OpenFOAM/C3/Exporting-geometry-from-Salome-to-OpenFOAM/English-timed

Time	Narration
00:01	Hello and welcome to the spoken tutorial on Exporting the geometry from Salome to OpenFOAM.
00:09	In this tutorial, we will see : To group the meshed geometry parts in Salome To export the geometry to OpenFOAM To create a case directory for simulation and To view the geometry in ParaView.
00:26	To record this tutorial, I am using: Linux operating system, Ubuntu version 12.10 OpenFOAM version 2.1.1 ParaView version 3.12.0 Salome version 6.6.0
00:41	To practice this tutorial, the learner should first perform the tutorial on Creating and meshing a Curved-Pipe Geometry in Salome.
00:52	Open Salome as shown in the previous tutorial. Go to file >> Open. Go to Desktop. Click on Curved-geometry.hdf.
01:04	Press Open. Go to mesh-module from Modules drop-down option.
01:12	Open the 'Mesh' tree from the object Browser.
01:17	Right-click on Mesh_1. Click on Show. We see the mesh on the geometry is visible.
01:28	Let me close the python console window.
01:32	Now, we have to name the meshed geometry parts as we require it in OpenFOAM.
01:39	To create Groups on this mesh, right-click on Mesh_1 and click on Create Group.
01:48	Select the Element Type as Face. Select the Group type as Group on Geometry.
01:57	Click on the button in front of Geometrical Object and select Direct Geometrical Selection.
02:07	Open the 'Geometry' tree in the Object Browser. Open the pipe_1 tree and select the inlet group in the geometry tree that we had created in the previous tutorial.
02:22	You can select the color as red.
02:26	Name the group as inlet. Click on Apply and close. inlet group is seen in the tree.
02:37	Similarly, create the outlet group. I have created the outlet group.
02:44	Now, to create the group of the whole outer surface, right-click on mesh_1 >> Create group .
02:53	Select Element Type as Face and the Group Type as Group on filter.
03:00	Click on Set filter. Click on the Add button. In the drop-down option below criterion menu, select Free Faces. Click on Apply and Close.
03:17	You can change the color to blue.
03:23	Again click on Apply and Close. Group_1 has been created.
03:31	Now, in the mesh menu at the top, click on Cut groups. Select the main object as Group_1. Select tool object as inlet.
03:45	Hold the shift key on your keyboard and also select the tool object as outlet.
03:54	Type the result name as walls.
03:58	You can select the color as purple. click on Apply and Close. 'We see walls group has been created.
04:10	Right click on the Group_1 and delete this group as we do not want to see it in OpenFOAM.
04:20	Save the work by clicking on save document option.
04:24	Now right click on mesh_1. Go to Export>> Unv File.
04:33	Name the file as bentpipe. I am saving this file on the Desktop. Close salome We see bentpipe.unv file on the desktop.
04:50	Create a folder named bentpipe on the desktop.
04:55	Now, move bentpipe.unv file to this folder.
05:01	To perform simulation on this geometry in OpenFOAM using icoFoam solver, Go to the icoFoam folder in OpenFOAM.
05:10	For the location of this folder, go to the tutorial on lid driven cavity.
05:15	Copy and Paste bentpipe folder on the desktop in this icoFoam folder.
05:22	Also, copy the system folder from cavity folder to this bentpipe folder.
05:32	Now, go inside the bentpipe folder throgh command terminal.I am inside the bentpipe folder.
05:41	Type ls and press Enter. We can see the system folder and the bentpipe.unv file.
05:49	Now, type ideasUnvToFoam bentpipe.(dot)unv, Note that U, T and F are capital. Press Enter.
06:11	Now Type ls. We see constant folder has been created. Type cd (space) Constant.
06:23	Type cd (space) polyMesh. Type ls. Press Enter.
06:31	We seegeometry files have been created.Come out of the polyMesh folder.
06:38	Come out of the constant folder.
06:42	Now, to convert the geometry scale to centimeters, typetransformPoints (space) -scale'(0.01 0.01 0.01)' and press Enter.The Geometry has been converted to centimeters.
07:17	Minimize the terminal.Go inside the bentpipe folder.
07:23	Go inside constant folder. We see that the transportProperties file is not there.
07:30	Copy the transportProperties file from the cavity folder and save it inside the constant folder.
07:37	I have copied the transport property file Now, come out of the constant folder.
07:44	We need the 0 (zero) folder having P and U files.Copy the 0 (zero) folder from the cavity folder.
07:55	I have copied the 0 (zero) folder. Go inside the 0 (zero) folder.
08:02	Open the p file .Make sure that you give boundary patches for inlet, outlet and walls as we had created in Salome.
08:15	Erase movingWall and type inlet. Erase fixedWall and type outlet.
08:25	Erase frontAndBack and type walls. Save the file and Close the file.
08:34	Similarly,Make changes in U file. For appropriate boundary conditions,you can refer to the tutorial on Hagen-Poiseuille flow.
08:46	I have made the changes and given the appropriate boundary conditions.
08:51	You may also make the changes in transportProperties and ControlDict files by refering to the tutorial on Hagen-Poiseuille flow.
09:00	Let's close the Home Folder.
09:03	Now, go to terminal.Type paraFoam. This will open ParaView. Click on Apply in the Object Inspector Menu.
09:16	In the drop down menu click on Surface with Edges. Lets have a closer look by zooming in.
09:28	We see hexahedral mesh. We also see the groups have been created as we had named it in Salome- Inlet outlet and walls.
09:38	Volume inside the surface is automatically grouped as internal mesh. In this tutorial we have learned: How to group the meshed geometry parts in Salome. How to export the geometry to OpenFOAM. How to create a case directory for simulation. And to view the geometry in ParaView.
10:00	For Assignment,Run the simulation by making appropriate changes in the files as described. Export the geometries that you have created on your own.And run the simulations on those geometries.
10:14	The video is available at the following 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.
10:24	The Spoken Tutorial Project Team Conducts workshops using spoken tutorials Gives certificates to those who pass an online test For more details, contact@spoken-tutorial.org
10:40	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 this mission is available at, http://spoken-tutorial.org/NMEICT-Intro
10:58	I am Saurabh Sawant, from IIT Bombay, Thank you.

Contributors and Content Editors

PoojaMoolya, Pratik kamble, Sandhya.np14