Homec4science
Diffusion akantu (features/28-getelementinradius-const-element-element-in-feengine-returns-always-0) Browse

rAKA/doc/manual/manual-structuralmechanicsmodel.tex
50d8507655b0features/28-getelementi…

Last Change
Raw File

manual-structuralmechanicsmodel.tex
View Options

\chapter{Structural Mechanics Model}
Static structural mechanics problems can be handled using the
class \code{StructuralMechanicsModel}. So far, \akantu provides 2D and 3D
Bernoulli beam elements \cite{frey2009}. This model is instantiated for a given
\code{Mesh}, as for the \code{SolidMechanicsModel}. The model will create its own \code{FEEngine} object to
compute the interpolation, gradient, integration and assembly
operations. The \code{StructuralMechanicsModel} constructor is called
in the following way:
\begin{cpp}
StructuralMechanicsModel model(mesh, spatial_dimension);
\end{cpp}
where \code{mesh} is a \code{Mesh} object defining the structure for
which the equations of statics are to be solved, and
\code{spatial\_dimension} is the dimensionality of the problem. If
\code{spatial\_dimension} is omitted, the problem is assumed to have
the same dimensionality as the one specified by the mesh.
\note[\ 1]{Dynamic computations are not supported to date.}
\note[\ 2]{Structural meshes are created and loaded as described in
Section~\ref{sect:common:mesh} with \code{MeshIOMSHStruct} instead of \code{MeshIOMSH}:}
\begin{cpp}
akantu::MeshIOMSHStruct mesh_io;
mesh_io.read("structural_mesh.msh", beams);
\end{cpp}
\vspace{1cm}
This model contains at least the following \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}. The \textbf{displacement} is 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\_rotation] contains the generalized displacements
(\textit{i.e.} displacements and rotations) 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[force\_moment] contains the generalized external forces (forces
and moments) applied to the nodes ($\vec{f_{\st{ext}}}$ in the
following).
\item[residual] contains the difference between the generalized external and internal
forces and moments. On the 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 the free degrees of freedom.
\end{description}
An example to help understand how to use this model will be presented in the
next section.
\section{Model Setup}
\label{sec:structMechMod:setup}
\subsection{Initialization}
The easiest way to initialize the structural mechanics model is:
\begin{cpp}
model.initFull();
\end{cpp}
The method \code{initFull} computes the shape functions, initializes
the internal vectors mentioned above and allocates the memory for the
stiffness matrix, unlike the solid mechanics model, its default argument is \code{\_static}.
Material properties are defined using the \code{StructuralMaterial}
structure described in
Table~\ref{tab:structMechMod:strucMaterial}. Such a definition could,
for instance, look like
\begin{cpp}
StructuralMaterial mat1;
mat.E=3e10;
mat.I=0.0025;
mat.A=0.01;
\end{cpp}
\begin{table}[htb] \centering
\begin{tabular}{cl}
\toprule
Field & Description \\
\midrule
\code{E} & Young's modulus \\
\code{A} & Cross section area \\
\code{I} & Second cross sectional moment of inertia (for 2D elements)\\
\code{Iy} & \code{I} around beam $y$--axis (for 3D elements)\\
\code{Iz} & \code{I} around beam $z$--axis (for 3D elements)\\
\code{GJ} & Polar moment of inertia of beam cross section (for 3D elements)\\
\bottomrule
\end{tabular}
\caption{Material properties for structural elements defined in
the class \code{StructuralMaterial}.}
\label{tab:structMechMod:strucMaterial}
\end{table}
Materials can be added to the model's \code{element\_material} vector using
\begin{cpp}
model.addMaterial(mat1);
\end{cpp}
They are successively numbered and then assigned to specific elements.
\begin{cpp}
for (UInt i = 0; i < nb_element_mat_1; ++i) {
model.getElementMaterial(_bernoulli_beam_2)(i,0) = 1;
}
\end{cpp}
\subsection{Setting Boundary Conditions}\label{sect:structMechMod:boundary}
As explained before, the Dirichlet boundary conditions are applied through the
array \textbf{blocked\_dofs}. Two options exist to define Neumann conditions.
If a nodal force is applied, it has to be directly set in the array
\textbf{force\_momentum}. For loads distributed along the beam length, the
method \code{computeForcesFromFunction} integrates them into nodal forces. The
method takes as input a function describing the distribution of loads along the
beam and a functor \code{BoundaryFunctionType} specifing if the function is
expressed in the local coordinates (\code{\_bft\_traction\_local}) or in the
global system of coordinates (\code{\_bft\_traction}).
\begin{cpp}
static void lin_load(double * position, double * load,
Real * normal, UInt surface_id){
memset(load,0,sizeof(Real)*3);
load[1] = position[0]*position[0]-250;
}
int main(int argc, char *argv[]){
...
model.computeForcesFromFunction<_bernoulli_beam_2>(lin_load,
_bft_traction_local);
...}
\end{cpp}
\section{Static Analysis\label{sect:structMechMod:static}}
The \code{StructuralMechanicsModel} class can perform static analyses
of structures. In this case, the equation to solve is the same as for
the \code{SolidMechanicsModel} used for static analyses
\begin{equation}\label{eqn:structMechMod:static}
\mat{K} \vec{u} = \vec{f_{\st{ext}}}~,
\end{equation}
where $\mat{K}$ is the global stiffness matrix, $\vec{u}$ the
generalized displacement vector and $\vec{f_{\st{ext}}}$ the vector of
generalized external forces applied to the system.
To solve such a problem, the static solver of the
\code{StructuralMechanicsModel}\index{StructuralMechanicsModel} object
is used. First a model has to be created and initialized.
\begin{cpp}
StructuralMechanicsModel model(mesh);
model.initFull();
\end{cpp}
\begin{itemize}
\item \code{model.initFull} initializes all internal vectors to zero.
\end{itemize}
Once the model is created and initialized, the boundary conditions can
be set as explained in Section~\ref{sect:structMechMod:boundary}.
Boundary conditions will prescribe the external forces or moments for
the free degrees of freedom $\vec{f_{\st{ext}}}$ and displacements or
rotations for the others. To completely define the system represented
by equation (\ref{eqn:structMechMod:static}), the global stiffness
matrix $\mat{K}$ must be assembled.
\index{StructuralMechanicsModel!assembleStiffnessMatrix}
\begin{cpp}
model.assembleStiffnessMatrix();
\end{cpp}
The computation of the static equilibrium is performed using the same
Newton-Raphson algorithm as described in
Section~\ref{sect:smm:static}.
\note{To date,
\code{StructuralMechanicsModel} handles only constitutively and
geometrically linear problems, the algorithm is therefore guaranteed
to converge in two iterations.}
\begin{cpp}
model.updateResidual();
model.solve();
\end{cpp}
\index{StructuralMechanicsModel!updateResidual}
\index{StructuralMechanicsModel!solve}
\begin{itemize}
\item \code{model.updateResidual} assembles the internal forces and
removes them from the external forces.
\item \code{model.solve} solves the Equation (\ref{eqn:structMechMod:static}).
The \textbf{increment} vector of the model will contain the new
increment of displacements, and the \textbf{displacement\_rotation}
vector is also updated to the new displacements.
\end{itemize}
%At the end of the analysis, the final solution is stored in the
%\textbf{displacement} vector. A full example of how to solve a
%structural mechanics problem is presented in the code
%\shellcode{\examplesdir/structural\_mechanics/test\_structural\_mechanics\_model\_bernoulli\_beam\_2\_exemple\_1\_1.cc}.
%This example is composed of a 2D beam, clamped at the left end and
%supported by two rollers as shown in Figure
%\ref{fig:structMechMod:exem1_1}. The problem is defined by the
%applied load $q=\SI{6}{\kilo\newton\per\metre}$, moment $\bar{M} =
%\SI{3.6}{\kilo\newton\metre}$, moments of inertia $I_1 =
%\SI{250\,000}{\power{\centi\metre}{4}}$ and $I_2 =
%\SI{128\,000}{\power{\centi\metre}{4}}$ and lengths $L_1 =
%\SI{10}{\metre}$ and $L_2 = \SI{8}{\metre}$. The resulting
%rotations at node two and three are $ \varphi_2 = 0.001\,167\
%\mbox{and}\ \varphi_3 = -0.000\,771.$
At the end of the analysis, the final solution is stored in the
\textbf{displacement\_rotation} vector. A full example of how to
solve a structural mechanics problem is presented in the code
\shellcode{\examplesdir/structural\_mechanics/bernoulli\_beam\_2\_example.cc}.
This example is composed of a 2D beam, clamped at the left end and
supported by two rollers as shown in Figure
\ref{fig:structMechMod:exem1_1}. The problem is defined by the
applied load $q=\SI{6}{\kilo\newton\per\metre}$, moment $\bar{M} =
\SI{3.6}{\kilo\newton\metre}$, moments of inertia $I_1 =
\SI{250\,000}{\centi\metre\tothe{4}}$ and $I_2 =
\SI{128\,000}{\centi\metre\tothe{4}}$ and lengths $L_1 =
\SI{10}{\metre}$ and $L_2 = \SI{8}{\metre}$. The resulting
rotations at node two and three are $ \varphi_2 = 0.001\,167\
\mbox{and}\ \varphi_3 = -0.000\,771.$
\begin{figure}[htb]
\centering
\includegraphics[scale=1.1]{figures/beam_example}
\caption{2D beam example}
\label{fig:structMechMod:exem1_1}
\end{figure}
%%% Local Variables:
%%% mode: latex
%%% TeX-master: "manual"
%%% End:
c4science · Help