OpenFOAM-version-7/C3/2D-Dam-Break-Simulation-using-OpenFOAM/English

Title of the script: 2D Dam Break Simulation using OpenFOAM

Author: Ashley Melvin

Keywords: OpenFOAM, ParaView, CFD, computational fluid dynamics, blockMesh, VOF, volume of fluid, multiphase flow, dam break, scotch decomposition, setFields, FOSSEE, spoken tutorial, video tutorial.

Visual Cue	Narration
Slide Opening Slide	Welcome to this tutorial on 2D Dam Break Simulation
Slide Learning Objectives	In this tutorial, we will learn how to, Set up a case of multiphase flow Decompose the domain using scotch decomposition method Specify a non-uniform initial condition, and View the results of a multiphase simulation in ParaView
Slide System Specifications	To record this tutorial, I am using, Ubuntu Linux OS version 22.04* OpenFOAM version 9 ParaView version 5.10.1, and gedit Text Editor
Slide Prerequisites* If not, please go through the prerequisite OpenFOAM tutorial on https://spoken-tutorial.org	As a prerequisite, You should have basic knowledge of multiphase flows. You should also be familiar with parallel computing in OpenFOAM. If not, please go through the prerequisite OpenFOAM tutorials on this website.
Slide Code Files	The files used in this tutorial are available in the Code Files link on this tutorial page Please download and extract them Make a copy and then use them while practicing Copy the damBreak folder into the run directory to follow along
Slide Breaking of a Dam	We will be solving the dam break problem shown in the figure. Initially, there is a water column in the domain, and It is surrounded by air.
Only Narration	Let’s see what happens when a dam, that holds the water column, suddenly breaks.
CTRL + ALT + T keys	Open the terminal by pressing Ctrl, Alt and T keys together.
[Terminal] Type: cd $FOAM_RUN	Type this command and press Enter to move into the run directory.
[Terminal] Type: cd damBreak	Let’s move into the damBreak folder using the following command.
[Terminal] Type: gedit system/blockMeshDict	Let’s open the blockMeshDict file in a text editor.
Slide Dam Break Geometry	The geometry is divided into 5 blocks as shown in the diagram.
[gedit - blockMeshDict] Highlight: Blocks List Link	The 5 blocks are defined as shown.
Slide Boundaries	The boundaries of the geometry are: leftWall rightWall lowerWall, and atmosphere It is named so, as it is exposed to the atmosphere.
[gedit - blockMeshDict] Highlight: Boundary List Link	The 4 faces are defined in the boundary list as shown.
[gedit - blockMeshDict] Close the window	Close the blockMeshDict file.
Only Narration	Now, let’s view the initial and boundary conditions files.
[Terminal] Type: gedit 0/p_rgh	Let’s view the initial and boundary values of p_rgh
Only Narration	p_rgh is the pressure without the hydrostatic contribution.
[gedit - p_rgh] Highlight: fixedFluxPressure Link	All three walls are imposed with fixedFluxPressure boundary conditions.
[gedit - p_rgh] Highlight: value uniform 0 Link	For the type fixedFluxPressure, value is just a placeholder for the first time-step.
[gedit - p_rgh] Highlight: atmosphere boundary condition Link	The top boundary is exposed to the atmosphere. Therefore, a totalPressure of 0 Pa is imposed.
Only Narration	The additional reading material has more details on p_rgh and its boundary conditions. Please refer to it.
[gedit - p_rgh] Close the window	Close the p_rgh file.
[Terminal] Type: gedit 0/alpha.water.orig	Let’s view the initial and boundary values of phase fraction of water.
[gedit - alpha.water.orig] Highlight: internalField uniform 0 Link	The domain is initialized uniformly with a value of 0. This means the entire domain consists of only air. We will be initializing the section of the domain with the water column later.
[gedit - alpha.water.orig] Highlight: zeroGradient Link Point to the contact angles and walls.	The surface tension effects between the walls and the fluid-interface are ignored. Thus, the contact angle between the walls and the fluid-interface is 90 degrees. Therefore, all three walls are imposed with zeroGradient boundary condition.
[gedit - alpha.water.orig] Highlight: type inletOutlet Link	The inletOutlet type boundary condition is imposed on the top boundary. It acts as a zeroGradient boundary condition for outflow.
[gedit - alpha.water.orig] Highlight: inletValue uniform 0 Link	For inflow, this type of boundary condition takes the inletValue as the fixedValue. We have specified the inletValue as 0, corresponding to 100 percent air.
[gedit - alpha.water.orig] Highlight: value uniform 0 Link	For the type inletOutlet, value is just a placeholder for the first time-step.
[gedit - alpha.water.orig] Close the window	Close the phase fraction file.
[Terminal] Type: gedit 0/U	Let’s view the initial and boundary values of U U is the Velocity Boundary Conditions file.
Slide Velocity Boundary Conditions* walls - noSlip top (atmosphere) - pressureInletOutletVelocity	Let’s look at the boundary conditions of velocity.* At the walls, noSlip condition is imposed At the top boundary, pressureInletOutletVelocity type boundary condition is imposed.
Slide pressureInletOutletVelocity	The pressureInletOutletVelocity Acts as a zeroGradient boundary condition for outflow. And for inflow, it acts as a fixedValue boundary condition.
[gedit - U] Close the window	Close the U file.
[Terminal] Type: ls constant	Let’s look at the constant files used in the simulation.
[Terminal] Highlight: momentumTransport	In this simulation, the flow is considered to be laminar. The same is specified in the momentumTransport file.
[Terminal] Type: gedit constant/momentumTransport	Let's view the contents of the momentumTransport file. The simulationType is specified as laminar.
[gedit - momentumTransport] Close the window	Close the momentumTransport file.
[Terminal] Highlight: g	The simulation requires the acceleration due to gravity, to be specified. The g file is used to specify the acceleration due to gravity. This has been discussed in the previous tutorials in this series.
Slide Transport Properties	These are the transport properties of water and air used in this simulation.
Slide Transport Properties Highlight: Newtonian Link	Both water and air are considered to be Newtonian fluids.
[Terminal] Type: gedit constant/transportProperties	Let’s open the transportProperties file in a text editor.
[gedit - transportProperties] Highlight: phases (water air) Link	The two phases in this simulation are water and air.
[gedit - transportProperties] Highlight: Properties of water and air Link	The properties of water and air are specified as shown.
[gedit - transportProperties] Highlight: sigma 0.07 Link	The surface tension between water and air is taken to be 0.07 Newton per meter.
[gedit - transportProperties] Close the window	Close the transportProperties file.
Only Narration	Now let’s look at how the domain is decomposed for the parallel run.
[Terminal] Type: gedit system/decomposeParDict	Let’s open the decomposePar dictionary in a text editor.
[gedit - decomposeParDict] Highlight: numberOfSubdomains 4 Link	The domain is decomposed into 4 sub-domains.
[gedit - decomposeParDict] Highlight: method scotch Link	The domain is decomposed using the scotch decomposition method. Scotch decomposition requires no geometric input. It attempts to minimize the number of processor boundaries.
[gedit - decomposeParDict] Close the window	Close the decomposeParDict file.
Only Narration	Now, let’s see how to initialize the section of the domain with a water column.
[Terminal] Type: gedit system/setFieldsDict	Such non-uniform initial conditions are specified using the setFields dictionary.
[gedit - setFieldsDict] Highlight: defaultFieldValues Link	The default value of fields for the domain is specified using the defaultFieldValues list.
[gedit - setFieldsDict] Highlight: Link volScalarFieldValue alpha.water 0	The default value of phase fraction of water is specified as 0.
[gedit - setFieldsDict] Highlight: regions Link	Next, we set the regions where the field values are different from the default values.
[gedit - setFieldsDict] Highlight: boxToCell Link	We specify the cells within a bounding box using boxToCell. This bounding box contains the cells that hold the water column.
Slide boxToCell* box (minx miny minz) (maxx maxy maxz)	boxToCell creates a bounding box within a vector minimum and maximum to define the cells This is the syntax of boxToCell
Slide Water Column	The section occupied by the water column is shown in the figure. We have considered the thickness of the geometry to be 0.1 meter.
Slide boxToCell	For the water column, The vector minimum is the origin, and The vector maximum is (0.5,1,0.1)
[gedit - setFieldsDict] Highlight: box (0 0 0) (0.5 1 0.1) Link	We specify the bounding box as shown.
[gedit - setFieldsDict] Highlight: fieldValues List Link	The fieldValues to be specified within the box is defined as shown.
[gedit - setFieldsDict] Highlight: alpha.water 1 Link	The phase fraction of water is specified to be 1 within the box. This means that the box is completely filled with water.
[gedit - setFieldsDict] Close the window	Close the setFieldsDict file.
[Terminal] Type: blockMesh	Let’s mesh the geometry using the blockMesh command.
[Terminal] Type: setFields	Then, let’s set the fields in the domain using the setFields command. Note that the setFields command should be executed only after meshing.
Only Narration	The additional reading material has more details on the setFields utility. Please refer to it.
[Terminal] Type: decomposePar	Let’s decompose the domain using the decomposePar command.
Slide interFoam* Captures the interface of 2 immiscible fluids using the volume of fluid (VOF) method.	We will use the interFoam solver to simulate this problem. It solves incompressible, isothermal, turbulent, multiphase flows. It captures the interface of 2 immiscible fluids using the volume of fluid method.
[Terminal] Type: mpirun -np 4 interFoam -parallel	Let’s start the simulation using the following command.
[Terminal] Type: reconstructPar	Since we had run our simulation in parallel, our solution is decomposed. Let’s reconstruct our solution using the reconstructPar command.
[Terminal] Type: paraFoam	Let’s now view the simulated results in ParaView.
[ParaView] Properties Tab Click on Apply	Click on the Apply button to view the geometry.
[ParaView] Active Variable Controls Click on vtkBlockColors >> Click on alpha.water Link	Let’s view the contours of phase fraction of water. Click on the vtkBlockColors dropdown in the Active Variable Controls and select alpha.water.
[ParaView] Layout Window Initial Phase Fraction Contour	You can see the initial contours of phase fraction of water showing the water column.
[ParaView] VCR Controls Click on Play Link	Let’s see how the contours change with time. Click on the Play button in the VCR Controls.
[ParaView] Layout Window Phase Fraction Contour animation	The animation shows the water flow for 5 seconds from the instance when the dam was broken.
[ParaView] Close ParaView	Close the ParaView window.
Only Narration	With this we have come to the end of the tutorial. Let’s summarize.
Slide Summary	In this tutorial, we have learnt to: Set up a case of multiphase flow Decompose the domain using scotch decomposition method Specify a non-uniform initial condition, and View the results of a multiphase simulation in ParaView
Slide Assignment	As an assignment:* For the same domain, increase the height of the water column to 1.5 meter, and Run the simulation.
Slide About the Spoken Tutorial Project	The video at the following link summarizes 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 the 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 Acknowledgement	The Spoken Tutorial project was established by the Ministry of Education, Govt. of India.
Only Narration	This tutorial is contributed by Ashley Melvin, Ashuthosh P S, John Pinto and Payel Mukherjee from IIT Bombay. Thank you for joining.

Contributors and Content Editors

Evan