Evan: Created page with "'''Title of the script''': 2D Dam Break Simulation using OpenFOAM '''Author''': Ashley Melvin '''Keywords''': OpenFOAM, ParaView, CFD, computational fluid dynamics, blockMes..."

2025-01-02T06:35:48Z

Created page with "'''Title of the script''': 2D Dam Break Simulation using OpenFOAM '''Author''': Ashley Melvin '''Keywords''': OpenFOAM, ParaView, CFD, computational fluid dynamics, blockMes..."

New page

'''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.

{| border=1
|-
| align=center| '''Visual Cue'''
| align=center| '''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 [https://imgur.com/4clg8w3.png 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 [https://imgur.com/OjuyDUc.png 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 '''[https://imgur.com/WmtpcPZ.png Link]
|| All three '''walls''' are imposed with '''fixedFluxPressure''' boundary conditions.
|-
|| [gedit - '''p_rgh'''] Highlight:

'''value uniform 0''' [https://imgur.com/QoMav70.png Link]
|| For the '''type fixedFluxPressure''', '''value''' is just a '''placeholder''' for the first '''time-step'''.
|-
|| [gedit - '''p_rgh'''] Highlight:

'''atmosphere''' boundary condition [https://imgur.com/JK3soLy.png 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''' [https://imgur.com/1aaDdh8.png 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 '''[https://imgur.com/v9BoZsx.png 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 '''[https://imgur.com/HN6b9Ve.png 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 '''[https://imgur.com/RGjo8lX.png 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''' [https://imgur.com/G78q4oa.png 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 [https://imgur.com/Pdn13Gv.png 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) '''[https://imgur.com/kpH02Yo.png Link]
|| The two '''phases''' in this simulation are '''water''' and '''air'''.
|-
|| [gedit - '''transportProperties'''] Highlight:

Properties of water and air [https://imgur.com/nKWp8rv.png Link]
|| The properties of '''water''' and '''air''' are specified as shown.
|-
|| [gedit - '''transportProperties'''] Highlight:

'''sigma 0.07 '''[https://imgur.com/bdnBZhj.png 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 '''[https://imgur.com/fbjxny0.png Link]
|| The domain is '''decomposed''' into '''4 sub-domains'''.
|-
|| [gedit - '''decomposeParDict'''] Highlight:

'''method scotch '''[https://imgur.com/50ehP2I.png 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 '''[https://imgur.com/Ii1maj0.png Link]
|| The default value of '''fields''' for the domain is specified using the '''defaultFieldValues''' list.
|-
|| [gedit - '''setFieldsDict'''] Highlight: [https://imgur.com/PlQWgJD.png Link]

'''volScalarFieldValue alpha.water 0'''
|| The default value of '''phase fraction''' of '''water''' is specified as '''0'''.
|-
|| [gedit - '''setFieldsDict'''] Highlight:

'''regions '''[https://imgur.com/caYouzm.png Link]
|| Next, we set the '''regions''' where the '''field''' values are different from the default values.
|-
|| [gedit - '''setFieldsDict'''] Highlight:

'''boxToCell '''[https://imgur.com/fuxtALG.png 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) '''[https://imgur.com/nHT9nNA.png Link]
|| We specify the '''bounding box''' as shown.
|-
|| [gedit - '''setFieldsDict'''] Highlight:

fieldValues List [https://imgur.com/32cJriX.png Link]
|| The '''fieldValues''' to be specified within the '''box''' is defined as shown.
|-
|| [gedit - '''setFieldsDict'''] Highlight:

'''alpha.water 1 '''[https://imgur.com/xJjpWjo.png 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 '''[https://imgur.com/1nOhPK9.png 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 '''[https://imgur.com/IFMlIWa.png 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.

|-
|}

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

Evan: Created page with "'''Title of the script''': 2D Dam Break Simulation using OpenFOAM '''Author''': Ashley Melvin '''Keywords''': OpenFOAM, ParaView, CFD, computational fluid dynamics, blockMes..."