OpenFOAM-version-7/C2/Setting-up-a-Test-Case-in-OpenFOAM/English-timed
From Script | Spoken-Tutorial
| Time | Narration |
| 00:01 | Hello and welcome to this tutorial on Setting up a test case in OpenFOAM. |
| 00:07 | In this tutorial, we will learn to:
Set up a case in OpenFOAM |
| 00:13 | Access the case files using terminal |
| 00:17 | Pre-process a case |
| 00:20 | Run a case, and Post-process a case |
| 00:25 | This tutorial is recorded using,
Ubuntu Linux OS version 18.04 |
| 00:34 | OpenFOAM version 7 |
| 00:37 | ParaView version 5.6.0, and gedit Text editor |
| 00:45 | You may use any other text editor of your choice. |
| 00:50 | As a prerequisite: You should be familiar with basic Linux commands. |
| 00:58 | If not, please go through the prerequisite Linux tutorials on this website. |
| 01:04 | In this tutorial, we will learn to set up the lid driven cavity case. |
| 01:10 | Lid driven cavity is one of the most widely used 2D test cases for the validation of a CFD code. |
| 01:19 | This is the diagram of Lid Driven Cavity Flow. |
| 01:24 | It consists of 3 fixed walls and a moving top wall. |
| 01:30 | Open a terminal by pressing the Ctrl, Alt and T keys together. |
| 01:37 | Here onwards please remember to press the Enter key after typing each command. |
| 01:44 | Now, let’s create a RUN directory. |
| 01:48 | To do so, type the command as shown. |
| 01:52 | Tutorial cases will later be copied into the RUN directory. |
| 01:57 | Go to the RUN directory using the cd command. |
| 02:02 | Now our present working directory is the RUN directory. |
| 02:07 | OpenFOAM installation comes with a set of test cases. |
| 02:12 | The TUTORIALS directory contains these test cases. |
| 02:17 | The Lid driven cavity case already exists inside the TUTORIALS directory. |
| 02:23 | We’ll now copy the Lid driven cavity case from the TUTORIALS directory into the RUN directory. |
| 02:31 | To do so, type the following command. |
| 02:36 | The mesh generator for OpenFOAM is a utility called blockMesh. |
| 02:42 | The input dictionary for blockMesh utility is blockMeshDict. |
| 02:49 | The blockMeshDict file is located in the system folder. |
| 02:55 | Open the blockMeshDict file in a text editor. |
| 03:00 | Now let’s look at the contents of the file. |
| 03:04 | The blockMeshDict contains details of the geometry like vertices, blocks, edges and boundaries. |
| 03:17 | Close the blockMeshDict file. |
| 03:20 | The 0 folder contains the initial and boundary conditions for the simulation. |
| 03:27 | Type the following command to move into the 0 folder inside the cavity case directory. |
| 03:35 | Type ls and press Enter to view the files in the 0 folder. |
| 03:41 | The 0 folder contains the kinematic pressure file p and the velocity file U. |
| 03:49 | Open the kinematic pressure file p in a text editor. |
| 03:54 | The p file contains the initial and boundary conditions of kinematic pressure. |
| 04:01 | The dimensions of kinematic pressure is meter squared per second squared. |
| 04:07 | The internalField defines the values in the interior of the domain. |
| 04:13 | The initial field is set as 0 kinematic pressure. |
| 04:17 | This field is uniform across the domain. |
| 04:21 | You can see that all walls are imposed with a zero gradient pressure boundary condition. |
| 04:29 | Let us close the p file. |
| 04:32 | Now open the velocity file U in a text editor. |
| 04:37 | The U file contains the initial and boundary conditions of velocity. |
| 04:43 | You can see that the moving wall is imposed with a velocity of 1 m/s in the x direction. |
| 04:52 | Also notice that the no-slip condition is imposed on the three fixed walls. |
| 04:59 | Now let us close the U file. |
| 05:02 | We’ll go back to the cavity folder.
Type cd (space)(dot)(dot) |
| 05:10 | Next, we will view the transport properties file which is in the constant folder. |
| 05:17 | The transportProperties file contains the details of kinematic viscosity. |
| 05:24 | The dimensions of kinematic viscosity is meter squared per second. |
| 05:30 | The kinematic viscosity is defined by: nu equals magnitude of U times d by Re |
| 05:41 | where velocity is 1 m per second |
| 05:45 | characteristic length is 0.1 meters |
| 05:50 | The Reynolds number (Re) for the flow is taken as 10. |
| 05:55 | The kinematic viscosity is therefore 0.01 meter squared per second |
| 06:01 | Now let me switch back to transportProperties file. |
| 06:05 | The value of kinematic viscosity is indicated in the transportProperties file. |
| 06:11 | Close the transportProperties file. |
| 06:14 | To move into the system folder, type the following command. |
| 06:19 | Type ls to view the contents of the system folder. |
| 06:24 | The system folder contains the following files:
blockMeshDict, controlDict, fvSchemes and fvSolution. |
| 06:37 | The fvSchemes dictionary contains the finite volume discretisation schemes. |
| 06:44 | The fvSolution dictionary contains the linear equation solvers and tolerances. |
| 06:51 | It contains other algorithm controls as well. |
| 06:56 | The controlDict dictionary contains the simulation control parameters. |
| 07:02 | The dictionary input includes the control of time and reading and writing of the solution data. |
| 07:09 | Let’s open the controlDict file in a text editor. |
| 07:14 | The start and stop times and the time step for the run must be set. |
| 07:21 | The start time is set at 0 seconds. |
| 07:25 | The time at which the simulation stops, is specified using the keyword stopAt. |
| 07:32 | Here, stopAt is specified using the keyword endTime. |
| 07:38 | The endTime is set at 0.5 seconds. |
| 07:43 | This means that simulation stops after 0.5 seconds. |
| 07:49 | The value of the keyword deltaT defines the time step for the simulation. |
| 07:56 | The time step for the current simulation is set as 0.005 seconds. |
| 08:03 | Temporal accuracy and numerical stability is essential while running the simulation. |
| 08:10 | To achieve this, a Courant number of less than 1 is required. |
| 08:16 | Keeping this in mind, the time step is set to 0.005 seconds. |
| 08:22 | Please refer to the additional reading material on this tutorial page for details. |
| 08:28 | It mentions the steps used to calculate the time-step. |
| 08:33 | icoFoam is the OpenFOAM solver used to simulate the lid driven cavity flow. |
| 08:39 | Close the controlDict file. |
| 08:42 | Go back to the cavity folder using cd command. |
| 08:47 | Type the command blockMesh and press Enter to mesh the geometry. |
| 08:53 | The command takes input from the blockMeshDict dictionary and creates the geometry and meshes it. |
| 09:01 | The meshing is now complete. |
| 09:04 | The lid driven cavity flow is an incompressible flow. |
| 09:09 | It is solved using the OpenFOAM solver icoFoam. |
| 09:14 | To start the simulation, type icoFoam in the terminal. |
| 09:20 | The iterations are now complete. |
| 09:23 | Let us view the simulated results in ParaView.
So, type paraFoam in the terminal. |
| 09:32 | In the ParaView window, go to the Properties tab on the left.
Then click on the green coloured Apply button. |
| 09:41 | Go to the Active Variable Controls at the top. |
| 09:46 | Click on the vtkBlockColors dropdown and select U. |
| 09:52 | Ensure that you click on the U option with a point icon and not the box icon, in the dropdown. |
| 10:00 | The box icon would display contours without any grading. |
| 10:04 | The velocity contour at the start of the simulation is now displayed in the layout. |
| 10:11 | Let us see how the velocity contours develop through the simulation. |
| 10:16 | To do so, go to the VCR Controls and click on the Play button. |
| 10:23 | The velocity contour at the end of the simulation is now displayed in the layout. |
| 10:30 | Close the ParaView window. |
| 10:34 | With this we have come to the end of the tutorial. |
| 10:36 | To summarise, in this tutorial we have learnt to: |
| 10:42 | Set up a case in OpenFOAM |
| 10:45 | Access the case files using terminal |
| 10:49 | Pre-process a case
Run a case, and |
| 10:54 | Post-process a case |
| 10:57 | The video at the following link summarises the Spoken Tutorial project.
Please download and watch it. |
| 11:05 | We conduct workshops using Spoken Tutorials and give certificates.
Please contact us. |
| 11:13 | Please post your timed queries in this forum. |
| 11:17 | Do you have any general/technical questions?
Please visit the forum given in this link. |
| 11:24 | The FOSSEE team coordinates solving feasible CFD problems of reasonable complexity using OpenFOAM. |
| 11:31 | We give honorarium and certificates to those who do this. |
| 11:35 | For more details, please visit these sites. |
| 11:39 | The Spoken Tutorial project is supported by MHRD, Govt. of India.
The script for this tutorial is contributed by Ashley Melvin. |
| 11:49 | And this is Swetha Sridhar from IIT Bombay signing off.
Thank you for joining. |
