1 files changed, 143 insertions, 0 deletions
diff --git a/CHAPTERS/chap3/chapter3.tex b/CHAPTERS/chap3/chapter3.tex
new file mode 100644
index 0000000..9b400e8
--- /dev/null
+++ b/CHAPTERS/chap3/chapter3.tex
@@ -0,0 +1,143 @@
+\chapter{Importing Mesh From Third Party Software in OpenFOAM}
+\thispagestyle{empty}
+\label{sec:chap3}
+\newcommand{\LocCHthreefig}{\Origin/CHAPTERS/chap3/figures}
+
+OpenFOAM can be used for creating and meshing geometrical shapes like Box, Pipe. When dealing with complex geometries like a turbine blade, aircraft,
+ship etc, we cannot use the blockMesh utility. In such cases it is always better to create the geometry and mesh in dedicated CAD and Meshing softwares 
+and solve those usiing OpenFOAM. As a prerequisite it is expected the user should have knowledge about creating geometry and generating mesh in softwares
+like Gmabit, Gmsh, Salome, ICEM etc. This chapter deals with the steps involved in importing mesh files in OpenFOAM using different mesh conversion tools.
+
+\section{Geometry}
+
+We will use the above problem of Flow over a square cylinder as an example for importing mesh file in OpenFOAM. Here we have a square cylinder
+of length 1m and height 1 m. Inlet velocity is set at 1 $\frac{m}{s}$ for Reynolds number (Re) 100. The size of the domain choosen is 60 m by 40 m.
+The boundary conditions are as shown in the , Fig \ref{square} below.
+
+\begin{figure}[t]  
+\centering  
+\includegraphics[width=\lgfig]{\LocCHthreefig/square.png}
+\caption{Flow over square Cylinder}
+\label{square}  
+\end{figure}
+
+\section{Meshing}
+
+We have generated a hexhedral mesh for the above geometry with 40000 cells and saved the mesh file as cylmesh.msh. 
+The mesh generated is as shown below, Fig \ref{mesh} 
+
+\begin{figure}[h]  
+\centering
+\includegraphics[width=\lgfig]{\LocCHthreefig/cylmesh.jpeg}
+\caption{Mesh}
+\label{mesh}
+  
+\end{figure}
+
+\section{Importing the mesh file}
+
+In incompressibel solvers go to icoFoam and create a solver inside it by the name \textbf{cylinder}. Now go inside the cavity case and copy the 
+\begin{itemize}
+\item 0
+\item system
+\end{itemize}
+
+\flushleft folder and paste it inside the cylinder folder. Please make a not here that we do not need the \textbf{constant} folder here. After this copy the 
+cylmesh.msh mesh file create earlier and paste this inside this folder. Thus the our case file is now ready. Now open the command terminal and type the
+path for the cylinder folder. Now since we have a Fluent (.msh) mesh file we will use the mesh conversion command as shown below followed by the file name \\
+\centering \textbf{fluentMeshToFoam file-name.msh} \newline
+
+\flushleft In the terminal window type the above command with the file name and press enter.
+
+\begin{figure}[h]  
+\centering
+\includegraphics[width=\lgfig]{\LocCHthreefig/conversion.png}
+\caption{convert}
+\label{mesh}
+\end{figure}
+
+\flushleft In case you have a 3D mesh file then you can use the command \\ \vspace{0.5cm}
+\centering {\textbf{fluent3DMeshToFoam file-name.msh}} \newline
+
+\flushleft The Fluent mesh file is converted into OpenFOAM mesh file. Now if we look back into our cylinder folder we can see that the "constant"
+folder is now generated. When we open the constant folder we will see that the transport properties file is missing. Since we had converted the 
+fluent mesh file into openfoam the fluid property files were missing. Copy the transport property file from the constant folder of cavity case
+and paste this inside the constant folder of cylinder. The trasnportProperties file contains the value of fluid viscosity, we can either change it
+or keep it default. \newline
+
+\flushleft Make a note here that we do not use the \textbf{blockMesh} command here
+
+\section{Boundary Conditions}
+
+When we import the geometry in OpenFOAM we need to be very careful with the boudnary names used while creating the mesh file. Since OpenFOAM is case
+sensitive in case of any mistake with the boundary names can create an error while running the solver. To view the boundary names in the command terminal
+go to polyMesh folder inside the constant. Inside polyMesh you can see a file by the name \textbf{boundary}. Open this file in any editor of your
+choice, eg, gedit boundary, Fig \ref{boundary}.
+
+\begin{figure}[h]  
+\centering
+\includegraphics[width=\lgfig]{\LocCHthreefig/boundary.png}
+\caption{Boundary file}
+\label{boundary}
+\end{figure}
+
+\flushleft The boundary names will be as shown in the domain shown above, Fig \ref{square}. In case of any error with the boundary names you can
+always refer to this boundary file. Now in your command terminal go to the 0 folder and open the pressure file. Make sure that the boundary names 
+match exactly the names in the boundary file, in case of errors make the necessary changes.
+
+\section{Solver settings}
+
+In the terminal window go to the controlDict file inside system and open it in any editor of your choice. Change the endTime from 0.5 to 1.5 seconds.
+Save the file and close it, Fig \ref{cd} and come back to the cylinder folder.
+
+\begin{figure}[h]  
+\centering
+\includegraphics[width=\lgfig]{\LocCHthreefig/controldict.png}
+\caption{controlDict file}
+\label{cd}
+\end{figure}
+
+\flushleft After making the necessary changes we can now run the solver. In the temrinal window type the name of the solver \textbf{icoFoam}
+and press enter. The iterations will be seen running on the terminal window. After the iterations stop we can now start with the visualization.
+
+\section{Post-Processing}
+
+Launch paraview by typing \textbf{paraFoam} in the terminal window and once it opens click on the Apply button to view the geometry, Fig \ref{geom}.
+In the active varialble control menu change from Solid Color to Velocity (U). You can now see the initial conditions for velocity, Fig \ref{vel}.
+To view the animation on the right hand top of paraview click on the play button of VCR menu. You can see the change in velocity in the paraview 
+window with the passage of time, Fig \ref {vel-1}.
+
+\begin{figure}[h]  
+\centering
+\includegraphics[width=\lgfig]{\LocCHthreefig/geom-paraview.png}
+\caption{Geometry in Paraview}
+\label{geom}
+\end{figure}
+
+\begin{figure}[h]  
+\centering
+\includegraphics[width=\lgfig]{\LocCHthreefig/vel.png}
+\caption{Initial velocity condition}
+\label{vel}
+\end{figure}
+
+\begin{figure}[h]  
+\centering
+\includegraphics[width=\lgfig]{\LocCHthreefig/vel-1.png}
+\caption{Velocity at 1 sec}
+\label{vel-1}
+\end{figure}
+
+\section{Mesh Conversion Commands}
+
+The user can also import mesh files from other meshing softwares as well. Here is a list of commands to import mesh files in OpenFOAM.
+
+\begin{itemize}
+\item ANSYS : ansysToFoam file-name
+\item IDEAS : ideasToFoam file-name
+\item CFX : cfxToFoam file-name
+\item SALOME : ideasUnvToFoam file-name
+\end{itemize}
+
+
+