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

Time	Narration
00:00	Hello and welcome to the spoken tutorial on Importing Mesh files in OpenFOAM
00:07	In this tutorial, you will learn to: import Mesh files from a meshing software in OpenFOAM.
00:14	To record this tutorial I am using Linux Operating system Ubuntu version 12.04. OpenFOAM version 2.1.1 ParaView version 3.12.0
00:26	As a pre-requisite, the user should know how to generate a Mesh in software like - Gambit, Ansys ICEM , CFX, Salome etc.
00:40	*Using blockMesh, we can easily make simple geometries.*For example- box, pipe etc. It is difficult to create complex geometries using blockMesh.
00:53	*But OpenFOAM supports importing mesh from third party meshing software. There are commands available in OpenFOAM, to import these mesh files.
01:05	We will now learn to import these files.
01:08	Here is the geometry of our case. We have a square cylinder length 1m and height 1m. Inlet velocity is 1 m/s
01:22	*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
01:36	This is the mesh file generated in a meshing software.
01:40	In your OpenFOAM working directory, go to the icoFoam solver and click on it.
01:47	Now Create a folder by the name cylinder
01:52	Now go to the cavity case.Copy the 0 and system folders from the cavity case.
01:59	Paste this inside the cylinder folder.Note that, you do not need the constant folder.
02:10	On my desktop, I have a Fluent mesh file with a .(dot) msh extension.It is named as cylmesh.msh
02:23	Copy-and-paste this file in the cylinder folder in icoFoam.Our setup is now ready.
02:32	Open the command terminal.Type run and press Enter.
02:37	Type cd tutorials; press Enter.
02:42	Type cd incompressible; press Enter.Type cd icoFoam; press EnterType cd cylinder and press Enter.
02:58	For a Fluent mesh file, in the command terminal we need to typefluentMeshToFoam note that (MTF) are capital here (space) cylmesh.mshand press Enter
03:20	On the terminal you will see that the mesh file is converted to openfoam data file
03:28	Now go back to the cylinder folder
03:31	The constant folder has been generated.Click on the constant folder to open it.
03:38	Transport Property file is missing from the constant folder
03:42	Go two levels back and copy the transport property from the constant folder of the cavity case.
03:53	Paste this inside the constant folder of cylinder which we created just now.We will keep the default viscosity.
04:05	Switch back to the terminal.
04:08	Note that we do not run blockMesh command here.To view the boundary conditions in the mesh file
04:15	Go to Constant > polyMesh.Type ls.You will see the boundary file.
04:25	Open it in any editor of your choice.
04:30	The boundary condition names are as seen in the geometry slide.
04:36	In case of any error with the boundary names, you can refer the boundary fileclose this.
04:45	In the terminal, go two levels back and go to the 0 folder.
04:52	Open the pressure file in the 0 folder.
04:57	Note that the boundary names should exactly match with the boundary file.Change them if needed.Close this file.
05:08	Go one level back and go to the system folder.
05:15	Open the controlDict file.
05:18	We will change the end time of controlDict file.Close this.
05:25	Go one level back.To start the iterations', type icoFoam and press EnterIterations running will be seen in the terminal.
05:39	To view the geometry, type paraFoam and press Enter.In the ParaView window, click on the Apply button in the object inspector menu.
05:53	You can see the geometry.In the Active variable control menu, change from solid color to U velocity
06:03	The initial velocity condition is seen here.
06:08	Click on the play button in the VCR menu on the top right-hand side.
06:15	We can see the velocity contours with the passage of time.
06:20	Close the paraview window.
06:23	Here is a list of command to import geometry from other meshing software. ANSYS : ansysMeshToFoam space <filename> IDEAS : ideasTofoam space <filename> CFX : cfxToFoam space <filename> SALOME : ideasUnvToFoam space <filename> This brings us to the end of the tutorial.
06:54	As an assignment Try importing the mesh file of circular cylinder. Mesh file by the name circcyl.mshis provided with this tutorial. Solve it using the icoFoam solver.
07:12	In this tutorial we learnt : Importing geometry from other meshing software.
07:18	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
07:30	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
07:46	Spoken Tutorials Project is a part of the 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-tutorialMore information on the same is available at the following URL linkhttp://spoken-tutorial.org/NMEICT-Intro
08:03	This is Rahul Joshi from IIT BOMBAY signing off.Thanks for joining

Contributors and Content Editors

PoojaMoolya, Pratik kamble, Sandhya.np14