OpenFOAM-version-7/C2/Creating-2D-Channel-Geometry-and-Mesh-in-OpenFOAM/English-timed
From Script | Spoken-Tutorial
| Time | Narration |
| 00:01 | Hello and welcome to this tutorial on Creating 2D Channel Geometry and Mesh in OpenFOAM. |
| 00:08 | In this tutorial, we will learn to:
Create a 2D channel geometry using blockMeshDict |
| 00:17 | Mesh a geometry |
| 00:20 | Label the boundary patches, and View the mesh in ParaView |
| 00:27 | To record this tutorial, I am using,
Ubuntu Linux OS version 18.04 |
| 00:36 | OpenFOAM version 7 |
| 00:39 | ParaView version 5.6.0, and gedit Text Editor |
| 00:47 | You may use any other editor of your choice. |
| 00:51 | The files used in this tutorial are available in the Code Files link on this tutorial page |
| 00:59 | Please download and extract them |
| 01:02 | Make a copy and then use them while practising |
| 01:07 | The problem description of 2D flow in a channel is as shown in the diagram. |
| 01:14 | This is the geometry for 2D flow in a channel. |
| 01:19 | The faces of the geometry are: Inlet and outlet |
| 01:25 | Bottom and top walls |
| 01:28 | Back face, and Front face |
| 01:32 | Open the terminal by pressing Ctrl, Alt & T keys. |
| 01:38 | At the prompt, type the following command to go to the RUN directory. |
| 01:45 | Here onwards, please remember to press the Enter key after typing each command in the terminal. |
| 01:52 | Let us now copy the case of flow in a channel from the TUTORIALS directory into the RUN directory. |
| 02:00 | Type the following command to do so. |
| 02:05 | We will only be creating and meshing the geometry. |
| 02:09 | Hence, we do not need the boundary conditions folder. |
| 02:13 | Type the following command to delete the boundary conditions folder. |
| 02:18 | The blockMeshDict file is located in the system folder. |
| 02:23 | Let us open it in any text editor. |
| 02:27 | I am doing it in gedit Text Editor. |
| 02:31 | We can now see the blockMeshDict file. |
| 02:35 | Select the contents of the file from vertices to the end of the document, as shown. |
| 02:42 | We don’t need the selected content as we will be entering the input parameters.
Hence, delete the selected section. |
| 02:52 | The remaining content is common for all blockMeshDict files. |
| 02:57 | The unit of the coordinates entered in the blockMesh dictionary needs to be specified. |
| 03:04 | It is defined using the keyword convertToMeters. |
| 03:09 | The value 1 indicates that the values of all the coordinates are in meters. |
| 03:17 | Open the channel.txt file, that you had downloaded, in a text editor. |
| 03:23 | Copy the entire content of the text file. |
| 03:27 | Let me switch back to the blockMeshDict file. |
| 03:32 | Paste the copied contents into the blockMeshDict file as shown. |
| 03:40 | The vertices of the channel geometry are numbered as indicated. |
| 03:46 | The vertex numbering starts from 0. |
| 03:50 | The coordinates of the vertices are entered as shown. |
| 03:55 | Note that the vertices are entered in the ascending order of their vertex numbers. |
| 04:01 | Vertex 0 is located at the origin. |
| 04:05 | Its coordinates are entered as shown. |
| 04:09 | The x, y and z coordinates of vertex 1 are 4, 0 and 0 respectively. |
| 04:18 | Its coordinates are entered as shown. |
| 04:22 | Similarly, the coordinates of vertex 2 and 3 are entered as shown. |
| 04:29 | The z coordinate of all the points on the front face is 2. |
| 04:35 | The coordinates of front face vertices 4, 5, 6 and 7 are entered as shown. |
| 04:44 | For meshing, OpenFOAM requires 3-dimensional blocks to be defined. |
| 04:51 | The blocks are specified using the vertices that define them. |
| 04:57 | We use a single block in our geometry. |
| 05:01 | The block is defined as shown. |
| 05:05 | We use hexahedral blocks for meshing. |
| 05:10 | The order in which the vertices are specified, define the block. |
| 05:16 | We first enter the vertices of the lower xy-plane, in this case, the back face. |
| 05:24 | We start from the origin and enter the vertices of the face. |
| 05:29 | When viewed along the negative z-direction, the vertices should be ordered counterclockwise. |
| 05:37 | The vertices of the back face are defined as shown. |
| 05:41 | The vertices of the front face are entered in the same order as that of the back face. |
| 05:48 | Let us start defining the meshing parameters of the block. |
| 05:53 | We first define the number of cells in each direction of the block. |
| 05:59 | The number of cells in each direction is defined as shown. |
| 06:04 | This indicates that there are 40 cells in x direction and 25 cells in y direction. |
| 06:13 | There is only one cell along z direction indicating that the simulation is 2D in xy-plane. |
| 06:22 | Next, let us define how the mesh is graded. |
| 06:27 | We use simpleGrading as the cells have uniform expansion in all directions. |
| 06:34 | Let us now define the expansion ratios in each direction. |
| 06:39 | Expansion ratio along a direction is the ratio of width of the end cell to that of the start cell in that direction. |
| 06:50 | Since the cell width is uniform in all directions, the expansion ratio is 1. |
| 06:57 | Please refer to the "Additional Reading Material" on this tutorial page for details.
It has more details on defining a block. |
| 07:07 | Now, let us define the edges. |
| 07:11 | Edges are used to define arc or spline edges. |
| 07:17 | Since all the edges of channel geometry are straight lines, we leave it empty. |
| 07:23 | Let us label the boundary patches. |
| 07:26 | The labels are used to impose boundary conditions on the respective faces. |
| 07:32 | Boundary labels are defined using the boundary list. |
| 07:37 | The bottom face of the geometry is named bottomWall. |
| 07:42 | The patch type of the boundary is defined using the keyword type. |
| 07:48 | The bottom face resembles the characteristics of a solid wall.
Hence, the face is of the type wall. |
| 07:57 | Vertices define a face. |
| 08:00 | The vertices and their order for a face, is defined using the keyword faces. |
| 08:07 | Since the block face is a quadrilateral, it is defined by 4 vertices. |
| 08:14 | When viewed from inside the block, the vertices of the face should be ordered clockwise. |
| 08:21 | Keeping this in mind, the vertices of the bottom wall are ordered as shown. |
| 08:28 | Following the same convention, the top face is named topWall and is defined as shown. |
| 08:36 | We are creating the geometry for a 2D simulation in xy-plane. |
| 08:42 | We do not need to solve in the z direction.
Hence, we keep the front and back faces empty. |
| 08:51 | The back and front faces are defined as shown. |
| 08:56 | The inlet and outlet faces need the application of boundary condition. |
| 09:02 | Since they do not contain any geometric or topological information, a generic label would suffice. |
| 09:10 | Such generic boundaries are labelled using the keyword patch. |
| 09:16 | The inlet and outlet faces are defined as shown. |
| 09:21 | We have finished labelling all the boundary patches. |
| 09:25 | Next, we merge faces using the mergePatchPairs field. |
| 09:31 | We merge faces when a patch face from one block is connected to a patch face of another block. |
| 09:39 | Our geometry has only one block and there are no patches to merge. |
| 09:45 | Therefore, we leave the mergePatchPairs field empty. |
| 09:51 | We have entered all the necessary fields.
Save and close the file. |
| 09:58 | In the terminal, type cd (space) channel395. |
| 10:05 | Let us mesh the geometry. |
| 10:08 | Type blockMesh and press Enter to do so. |
| 10:13 | The meshing is complete. |
| 10:16 | To view the mesh in ParaView, type paraFoam and press Enter. |
| 10:24 | Click on the green coloured Apply on the left side of your window in the Properties tab. |
| 10:31 | Click on Surface available in the Representation Toolbar and change it to Surface with Edges. |
| 10:40 | You can now see the mesh structure of the front face. |
| 10:45 | Close the ParaView window. |
| 10:48 | With this we have come to the end of the tutorial.
Let us summarize. |
| 10:55 | In this tutorial, we have learnt to: Create a 2D channel geometry using blockMeshDict |
| 11:03 | Mesh a geometry
Label the boundary patches, and |
| 11:08 | View the mesh in ParaView |
| 11:11 | As an assignment: Create a geometry having dimensions 5 metres, 4 metres and 3 metres along x, y and z axis |
| 11:24 | Mesh the geometry such that it has 50, 40 and 1 cell along x, y and z axis, and |
| 11:35 | View the mesh in ParaView |
| 11:38 | The video at the following link summarises the Spoken Tutorial project.
Please download and watch it. |
| 11:46 | We conduct workshops using spoken tutorials and give certificates.
Please contact us. |
| 11:54 | Please post your timed queries in this forum. |
| 11:59 | Do you have any general/technical questions?
Please visit the forum given in this link. |
| 12:07 | The FOSSEE team coordinates solving feasible CFD problems of reasonable complexity using OpenFOAM. |
| 12:16 | We give honorarium and certificates to those who do this.
For more details, please visit these sites. |
| 12:25 | The Spoken Tutorial project is supported by MHRD, Govt. of India.
The script for this tutorial is contributed by Ashley Melvin. |
| 12:36 | And this is Swetha Sridhar from IIT Bombay signing off.
Thank you for joining. |
