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 to: import Mesh files from a meshing software in OpenFOAM.
Slide 3: 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 4  : 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 5:	Using blockMesh, we can easily make simple geometries. For example- box, pipe etc. It is difficult to create complex geometries using blockMesh.
Slide 6:	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 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 40m by 60m 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) ..	Now go to the cavity case.
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	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 the command terminal.
In the terminal window >> type run >> press Enter.	Type run and press Enter.
	Type cd tutorials; press Enter.
Type incompressible and press Enter	Type cd incompressible; press Enter
Type icoFoam and press Enter	Type cd icoFoam; press Enter
Type cylinder and press Enter	Type cd 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	Now go back 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 the transport property from the constant folder of the 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. Type ls. You will see the 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 the boundary names, you can refer to boundary file
polyMesh >> constant >> 0 folder	In the terminal, go two levels back and go to the 0 folder.
Open the ' p ' file	Open the pressure file in the 0 folder.
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 file.
' p '>> 0 >> system folder	Go one level back and go to the system folder.
Open the controlDict file.	Open the controlDict file.
Edit the control dict file	We will change the end time of controlDict file. Close this.
	Go one level back.
Type icoFoam and press enter	To start the iterations, type icoFoam and press Enter
Iterations running in terminal window	Iterations running will be seen 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.
Slide : List of commands to import mesh files	Here is a list of command to import geometry from other meshing software. ANSYS : ansysMeshToFoam space <filename> CFX : cfxToFoam space <filename> IDEAS : ideasTofoam space <filename> SALOME : ideasUnvToFoam space <filename> 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 geometry from other meshing software.
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