View source for OpenFOAM-version-7/C2/Simulation-a-2D-Turbulent-Flow-in-a-Channel-using-OpenFOAM/English

'''Title of the script:''' Simulation of a Turbulent Flow in a 2D Channel using OpenFOAM

'''Author:''' Padmini Priyadarshini

'''Keywords:''' OpenFOAM, Turbulence, k-epsilon, yplus, expansion ratio, blockMesh, wall function, channel flow, simpleFoam, ParaView, video tutorial



{| border = "1"
|- 
|| '''Visual Cue'''
|| '''Narration'''
|- 
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Simulation of Turbulent Flow in a 2D Channel using OpenFOAM.'''
|- 
|| Slide: Learning Objective
|| In this tutorial, we will learn how to:
* Implement '''k-epsilon model'''
* Set up '''turbulence''' '''parameters'''
* '''Run '''the '''simulation'''
|- 
|| Slide: System Specifications
|| To record this tutorial, I am using,
* '''Linux Mint OS''' version 18.3
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0
* '''gedit Text Editor'''

However, you may use any other '''text editor''' of your choice.

The steps explained in this tutorial are identical in '''Ubuntu Linux OS'''.
|-
|| 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 '''turbulent flows''' and '''fluid dynamics'''.
* You should also be familiar with '''simulating''' a '''flow''' through a '''pipe''' 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: Solver detail
|| We will use the '''simpleFoam solver''' to '''simulate''' this problem.


'''simpleFoam''' is a '''steady-state solver''' for '''incompressible''', '''turbulent flow'''.
|-
|| Slide: Problem statement
|| The diagram shows a''' 2D channel '''of length '''65 m '''and width '''1 m'''.


The '''kinematic viscosity''' is '''1e-05 m<sup>2</sup>/s  (1e to the power of minus 5 metre squared per second).'''


The '''Inlet velocity '''is '''20 metres per second. '''


'''Outlet pressure '''is set to '''0 atmosphere.'''
|-
|| Slide: Flow Properties
|| '''Reynolds number''' is '''2 million'''.


And the '''flow''' is '''turbulent.'''
|- 
|| Slide: K-Epsilon turbulence model
|| '''K-epsilon '''is a widely used '''RAS''' '''turbulence model.'''


It is a '''two-equation model'''.


It solves:
* The '''turbulent kinetic energy''' '''transport equation''', and
* The '''turbulent dissipation rate transport''' '''equation'''
|- 
|| Only Narration
|| Let us set up the '''case.'''
|-
|| Only Narration
|| Download the '''kepsilon '''folder provided in the '''Code file''' and extract it.
|-
|| CTRL + ALT + T
|| Open the '''terminal''' by pressing '''Ctrl''', '''Alt''' & '''T''' keys.
|-
|| [Terminal]

Only Narration
|| From now onwards please remember to press the '''Enter''' key after typing each '''command '''in the''' Terminal.'''
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| Let us''' '''open the '''RUN directory'''.


To do so, type the following '''command.'''
|-
|| [Terminal] Type:

'''cp -r ~/Downloads/kepsilon .'''
|| And copy the downloaded file into the '''RUN directory'''.


To do so, type the following '''command.'''
|-
|| Only Narration 
|| I have downloaded the file into my '''Downloads directory.'''


Please change the '''path''' as per your machine.
|-
|| [Terminal] Type:

'''cd kepsilon'''
|| With this '''command''', we will navigate to the '''kepsilon directory'''.
|-
|| Slide: Y plus
|| '''YPlus '''is the '''dimensionless wall distance.'''


For '''wall function''' '''approach,''' '''yplus''' value should be between '''30 '''and '''300.'''
|-
|| Slide: Wall distance, yp
|| Let “'''yp'''” be the distance between the '''wall''' and the nearest '''cell centre.'''


For our '''case, yp''' is '''0.00155''' for a '''yplus''' value of '''100.'''


For '''channel flow, '''the''' skin friction coefficient, Cf''' is given by this formula.
|-
|| Only Narration
|| The '''Additional Reading Material''' has more details on the''' wall function approach'''.


It mentions the steps used to calculate '''yp'''.
|-
|| [Terminal] Type:


'''ls system'''
|| Type the following''' command''' to view the content of the '''system directory'''.
|-
|| [Terminal] Highlight: 


'''blockMeshDict'''
|| This '''directory''' contains the '''blockMeshDict''' file.
|-
|| Only Narration
|| I have already set up the '''blockMesh''' file for a '''2D multi-block channel '''with this''' yp value'''.
|-
|| Only Narration
|| Let us take a look at the''' initial''' and '''boundary conditions''' of the '''flow variables.'''
|-
|| Slide: Inlet Boundary Condition - k
|| Let us take a look at the '''inlet boundary condition '''for '''kappa.'''


We will use '''turbulentIntensityKineticEnergyInlet'''


This calculates''' kappa '''using the user-specified '''turbulence intensity'''.


For our '''case, turbulent intensity''' is '''0.0261 '''and '''Turbulent kinetic energy''' is '''0.41 m<sup>2</sup>/s<sup>2'''</sup> (metre squared per second squared)
|-
|| Slide: Inlet Boundary Condition - epsilon



|| Let us take a look at the '''inlet boundary condition '''for '''epsilon.'''


We will use '''turbulentMixingLengthDissipationRateInlet '''


This calculates '''epsilon''' using '''kappa '''and user-specified '''mixingLength'''.


'''mixingLength '''refers to the''' turbulent length scale.'''


'''Kappa''' value is automatically put in by the '''solver'''.


Here, the''' turbulent length scale''' is '''0.07 m'''.


And, the value of the '''turbulent dissipation rate''' is '''0.61 m<sup>2</sup>/s<sup>3'''</sup> (metre squared per seconds cubed)
|-
|| Slide: Wall Boundary Condition 
|| Next, let us take a look at the '''wall boundary conditions '''to be used. 


* '''turbulent kinetic energy '''is set to '''kqRWallFunction '''
* '''turbulent dissipation '''is set to '''epsilonWallFunction'''
|-
|| Slide: Outlet Boundary Condition 
|| This slide shows the '''outlet boundary condition.'''


'''zeroGradient boundary condition''' is imposed at the '''outlet '''for both '''parameters'''.
|-
|| Slide: Kinematic eddy viscosity, nut
|| '''Kinematic eddy viscosity''' is a dependent '''variable'''.


Hence, its value is calculated by the''' solver'''.


At the '''wall, nutWallFunction''' is used.
|-
|| Only Narration
|| The '''Additional Reading Material''' has more details on the '''boundary conditions'''.


Please refer to it.


Let us take a look at the '''boundary''' and '''initial conditions''' for '''turbulent kinetic energy'''.
|-
|| [Terminal] Type:


'''gedit 0/k'''
|| Open the '''k''' file in a '''text editor.'''
|-
|| [gedit -'''k'''] Highlight: 


'''internalField uniform 0.41;'''
|| The''' internalField''' is initialised as '''0.41'''
|-
|| [gedit -'''k'''] Highlight:''' '''


'''type turbulentIntensityKineticEnergyInlet'''
|| The''' inlet boundary type''' is set to '''turbulentIntensityKineticEnergyInlet'''
|-
|| [gedit -'''k'''] Highlight:''' '''


'''intensity 0.0261;'''
|| The '''keyword intensity '''represents the '''turbulent intensity''', and is set to '''0.0261'''
|-
|| [gedit -'''k'''] Highlight: 


'''value $internalField;'''
|| We have passed the '''internalField''' value to the '''patch field''' value.
|-
|| [gedit -'''k'''] Highlight: 


'''zeroGradient;'''
|| '''outlet''' is set to '''zeroGradient.'''
|-
|| [gedit -'''k'''] Highlight: 


'''kqRWallFunction'''
|| The '''patch type''' for both walls are set to '''kqRWallFunction'''.
|-
|| [gedit -'''k'''] Highlight: 


'''value $internalField; '''
|| The''' internalField''' value is passed to the '''patch field '''value.
|-
|| [gedit -'''k'''] Highlight: 


'''type empty;'''
|| The '''frontAndBack patch '''is set as '''empty.'''
|-
|| [gedit - '''k'''] Close Text Editor
|| Close the '''k''' file.
|-
|| Only Narration
|| Let’s take a look at the '''epsilon''' file.
|-
|| [Terminal] Type: 


'''gedit 0/epsilon'''
|| Open the '''epsilon''' file in a '''text editor.'''
|-
|| [gedit -'''epsilon'''] Highlight: 


'''0.61'''
|| The '''internalField '''value is initialized to '''0.61'''
|-
|| [gedit -'''epsilon'''] Highlight: 


'''turbulentMixingLengthDissipationRateInlet'''
|| The '''inlet type''' is defined as '''turbulentMixingLengthDissipationRateInlet'''
|-
|| [gedit -'''epsilon'''] Highlight: 


'''0.07'''
|| The field''' mixingLength''' is set to '''0.07'''
|-
|| [gedit -'''epsilon'''] Highlight: 


'''$internalField'''
|| The '''internalField''' value is passed to the '''patch field '''value.
|-
|| [gedit -'''epsilon'''] Highlight: 


'''zeroGradient'''
|| The '''outlet patch''' is defined as '''zeroGradient.'''
|-
|| [gedit -'''epsilon'''] Highlight: 


'''epsilonWallFunction'''
|| The '''wall patch type '''is set to '''epsilonWallFunction.'''
|-
|| [gedit - e'''psilon'''] Close Text Editor
|| Close the '''epsilon''' file.
|-
|| [Terminal] Type:


'''gedit 0/nut'''
|| Now, let’s open the '''nut '''file in a '''text editor.'''
|-
|| [gedit -'''nut'''] Highlight: 


'''calculated'''
|| The '''inlet''' and '''outlet patches''' are set to '''calculated.'''
|-
|| [gedit -'''nut'''] Highlight: 


'''type nutkWallFunction;'''
|| The '''wall patch type '''is set as '''nutkWallFunction'''.
|-
|| [gedit - '''nut'''] Close Text Editor
|| Close the '''nut''' file.
|-
|| [Terminal] Type: 


'''gedit 0/U'''
|| Next, open the '''velocity '''file in a '''text editor.'''
|-
|| [gedit -'''U'''] Highlight: 


'''(20 0 0)'''
|| The '''inlet patch''' is given a fixed value of '''20 '''along the axis.
|-
|| [gedit -'''U'''] Highlight: 


'''zeroGradient'''
|| The '''outlet patch''' is set to '''zeroGradient.'''
|- 
|| [gedit -'''U]''' Close Text Editor
|| Close the '''U''' file.
|- 
|| Only Narration
|| The '''case '''is ready to be '''run. '''
|-
|| [Terminal] Type: 


'''blockMesh'''
|| Type '''blockMesh''' to '''mesh''' the geometry.
|-
|| [Terminal] Type: 


'''simpleFoam'''
|| Type '''simpleFoam''' in the '''terminal.'''
|-
|| Only Narration
|| The '''simulation''' will take some time depending on your computer’s '''hardware'''.
|-
|| [Terminal] Highlight:


'''End'''
|| The word '''End''' indicates that the '''simulation''' has finished successfully.
|-
|| Slide: Outlet Velocity Profile 
|| The slide shows the '''velocity profile''' at the '''channel exit.'''
|-
|| Only Narration
|| With this we have come to the end of the tutorial.


Let us summarize.
|- 
|| Slide: Summary
|| In this tutorial, we learnt to,
* Implement '''k-epsilon turbulence model'''
* Set up the''' initial '''and '''boundary conditions''' for''' turbulence parameters'''
* '''Run''' the '''simulation'''
|-
|| Slide: Assignment
|| As an assignment:
* Change the '''inlet boundary condition''' for '''kappa '''and''' epsilon''' to''' fixedValue'''
* Repeat the '''simulation''' for a '''velocity '''value of '''40 m/s''', change '''kappa '''and '''epsilon''' accordingly
|-
|| 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: Spoken Tutorial 
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.


The script for this tutorial is contributed by Padmini.


And this is Swetha from IIT Bombay signing off.


Thank you for joining.
|-
|}