OpenFOAM/C3/Exporting-geometry-from-Salome-to-OpenFOAM/English-timed
From Script | Spoken-Tutorial
Revision as of 11:42, 26 November 2015 by Pratik kamble (Talk | contribs)
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 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 dropdown 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 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 button in front of Geometrical Object and select Direct Geometry 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 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. |
Also, copy and paste the system folder from cavity folder to this bentpipe folder. | |
Now, go inside the bentpipe folder throgh command terminal.I am inside the bentpipe folder. | |
Type ls and press Enter. We can see the system folder and the bentpipe.unv file. | |
Now, type ideasUnvToFoam bentpipe.(dot)unv, Note that U, T and F are capital. Press Enter. | |
Type ls. We can see the constant folder has been created. Type cd (space) Constant. | |
Type cd (space) polyMesh. Type ls. Press Enter. | |
We see that the geometry files have been created.Come out of the polyMesh folder. | |
Come out of the geometry folder. | |
Now, to convert the geometry scale to centimeters, typetransformPoints (space) -'(0.01 0.01 0.01)' and press Enter. Geometry has been converted to centimeters. | |
Minimize the terminal.Go inside the bentpipe folder. | |
Go inside constant folder. We see that the transportProperties file is not there. | |
Copy the transportProperties file from the cavity folder and save it inside the constant folder. | |
Now, come out of the constant folder. | |
We need the 0 (zero) folder having P and U files.Copy the 0 (zero) folder from the cavity folder. | |
I have copied the 0 (zero) folder. Go inside the 0 (zero) folder. | |
Open the p file .Make sure that you give boundary patches for inlet, outlet and walls as we had created in Salome. | |
Erase movingWall and type inlet. Erase fixedWall and type outlet. | |
Erase frontAndBack and type walls. Save the file and Close the file. | |
Similarly,Make changes in U file. For appropriate boundary conditions, refer to the tutorial on Hagen-Poiseuille flow. | |
I have made the changes and given the appropriate boundary conditions. | |
You may also make the changes in transportProperties and ControlDict files by refering to the tutorial on Hagen-Poiseuille flow. | |
Let's close the Home Folder. | |
Now, go to terminal.Type paraFoam. This will open ParaView. Click on Apply in the Object Inspector Menu. | |
In the drop down menu click on Surface with Edges. Lets have a closer view by zooming in. | |
We see hexahedral mesh. We see the groups have been created as we had named it in Salome- Inlet outlet and walls. | |
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. | |
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.
| |
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. | |
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 | |
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 | |
I am Saurabh Sawant, from IIT Bombay, Thank you. |