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 prerequisite, the user should know how to generate a Mesh in softwares 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' (zero0 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 space tutorials; press Enter. |
| 02:42 | Type: cd space incompressible and press Enter. Type cd space icoFoam; press Enter. Type cd space cylinder and press Enter. |
| 02:58 | For a Fluent mesh file, in the command terminal, we need to type "fluentMeshToFoam" (Note that M, T, F are capital here) (space) "cylmesh.msh" and press Enter. |
| 03:20 | On the terminal, you will see that the mesh file is now 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 file. Close this. |
| 04:45 | In the terminal, go two levels back and go to the '0' (zero) folder. |
| 04:52 | Open the pressure file in the '0' (zero) 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 the controlDict file. Close this. |
| 05:25 | Go one level back. To start the iterations, type "icoFoam" and press Enter. Iterations 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 commands to import geometry from other meshing software.
ANSYS : ansysToFoam 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 a 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 softwares. |
| 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 Tutorial 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. More information on this mission is available at the following URL: |
| 08:03 | This is Rahul Joshi from IIT Bombay, signing off. Thanks for joining. |
