Diffusion akantu (bugfixes/27-bug-in-the-python-interface) Browse

27-bug-in-the…

manual-solidmechanicsmodel.tex
View Options

			\chapter{Solid Mechanics Model\index{SolidMechanicsModel}\label{sect:smm}}

			The solid mechanics model is a specific implementation of the
			\code{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 \code{FEEngine} object to compute the interpolation,
			gradient, integration and assembly operations. A
			\code{SolidMechanicsModel} object can simply be created like this:
			\begin{cpp}
			SolidMechanicsModel model(mesh);
			\end{cpp}
			where \code{mesh} is the mesh for which the equations are to be
			solved. A second parameter called \code{spatial\_dimension} can be
			added after \code{mesh} if the spatial dimension of the problem is
			different than that of the mesh.

			This model contains at least the the following six \code{Arrays}:
			\begin{description}
			\item[blocked\_dofs] 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
			\textbf{blocked\_dofs} value of a degree of freedom to \code{true}.
			A Neumann boundary condition can be applied by setting the
			\textbf{blocked\_dofs} value of a degree of freedom to \code{false}.
			The \textbf{displacement}, \textbf{velocity} and
			\textbf{acceleration} are computed for all degrees of freedom for
			which the \textbf{blocked\_dofs} value is set to \code{false}. For
			the remaining degrees of freedom, the imposed values (zero by
			default after initialization) are kept.
			\item[displacement] 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).
			\item[velocity] contains the velocities of all degrees of freedom. As
			\textbf{displacement}, it contains computed or imposed velocities
			depending on the nature of the degrees of freedom ($\dot{\vec{u}}$
			in the following).
			\item[acceleration] contains the accelerations of all degrees of
			freedom. As \textbf{displacement}, it contains computed or imposed
			accelerations depending on the nature of the degrees of freedom
			($\ddot{\vec{u}}$ in the following).
			\item[force] contains the external forces applied on the nodes
			($\vec{f}_{\st{ext}}$ in the following).
			\item[residual] contains the difference between external and internal
			forces. On blocked degrees of freedom, \textbf{residual} contains
			the support reactions. ($\vec{r}$ in the following). It should be
			mentioned that at equilibrium \textbf{residual} should be zero on
			free degrees of freedom.
			\end{description}

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

			\section{Model Setup}


			\subsection{Setting Initial Conditions \label{sect:smm:initial_condition}}

			For a unique solution of the equations of motion, initial
			displacements and velocities for all degrees of freedom must be
			specified:
			\begin{eqnarray}
			\vec{u}(t=0) = \vec{u}_0\\
			\dot{\vec u}(t=0) =\vec{v}_0
			\end{eqnarray} The solid mechanics model can be initialized as
			follows:
			\begin{cpp}
			model.initFull()
			\end{cpp}
			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.
			\begin{cpp}
			Array<Real> & disp = model.getDisplacement();
			Array<Real> & velo = model.getVelocity();
			for (UInt i = 0; i < mesh.getNbNodes(); ++i) {
			disp(i, 0) = 0.1;
			velo(i, 1) = 1.;
			}
			\end{cpp}

			\subsection{Setting Boundary Conditions\label{sect:smm:boundary}}
			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.~\ref{fig:smm:boundaries}):
			\begin{equation}
			\vec{u} = \bar{\vec u} \quad \forall \vec{x}\in
			\Gamma_{u}
			\end{equation}
			A Neumann boundary condition imposes the value of the gradient of the
			solution at the boundary $\Gamma_t$ of the problem domain
			(Fig.~\ref{fig:smm:boundaries}):
			\begin{equation}
			\vec{t} = \mat{\sigma} \vec{n} = \bar{\vec t} \quad
			\forall \vec{x}\in \Gamma_{t}
			\end{equation}

			\begin{figure} \centering
			\def\svgwidth{0.5\columnwidth}
			\input{figures/problemDomain.pdf_tex}
			\caption{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.\label{fig:smm:boundaries}}
			\label{fig:problemDomain}
			\end{figure}

			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. Figure~\ref{fig:smm:dirichlet_bc} 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 as shown in the following code:

			\begin{cpp}
			Array<bool> & blocked = model.getBlockedDOFs();
			const Array<Real> & pos = mesh.getNodes();

			UInt nb_nodes = mesh.getNbNodes();

			for (UInt i = 0; i < nb_nodes; ++i) {
			if(Math::are_float_equal(pos(i, 0), 0)) {
			blocked(i, 0) = true; //block displacement in x-direction
			blocked(i, 1) = true; //block displacement in y-direction
			disp(i, 0) = 0.; //fixed displacement in x-direction
			disp(i, 1)= 0.; //fixed displacement in y-direction
			}
			}
			\end{cpp}

			\begin{figure}[!htb]
			\centering
			\includegraphics[scale=0.4]{figures/dirichlet}
			\caption{Beam with fixed support.\label{fig:smm:dirichlet_bc}}
			\end{figure}

			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 \code{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 \code{tag\_0}, \code{tag\_1} or
			\code{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
			\code{physical\_names} to the function
			\code{createGroupsFromMeshData}. Boundary conditions can also be
			created from the geometry by calling
			\code{createBoundaryGroupFromGeometry}. This function gathers all the
			elements on the boundary of the geometry.

			To apply the required boundary conditions, the function \code{applyBC}
			needs to be called on a \code{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: \code{FlagOnly, FixedValue,}
			and \code{IncrementValue}. The functor \code{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 \code{FixedValue}
			functor is used when a displacement value is applied in a fixed
			direction. The \code{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 file:

			\begin{cpp}
			mesh.createGroupsFromMeshData<std::string>("physical_names");

			model.applyBC(BC::Dirichlet::FixedValue(13.0, BC::_y), "Top");

			model.applyBC(BC::Dirichlet::FlagOnly(BC::_x), "Bottom");

			model.applyBC(BC::Dirichlet::IncrementValue(13.0, BC::_x), "Side");
			\end{cpp}

			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 \code{FromTraction} of Neumann boundary
			conditions is called. Otherwise, the functor \code{FromStress} should
			be called which gets the stress tensor as an input parameter.

			\begin{cpp}
			Array<Real> surface_traction(3);
			surface_traction(0)=0.0;
			surface_traction(1)=0.0;
			surface_traction(2)=-1.0;

			Matrix<Real> surface_stress(3, 3, 0.0);
			surface_stress(0,0)=0.0;
			surface_stress(1,1)=0.0;
			surface_stress(2,2)=-1.0;

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

			model.applyBC(BC::Neumann::FromStress(surface_stress), "Top");
			\end{cpp}

			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.

			\begin{cpp}
			model.applyBC(BC::Neumann::FreeBoundary(), "Side");
			\end{cpp}

			User specified functors can also be implemented. A full example for
			setting both initial and boundary conditions can be found in
			\shellcode{\examplesdir/boundary\_conditions.cc}. The problem solved
			in this example is shown in Fig.~\ref{fig:smm:bc_and_ic}. 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.
			\begin{figure}[!htb]
			\centering
			\includegraphics[scale=0.8]{figures/bc_and_ic_example}
			\caption{Plate on movable supports.\label{fig:smm:bc_and_ic}}
			\end{figure}

			\subsection{Material Selector\label{sect:smm:materialselector}}

			If the user wants to assign different materials to the different
			finite elements of choice 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. \code{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.

			\begin{cpp}
			MeshDataMaterialSelector<std::string> * mat_selector;
			mat_selector = new MeshDataMaterialSelector<std::string>("physical_names", model);
			model.setMaterialSelector(*mat_selector);
			\end{cpp}

			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:

			\begin{cpp}
			MeshDataMaterialSelector<UInt> * mat_selector;
			mat_selector = new MeshDataMaterialSelector<UInt>("tag_1", model);
			model.setMaterialSelector(*mat_selector);
			\end{cpp}

			where \code{tag\_1} of the mesh file is used as the classifier index
			and the elements that have index value equal to one will be assigned
			to the second material in the material file.

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

			For cohesive material, \akantu has a pre-defined material selector to assign
			the first cohesive material by default to the cohesive elements which is called
			\code{DefaultMaterialCohesiveSelector} and it inherits its properties from
			\code{DefaultMaterialSelector}. Multiple cohesive materials can be assigned
			using mesh data information (for more details, see \ref{intrinsic_insertion}).

			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.

			% An application of \code{DefaultMaterialCohesiveSelector} and usage in
			% a customly generated material selector class can be seen in
			% \shellcode{\examplesdir/cohesive\_element/cohesive\_extrinsic\_IG\_TG/cohesive\_extrinsic\_IG\_TG.cc}.

			\IfFileExists{manual-cohesive_elements_insertion.tex}{\input{manual-cohesive_elements_insertion}}{}

			\section{Static Analysis\label{sect:smm:static}}

			The \code{SolidMechanicsModel} class can handle different analysis
			methods, the first one being presented is the static case. In this
			case, the equation to solve is
			\begin{equation}
			\label{eqn:smm:static} \mat{K} \vec{u} =
			\vec{f}_{\st{ext}}
			\end{equation}
			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
			\code{SolidMechanicsModel}\index{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
			\code{SolidMechanicsModel} is obtained, the easiest way to initialize
			it is to use the \code{initFull}\index{SolidMechanicsModel!initFull}
			method by giving the \code{SolidMechanicsModelOptions}. These options
			specify the type of analysis to be performed and whether the materials
			should be initialized or not.
			\begin{cpp}
			SolidMechanicsModel model(mesh);
			model.initFull(SolidMechanicsModelOptions(_static));
			\end{cpp}
			Here, a static analysis is chosen by passing the argument
			\code{\_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 \code{initFull}. The method \code{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~\ref{sect:smm:boundary}. 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
			\code{solveStep}\index{SolidMechanicsModel!solveStep} can be called:
			\begin{cpp}
			model.solveStep<_scm_newton_raphson_tangent_modified, _scc_residual>(1e-4, 1);
			\end{cpp}
			This function is templated by the solving method and the convergence
			criterion and takes two arguments: the tolerance and the maximum
			number of iterations, which are $\num{1e-4}$ and $1$ for this example. The
			modified Newton-Raphson method is chosen to solve the system. In this
			method, the equilibrium equation (\ref{eqn:smm:static}) is modified in
			order to apply a Newton-Raphson convergence algorithm:
			\begin{align}\label{eqn:smm:static-newton-raphson}
			\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}~,\nonumber
			\end{align}
			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 \code{solveStep} method in the
			first step, the global stiffness matrix $\mat{K}$ from
			Equation~(\ref{eqn:smm:static}) 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 (\code{\_scc\_residual}), \ie
			$\|\|\vec{r}\|\| < \mbox{\code{\_scc\_residual}}$. One can also iterate
			until the increment of displacement is zero (\code{\_scc\_increment})
			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. $100$:
			\begin{cpp}
			model.solveStep<_scm_newton_raphson_tangent_modified,_scc_residual>(1e-4, 100)
			\end{cpp}
			At the end of the analysis, the final solution is stored in the
			\textbf{displacement} vector. A full example of how to solve a static
			problem is presented in the code \code{\examplesdir/static/static.cc}.
			This example is composed of a 2D plate of steel, blocked with rollers
			on the left and bottom sides as shown in Figure \ref{fig:smm:static}.
			The nodes from the right side of the sample are displaced by $0.01\%$
			of the length of the plate.

			\begin{figure}[!htb]
			\centering
			\includegraphics[scale=1.05]{figures/static}
			\caption{Numerical setup\label{fig:smm:static}}
			\end{figure}

			The results of this analysis is depicted in
			Figure~\ref{fig:smm:implicit:static_solution}.

			\begin{figure}[!htb]
			\centering
			\includegraphics[width=.7\linewidth]{figures/static_analysis}
			\caption{Solution of the static analysis. Left: the initial
			condition, right: the solution (deformation magnified 50 times)}
			\label{fig:smm:implicit:static_solution}
			\end{figure}

			\section{Dynamic Methods} \label{sect:smm: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:
			\begin{equation}
			\label{eqn:equation-motion}
			\mat{M}\ddot{\vec{u}} +
			\mat{C}\dot{\vec{u}} + \mat{K}\vec{u} = \vec{f}_{\st{ext}}~,
			\end{equation}
			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, (\ref{eqn:equation-motion}) becomes a
			system of three equations (see \cite{curnier92a} \cite{hughes-83a} for
			more details):
			\begin{align}
			\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}
			\label{eqn:equation-motion-discret} \\
			\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} \label{eqn:finite-difference-1}\\
			\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} \label{eqn:finite-difference-2}
			\end{align}

			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 equations
			(\ref{eqn:finite-difference-1}) and (\ref{eqn:finite-difference-2})
			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 $0 < \alpha <
			1/2$.

			\begin{center}
			\begin{tabular}{cll}
			\toprule
			$\alpha$ & Method ($\beta = 1/2$) & Type\\
			\midrule
			$0$ & central difference & explicit\\
			$1/6$ & Fox-Goodwin (royal road) &implicit\\
			$1/3$ & Linear acceleration &implicit\\
			$1/2$ & Average acceleration (trapezoidal rule)& implicit\\
			\bottomrule
			\end{tabular}
			\end{center}

			The solution of this system of equations,
			(\ref{eqn:equation-motion-discret})-(\ref{eqn:finite-difference-2}) 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:

			\begin{enumerate}
			\item \textit{Predictor:}
			\begin{align}
			\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{align}

			\item \textit{Solve:}
			\begin{align}
			\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{align}

			\item \textit{Corrector:}
			\begin{align}
			\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{align}
			\end{enumerate}

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

			\begin{center}
			\begin{tabular}{lcccc}
			\toprule
			& $\vec{w}$ & $e$ & $d$ & $c$\\
			\midrule
			in acceleration &$ \delta\ddot{\vec{u}}$ & $\alpha \beta\Delta t^2$ &$\beta \Delta t$ &$1$\\
			in velocity & $ \delta\dot{\vec{u}}$& $\frac{1}{\beta} \Delta t$ & $1$ & $\alpha\Delta t$\\
			in displacement &$\delta\vec{u}$ & $ 1$ & $\frac{1}{\alpha} \Delta t$ & $\frac{1}{\alpha \beta} \Delta t^2$\\
			\bottomrule
			\end{tabular}
			\end{center}

			%\note{If you want to use the implicit solver \akantu should be compiled at least with one sparse matrix solver such as Mumps\cite{mumps}.}


			\subsection{Implicit Time Integration}
			To solve a problem with an implicit time integration scheme, first a
			\code{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.

			\begin{cpp}
			SolidMechanicsModel model(mesh);
			model.initFull(SolidMechanicsModelOptions(_implicit_dynamic));
			/Boundary conditions see Section~%\ref{sect:smm:boundary}% /
			\end{cpp}
			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. \index{SolidMechanicsModel!setTimeStep}
			\begin{cpp}
			model.setTimeStep(time_step);
			\end{cpp}
			Since the system has to be solved for a given amount of time, the
			method \code{solveStep()}, (which has already been used in the static
			example in Section~\ref{sect:smm:static}), is called inside a time
			loop:
			\begin{cpp}
			/// time loop
			Real time = 0.;
			for (UInt s = 1; time <max_time; ++s, time += time_step) {
			model.solveStep<_scm_newton_raphson_tangent_modified,_scc_increment>(1e-12, 100);
			}
			\end{cpp}
			An example of solid mechanics with an implicit time integration scheme
			is presented in
			\shellcode{\examplesdir/implicit/implicit\_dynamic.cc}. This example
			consists of a 3D beam of
			$\SI{10}{\metre}\,\times\,\SI{1}{\metre}\,\times\,\SI{1}{\metre}$
			blocked on one side and is on a roller on the other side. A constant
			force of \SI{5}{\kilo\newton} is applied in its middle.
			Figure~\ref{fig:smm:implicit:dynamic} presents the geometry of this
			case. The material used is a fictitious linear elastic material with a
			density of \SI{1000}{\kilo\gram\per\cubic\metre}, a Young's Modulus of
			\SI{120}{\mega\pascal} 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:
			\begin{equation}
			\label{eqn:smm:implicit}
			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)
			\end{equation}

			\begin{figure}[!htb]
			\centering
			\includegraphics[scale=.6]{figures/implicit_dynamic}
			\caption{Numerical setup}
			\label{fig:smm:implicit:dynamic}
			\end{figure}

			Figure \ref{fig:smm:implicit:dynamic_solution} presents the deformed
			beam at 3 different times during the simulation: time steps 0, 1000 and
			2000.

			\begin{figure}[!htb]
			\centering
			\setlength{\unitlength}{0.1\textwidth}
			\begin{tikzpicture}
			\node[above right] (img) at (0,0)
			{\includegraphics[width=.6\linewidth]{figures/dynamic_analysis}};
			\node[left] at (0pt,20pt) {$0$}; \node[left] at (0pt,60pt) {$1000$};
			\node[left] at (0pt,100pt) {$2000$};
			\end{tikzpicture}

			\caption{Deformed beam at 3 different times (displacement are
			magnified by a factor 10).}
			\label{fig:smm:implicit:dynamic_solution}
			\end{figure}

			\subsection{Explicit Time Integration}
			\label{ssect:smm:expl-time-integr}

			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
			\code{SolidMechanicsModel} class. In the initialization, the explicit
			scheme is selected using the \code{\_explicit\_lumped\_mass} constant.

			\begin{cpp}
			SolidMechanicsModel model(mesh);
			model.initFull(SolidMechanicsModelOptions(_explicit_lumped_mass));
			\end{cpp}
			\index{SolidMechanicsModel!initFull}
			\note{Writing \code{model.initFull()} or \code{model.initFull(SolidMechanicsModelOptions());} is
			equivalent to use the \code{\_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 \textbf{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:

			\begin{cpp}
			critical_time_step = model.getStableTimeStep();
			\end{cpp} \index{SolidMechanicsModel!StableTimeStep}

			The stable time step corresponds to the time the fastest wave (the compressive
			wave) needs to travel the characteristic length of the mesh:
			\begin{equation}
			\label{eqn:smm:explicit:stabletime}
			\Delta t_{\st{crit}} = \frac{\Delta x}{c}
			\end{equation}
			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.

			\begin{cpp}
			const Real safety_time_factor = 0.8;
			Real applied_time_step = critical_time_step * safety_time_factor;
			model.setTimeStep(applied_time_step);
			\end{cpp}
			\index{SolidMechanicsModel!setTimeStep} 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$-\beta$ equations with $\beta=1/2$ and $\alpha=0$. In \akantu
			these computations at each time step are invoked by calling the
			function \code{solveStep}:
			\begin{cpp}
			for (UInt s = 1; (s-1)*applied_time_step < total_time; ++s) {
			model.solveStep();
			}
			\end{cpp} \index{SolidMechanicsModel!solveStep}
			The method
			\code{solveStep} wraps the four following functions:
			\begin{itemize}
			\item \code{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
			\code{model.explicitCorr()}. The equations are:
			\begin{align}
			\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}
			\label{eqn:smm:explicit:onehalfvelocity}
			\end{align}

			\item \code{model.updateResidual()} and
			\code{model.updateAcceleration()} compute the acceleration increment
			$\delta \vec{\ddot{u}}$:
			\begin{equation}
			\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}}_{n} - \mat{M} \vec{\ddot{u}}_{n}
			\end{equation}

			\note{The internal force $\vec{f}_{\st{int}\, n+1}$ is computed from
			the displacement $\vec{u}_{n+1}$ based on the constitutive law.}

			\item \code{model.explicitCorr()} computes the velocity and
			acceleration fields at $t+1$:
			\begin{align}
			\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{align}
			\end{itemize}

			The use of an explicit time integration scheme is illustrated by the
			example:\par
			\noindent \shellcode{\examplesdir/explicit/explicit\_dynamic.cc}\par
			\noindent 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
			Figure~\ref{fig:smm:explicit}.

			\begin{figure}[!htb] \centering
			\begin{tikzpicture}
			\coordinate (c) at (0,2);
			\draw[shift={(c)},thick, color=blue] plot [id=x, domain=-5:5, samples=50] ({\x, {(40 * sin(0.1pi3\x) exp(- (0.1pi3\x)(0.1pi3*\x) / 4))}});
			\draw[shift={(c)},-latex] (-6,0) -- (6,0) node[right, below] {$x$};
			\draw[shift={(c)},-latex] (0,-0.7) -- (0,1) node[right] {$u$};
			\draw[shift={(c)}] (-0.1,0.6) node[left] {$A$}-- (1.5,0.6);

			\coordinate (l) at (0,0.6);
			\draw[shift={(0,-0.7)}] (-5, 0) -- (5,0) -- (5, 1) -- (-5, 1) -- cycle;
			\draw[shift={(l)}, latex-latex] (-5,0)-- (5,0) node [midway, above] {$L$};
			\draw[shift={(l)}] (5,0.2)-- (5,-0.2);
			\draw[shift={(l)}] (-5,0.2)-- (-5,-0.2);

			\coordinate (h) at (5.3,-0.7);
			\draw[shift={(h)}, latex-latex] (0,0)-- (0,1) node [midway, right] {$h$};
			\draw[shift={(h)}] (-0.2,1)-- (0.2,1);
			\draw[shift={(h)}] (-0.2,0)-- (0.2,0);
			\end{tikzpicture}

			\caption{Numerical setup \label{fig:smm:explicit}}
			\end{figure}

			The length and height of the beam are $L=\SI{10}{\metre}$ and
			$h = \SI{1}{\metre}$, respectively. The material is linear elastic,
			homogeneous and isotropic (density:
			\SI{7800}{\kilo\gram\per\cubic\metre}, Young's modulus:
			\SI{210}{\giga\pascal} and Poisson's ratio: $0.3$). The imposed
			displacement follow a Gaussian function with a maximum amplitude of $A = \SI{0.01}{\meter}$. The
			potential, kinetic and total energies are computed. The safety factor
			is equal to $0.8$.

			\input{manual-constitutive-laws}

			\section{Adding a New Constitutive Law}\index{Material!create a new
			material}

			There are several constitutive laws in \akantu as described in the
			previous Section~\ref{sect:smm:CL}. 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 (\code {material\_XXX.hh} and \code{material\_XXX.cc}) have
			to be provided where \code{XXX} is the name of the new material. The
			header file \code {material\_XXX.hh} defines the interface of your
			custom material. Its implementation is provided in the
			\code{material\_XXX.cc}. The new law must inherit from the
			\code{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:
			\begin{cpp}
			/* ---------------------------------------------------------------------- */
			#include "material.hh"
			/* ---------------------------------------------------------------------- */

			#ifndef __AKANTU_MATERIAL_XXX_HH__
			#define __AKANTU_MATERIAL_XXX_HH__

			__BEGIN_AKANTU__

			class MaterialXXX : public Material {

			/// declare here the interface of your material

			};
			\end{cpp}
			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 Lam\'{e} coefficients and its
			bulk modulus. Furthermore, the user has to add a new internal variable
			\code{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:
			\begin{cpp}
			class LocalMaterialDamage : public Material {

			/// declare constructors/destructors here

			/// declare methods and accessors here

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

			AKANTU_GET_MACRO_BY_ELEMENT_TYPE_CONST(Damage, damage, Real);
			private:

			/// 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;

			};
			\end{cpp}
			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:
			\begin{cpp}
			for (UInt m = 0; m < model.getNbMaterials(); ++m)
			std::cout << model.getMaterial(m) << std::endl;
			\end{cpp}
			the standard output stream operator has to be redefined. This should be done at the end of the header file:
			\begin{cpp}
			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)
			{
			_this.printself(stream);
			return stream;
			}
			\end{cpp}
			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 \code{material\_XXX.cc}
			file. However, the declaration has to be provided in the
			\code{material\_XXX.hh} file:
			\begin{cpp}
			class LocalMaterialDamage : public Material {
			/* -------------------------------------------------------------------- */
			/* Constructors/Destructors */
			/* -------------------------------------------------------------------- */
			public:

			LocalMaterialDamage(SolidMechanicsModel & model, const ID & id = "");
			};
			\end{cpp}
			The user can now define the implementation of the constructor in the
			\code{material\_XXX.cc} file:
			\begin{cpp}
			/* ---------------------------------------------------------------------- */
			#include "local_material_damage.hh"
			#include "solid_mechanics_model.hh"

			__BEGIN_AKANTU__

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

			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);

			damage.initialize(1);

			AKANTU_DEBUG_OUT();
			}
			\end{cpp}
			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:
			\code{registerParam}\index{Material!registerParam}:
			\begin{cpp}
			void registerParam(name of the parameter (key in the material file),
			member variable,
			default value (optional parameter),
			access permissions,
			description);
			\end{cpp}
			The available access permissions are as follows:
			\begin{itemize}
			\item \code{\_pat\_internal}: Parameter can only be output when the material is printed.
			\item \code{\_pat\_writable}: User can write into the parameter. The parameter is output when the material is printed.
			\item \code{\_pat\_readable}: User can read the parameter. The parameter is output when the material is printed.
			\item \code{\_pat\_modifiable}: Parameter is writable and readable.
			\item \code{\_pat\_parsable}: Parameter can be parsed, \textit{i.e.} read from the input file.
			\item \code{\_pat\_parsmod}: Parameter is modifiable and parsable.
			\end{itemize}

			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:
			\begin{cpp}
			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);
			\end{cpp}
			In the following a detailed description of these functions is provided:
			\begin{itemize}

			\item \code{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.

			\item \code{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:
			\begin{equation}
			\label{eqn:smm:constitutive_elastic}
			\mat{\sigma } =\lambda\mathrm{tr}(\mat{\varepsilon})\mat{I}+2 \mu \mat{\varepsilon}
			\end{equation}

			Therefore, this method contains a loop on all quadrature points
			assigned to the material using the two macros:\par
			\code{MATERIAL\_STRESS\_QUADRATURE\_POINT\_LOOP\_BEGIN}\par
			\code{MATERIAL\_STRESS\_QUADRATURE\_POINT\_LOOP\_END}

			\begin{cpp}
			MATERIAL_STRESS_QUADRATURE_POINT_LOOP_BEGIN(element_type);

			// sigma <- f(grad_u)

			MATERIAL_STRESS_QUADRATURE_POINT_LOOP_END;
			\end{cpp}

			\note{The strain vector in \akantu contains the values of $\nabla
			\vec{u}$, i.e. it is really the \emph{displacement gradient},}

			\item \code{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:
			\begin{equation}
			\label{eqn:smm:constitutive_elasc} \mat{K }
			=\int{\mat{B^T}\mat{D(\varepsilon)}\mat{B}}
			\end{equation}

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

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

			\begin{figure}[!htb]
			\begin{center}
			\includegraphics[width=0.4\textwidth,keepaspectratio=true]{figures/tangent.pdf}
			\caption{Tangent to the stress-strain curve.}
			\label{fig:smm:AL:K}
			\end{center}
			\end{figure}

			\item \code{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~\code{getPushWaveSpeed}.
			\end{itemize}
			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:
			\begin{cpp}
			#include "material_XXX.hh"
			\end{cpp}
			For existing materials, as mentioned in Section~\ref{sect:smm:CL}, by
			default, the materials are initialized inside the method
			\code{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:
			\begin{cpp}
			/// model initialization
			model.initFull(SolidMechanicsModelOptions(_explicit_lumped_mass,true));
			\end{cpp}
			Once the model has been initialized, the local material needs
			to be registered in the model:
			\begin{cpp}
			model.registerNewCustomMaterials<XXX>("name_of_local_material");
			\end{cpp}
			Only at this point the material can be initialized:
			\begin{cpp}
			model.initMaterials();
			\end{cpp}
			A full example for adding a new damage law can be found in
			\shellcode{\examplesdir/new\_material}.

			%%% Local Variables: %%% mode: latex %%% TeX-master: "manual" %%% End:

rAKA/doc/manual/manual-solidmechanicsmodel.tex72e4960f4c2cbugfixes/27-bug-in-the…

manual-solidmechanicsmodel.texView Options

rAKA/doc/manual/manual-solidmechanicsmodel.tex
72e4960f4c2cbugfixes/27-bug-in-the…

manual-solidmechanicsmodel.tex
View Options