OpenFOAM/C3/Importing-mesh-file-in-OpenFOAM/English

Visual Cue	Narration
Slide 1	Hello and welcome to the spoken tutorial on Importing Mesh files in OpenFOAM
Slide 2 : Learning Objectives	In this tutorial, you will learn how to: import Mesh files from a meshing software in OpenFOAM.
Slide 3  : Pre-requisite	As a pre-requisite, the user should know how to generate a Mesh in software like -Gambit, Ansys ICEM , CFX, Salome etc.
Slide 4: System Requirement	To record this tutorial I am using Linux Operating system Ubuntu version 12.04. OpenFOAM version 2.1.1 ParaView version 3.12.0
Slide 5:.	Using blockMesh, we can easily make simple geometries. For example- pipe, box, etc.
Narration, no visual cue	It is difficult to create complex geometries using blockMesh. But OpenFOAM supports importing mesh from third party meshing software.
	There are commands available in OpenFOAM, to import these mesh files. We will now learn how to import these files
Slide 7 : geometry for the case Point over the square cylinder point over its length and height point on inlet velocity	Here is the geometry of our case. We have a square cylinder length 1m and height 1m. Inlet velocity is 1 m/s We are solving this for a Reynolds Number (Re) = 100 The domain chosen is 40 by 60 The Boundary conditions are as shown in the diagram
Slide 8 :	This is the mesh file generated in a meshing software
Go to the OpenFOAM > xyz- 2.1.1>run>tutorials>incompressible >icoFoam	In your OpenFOAM working directory, go to the icoFoam solver and click on it
Create a folder : cylinder	Create a folder by the name cylinder
Type cd (space) ..	Go one level back
Copy 0 and system folder from cavity folder in icoFoam	Copy the 0 and system folders from the cavity case.
Paste it in cylinder folder	Then paste it inside the cylinder folder.
No constant folder	Note that you do not need the constant folder.
Point over the .msh file on the desktop	On my desktop, I have a Fluent mesh file with a .(dot) msh extension It is named as cylmesh.msh
Copy-and-paste >> cylinder folder.	Copy-and-paste this file in the cylinder folder in icoFoam. Our setup is now ready
Ctrl+Alt+t keys simultaneously	Open a command terminal and press Enter.
In the terminal window >> type run >> press Enter.	Type run and press Enter.
Type Incompressible and press Enter	Type Incompressible and press Enter
Type icoFoam and press Enter	Type icoFoam and press Enter
Type cylinder and press Enter	Type cylinder and press Enter.
On the terminal >> type fluentMeshToFoam cylmesh.msh >>Enter	For a Fluent mesh file, in the command terminal we need to type fluentMeshToFoam ( space ) cylmesh.msh and press Enter
The command terminal will show the conversion	On the terminal you will see that the mesh file is converted to openfoam data file
Click on cylinder folder	Go to the cylinder folder
Point to the constant folder Click on constant folder	The constant folder has been generated Click on the constant folder to open it.
Point showing no transport property file.	Transport Property file is missing from the constant folder
constant >> cylinder >> cavity >> constant – copy the transport property file	Go two levels back and copy transport property from cavity case
Paste inside the constant folder of cylinder do not change the viscosity	Paste it inside the constant folder of cylinder which we created just now We will keep the default viscosity
Command Terminal	Switch back to the terminal.
Do not run blockMesh command	Note that we do not run blockMesh command here.
Boundary conditions in the mesh file	To view the boundary conditions in the mesh file
From the command terminal go to the boudary file	Go to Constant > polyMesh > boundary file.
Open the file in the text editor	Open it in any editor of your choice.
Names are same as sown in the geometry slide	The boundary condition names are same as seen in the geometry slide.
In case of boundary name error check this file	In case of any error with boundary names, you can refer to the boundary file
polyMesh >> constant >> 0 folder	Go two levels back and go to the 0 folder.
Open the ' p ' file	Now, open the 0 folder and then open the pressure file in an editor
Point over the boundary name and change it to the ones shown in the boundary file	Note that the boundary names should exactly match with the boundary file. Change them if needed. Close this
' p '>> 0 >> system folder	Now go two levels back and go to the system folder
Make changes in the system folder	We can make some changes in the files of 'system folder
Edit the control dict file	We will change the end time of controlDict file in our case Open the file in a editor
Edit and change end time from 5 to 100	Change it from 5 to 100 and close it.
Go to the cylinder folder in terminal	Close this and go two levels back
Type icoFoam and press enter	To start the iterations, type icoFoam and press Enter
Iterations running in terminal window	Iterations will be seen running in the terminal
Open paraview	To view the geometry, type paraFoam and press Enter
Click on Apply button	In the paraFoam window, click on the Apply button in the object inspector menu
Point over the geometry	You can see the geometry
Point over the solid color and change it to U	In the Active variable control menu, change from solid color to U velocity
Point over the velocity condition	The initial velocity condition is seen here
Click on the play button of VCR controls	Click on the play button of the VCR menu on the top right hand side
Point over the geometry	We can see the velocity contours with the passage of time
Close paraview	Close the paraview window
	Let me switch back to the slides
Slide : List of commands to import mesh files	Here is a list of command to import geometry from other meshing software. ANSYS : ansysMeshToFoam space <name of the file> CFX : cfxToFoam space <name of the file> IDEAS : ideasTofoam space <name of the file> SALOME : ideasUnvToFoam space <name of the file> This brings us to the end of the tutorial
Slide :	As an assignment Try importing the mesh file of circular cylinder. Mesh file by the name circcyl.msh provided with this tutorial Solve it using the icoFoam solver
Slide : Summary	In this tutorial we learnt : Importing mesh files from third party software into OpenFOAM.
Slide 11 : About Spoken tutorials	Watch the video available at this URL: http://spoken-tutorial.org/What_is_a_Spoken_Tutorial It summarizes the Spoken Tutorial project. If you do not have good bandwidth, you can download and watch it
Slide 12: About Spoken tutorials	The Spoken Tutorial Project Team -Conducts workshops using spoken tutorials -Gives certificates to those who pass an online test -For more details, please write to contact@spoken-tutorial.org
Slide 13: Acknowledgement	Spoken Tutorials are part of Talk to a Teacher project, It is supported by the National Mission on Education through ICT, MHRD, Government of India. This project is coordinated by http://spoken-tutorial More information on the same is available at the following URL link http://spoken-tutorial.org/NMEICT-Intro
About the contributor	This is Rahul Joshi from IIT BOMBAY signing off. Thanks for joining

Contributors and Content Editors

Nancyvarkey, Rahuljoshi