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 the 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 the 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 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 the "bentpipe" folder on the desktop, in this icoFoam folder.
05:22	Also, copy the system folder from the cavity folder to this bentpipe folder.
05:32	Now, go inside this bentpipe folder throgh command terminal. I am inside the bentpipe folder.
05:41	Type "ls" and press Enter. We see the systemfolder and the bentpipe.unv file.
05:49	Now, type: ideasUnvToFoam space 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 see geometry 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, type: transformPoints (space) -scale space '(0.01 space 0.01 space 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 the 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 Properties 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 fixedWalls 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 referring 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. Let's 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, please write to: contact@spoken-tutorial.org
10:40	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: 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