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

Title of the script: Setting-up a test case in OpenFOAM

Author: Ashley Melvin

Keywords: OpenFOAM, ParaView, lid driven cavity, pre-processing, blockMesh, controlDict, post-processing, video tutorial

Visual Cue	Narration
Slide: Opening Slide	Hello and welcome to this tutorial on Setting up a test case in OpenFOAM.
Slide: Learning Objective	In this tutorial, we will learn to: Set up a case in OpenFOAM Access the case files using terminal Pre-process a case Run a case, and Post-process a case
Slide: System Specifications	This tutorial is recorded using, Ubuntu Linux OS version 18.04 OpenFOAM version 7 ParaView version 5.6.0, and gedit Text editor You may use any other text editor of your choice.
Slide: Prerequisites	As a prerequisite: You should be familiar with basic Linux commands. If not, please go through the prerequisite Linux tutorials on this website.
Slide: Lid Driven Cavity	In this tutorial, we will learn to set up the lid driven cavity case. Lid driven cavity is one of the most widely used 2D test cases for the validation of a CFD code.
Slide: Diagram	This is the diagram of Lid Driven Cavity Flow. It consists of 3 fixed walls and a moving top wall.
Highlight Terminal on the machine	Open a terminal by pressing the Ctrl, Alt and T keys together.
Only Narration	Here onwards please remember to press the Enter key after typing each command.
[Terminal] Type: mkdir -p $FOAM_RUN	Now, let’s create a RUN directory. To do so, type the command as shown.
[Terminal] Highlight FOAM_RUN	Tutorial cases will later be copied into the RUN directory.
[Terminal] Type: cd $FOAM_RUN	Go to the RUN directory using the cd command. Now our present working directory is the RUN directory.
Only Narration	OpenFOAM installation comes with a set of test cases. The tutorials directory contains these test cases. The Lid driven cavity case already exists inside the tutorials directory.
[Terminal] Type: cp -r $FOAM_TUTORIALS/incompressible/icoFoam/cavity/cavity .	We’ll now copy the Lid driven cavity case from the tutorials directory into the RUN directory. To do so, type the following command.
Slide: blockMesh	The mesh generator for OpenFOAM is a utility called blockMesh. The input dictionary for blockMesh utility is blockMeshDict.
[Terminal] Type: gedit cavity/system/blockMeshDict	The blockMeshDict file is located in the system folder. Open the blockMeshDict file in a text editor.
[gedit - blockMeshDict] Highlight vertices, blocks, edges and boundary	Now let’s look at the contents of the file. The blockMeshDict contains details of the geometry like vertices, blocks, edges and boundaries.
[gedit - blockMeshDict] Close the window	Close the blockMeshDict file.
[Terminal] Type: cd cavity/0	The 0 folder contains the initial and boundary conditions for the simulation. Type the following command to move into the 0 folder inside the cavity case directory.
[Terminal] Type: ls	Type ls and press Enter to view the files in the 0 folder.
[Terminal] Highlight p and U	The 0 folder contains the kinematic pressure file p and the velocity file U.
[Terminal] Type: gedit p	Open the kinematic pressure file p in a text editor.
Only Narration	The p file contains the initial and boundary conditions of kinematic pressure.
[gedit - p] Highlight dimensions [0 2 -2 0 0 0 0]	The dimensions of kinematic pressure is meter squared per second squared.
[gedit - p] Highlight internalField	The internalField defines the values in the interior of the domain.
[gedit - p] Highlight uniform 0	The initial field is set as 0 kinematic pressure. This field is uniform across the domain.
[gedit - p] Highlight Both the zeroGradient	You can see that all walls are imposed with a zero gradient pressure boundary condition.
[gedit - p] Close the window	Let us close the p file.
[Terminal] Type: gedit U	Now open the velocity file U in a text editor.
Only Narration	The U file contains the initial and boundary conditions of velocity.
[gedit - U] Highlight uniform (1 0 0);	You can see that the moving wall is imposed with a velocity of 1 m/s in the x direction.
[gedit - U] Highlight noSlip	Also notice that the no-slip condition is imposed on the three fixed walls.
[gedit - U] Close the window	Now let us close the U file.
[Terminal] Type: cd ..	We’ll go back to the cavity folder. Type cd (space)(dot)(dot)
[Terminal] Type: gedit constant/transportProperties	Next, we will view the transport properties file which is in the constant folder.
[gedit - transportProperties] Highlight nu	The transportProperties file contains the details of kinematic viscosity.
[gedit - transportProperties] Highlight [0 2 -1 0 0 0 0]	The dimensions of kinematic viscosity is meter squared per second.
Slide: Kinematic Viscosity	The kinematic viscosity is defined by: nu equals magnitude of U times d by Re where velocity is 1 m per second characteristic length is 0.1 meters The Reynolds number (Re) for the flow is taken as 10. The kinematic viscosity is therefore 0.01 meter squared per second
Narration Only	Now let me switch back to transportProperties file.
[gedit - transportProperties] Highlight 0.01	The value of kinematic viscosity is indicated in the transportProperties file.
[gedit - transportProperties] Close the window	Close the transportProperties file.
[Terminal] Type: cd system	To move into the system folder, type the following command.
[Terminal] Type: ls	Type ls to view the contents of the system folder.
[Terminal] Highlight blockMeshDict controlDict fvSchemes fvSolution	The system folder contains the following files: blockMeshDict, controlDict, fvSchemes and fvSolution.
[Terminal] Highlight fvSchemes	The fvSchemes dictionary contains the finite volume discretisation schemes.
[Terminal] Highlight fvSolution	The fvSolution dictionary contains the linear equation solvers and tolerances. It contains other algorithm controls as well.
[Terminal] Highlight controlDict	The controlDict dictionary contains the simulation control parameters. The dictionary input includes the control of time and reading and writing of the solution data.
[Terminal] Type: gedit controlDict	Let’s open the controlDict file in a text editor.
[Terminal] Highlight startFrom and startTime	The start and stop times and the time step for the run must be set.
[gedit - controlDict] Highlight startTime 0;	The start time is set at 0 seconds.
[gedit - controlDict] Highlight stopAt endTime;	The time at which the simulation stops, is specified using the keyword stopAt. Here, stopAt is specified using the keyword endTime.
[gedit - controlDict] Highlight endTime 0.5;	The endTime is set at 0.5 seconds. This means that simulation stops after 0.5 seconds.
[gedit - controlDict] Highlight deltaT 0.005;	The value of the keyword deltaT defines the time step for the simulation. The time step for the current simulation is set as 0.005 seconds. Temporal accuracy and numerical stability is essential while running the simulation. To achieve this, a Courant number of less than 1 is required. Keeping this in mind, the time step is set to 0.005 seconds.
[gedit - controlDict] Highlight application icoFoam;	icoFoam is the OpenFOAM solver used to simulate the lid driven cavity flow.
[gedit - controlDict] Close the window	Close the controlDict file.
[Terminal] Type: cd ..	Go back to the cavity folder using cd command.
[Terminal] Type: blockMesh >> Enter	Type the command blockMesh and press Enter to mesh the geometry. The command takes input from the blockMeshDict dictionary and creates the geometry and meshes it.
[Terminal] Highlight End	The meshing is now complete.
[Terminal] Type: icoFoam	The lid driven cavity flow is an incompressible flow. It is solved using the OpenFOAM solver icoFoam. To start the simulation, type icoFoam in the terminal.
[Terminal] Highlight End	The iterations are now complete.
[Terminal] Type: paraFoam	Let us view the simulated results in ParaView. So, type paraFoam in the terminal.
[ParaView] Properties Tab Click on Apply	In the ParaView window, go to the Properties tab on the left. Then click on the green coloured Apply button.
[ParaView] Click on vtkBlockColors >> Click on U	Go to the Active Variable Controls at the top. Click on the vtkBlockColors dropdown and select U. Ensure that you click on the U option with a point icon and not the box icon, in the dropdown. The box icon would display contours without any grading.
[ParaView] Velocity Contours in the Layout	The velocity contour at the start of the simulation is now displayed in the layout.
[ParaView] Go to VCR Controls and click on the Play Button	Let us see how the velocity contours develop through the simulation. To do so, go to the VCR Controls and click on the Play button.
[ParaView] Final Velocity Contours in the Layout	The velocity contour at the end of the simulation is now displayed in the layout.
[ParaView] Close the Window	Close the ParaView window.
Only Narration	With this we have come to the end of the tutorial.
Slide: Summary	To summarise, in this tutorial we have learnt to: Set up a case in OpenFOAM Access the case files using terminal Pre-process a case Run a case, and Post-process a case
Slide: About the Spoken Tutorial Project	The video at the following link summarises the Spoken Tutorial project. Please download and watch it.
Slide: Spoken Tutorial Workshops	We conduct workshops using Spoken Tutorials and give certificates. Please contact us.
Slide: Spoken Tutorial Forum	Please post your timed queries in this forum.
Slide: FOSSEE Forum	Do you have any general/technical questions? Please visit the forum given in this link.
Slide: FOSSEE Case Study Project	The FOSSEE team coordinates solving feasible CFD problems of reasonable complexity using OpenFOAM. We give honorarium and certificates to those who do this. For more details, please visit these sites.
Slide: Spoken Tutorial	The Spoken Tutorial project is supported by MHRD, Govt. of India. The script for this tutorial is contributed by Ashley Melvin. And this is Swetha Sridhar from IIT Bombay signing off. Thank you for joining.

Contributors and Content Editors

Ashleymelvin, Nancyvarkey