OpenFOAM-version-7/C2/Setting-up-a-Test-Case-in-OpenFOAM/English-timed

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.

Contributors and Content Editors

PoojaMoolya