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

'''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/s<sup>2'''</sup>.
|- 
|| [gedit - '''g'''] Highlight:


'''value (0 -10 0) '''
|| The '''magnitude''' of '''g''' is '''10''' '''m/s<sup>2'''</sup>.
|- 
|| [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/m<sup>3'''</sup>.


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<sup>-2</sup> K<sup>-1'''</sup>.
|- 
|| [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.
|-
|}