Script | Spoken-Tutorial - User contributions [en]

OpenFOAM-version-9/C3/Simulating-Natural-Convection-in-a-Cavity/English

2025-01-28T04:28:18Z

Evan: Created page with "'''Title of the script''': Simulating Natural Convection in a Cavity '''Author''': Divyesh Variya '''Keywords''': OpenFOAM, ParaView, CFD, computational fluid dynamics, bloc..."

'''Title of the script''': Simulating Natural Convection in a Cavity

'''Author''': Divyesh Variya

'''Keywords''': OpenFOAM, ParaView, CFD, computational fluid dynamics, blockMesh, buoyancy driven flow, heat transfer, natural convection, buoyantSimpleFoam, thermophysical properties, FOSSEE, spoken tutorial, video tutorial.

{| border=1
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide:

'''Opening Slide'''
|| Welcome to the spoken tutorial on '''Simulating Natural Convection in a Cavity'''.
|-
|| Slide:

'''Learning Objective'''
|| In this tutorial, we will learn to:
* Set up a case of '''heat transfer''' in '''OpenFOAM'''
* Simulate a '''buoyancy-driven flow''', and
* Set up '''thermophysical properties''' in '''OpenFOAM'''

|-
|| Slide:

'''System Specifications'''
|| To record this tutorial, I am using,
* '''Ubuntu Linux''' OS version 22.04
* '''OpenFOAM''' version 9
* '''ParaView''' version 5.6.0, and
* '''gedit''' Text editor

However, you may use any other editor of your choice.
|-
|| Slide:

'''Prerequisites'''

* If not, please go through the prerequisite '''OpenFOAM '''tutorials on https://spoken-tutorial.org

|| As a prerequisite:
* You should have basic knowledge of '''convective heat transfer'''.
* You should be familiar with '''setting up a case''' in '''OpenFOAM'''.
* If not, please go through the prerequisite '''OpenFOAM '''tutorial 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 practising

|-
|| Slide:

'''Natural Convection in a Cavity'''
|| We will be solving a '''2D flow''' in a square '''cavity'''.

All '''4 walls''' of the '''cavity''' are '''fixed'''.
|-
|| Slide:

'''Natural Convection in a Cavity'''
||
* The '''bottom wall''' is maintained at a higher '''temperature''' compared to the '''top wall'''.
* The '''side walls''' are '''adiabatic'''.

|-
|| Slide:

'''Natural Convection in a Cavity'''
||
* The '''gravity''' is acting '''downwards''', in the '''negative y-direction'''.

* Inside the '''cavity''', the fluid close to the '''hot wall''' at the '''bottom''' is lighter.

* The fluid close to the '''cold wall''' on '''top''' is heavier.

* This difference in density causes a continuous circulation in the '''cavity'''.

|-
|| Only Narration
|| Let’s '''simulate''' this problem in '''OpenFOAM'''.
|-
|| CTRL + ALT + T
|| Open the '''terminal''' by pressing '''Ctrl''', '''Alt''' and '''T''' keys.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| Type the following '''command''' and press '''Enter''' to move into the '''run directory'''.
|-
|| Only Narration
|| Please remember to press the '''Enter''' key after typing each '''command''' in the '''terminal'''.
|-
|| [Terminal] Type: '''cp -r ~/Downloads/cavityConvection .'''
|| Let’s copy the case folder that is downloaded and extracted into the '''run directory'''.
|-
|| [Terminal] Type:

'''cd cavityConvection'''
|| Let’s change the directory to '''cavityConvection''' using the '''cd''' '''command'''.
|-
|| Slide:

'''Geometry'''
|| In this '''simulation''', we consider a '''square cavity''' with an edge '''length''' of '''1 m'''.
|-
|| Slide:

'''Boundaries'''
|| The '''computational domain''' has 4''' boundaries''', namely '''top''', '''bottom''', '''left''', and '''right'''.

All 4 '''boundaries''' are '''fixed walls'''.
|-
|| [Terminal] Type:

'''gedit system/blockMeshDict'''
|| Type the following command to open the '''blockMeshDict''' file in a text editor.
|-
|| [gedit blockMeshDict]:

Only Narration
|| We have a '''cubical''' geometry with a single '''block''' and four '''walls'''.

|-
|| [Terminal] Type:

'''Ctrl + Q'''
|| Close this file by pressing '''Ctrl + Q'''
|-
|| Slide: '''Boundary Conditions'''
|| Let’s look at the '''boundary conditions''' in this simulation.

* The '''bottom hot wall''' is maintained at '''1 K'''.
* The '''top cold wall''' is maintained at '''0 K'''.
* The '''left''' and the '''right''' '''walls''' are '''adiabatic'''.
* Therefore, they have '''zero gradient temperature boundary conditions'''.

|-
|| Slide:

'''Boundary Conditions'''
|| The '''boundary conditions '''used in the '''simulation''' are as shown in the table.
|-
|| [Terminal] Type:

'''ls 0'''
|| The '''boundary conditions''' are defined in the '''0 folder'''.

Let’s view its contents.
|-
|| [Terminal] Highlight:

'''p p_rgh T U'''
|| You will see two '''pressure files''' along with the '''temperature''' and the '''velocity files'''.

One is the '''pressure file''', '''p''' and the other is the '''modified pressure file''', '''p_rgh'''.
|-
|| Slide:

'''p_rgh'''

* In solvers involving external forces, such as gravity, a modified pressure is used.
* In this case, a pressure without the hydrostatic pressure is used.

'''Highlight >> p_rgh = p – rho*g*h'''

* It is numerically convenient to solve for this modified pressure term, p_rgh
* The pressure, p is calculated from the p_rgh pressure

||
* In '''solvers''' involving '''body forces''', such as '''gravity''', a '''modified pressure''' is used.
* In this case, a '''pressure''' without '''hydrostatic pressure''' is used.
* This '''modified pressure''', '''p_rgh''' is defined as:

'''p_rgh = p - rho*g*h'''
* It is numerically convenient to solve for this '''modified pressure''' term, '''p_rgh'''
* The '''pressure''', '''p''' is calculated from the '''p_rgh pressure'''

|-
|| [Terminal] Type: '''gedit 0/T'''
|| Let’s first open the '''temperature file''', '''T'''.
|-
|| [gedit - '''T'''] Highlight:

'''internalField uniform 1 '''
|| The '''domain''' is initialized with '''1 K'''.
|-
|| [gedit - '''T'''] Highlight:

'''bottom '''boundary condition
|| The '''bottom wall''' is maintained at a '''constant temperature''' of '''1 K'''.
|-
|| [gedit - '''T'''] Highlight:

'''top '''boundary condition
|| The '''top wall''' is maintained at a '''temperature''' of '''0 K'''.
|-
|| [gedit - '''T'''] Highlight:

'''left '''&''' right '''boundary condition
|| The '''left''' and '''right walls''' have '''zero gradient temperature boundary condition'''.
|-
|| [gedit - '''T'''] Close the window
|| Close the '''temperature''' '''file'''.
|-
|| [Terminal] Type: '''gedit 0/p_rgh'''
|| Let’s open the '''p_rgh file'''.
|-
|| [gedit - '''p_rgh'''] Highlight:

all''' walls '''boundary condition
|| All '''4 walls''' have been assigned the '''fixedFluxPressure''' '''boundary condition'''.
|-
|| Slide:

'''fixedFluxPressure'''
|| The '''fixedFluxPressure boundary condition''' is:

* Analogous to the '''zeroGradient''' '''pressure boundary condition'''
* Used when '''body forces''' such as '''gravity''' and '''surface tension''' are present
* It adjusts the '''pressure gradient''' at the '''wall''' based on the '''body forces'''

|-
|| [gedit - '''p_rgh'''] Highlight:

all''' walls '''boundary condition
|| Our '''simulation''' takes '''gravitational''' '''force''' into consideration.

Therefore, we will use the '''fixedFluxPressure''' condition at the '''walls'''.
|-
|| [gedit - '''p_rgh'''] Close the window
|| Close the '''p_rgh''' file.
|-
|| [Terminal] Type: '''gedit 0/p'''
|| Let’s open the '''pressure '''file,''' p'''.
|-
|| [gedit - '''p'''] Highlight:

all''' walls '''boundary condition
|| The '''pressure''' values at the '''boundaries''' are calculated from the '''p_rgh''' values.

Therefore, all '''4 walls''' have been assigned the '''calculated''' '''boundary condition'''.
|-
|| [gedit - '''p'''] Highlight:

'''value $internalField;'''
|| The '''value''' has been specified to be the same as the '''internalField'''.
|-
|| [gedit - '''p'''] Close the window
|| Close the '''p''' file.
|-
|| [Terminal] Type:

'''ls constant'''
|| Let’s now see the contents of the '''constant''' folder using the '''ls command'''.
|-
|| [Terminal] Highlight:

'''g momentumTransport thermophysicalProperties'''
|| We see that there are 3 files in the '''constant''' folder.
|-
|| [Terminal] Type: '''gedit constant/g'''
|| Let’s open the '''g '''file.
|-
|| [gedit - '''g'''] Highlight:

'''dimensions [0 1 -2 0 0 0 0] '''
|| The '''dimension''' of '''g''' is '''m/s2'''.
|-
|| [gedit - '''g'''] Highlight:

'''value (0 -10 0) '''
|| The '''magnitude''' of '''g''' is '''10''' '''m/s2'''.
|-
|| [gedit - '''g'''] Close the window
|| Close the '''g''' file.
|-
|| [Terminal] Type: '''gedit constant/momentumTransport'''
|| Let’s open the '''momentumTransport '''file.
|-
|| [gedit - '''momentumTransport'''] Highlight: '''simulationType laminar'''
|| Our '''simulation''' will be a '''laminar''' one.
|-
|| [gedit - '''momentumTransport'''] Close the window
|| Close the '''momentumTransport''' file.
|-
|| [Terminal] Type: '''gedit constant/thermophysicalProperties'''
|| Next, let’s open the '''thermophysicalProperties''' file.
|-
|| [gedit - '''thermophysicalProperties''']:

Only Narration
|| In this file, the '''properties''' of the '''fluid''' used in our '''simulation''' are specified.

We’ll be '''simulating''' the '''flow''' inside the '''cavity'''.
|-
|| [gedit - '''thermophysicalProperties'''] Highlight: '''thermoType''' field
|| '''OpenFOAM''' contains various '''thermophysical''' modelling packages.

The '''thermoType''' assembles the various '''thermophysical''' modelling packages.
|-
|| Only Narration
|| The '''additional reading material''' has more details on the '''thermophysical''' modelling packages.

Please refer to it.
|-
|| Slide:

'''Fluid Properties'''
|| The various properties used in this '''simulation''' are shown in the table.
|-
|| [gedit - '''thermophysicalProperties'''] Highlight: '''equationOfState Boussinesq'''
|| We’ll be using the '''Boussinesq approximation''' for the '''equation of state'''.
|-
|| Slide: '''Boussinesq Approximation'''

'''Higlight: '''equation from slide in 3rd point
|| The '''Boussinesq approximation''' is:
* Used in '''buoyancy-driven flows'''.
* It acts as an '''equation of state''' while solving the '''governing equations'''
* Mathematically, it defines the '''density field''' as shown in the equation

|-
|| Slide:

'''Boussinesq Approximation'''
|| '''Where, the reference density''' and '''coefficient of volumetric expansion''' are properties of fluid.
|-
|| Slide:

'''Reference Temperature'''
|| The '''reference temperature''' is taken to be the '''average''' of '''hot''' and '''cold''' '''wall temperatures'''.

Therefore, the '''reference temperature''' for our '''simulation''' is '''0.5 K'''.
|-
|| Only Narration
|| The '''additional reading material''' has more details on the '''Boussinesq approximation'''.

Please refer to it.
|-
|| [gedit - '''thermophysicalProperties'''] Highlight: '''molWeight 28.9 '''
|| The '''molecular weight''' of the''' '''fluid is specified as '''28.9 g/mol'''.
|-
|| [gedit - '''thermophysicalProperties'''] Highlight: '''rho0 1;'''

'''T0 0.5; '''
|| For the fluid in our '''simulation''', the '''reference density''' is specified to be '''1 kg/m3'''.

This is the '''reference density''' at a '''reference temperature''' of '''0.5 K'''.
|-
|| [gedit - '''thermophysicalProperties'''] Highlight: '''beta 3.4e-02 '''
|| The '''coefficient of volumetric expansion''' is '''3.4X10-2 K-1'''.
|-
|| [gedit - '''thermophysicalProperties'''] Highlight: '''Cp 1000 '''
|| The '''specific heat at constant pressure''' is taken to be '''1000 kJ/kg-K'''.
|-
|| [gedit - '''thermophysicalProperties'''] Highlight: '''Hf 0 '''
|| Since no '''phase change''' is considered in this '''simulation''', the '''heat of fusion''' is '''0'''.
|-
|| [gedit - '''thermophysicalProperties'''] Highlight: '''transport'''

'''{'''

'''mu 4.91e-03;'''

'''Pr 0.71;'''

'''} '''
|| For '''transport properties''', '''dynamic viscosity''' and '''Prandtl number''' are to be specified.

They are specified as shown here.
|-
|| [gedit - '''thermophysicalProperties'''] Close the window
|| Close the '''thermophysicalProperties''' file.
|-
|| [Terminal] Type: '''Ctrl + L'''
|| Clear the screen by pressing '''Ctrl''' and '''L''' keys together.
|-
|| [Terminal] Type: '''blockMesh'''
|| Let’s '''mesh''' the geometry using the '''blockMesh''' '''command'''.
|-
|| Slide:

'''buoyantSimpleFoam'''
|| We will be using the '''buoyantSimpleFoam''' solver in this simulation.

* It is a '''steady-state''' '''compressible flow '''solver for '''buoyant''' and '''turbulent flows'''.
* It solves the '''mass''', '''momentum''' and '''energy equations''' along with an '''equation of state'''.
* The '''equation of state''' we have considered is based on the '''Boussinesq approximation'''.

|-
|| [Terminal] Type: '''buoyantSimpleFoam'''
|| Let’s start the '''simulation''' using the following '''command'''.
|-
|| Only Narration
|| The '''simulation''' may take some time to complete.
|-
|| [Terminal] Highlight: '''End'''
|| The '''simulation''' is now complete.
|-
|| [Terminal] Type: '''paraFoam'''
|| Let’s 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 '''U '''
|| Let’s view the '''velocity contours''' for the simulation.

Click on the '''vtkBlockColors''' dropdown in the '''Active Variable Controls''' and select '''U'''.
|-
|| [ParaView] '''VCR Controls'''

Click on '''Last Frame '''
|| Let’s view the '''contours''' at the end of the simulation.

Click on the '''Last Frame''' button in the '''VCR Controls'''.
|-
|| [ParaView]

Click on '''Rescale to Visible Data Range '''
|| Click on the '''Rescale to Visible Data Range.'''
|-
|| [ParaView] '''Layout Window'''

Point to Circulation
|| We can see the '''steady-state circulation''' in the cavity.

This is an example of the '''Rayleigh-Benard convection'''.
|-
|| [ParaView] '''Close ParaView'''
|| Close the '''ParaView''' window.
|-
|| Only Narration
|| 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 '''heat transfer''' in '''OpenFOAM'''
* Simulate a '''buoyancy-driven flow''', and
* Set up '''thermophysical properties''' in '''OpenFOAM'''

|-
|| Slide: '''Assignment'''
|| As an assignment:* Increase the '''length''' of the '''cavity''' in the '''x-direction''' to '''2 m'''
* Keep all the other parameters unaltered in your '''simulation'''
* '''Simulate''' the '''flow '''in this '''rectangular cavity'''
* View the '''steady-state velocity contours'''

|-
|| 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 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: '''Acknowledgements'''
|| The Spoken Tutorial project was established by the Ministry of Education, Govt. of India.
|-
|| Only Narration
|| This tutorial is contributed by Diveysh variya, Aabhushan Regmi, Biraj Khadka, and Payel Mukharjee.

Thanks for joining.
|-
|}

OpenFOAM-version-7/C3/Parallel-Computing-in-OpenFOAM/English

2025-01-09T05:06:44Z

Evan: Created page with "'''Title of the script:''' Parallel Computing in OpenFOAM '''Script:''' Divyesh Variya, Ashuthosh Shridhar '''Video & Narration:''' John Pinto, Payel Mukherjee '''Keywords..."

'''Title of the script:''' Parallel Computing in OpenFOAM

'''Script:''' Divyesh Variya, Ashuthosh Shridhar

'''Video & Narration:''' John Pinto, Payel Mukherjee

'''Keywords:''' OpenFOAM, Parallel Computing, Hierarchical, Manual, Scotch, Simple, decomposition, mpirun, Paraview, Video-Tutorial

{|border=1
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| '''Slide 1:'''

'''Opening Slide'''
|| Welcome to this spoken tutorial on '''Parallel Computing in OpenFOAM.'''
|-
|| '''Slide 2:'''

'''Learning Objectives'''
|| In this tutorial, we will learn to,
* '''Decompose''' a domain
* '''Run''' a '''simulation''' using '''Simple decomposition '''method
* '''Reconstruct''' a domain
|-
|| '''Slide 3:'''

'''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 4:'''

'''Prerequisites'''

* If not, please go through the prerequisite '''OpenFOAM '''tutorial on '''https://spoken-tutorial.org'''
|| To practice this tutorial, learner should have,
* Basic knowledge of '''OpenFOAM '''software
* If not, please go through the prerequisite '''OpenFOAM '''tutorials on this website.
|-
|| '''Slide 5:'''

'''Parallel Computing'''
|| In''' parallel computing, '''a large domain is split into multiple '''domains''' of smaller size.

Each of the smaller domains is assigned an individual '''processor'''.

The '''processors''' run simultaneously and communicate with each other.

'''OpenFoam''' uses the '''OpenMPI''' library to do this.

Thus, we can speed up the '''simulation'''.
|-
|| '''Slide 6:'''

'''Processes Involved'''
|| There are three main processes involved in '''parallel computing.'''

* '''Decomposition''' of the '''domain.'''
* '''Simulation''' of the '''decomposed tasks''' in separate '''processors.'''
* '''Reconstruction''' of the '''domain.'''
|-
|| '''Slide 7:'''

'''Decomposition Methods'''
|| The four main '''decomposition methods''' available in OpenFOAM are:

* '''Simple'''
* '''Hierarchical'''
* '''Scotch '''and
* '''Manual'''
|-
|| Only Narration
|| Let us learn about Simple Decomposition method using a 2 Dimensional example.
|-
|| '''Slide 8:'''

'''Simple Decomposition'''
|| Simple decomposition method divides the domain''' '''in equal parts'''.'''

The splitting is done according to the user-specified '''coefficients'''.
|-
|| '''Slide 9:'''

'''Input Parameter - Simple'''
|| '''Simple decomposition''' requires two inputs.
* '''Decomposition coefficients''' and
* '''cell skewness factor, delta'''

A typical value for '''delta''' is 10 to the power of minus 3('''10^-3).'''
|-
|| '''Slide 10:'''

'''Decomposition Coefficients'''
|| '''Decomposition coefficients''' represent the number of '''subdomains''' in a particular direction.

Thus, the product of '''nx, ny, nz '''must be equal to the total number of '''subdomains.'''
|-
|| '''Slide 11:'''

'''Simple Decomposition - n (2 2 1)'''
|| This slide shows the '''decomposition domain''' for the '''decomposition coefficients''' of (2 2 1).
|-
|| '''Slide 12:'''

'''Simple Decomposition - n (4 1 1)'''
|| This slide shows the '''decomposed domain''' for the''' decomposition coefficients '''of (4 1 1).
|-
|| Only Narration
|| For more information on '''decomposition methods, '''Please refer to '''Additional Reading material.'''
|-
|| Only Narration
|| Let us set up a '''case.'''
|-
|| '''Press CTRL + ALT + T keys.'''
|| Open the '''terminal''' by pressing '''Ctrl''', '''Alt''' and '''T''' keys.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| At the '''prompt''', type this '''command''' to go to the '''run directory'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/icoFoam/cavity/cavity .'''
|| Copy the '''cavity''' '''case''' from the '''tutorial directory''' into the '''run directory'''.
|-
|| [Terminal] Type:

'''cd cavity'''
|| Navigate to the '''cavity case'''.
|-
|| [Terminal] Type:

'''blockMesh'''
|| Run the '''blockMesh''' command to execute the '''mesh'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/multiphase/interFoam/laminar/damBreak/damBreak/system/decomposeParDict system/'''
|| Copy a''' decomposeParDict''' file from''' '''the '''dam break''' '''tutorial''' to the '''system '''folder.
|-
|| Only Narration
|| To see the maximum number of '''processors''' available in your '''machine''', do the following.
|-
|| [Terminal] Type:

'''lscpu'''
|| Type '''lscpu''' on the '''terminal.'''
|-
|| [gedit - '''terminal'''] Highlight

'''CPU(s): 24'''
|| My '''machine''' has '''24 CPUs .'''
|-
|| [gedit - '''terminal'''] Highlight

'''Thread(s) per core…. 2'''
|| '''12 physical cores''' per '''socket '''and '''2 threads''' per '''physical core.'''
|-
|| '''Slide 13:'''

'''Number of processors'''
|| Multiplication of these 3 quantities gives the number of '''logical cores.'''

This is equal to the maximum number of '''processors'''.
|-
|| Only Narration
|| We will run this case in 4''' processors'''.
|-
|| Only Narration
|| Note:

Please assign at least 4 processors to your Virtual Machine.
|-
|| [Terminal] Type:

'''gedit system/decomposeParDict'''
|| Open the '''decomposeparDict '''in a '''text editor.'''
|-
|| [gedit '''decomposeParDict'''] Highlight numberOfSubdomains '''4'''<nowiki>;</nowiki>
|| The '''number of subdomains '''is defined as '''4.'''
|-
|| [gedit '''decomposeParDict''']

'''method simple;'''
|| '''Simple''' method of decomposition is being used.
|-
|| [gedit '''decomposeParDict'''] Highlight '''coeffs'''
|| Go to '''coeffs sub-dictionary.'''
|-
|| [gedit '''decomposeParDict''': Highlight '''n'''
|| '''n '''represents the Decomposition coefficients in each direction.

I will modify''' n '''so that we have:
* 2 '''divisions''' in '''x''' and''' y''' directions.
* And 1 division in '''z '''direction.
|-
|| [gedit '''decomposeParDict''']

Save >> Close the window
|| '''Save''' and Close the file.
|-
|| [Terminal] Type:

'''decomposePar -cellDist'''
|| To '''decompose '''the '''domain''', type the following '''command.'''
|-
|| [Terminal] Highlight:

'''cellDist'''
|| The argument '''cellDist''' writes a file named '''cellDecomposition''' inside the '''constant''' folder.

This file contains the details of the '''processor '''allocation.
|-
|| Only Narration
|| The '''domain''' is decomposed.
|-
|| Only Narration
|| The '''command''' '''decomposePar''' creates a directory for each '''processor'''.

These directories contain the '''subdomain''' and the corresponding''' geometric fields.'''
|-
|| [Terminal] Type:

'''ls'''
|| Type '''ls''' to view the folders assigned to each '''processor.'''
|-
|| [cavity - '''directory'''] Highlight

'''Processor0 …..Processor3'''
|| Since we use''' '''4''' processors''', we have 4''' processor''' directories.
|-
|| [Terminal] Type:

'''ls processor0'''
|| Type '''ls''' '''processor0 '''to view the content of''' processor0.'''
|-
|| [Terminal] Highlight

'''0 constant'''
|| It contains the '''0''' and '''constant '''directories.
|-
|| Point to '''0 directory'''.

Point to '''Constant directory'''.
|| '''0''' directory contains the '''decomposed geometric field'''.

The''' Constant '''directory contains the '''decomposed mesh files.'''
|-
|| [Terminal] Type:

'''gedit constant/cellDecomposition'''
|| Open the''' cellDecomposition '''file from the Constant folder in a '''text editor.'''
|-
|| [gedit - '''cellDecomposition'''] Highlight '''400'''
|| The number on the first line represents the number of '''cells''' in the '''domain.'''
|-
|| [gedit - '''cellDecomposition'''] Highlight

'''(.......'''
|| The entries within the bracket represent the '''processor''' number.
|-
|| [gedit - '''cellDecomposition'''] Highlight

'''0'''
|| '''0''' here indicates the '''processor''' number that is assigned to the corresponding '''cell.'''
|-
|| [gedit - '''cellDecomposition''']

Close the window
|| Close the file.
|-
|| Only Narration
|| Let’s view the '''subdomains''' in '''paraview.'''
|-
|| [Terminal] Type:

'''paraFoam'''
|| Type '''paraFoam '''on the '''terminal.'''
|-
|| [ParaView] Uncheck:

'''Properties Tab >> Scroll Down - Mesh Parts >> Uncheck fixedWalls & movingWall'''
|| Uncheck all other fields other than '''internalMesh''' from '''Mesh Parts'''.
|-
|| [ParaView] Click:

'''Properties Tab >> Scroll Down - Fields'''

'''>> check cellDist'''
|| Check all '''Volume Fields''' in the '''Properties tab'''.
|-
|| [ParaView] Click:

'''Apply'''
|| Click on the '''Apply''' button in the '''Properties tab.'''
|-
|| [ParaView]

'''Click on Solid Color >> Click on cell Dist'''
|| Click on '''Solid Color '''available in the '''Active Variable'''

'''Controls.'''

Select '''cellDist''' with a '''block''' from the '''menu.'''
|-
|| Point to the dark blue block and the light blue block.

Point to the beige block and the maroon block.
|| One can see the divided''' '''domain.

The '''dark blue''' '''block''' belongs to '''processor number 0'''

The''' light blue''' '''block''' belongs to '''processor number 1'''

The '''beige block''' belongs to '''processor number 2''',

And the''' maroon '''belongs to '''processor number 3'''
|-
|| ['''paraview''']

Close the window
|| Close the '''ParaView''' window.
|-
|| '''Slide 14:'''

'''Command - Parallel run'''
|| '''OpenFOAM '''uses''' '''the '''openMPI '''library for '''parallelization'''.

* '''mpirun''' is the '''process''' '''launcher'''.
* The '''argument''' '''np''' represents the number of '''processors'''.
* In our case we use '''4 processors.'''
* Then the name of the '''application '''entered.
* We need to specify that the '''application''' has to be run in '''parallel'''.
* The '''output''' of the '''simulation''' is written in a file named '''log.'''
* This is done by using the '''right''' '''angle''' '''bracket'''.
* The '''&''' indicates that the '''process''' will be '''run''' in the '''background'''.

This allows us to use the current '''terminal''' when the '''application''' is '''running'''.
|-
|| [Terminal] Type:

'''mpirun -np 4 icoFoam -parallel > log &'''
|| Type this '''command''' in the '''terminal.'''
|-
|| [Terminal] Type:

'''tail log'''
|| Type the following '''command''' to view the end of the '''log '''file.
|-
|| [Terminal]

Highlight''' End'''
|| The '''simulation '''is complete.
|-
|| Only Narration
|| To post-process the case, we need to '''reconstruct''' the domain.
|-
|| [Terminal] Type:

'''reconstructPar'''
|| To do that, type''' reconstructPar''' in the '''terminal.'''
|-
|| [Terminal] Type:

'''ls'''
|| Type''' ls'''
|-
|| [Terminal] Highlight

'''0.5'''
|| The end time directory is reconstructed.
|-
|| '''Slide 15:'''

'''Summary'''
|| With this we come to the end of this tutorial. Let us summarize.

In this tutorial, we have learned to,
* '''Decompose''' a domain
* Run''' '''the simulation using the '''simple decomposition method'''
* '''Reconstruct''' a '''domain'''
|-
|| '''Slide 16:'''

'''Assignment'''
|| As an assignment:

Simulate the same '''case''' using,
* '''Simple decomposition''' with '''2''' '''processor'''
* '''Scotch decomposition''' with '''processor weight'''
|-
|| '''Slide 17:'''

'''About the Spoken Tutorial Project'''
|| The video at the following link summarizes the Spoken Tutorial project.

Please download and watch it.
|-
|| '''Slide 18:'''

'''Spoken Tutorial Workshops'''
|| We conduct workshops using Spoken Tutorials and give certificates.

Please contact us.
|-
|| '''Slide 19:'''

'''Spoken Tutorial Forum'''
|| Please post your timed queries in this forum.
|-
|| '''Slide 20:'''

'''FOSSEE Forum'''
||
* Do you have any general/technical questions?
* Please visit the forum given in this link.
|-
|| '''Slide 21:'''

'''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 22: Spoken Tutorial'''
|| Spoken Tutorial project was established by the Ministry of Education, Govt. of India

This tutorial is contributed by Divyesh Varya, Nishit Pachpande, John Pinto and Payel Mukherjee from IIT Bombay.

Thank you for joining.
|-
|}

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

2025-01-02T06:35:48Z

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..."

'''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.

|-
|}