 2D plate of steel, blocked with rollers on the left and bottom sides as shown in Fig. 10. The nodes from the right side of the sample are displaced by \(0.01\%\) of the length of the plate.


Fig. 10 Numerical setup.

The results of this analysis is depicted in Fig. 11.


Fig. 11 Solution of the static analysis. Left: the initial condition, right: the solution (deformation magnified 50 times).

Dynamic Methods

Different ways to solve the equations of motion are implemented in the solid mechanics model. The complete equations that should be solved are:

(4)\[\mat{M}\ddot{\vec{u}} + \mat{C}\dot{\vec{u}} + \mat{K}\vec{u} = \vec{f}_{\mathrm{ext}}\]

where \(\mat{M}\), \(\mat{C}\) and \(\mat{K}\) are the mass, damping and stiffness matrices, respectively.

In the previous section, it has already been discussed how to solve this equation in the static case, where \(\ddot{\vec{u}} = \dot{\vec{u}} = 0\). Here the method to solve this equation in the general case will be presented. For this purpose, a time discretization has to be specified. The most common discretization method in solid mechanics is the Newmark-\(\beta\) method, which is also the default in Akantu.

For the Newmark-\(\beta\) method, (Eq. 4) becomes a system of three equations (see [curnier92a][hughes-83a] for more details):

(5)\[\begin{split}\begin{eqnarray} \mat{M} \ddot{\vec{u}}_{n+1} + \mat{C}\dot{\vec{u}}_{n+1} + \mat{K} \vec{u}_{n+1} &={\vec{f}_{\st{ext}}}_{\, n+1}\\ \vec{u}_{n+1} &= \vec{u}_{n} + \left(1 - \alpha\right) \Delta t \dot{\vec{u}}_{n} + \alpha \Delta t \dot{\vec{u}}_{n+1} + \left(\frac{1}{2} - \alpha\right) \Delta t^2 \ddot{\vec{u}}_{n}\\ \dot{\vec{u}}_{n+1} &= \dot{\vec{u}}_{n} + \left(1 - \beta\right) \Delta t \ddot{\vec{u}}_{n} + \beta \Delta t \ddot{\vec{u}}_{n+1} \end{eqnarray}\end{split}\]

In these new equations, \(\ddot{\vec{u}}_{n}\), \(\dot{\vec{u}}_{n}\) and \(\vec{u}_{n}\) are the approximations of \(\ddot{\vec{u}}(t_n)\), \(\dot{\vec{u}}(t_n)\) and \(\vec{u}(t_n)\). Equation~(ref{eqn:equation-motion-discret}) is the equation of motion discretized in space (finite-element discretization), and the equations above are discretized in both space and time (Newmark discretization). The \(\alpha\) and \(\beta\) parameters determine the stability and the accuracy of the algorithm. Classical values for \(\alpha\) and \(\beta\) are usually \(\beta = 1/2\) for no numerical damping and \(0 < \alpha < 1/2\).


Method (\(beta= 1/2\))



central difference



Fox-Goodwin(royal road)



Linear acceleration



Average acceleration (trapeziodal rule)


The solution of this system of equations, (Eq. 5)) is split into a predictor and a corrector system of equations. Moreover, in the case of a non-linear equations, an iterative algorithm such as the Newton-Raphson method is applied. The system of equations can be written as:

  • Predictor:

    \[\begin{split}\vec{u}_{n+1}^{0} &= \vec{u}_{n} + \Delta t \dot{\vec{u}}_{n} + \frac{\Delta t^2}{2} \ddot{\vec{u}}_{n} \\ \dot{\vec{u}}_{n+1}^{0} &= \dot{\vec{u}}_{n} + \Delta t \ddot{\vec{u}}_{n} \\ \ddot{\vec{u}}_{n+1}^{0} &= \ddot{\vec{u}}_{n}\end{split}\]
  • Solve:

    \[\begin{split}\left(c \mat{M} + d \mat{C} + e \mat{K}_{n+1}^i\right) \vec{w} &= {\vec{f}_{\st{ext}}}_{\,n+1} - {\vec{f}_{\st{int}}}_{\,n+1}^i - \mat{C} \dot{\vec{u}}_{n+1}^i - \mat{M} \ddot{\vec{u}}_{n+1}^i\\ &= \vec{r}_{n+1}^i\end{split}\]
  • Corrector:

    \[\begin{split}\ddot{\vec{u}}_{n+1}^{i+1} &= \ddot{\vec{u}}_{n+1}^{i} +c \vec{w} \\ \dot{\vec{u}}_{n+1}^{i+1} &= \dot{\vec{u}}_{n+1}^{i} + d\vec{w} \\ \vec{u}_{n+1}^{i+1} &= \vec{u}_{n+1}^{i} + e \vec{w}\end{split}\]

where \(i\) is the Newton-Raphson iteration counter and \(c\), \(d\) and \(e\) are parameters depending on the method used to solve the equations





in acceleration


\(\alpha\beta\Delta t^2\)

\(\beta\Delta t\)


in velocity


\(\alpha\Delta t\)


\(\frac{1}{\beta\Delta t}\)

in displacement



\(\frac{1}{\alpha\Delta t}\)

\(\frac{1}{\alpha\beta \Delta t^2}\)


If you want to use the implicit solver Akantu should be compiled at least with one sparse matrix solver such as Mumps [mumps].

Implicit Time Integration

To solve a problem with an implicit time integration scheme, first a SolidMechanicsModel object has to be created and initialized. Then the initial and boundary conditions have to be set. Everything is similar to the example in the static case (Section~ref{sect:smm:static}), however, in this case the implicit dynamic scheme is selected at the initialization of the model:

SolidMechanicsModel model(mesh);
model.initFull(_analysis_method = _implicit_dynamic);

Because a dynamic simulation is conducted, an integration time step \(\Delta t\) has to be specified. In the case of implicit simulations, Akantu implements a trapezoidal rule by default. That is to say \(\alpha = 1/2\) and \(\beta = 1/2\) which is unconditionally stable. Therefore the value of the time step can be chosen arbitrarily within reason:


Since the system has to be solved for a given amount of time steps, the method solveStep(), (which has already been used in the static example in Section~ref{sect:smm:static}), is called inside a time loop:

/// time loop
Real time = 0.;

auto & solver = model.getNonLinearSolver();
solver.set("max_iterations", 100);
solver.set("threshold", 1e-12);
solver.set("convergence_type", SolveConvergenceCriteria::_solution);

for (UInt s = 1; time <max_time; ++s, time += time_step) {

An example of solid mechanics with an implicit time integration scheme is presented in examples/implicit/ This example consists of a 3D beam of \(10\mathrm{m}\times1\mathrm{m}\times1\mathrm{m}\) blocked on one side and is on a roller on the other side. A constant force of \(5\mathrm{kN}\) is applied in its middle. Fig. 12 presents the geometry of this case. The material used is a fictitious linear elastic material with a density of \(1000 \mathrm{kg/m}^3\), a Young’s Modulus of \(120 \mathrm{MPa}\) and Poisson’s ratio of \(0.3\). These values were chosen to simplify the analytical solution.

An approximation of the dynamic response of the middle point of the beam is given by:

\[u\left(\frac{L}{2}, t\right) = \frac{1}{\pi^4} \left(1 - cos\left(\pi^2 t\right) + \frac{1}{81}\left(1 - cos\left(3^2 \pi^2 t\right)\right) + \frac{1}{625}\left(1 - cos\left(5^2 \pi^2 t\right)\right)\right)\]

Fig. 12 Numerical setup.

Figure Fig. 13 presents the deformed beam at 3 different times during the simulation: time steps 0, 1000 and 2000.


Fig. 13 Deformed beam at three different times (displacement \(\times 10\)).

Explicit Time Integration

The explicit dynamic time integration scheme is based on the Newmark-\(\beta\) scheme with \(\alpha=0\) (see equations ref{eqn:equation-motion-discret}-ref{eqn:finite-difference-2}). In Akantu, \(\beta\) is defaults to \(\beta=1/2\), see section ref{sect:smm:Dynamic_methods}.

The initialization of the simulation is similar to the static and implicit dynamic version. The model is created from the SolidMechanicsModel class. In the initialization, the explicit scheme is selected using the _explicit_lumped_mass constant:

SolidMechanicsModel model(mesh);
model.initFull(_analysis_method = _explicit_lumped_mass);


Writing model.initFull() or model.initFull(); is equivalent to use the _explicit_lumped_mass keyword, as this is the default case.

The explicit time integration scheme implemented in Akantu uses a lumped mass matrix \(\mat{M}\) (reducing the computational cost). This matrix is assembled by distributing the mass of each element onto its nodes. The resulting \(\mat{M}\) is therefore a diagonal matrix stored in the mass vector of the model.

The explicit integration scheme is conditionally stable. The time step has to be smaller than the stable time step which is obtained in Akantu as follows:

critical_time_step = model.getStableTimeStep();

The stable time step corresponds to the time the fastest wave (the compressive wave) needs to travel the characteristic length of the mesh:

\[\Delta t_{\st{crit}} = \frac{\Delta x}{c}\]

where \(\Delta x\) is a characteristic length (eg the inradius in the case of linear triangle element) and \(c\) is the celerity of the fastest wave in the material. It is generally the compressive wave of celerity \(c = \sqrt{\frac{2 \mu + \lambda}{\rho}}\), \(\mu\) and \(\lambda\) are the first and second Lame’s coefficients and \(\rho\) is the density. However, it is recommended to impose a time step that is smaller than the stable time step, for instance, by multiplying the stable time step by a safety factor smaller than one:

const Real safety_time_factor = 0.8;
Real applied_time_step = critical_time_step * safety_time_factor;

The initial displacement and velocity fields are, by default, equal to zero if not given specifically by the user (see ref{sect:smm:initial_condition}).

Like in implicit dynamics, a time loop is used in which the displacement, velocity and acceleration fields are updated at each time step. The values of these fields are obtained from the Newmark:math:-beta equations with \(\beta=1/2\) and \(\alpha=0\). In Akantu these computations at each time step are invoked by calling the function solveStep:

for (UInt s = 1; (s-1)*applied_time_step < total_time; ++s) {

The method solveStep wraps the four following functions:

  • model.explicitPred() allows to compute the displacement

    field at \(t+1\) and a part of the velocity field at \(t+1\), denoted by \(\vec{\dot{u}^{\st{p}}}_{n+1}\), which will be used later in the method model.explicitCorr(). The equations are:

    \[\begin{split}\vec{u}_{n+1} &= \vec{u}_{n} + \Delta t \vec{\dot{u}}_{n} + \frac{\Delta t^2}{2} \vec{\ddot{u}}_{n}\\ \vec{\dot{u}^{\st{p}}}_{n+1} &= \vec{\dot{u}}_{n} + \Delta t \vec{\ddot{u}}_{n}\end{split}\]
  • model.updateResidual() and model.updateAcceleration() compute the acceleration increment

    \(\delta \vec{\ddot{u}}\):

    \[\left(\mat{M} + \frac{1}{2} \Delta t \mat{C}\right) \delta \vec{\ddot{u}} = \vec{f_{\st{ext}}} - \vec{f}_{\st{int}\, n+1} - \mat{C} \vec{\dot{u}^{\st{p}}}_{n+1} - \mat{M} \vec{\ddot{u}}_{n}\]
    The internal force \(\vec{f}_{\st{int}\, n+1}\) is computed from the

    displacement \(\vec{u}_{n+1}\) based on the constitutive law.

  • model.explicitCorr() computes the velocity and

    acceleration fields at \(t+1\):

    \[\begin{split}\vec{\dot{u}}_{n+1} &= \vec{\dot{u}^{\st{p}}}_{n+1} + \frac{\Delta t}{2} \delta \vec{\ddot{u}} \\ \vec{\ddot{u}}_{n+1} &= \vec{\ddot{u}}_{n} + \delta \vec{\ddot{u}}\end{split}\]

The use of an explicit time integration scheme is illustrated by the example: examples/explicit/ This example models the propagation of a wave in a steel beam. The beam and the applied displacement in the \(x\) direction are shown in Fig. 14.


Fig. 14 Numerical setup.

The length and height of the beam are \(L={10}\textrm{m}\) and \(h = {1}\textrm{m}\), respectively. The material is linear elastic, homogeneous and isotropic (density: SI{7800}{kilogrampercubicmetre}, Young’s modulus: SI{210}{gigapascal} and Poisson’s ratio: \(0.3\)). The imposed displacement follow a Gaussian function with a maximum amplitude of \(A = {0.01}\textrm{m}\). The potential, kinetic and total energies are computed. The safety factor is equal to \(0.8\).

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 [sect:io:material]).
In order to conveniently store values at each quadrature in a material point Akantu provides a special data structure, the at InternalField. The internal fields are inheriting from the at ElementTypeMapArray. Furthermore, it provides several functions for initialization, auto-resizing and auto removal of quadrature points.

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 \(base\) value to which we add a random number that follows the chosen distribution.

The Uniform distribution is gives a random values between in \([min, max)\). The Weibull distribution is characterized by the following cumulative distribution function:

\[F(x) = 1- e^{-\left({x/\lambda}\right)^m}\]

which depends on \(m\) and \(\lambda\), 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:

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:


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. In Appendix 7 a summary of the parameters for all materials of Akantu is provided.


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 \(\boldsymbol{\sigma} = \boldsymbol{C}:\boldsymbol{\varepsilon}\) with where \(\boldsymbol{\sigma}\) is the Cauchy stress tensor, \(\boldsymbol{\varepsilon}\) represents the infinitesimal strain tensor and \(\boldsymbol{C}\) is the elastic modulus tensor.

Linear isotropic

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 Figure [fig:smm:cl:elastic].

The equation that relates the strains to the displacements is: point) from the displacements as follows:

\[\label{eqn:smm:strain_inf} \boldsymbol{\varepsilon} = \frac{1}{2} \left[ \nabla_0 \boldsymbol{u}+\nabla_0 \boldsymbol{u}^T \right]\]

where \(\boldsymbol{\varepsilon}\) represents the infinitesimal strain tensor, \(\nabla_{0}\boldsymbol{u}\) the displacement gradient tensor according to the initial configuration. The constitutive equation for isotropic homogeneous media can be expressed as:

\[\label{eqn:smm:material:constitutive_elastic} \boldsymbol{\sigma } =\lambda\mathrm{tr}(\boldsymbol{\varepsilon})\boldsymbol{I}+2 \mu\boldsymbol{\varepsilon}\]

where \(\boldsymbol{\sigma}\) is the Cauchy stress tensor (\(\lambda\) and \(\mu\) are the the first and second Lame’s coefficients).

In Voigt notation this correspond to

\[\begin{split}\begin{aligned} \left[\begin{array}{c} \sigma_{11}\\ \sigma_{22}\\ \sigma_{33}\\ \sigma_{23}\\ \sigma_{13}\\ \sigma_{12}\\ \end{array}\right] &= \frac{E}{(1+\nu)(1-2\nu)}\left[ \begin{array}{cccccc} 1-\nu & \nu & \nu & 0 & 0 & 0\\ \nu & 1-\nu & \nu & 0 & 0 & 0\\ \nu & \nu & 1-\nu & 0 & 0 & 0\\ 0 & 0 & 0 & \frac{1-2\nu}{2} & 0 & 0 \\ 0 & 0 & 0 & 0 & \frac{1-2\nu}{2} & 0 \\ 0 & 0 & 0 & 0 & 0 & \frac{1-2\nu}{2} \\ \end{array}\right] \left[\begin{array}{c} \varepsilon_{11}\\ \varepsilon_{22}\\ \varepsilon_{33}\\ 2\varepsilon_{23}\\ 2\varepsilon_{13}\\ 2\varepsilon_{12}\\ \end{array}\right]\end{aligned}\end{split}\]

Linear anisotropic

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. For this we define the elastic modulus tensor as follow:

\[\begin{split}\begin{aligned} \left[\begin{array}{c} \sigma_{11}\\ \sigma_{22}\\ \sigma_{33}\\ \sigma_{23}\\ \sigma_{13}\\ \sigma_{12}\\ \end{array}\right] &= \left[ \begin{array}{cccccc} c_{11} & c_{12} & c_{13} & c_{14} & c_{15} & c_{16}\\ c_{21} & c_{22} & c_{23} & c_{24} & c_{25} & c_{26}\\ c_{31} & c_{32} & c_{33} & c_{34} & c_{35} & c_{36}\\ c_{41} & c_{42} & c_{43} & c_{44} & c_{45} & c_{46}\\ c_{51} & c_{52} & c_{53} & c_{54} & c_{55} & c_{56}\\ c_{61} & c_{62} & c_{63} & c_{64} & c_{65} & c_{66}\\ \end{array}\right] \left[\begin{array}{c} \varepsilon_{11}\\ \varepsilon_{22}\\ \varepsilon_{33}\\ 2\varepsilon_{23}\\ 2\varepsilon_{13}\\ 2\varepsilon_{12}\\ \end{array}\right]\end{aligned}\end{split}\]

To simplify the writing of input files the \(\boldsymbol{C}\) tensor is expressed in the material basis. And this basis as to be given too. This basis \(\Omega_{{\mathrm{mat}}} = \{\boldsymbol{n_1}, \boldsymbol{n_2}, \boldsymbol{n_3}\}\) is used to define the rotation \(R_{ij} = \boldsymbol{n_j} . \boldsymbol{e_i}\). And \(\boldsymbol{C}\) can be rotated in the global basis \(\Omega = \{\boldsymbol{e_1}, \boldsymbol{e_2}, \boldsymbol{e_3}\}\) as follow:

\[\begin{split}\begin{aligned} \boldsymbol{C}_{\Omega} &= \boldsymbol{R}_1 \boldsymbol{C}_{\Omega_{{\mathrm{mat}}}} \boldsymbol{R}_2\\ \boldsymbol{R}_1 &= \left[ \begin{array}{cccccc} R_{11} R_{11} & R_{12} R_{12} & R_{13} R_{13} & R_{12} R_{13} & R_{11} R_{13} & R_{11} R_{12}\\ R_{21} R_{21} & R_{22} R_{22} & R_{23} R_{23} & R_{22} R_{23} & R_{21} R_{23} & R_{21} R_{22}\\ R_{31} R_{31} & R_{32} R_{32} & R_{33} R_{33} & R_{32} R_{33} & R_{31} R_{33} & R_{31} R_{32}\\ R_{21} R_{31} & R_{22} R_{32} & R_{23} R_{33} & R_{22} R_{33} & R_{21} R_{33} & R_{21} R_{32}\\ R_{11} R_{31} & R_{12} R_{32} & R_{13} R_{33} & R_{12} R_{33} & R_{11} R_{33} & R_{11} R_{32}\\ R_{11} R_{21} & R_{12} R_{22} & R_{13} R_{23} & R_{12} R_{23} & R_{11} R_{23} & R_{11} R_{22}\\ \end{array}\right]\\ \boldsymbol{R}_2 &= \left[ \begin{array}{cccccc} R_{11} R_{11} & R_{21} R_{21} & R_{31} R_{31} & R_{21} R_{31} & R_{11} R_{31} & R_{11} R_{21}\\ R_{12} R_{12} & R_{22} R_{22} & R_{32} R_{32} & R_{22} R_{32} & R_{12} R_{32} & R_{12} R_{22}\\ R_{13} R_{13} & R_{23} R_{23} & R_{33} R_{33} & R_{23} R_{33} & R_{13} R_{33} & R_{13} R_{23}\\ R_{12} R_{13} & R_{22} R_{23} & R_{32} R_{33} & R_{22} R_{33} & R_{12} R_{33} & R_{12} R_{23}\\ R_{11} R_{13} & R_{21} R_{23} & R_{31} R_{33} & R_{21} R_{33} & R_{11} R_{33} & R_{11} R_{23}\\ R_{11} R_{12} & R_{21} R_{22} & R_{31} R_{32} & R_{21} R_{32} & R_{11} R_{32} & R_{11} R_{22}\\ \end{array}\right]\\\end{aligned}\end{split}\]

Linear orthotropic

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.

\[\begin{split}\begin{aligned} \left[\begin{array}{c} \sigma_{11}\\ \sigma_{22}\\ \sigma_{33}\\ \sigma_{23}\\ \sigma_{13}\\ \sigma_{12}\\ \end{array}\right] &= \left[ \begin{array}{cccccc} c_{11} & c_{12} & c_{13} & 0 & 0 & 0 \\ & c_{22} & c_{23} & 0 & 0 & 0 \\ & & c_{33} & 0 & 0 & 0 \\ & & & c_{44} & 0 & 0 \\ & \multicolumn{2}{l}{\text{sym.}} & & c_{55} & 0 \\ & & & & & c_{66}\\ \end{array}\right] \left[\begin{array}{c} \varepsilon_{11}\\ \varepsilon_{22}\\ \varepsilon_{33}\\ 2\varepsilon_{23}\\ 2\varepsilon_{13}\\ 2\varepsilon_{12}\\ \end{array}\right]\end{aligned}\end{split}\]
\[\begin{split}\begin{aligned} c_{11} &= E_1 (1 - \nu_{23}\nu_{32})\Gamma \qquad c_{22} = E_2 (1 - \nu_{13}\nu_{31})\Gamma \qquad c_{33} = E_3 (1 - \nu_{12}\nu_{21})\Gamma\\ c_{12} &= E_1 (\nu_{21} - \nu_{31}\nu_{23})\Gamma = E_2 (\nu_{12} - \nu_{32}\nu_{13})\Gamma\\ c_{13} &= E_1 (\nu_{31} - \nu_{21}\nu_{32})\Gamma = E_2 (\nu_{13} - \nu_{21}\nu_{23})\Gamma\\ c_{23} &= E_2 (\nu_{32} - \nu_{12}\nu_{31})\Gamma = E_3 (\nu_{23} - \nu_{21}\nu_{13})\Gamma\\ c_{44} &= \mu_{23} \qquad c_{55} = \mu_{13} \qquad c_{66} = \mu_{12} \\ \Gamma &= \frac{1}{1 - \nu_{12} \nu_{21} - \nu_{13} \nu_{31} - \nu_{32} \nu_{23} - 2 \nu_{21} \nu_{32} \nu_{13}}\end{aligned}\end{split}\]

The Poisson ratios follow the rule \(\nu_{ij} = \nu_{ji} E_i / E_j\).


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.

Neo-hookean Stress-strain curve.

Fig. 15 Neo-hookean Stress-strain curve.

As illustrated in Figure 4.6, 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 [Belytschko:2000].

The strain energy stored in the material is given by:

\[\label{eqn:smm:constitutive:neohookean_potential} \Psi(\boldsymbol{C}) = \frac{1}{2}\lambda_0\left(\ln J\right)^2-\mu_0\ln J+\frac{1}{2} \mu_0\left(\mathrm{tr}(\boldsymbol{C})-3\right)\]

where \(\lambda_0\) and \(\mu_0\) are, respectively, Lamé’s first parameter and the shear modulus at the initial configuration. \(J\) is the jacobian of the deformation gradient (\(\boldsymbol{F}=\nabla_{\!\!\boldsymbol{X}}\boldsymbol{x}\)): \(J=\text{det}(\boldsymbol{F})\). Finally \(\boldsymbol{C}\) 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 (\(\boldsymbol{\sigma}\)) should be computed through the second Piola-Kirchhoff stress tensor \(\boldsymbol{S}\):

\[\boldsymbol{\sigma } = \frac{1}{J}\boldsymbol{F}\boldsymbol{S}\boldsymbol{F}^T\]

Finally the second Piola-Kirchhoff stress tensor is given by:

\[\boldsymbol{S} = 2\frac{\partial\Psi}{\partial\boldsymbol{C}} = \lambda_0\ln J \boldsymbol{C}^{-1}+\mu_0\left(\boldsymbol{I}-\boldsymbol{C}^{-1}\right)\]

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).


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 Figure [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).

The standard rheological linear solid model (see Sections 10.2 and 10.3 of [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 Figure [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):

\[\frac{d\varepsilon(t)}{dt} = \left ( E + E_V \right ) ^ {-1} \cdot \left [ \frac{d\sigma(t)}{dt} + \frac{E_V}{\eta}\sigma(t) - \frac{EE_V}{\eta}\varepsilon(t) \right ]\]

where \(\eta\) is the viscosity. The equilibrium condition is unique and is attained in the limit, as \(t \to \infty\). At this stage, the response is elastic and depends on the Young’s modulus \(E\). 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.

Small-Deformation Plasticity

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. Figure 4.7 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

\[\begin{split}\boldsymbol{\varepsilon} &= \boldsymbol{\varepsilon}^e +\boldsymbol{\varepsilon}^p\\ \boldsymbol{\sigma} &= 2G(\boldsymbol{\varepsilon}^e) + \lambda \mathrm{tr}(\boldsymbol{\varepsilon}^e)\boldsymbol{I}\end{split}\]

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.

\[\label{eqn:smm:constitutive:von Mises} f = \sigma_{{\mathrm{eff}}} - \sigma_y = \left(\frac{3}{2} {\boldsymbol{\sigma}}^{{\mathrm{tr}}} : {\boldsymbol{\sigma}}^{{\mathrm{tr}}}\right)^\frac{1}{2}-\sigma_y (\boldsymbol{\varepsilon}^p)\]
\[\label{eqn:smm:constitutive:yielding} f < 0 \quad \textrm{Elastic deformation,} \qquad f = 0 \quad \textrm{Plastic deformation}\]

where \(\sigma_y\) is the yield strength of the material which can be function of plastic strain in case of hardening type of materials and \({\boldsymbol{\sigma}}^{{\mathrm{tr}}}\) is the deviatoric part of stress given by

\[\label{eqn:smm:constitutive:deviatoric stress} {\boldsymbol{\sigma}}^{{\mathrm{tr}}}=\boldsymbol{\sigma} - \frac{1}{3} \mathrm{tr}(\boldsymbol{\sigma}) \boldsymbol{I}\]

After yielding \((f = 0)\), 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

\[\label{eqn:smm:constitutive:plastic contitutive equation} \Delta {\boldsymbol{\varepsilon}}^p = \Delta p \frac {\partial{f}}{\partial{\boldsymbol{\sigma}}}=\frac{3}{2} \Delta p \frac{{\boldsymbol{\sigma}}^{{\mathrm{tr}}}}{\sigma_{{\mathrm{eff}}}}\]

In these expressions, the direction of the plastic strain increment (or equivalently, plastic strain rate) is given by \(\frac{{\boldsymbol{\sigma}}^{{\mathrm{tr}}}}{\sigma_{{\mathrm{eff}}}}\) while the magnitude is defined by the plastic multiplier \(\Delta p\). 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:

  1. Compute the trial stress:

    \[{\boldsymbol{\sigma}}^{{\mathrm{tr}}} = {\boldsymbol{\sigma}}_t + 2G\Delta \boldsymbol{\varepsilon} + \lambda \mathrm{tr}(\Delta \boldsymbol{\varepsilon})\boldsymbol{I}\]
  2. Check the Yielding criteria:

    \[f = (\frac{3}{2} {\boldsymbol{\sigma}}^{{\mathrm{tr}}} : {\boldsymbol{\sigma}}^{{\mathrm{tr}}})^{1/2}-\sigma_y (\boldsymbol{\varepsilon}^p)\]
  3. Compute the Plastic multiplier:

    \[\begin{split}\begin{aligned} d \Delta p &= \frac{\sigma^{tr}_{eff} - 3G \Delta P^{(k)}- \sigma_y^{(k)}}{3G + h}\\ \Delta p^{(k+1)} &= \Delta p^{(k)}+ d\Delta p\\ \sigma_y^{(k+1)} &= (\sigma_y)_t+ h\Delta p \end{aligned}\end{split}\]
  4. Compute the plastic strain increment:

    \[\Delta {\boldsymbol{\varepsilon}}^p = \frac{3}{2} \Delta p \frac{{\boldsymbol{\sigma}}^{{\mathrm{tr}}}}{\sigma_{{\mathrm{eff}}}}\]
  5. Compute the stress increment:

    \[{\Delta \boldsymbol{\sigma}} = 2G(\Delta \boldsymbol{\varepsilon}-\Delta \boldsymbol{\varepsilon}^p) + \lambda \mathrm{tr}(\Delta \boldsymbol{\varepsilon}-\Delta \boldsymbol{\varepsilon}^p)\boldsymbol{I}\]
  6. Update the variables:

    \[\begin{split}\begin{aligned} {\boldsymbol{\varepsilon^p}} &= {\boldsymbol{\varepsilon}}^p_t+{\Delta {\boldsymbol{\varepsilon}}^p}\\ {\boldsymbol{\sigma}} &= {\boldsymbol{\sigma}}_t+{\Delta \boldsymbol{\sigma}} \end{aligned}\end{split}\]

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: \(\sigma_y\) (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).


In the simplified case of a linear elastic and brittle material, isotropic damage can be represented by a scalar variable \(d\), which varies from \(0\) to \(1\) for no damage to fully broken material respectively. The stress-strain relationship then becomes:

\[\boldsymbol{\sigma} = (1-d)\, \boldsymbol{C}:\boldsymbol{\varepsilon}\]

where \(\boldsymbol{\sigma}\), \(\boldsymbol{\varepsilon}\) are the Cauchy stress and strain tensors, and \(\boldsymbol{C}\) 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.


This damage evolution law is energy based as defined by Marigo [marigo81a][ lemaitre96a]. It is an isotropic damage law.

\[\begin{split}\begin{aligned} Y &= \frac{1}{2}\boldsymbol{\varepsilon}:\boldsymbol{C}:\boldsymbol{\varepsilon}\\ F &= Y - Y_d - S d\\ d &= \left\{ \begin{array}{l l} \mathrm{min}\left(\frac{Y-Y_d}{S},\;1\right) & \mathrm{if}\; F > 0\\ \mathrm{unchanged} & \mathrm{otherwise} \end{array} \right.\end{aligned}\end{split}\]

In this formulation, \(Y\) is the strain energy release rate, \(Y_d\) the rupture criterion and \(S\) the damage energy. The non-local version of this damage evolution law is constructed by averaging the energy \(Y\).


This law introduced by Mazars [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 \(\varepsilon_{{\mathrm{eq}}} = \sqrt{<\boldsymbol{\varepsilon}>_+:<\boldsymbol{\varepsilon}>_+}\), with \(<.>_+\) the positive part of the tensor. This part is defined in the principal coordinates (I, II, III) as \(\varepsilon_{{\mathrm{eq}}} = \sqrt{<\boldsymbol{\varepsilon_I}>_+^2 + <\boldsymbol{\varepsilon_{II}}>_+^2 + <\boldsymbol{\varepsilon_{III}}>_+^2}\). The damage is defined as:

\[\begin{split}\begin{aligned} D &= \alpha_t^\beta D_t + (1-\alpha_t)^\beta D_c\\ D_t &= 1 - \frac{\kappa_0 (1- A_t)}{\varepsilon_{{\mathrm{eq}}}} - A_t \exp^{-B_t(\varepsilon_{{\mathrm{eq}}}-\kappa_0)}\\ D_c &= 1 - \frac{\kappa_0 (1- A_c)}{\varepsilon_{{\mathrm{eq}}}} - A_c \exp^{-B_c(\varepsilon_{{\mathrm{eq}}}-\kappa_0)}\\ \alpha_t &= \frac{\sum_{i=1}^3<\varepsilon_i>_+\varepsilon_{{\mathrm{nd}}\;i}}{\varepsilon_{{\mathrm{eq}}}^2}\end{aligned}\end{split}\]

With \(\kappa_0\) the damage threshold, \(A_t\) and \(B_t\) the damage parameter in traction, \(A_c\) and \(B_c\) the damage parameter in compression, \(\beta\) is the shear parameter. \(\alpha_t\) is the coupling parameter between traction and compression, the \(\varepsilon_i\) are the eigenstrain and the \(\varepsilon_{{\mathrm{nd}}\;i}\) are the eigenvalues of the strain if the material were undamaged.

The coefficients \(A\) and \(B\) are the post-peak asymptotic value and the decay shape parameters.

Adding a New Constitutive Law

There are several constitutive laws in Akantu as described in the previous Section Constitutive Laws. It is also possible to use a user-defined material for the simulation. These materials are referred to as local materials since they are local to the example of the user and not part of the Akantu library. To define a new local material, two files (material_XXX.hh and have to be provided where XXX is the name of the new material. The header file material_XXX.hh defines the interface of your custom material. Its implementation is provided in the The new law must inherit from the Material class or any other existing material class. It is therefore necessary to include the interface of the parent material in the header file of your local material and indicate the inheritance in the declaration of the class:

auto & solver = model.getNonLinearSolver();
solver.set("max_iterations", 1);
solver.set("threshold", 1e-4);
solver.set("convergence_type", SolveConvergenceCriteria::_residual);


/* ---------------------------------------------------------------------- */
#include "material.hh"
/* ---------------------------------------------------------------------- */


namespace akantu {

class MaterialXXX : public Material {

/// declare here the interface of your material


In the header file the user also needs to declare all the members of the new material. These include the parameters that a read from the material input file, as well as any other material parameters that will be computed during the simulation and internal variables.

In the following the example of adding a new damage material will be presented. In this case the parameters in the material will consist of the Young’s modulus, the Poisson coefficient, the resistance to damage and the damage threshold. The material will then from these values compute its Lamé coefficients and its bulk modulus. Furthermore, the user has to add a new internal variable damage in order to store the amount of damage at each quadrature point in each step of the simulation. For this specific material the member declaration inside the class will look as follows:

class LocalMaterialDamage : public Material {

/// declare constructors/destructors here

/// declare methods and accessors here

  /* -------------------------------------------------------------------- */
  /* Class Members                                                        */
  /* -------------------------------------------------------------------- */


  /// the young modulus
  Real E;

  /// Poisson coefficient
  Real nu;

  /// First Lame coefficient
  Real lambda;

  /// Second Lame coefficient (shear modulus)
  Real mu;

  /// resistance to damage
  Real Yd;

  /// damage threshold
  Real Sd;

  /// Bulk modulus
  Real kpa;

  /// damage internal variable
  InternalField<Real> damage;


In order to enable to print the material parameters at any point in the user’s example file using the standard output stream by typing:

for (UInt m = 0; m  < model.getNbMaterials(); ++m)
  std::cout << model.getMaterial(m) << std::endl;

the standard output stream operator has to be redefined. This should be done at the end of the header file:

class LocalMaterialDamage : public Material {

  /// declare here the interace of your material

/* ---------------------------------------------------------------------- */
/* inline functions                                                       */
/* ---------------------------------------------------------------------- */
/// standard output stream operator
inline std::ostream & operator <<(std::ostream & stream, const LocalMaterialDamage & _this)
  return stream;

However, the user still needs to register the material parameters that should be printed out. The registration is done during the call of the constructor. Like all definitions the implementation of the constructor has to be written in the file. However, the declaration has to be provided in the material_XXX.hh file:

class LocalMaterialDamage : public Material {
  /* -------------------------------------------------------------------- */
  /* Constructors/Destructors                                             */
  /* -------------------------------------------------------------------- */

  LocalMaterialDamage(SolidMechanicsModel & model, const ID & id = "");

The user can now define the implementation of the constructor in the file:

/* ---------------------------------------------------------------------- */
#include "local_material_damage.hh"
#include "solid_mechanics_model.hh"

namespace akantu {

/* ---------------------------------------------------------------------- */
LocalMaterialDamage::LocalMaterialDamage(SolidMechanicsModel & model,
           const ID & id)  :
  Material(model, id),
  damage("damage", *this) {

  this->registerParam("E", E, 0., _pat_parsable, "Young's modulus");
  this->registerParam("nu", nu, 0.5, _pat_parsable, "Poisson's ratio");
  this->registerParam("lambda", lambda, _pat_readable, "First Lame coefficient");
  this->registerParam("mu", mu, _pat_readable, "Second Lame coefficient");
  this->registerParam("kapa", kpa, _pat_readable, "Bulk coefficient");
  this->registerParam("Yd", Yd,   50., _pat_parsmod);
  this->registerParam("Sd", Sd, 5000., _pat_parsmod);



During the intializer list the reference to the model and the material id are assigned and the constructor of the internal field is called. Inside the scope of the constructor the internal values have to be initialized and the parameters, that should be printed out, are registered with the function: registerParam:

void registerParam(name of the parameter (key in the material file),
       member variable,
       default value (optional parameter),
       access permissions,

The available access permissions are as follows: - _pat_internal: Parameter can only be output when the material is printed. - _pat_writable: User can write into the parameter. The parameter is output when the material is printed. - _pat_readable: User can read the parameter. The parameter is output when the material is printed. - _pat_modifiable: Parameter is writable and readable. - _pat_parsable: Parameter can be parsed, i.e. read from the input file. - _pat_parsmod: Parameter is modifiable and parsable.

In order to implement the new constitutive law the user needs to specify how the additional material parameters, that are not defined in the input material file, should be calculated. Furthermore, it has to be defined how stresses and the stable time step should be computed for the new local material. In the case of implicit simulations, in addition, the computation of the tangent stiffness needs to be defined. Therefore, the user needs to redefine the following functions of the parent material:

void initMaterial();

// for explicit and implicit simulations void
computeStress(ElementType el_type, GhostType ghost_type = _not_ghost);

// for implicit simulations
void computeTangentStiffness(const ElementType & el_type,
           Array<Real> & tangent_matrix,
           GhostType ghost_type = _not_ghost);

// for explicit and implicit simulations
Real getStableTimeStep(Real h, const Element & element);

In the following a detailed description of these functions is provided:

  • initMaterial: This method is called after the material file is fully read and the elements corresponding to each material are assigned. Some of the frequently used constant parameters are calculated in this method. For example, the Lam'{e} constants of elastic materials can be considered as such parameters.

  • computeStress: In this method, the stresses are computed based on the

    constitutive law as a function of the strains of the quadrature points. For example, the stresses for the elastic material are calculated based on the following formula:

    \[\mat{\sigma } =\lambda\mathrm{tr}(\mat{\varepsilon})\mat{I}+2 \mu \mat{\varepsilon}\]

    Therefore, this method contains a loop on all quadrature points assigned to the material using the two macros: MATERIAL_STRESS_QUADRATURE_POINT_LOOP_BEGIN and MATERIAL_STRESS_QUADRATURE_POINT_LOOP_END

    // sigma <- f(grad_u)

    The strain vector in Akantu contains the values of \(\nabla \vec{u}\), i.e. it is really the displacement gradient,

  • computeTangentStiffness: This method is called when the tangent to the

    stress-strain curve is desired (see Fig ref {fig:smm:AL:K}). For example, it is called in the implicit solver when the stiffness matrix for the regular elements is assembled based on the following formula:

    \[\label{eqn:smm:constitutive_elasc} \mat{K } =\int{\mat{B^T}\mat{D(\varepsilon)}\mat{B}}\]

    Therefore, in this method, the tangent matrix (mat{D}) is computed for a given strain.

    The tangent matrix is a \(4^{th}\) order tensor which is stored as a matrix in Voigt notation.


    Fig. 16 Tangent to the stress-strain curve.

  • getCelerity: The stability criterion of the explicit integration scheme depend on the fastest wave celerity~eqref{eqn:smm:explicit:stabletime}. This celerity depend on the material, and therefore the value of this velocity should be defined in this method for each new material. By default, the fastest wave speed is the compressive wave whose celerity can be defined in getPushWaveSpeed.

Once the declaration and implementation of the new material has been completed, this material can be used in the user’s example by including the header file:

#include "material_XXX.hh"

For existing materials, as mentioned in Section~ref{sect:smm:CL}, by default, the materials are initialized inside the method initFull. If a local material should be used instead, the initialization of the material has to be postponed until the local material is registered in the model. Therefore, the model is initialized with the boolean for skipping the material initialization equal to true:

/// model initialization
model.initFull(_analysis_method = _explicit_lumped_mass);

Once the model has been initialized, the local material needs to be registered in the model:


Only at this point the material can be initialized:


A full example for adding a new damage law can be found in examples/new_material.

Adding a New Non-Local Constitutive Law

In order to add a new non-local material we first have to add the local constitutive law in Akantu (see above). We can then add the non-local version of the constitutive law by adding the two files (material_XXX_non_local.hh and where XXX is the name of the corresponding local material. The new law must inherit from the two classes, non-local parent class, such as the MaterialNonLocal class, and from the local version of the constitutive law, i.e. MaterialXXX. It is therefore necessary to include the interface of those classes in the header file of your custom material and indicate the inheritance in the declaration of the class:

/* ---------------------------------------------------------------------- */
#include "material_non_local.hh" // the non-local parent
#include "material_XXX.hh"
/* ---------------------------------------------------------------------- */


namespace akantu {

class MaterialXXXNonLocal : public MaterialXXX,
                            public MaterialNonLocal {

/// declare here the interface of your material


As members of the class we only need to add the internal fields to store the non-local quantities, which are obtained from the averaging process:

/* -------------------------------------------------------------------------- */
/* Class members                                                              */
/* -------------------------------------------------------------------------- */
  InternalField<Real> grad_u_nl;

The following four functions need to be implemented in the non-local material:

/// initialization of the material
void initMaterial();
/// loop over all element and invoke stress computation
virtual void computeNonLocalStresses(GhostType ghost_type);
/// compute stresses after local quantities have been averaged
virtual void computeNonLocalStress(ElementType el_type, GhostType ghost_type)
/// compute all local quantities
void computeStress(ElementType el_type, GhostType ghost_type);

In the intialization of the non-local material we need to register the local quantity for the averaging process. In our example the internal field grad_u_nl is the non-local counterpart of the gradient of the displacement field (grad_u_nl):

void MaterialXXXNonLocal::initMaterial() {
  /// register the non-local variable in the manager
    spatial_dimension * spatial_dimension);

The function to register the non-local variable takes as parameters the name of the local internal field, the name of the non-local counterpart and the number of components of the field we want to average. In the computeStress we now need to compute all the quantities we want to average. We can then write a loop for the stress computation in the function computeNonLocalStresses and then provide the constitutive law on each integration point in the function computeNonLocalStress.