View source for OpenFOAM-version-7/C3/Heat-source-addition-in-a-simulation-using-buoyantSimpleFoam/English

'''Title of the script''': Heat source addition to buoyantSimpleFoam

'''Author''': Mano Prithvi Raj, Binayak Lohani, Biraj Khadka

'''Keywords''': OpenFOAM, ParaView, CFD, computational fluid dynamics, blockMesh, buoyancy driven flow, heat transfer, heat source, topoSetDict, fvModels, buoyantSimpleFoam, thermophysical properties, FOSSEE, spoken tutorial, video tutorial

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

'''Opening Slide'''
| Welcome to the spoken tutorial on '''Heat''' '''source addition to buoyantSimpleFoam.'''
|-
|
'''Slide:'''

'''Learning Objective'''
|
In this tutorial, we will learn to:

<ul>
<li><blockquote><p>Set up a case of '''heat transfer''' in '''OpenFOAM'''</p></blockquote></li>
<li><blockquote><p>Simulate a '''buoyancy-driven flow''' with a heat source, and</p></blockquote></li>
<li><blockquote><p>Set up '''topoSetDict''' and '''fvModels''' in '''OpenFOAM'''</p></blockquote></li></ul>
|-
|
'''Slide:'''

'''System Specifications'''
|
To record this tutorial, I am using,

<ul>
<li><blockquote><p>'''Ubuntu Linux''' OS version 22.04</p></blockquote></li>
<li><blockquote><p>'''OpenFOAM''' version 9</p></blockquote></li>
<li><blockquote><p>'''ParaView''' version 5.6.0, and</p></blockquote></li>
<li><blockquote><p>'''gedit''' Text editor</p></blockquote></li></ul>

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

'''Prerequisites'''

<ul>
<li><blockquote><p>If not, please go through the prerequisite '''OpenFOAM''' tutorials on https://spoken-tutorialorg</p></blockquote></li></ul>
|
As a prerequisite:

<ul>
<li><blockquote><p>You should have basic knowledge of '''convective heat transfer'''</p></blockquote></li>
<li><blockquote><p>You should be familiar with setting up a '''case''' in '''OpenFOAM'''</p></blockquote></li>
<li><blockquote><p>If not, please go through the prerequisite '''OpenFOAM''' tutorials on this website</p></blockquote></li></ul>
|-
|
'''Slide:'''

'''Code Files'''
|
<ul>
<li><blockquote><p>The files used in this tutorial are available in the '''Code''' '''Files''' link on this tutorial page</p></blockquote></li>
<li><blockquote><p>Please download and extract them</p></blockquote></li>
<li><blockquote><p>Make a copy and then use them while practicing</p></blockquote></li></ul>
|-
|
'''Slide:'''

'''Problem Statement'''
|
We will be solving a '''2D flow''' in a square '''cavity'''

'''Top wall''' is moving other '''3 walls''' of the '''cavity''' are fixed
|-
|
'''Slide:'''

'''Problem Statement'''
|
<ul>
<li><blockquote><p>'''Bottom wall''' is maintained at a higher temperature compared to the '''top wall'''</p></blockquote></li>
<li><blockquote><p>The '''side walls''' are '''adiabatic'''</p></blockquote></li></ul>
|-
|
'''Slide:'''

'''Problem Statement'''
|
<ul>
<li><blockquote><p>A '''2D''' rectangular '''heat source''' of 100 '''Watts''' is added in the middle of the cavity</p></blockquote></li></ul>
|-
|
'''Slide:'''

'''Problem Statement'''
|
<ul>
<li><blockquote><p>'''Gravity''' is acting downwards, in the '''negative y-direction'''</p></blockquote></li></ul>

<ul>
<li><blockquote><p>Inside the '''cavity''', the fluid close to the '''hot wall''' at the bottom is lighter</p></blockquote></li></ul>

<ul>
<li><blockquote><p>Fluid close to the '''cold wall''' on the top is heavier</p></blockquote></li></ul>

<ul>
<li><blockquote><p>Moving '''top wall''' creates '''circulation''' in '''cavity''' due to '''density''' and '''shear flow''' difference</p></blockquote></li>
<li><blockquote><p>The addition of '''heat source''' and its magnitude affects the '''circulation''' of fluid</p></blockquote></li></ul>
|-
| Only Narration
| Let’s '''simulate''' this problem in '''OpenFOAM'''
|-
| '''CTRL + ALT + T'''
| 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: '''cp -r ~/Downloads/sourceAddition'''
|
I have downloaded and extracted the '''case folder''' to the '''Downloads''' folder

Let’s copy it into the '''run directory'''
|-
|
[Terminal] Type:

'''cd sourceAddition'''
| Let’s move into the '''case folder''' using the '''cd''' '''command'''
|-
|
'''Slide:'''

'''Geometry'''
|
<ul>
<li><blockquote><p>In this '''simulation''', we consider a '''square cavity''' with an '''edge length''' of '''1 m'''</p></blockquote></li>
<li><blockquote><p>There will be a '''heat source''' in the middle of the '''square cavity'''</p></blockquote></li>
<li><blockquote><p>The magnitude of '''power Q''' is '''100 Watts'''</p></blockquote></li></ul>
|-
| '''Slide: Boundaries'''
| The '''computational domain''' has '''4 boundaries''',
|-
|
'''Slide:'''

'''Boundary Conditions'''
| The '''boundary conditions''' used in the '''simulation''' are as shown in the table
|-
| Only Narration
| Let’s see how the '''boundary conditions''' are defined.
|-
|
[Terminal] Type:

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

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

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

One is the '''pressure file''', '''p''' and other is '''modified pressure file''', '''p_rgh'''

The significance of '''p_rgh''' has been explained earlier.
|-
| [Terminal] Type: '''gedit 0/T'''
| Let’s first open the '''temperature file''', '''T'''
|-
|
[gedit - '''T'''] Highlight:

'''internalField uniform 1''' [https://imgur.com/iDwsCri.png <span class="underline">Link</span>]
| The '''domain''' is '''initialised''' with '''1 K'''
|-
|
[gedit - '''T'''] Highlight: [https://imgur.com/J0KUmot.png <span class="underline">Link</span>]

'''bottom''' boundary condition
| The '''bottom wall''' is maintained at a constant temperature of '''1 K'''
|-
|
[gedit - '''T'''] Highlight: [https://imgur.com/G3JaouD.png <span class="underline">Link</span>]

'''top''' boundary condition
| The '''top wall''' is maintained at a temperature of '''0 K'''
|-
|
[gedit - '''T'''] Highlight: [https://imgur.com/5UflERt.png <span class="underline">Link</span>]

'''left''' &amp; '''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: [https://imgur.com/kp8xjSs.png <span class="underline">Link</span>]

all '''walls''' boundary condition
| All '''4 walls''' have been assigned the '''fixedFluxPressure''' '''boundary condition'''
|-
|
[gedit - '''p_rgh'''] Highlight: [https://imgur.com/kp8xjSs.png <span class="underline">Link</span>]

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

Therefore, we will be using 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: [https://imgur.com/FW5pj5M.png <span class="underline">Link</span>]

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: [https://imgur.com/R2wzPxe.png <span class="underline">Link</span>]

'''value $internalField;'''
|
The '''type calculated''', '''value''' is just a '''placeholder''' for the first '''time-step'''

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

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

'''topoSetDict'''
| We see the '''topoSetDict''' file in the '''system''' folder
|-
|
'''Slide:'''

'''topoSetDict'''
|
<ul>
<li><blockquote><p>'''topoSetDict''' is used to select cells, faces or points in the computational domain</p></blockquote></li>
<li><blockquote><p>'''topoSetDict''' is used to select a set of cells to define the location of '''heat source'''</p></blockquote></li></ul>
|-
| [Terminal] Type: '''gedit system/topoSetDict'''
| Let’s open the '''topoSetDict''' file
|-
|
[gedit - '''topoSetDict'''] Highlight:

'''Actions''' [https://i.imgur.com/i1Cy0QH.png <span class="underline">Link</span>]
|
<ul>
<li><blockquote><p>'''addedHeatSource''' is the name of the cellSet</p></blockquote></li>
<li><blockquote><p>The dimensions of the box for the '''boxToCell''' option are defined under '''sourceInfo'''</p></blockquote></li>
<li><blockquote><p>Let’s see how the box dimensions are defined</p></blockquote></li></ul>
|-
|
'''Slide:'''

'''boxToCell'''
|
<ul>
<li><blockquote><p>Here, we can see the domain, and the region where heat source is to be applied</p></blockquote></li>
<li><blockquote><p>'''boxToCell''' option chooses all the cells inside the box region for the '''cellSet'''</p></blockquote></li></ul>
|-
|
'''Slide:'''

'''boxToCell'''
|
Box is defined as below

Smallest coordinates are mentioned first followed by the greatest coordinates
|-
|
[gedit - '''topoSetDict'''] Highlight:

'''actions''' [https://i.imgur.com/bCzN8aa.png <span class="underline">Link</span>]
|
<ul>
<li><blockquote><p>In our case, the coordinates would be '''(0.4 0.4 -0.1''') followed by '''(0.6 0.6 0.1)'''</p></blockquote></li></ul>
|-
| [gedit - '''topoSetDict'''] Close the window
| Close the '''topoSetDict''' 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 4 files in the '''constant''' folder
|-
|
'''Slide:'''

'''constant Folder'''
|
<ul>
<li><blockquote><p>'''fvModels''' file contains the '''source term''' type and magnitude</p></blockquote></li>
<li><blockquote><p>The '''g''' file contains the details of the '''gravitational force'''</p></blockquote></li>
<li><blockquote><p>The '''momentumTransport''' file contains the details of '''turbulence properties'''</p></blockquote></li>
<li><blockquote><p>The '''thermophysicalProperties''' file contains the '''properties''' of the '''fluid''' used</p></blockquote></li></ul>
|-
|
'''Slide:'''

'''fvModels'''
|
<ul>
<li><blockquote><p>'''fvModels''' file is used to add source terms to the governing equations of solvers</p></blockquote></li>
<li><blockquote><p>The '''source term''' can be a '''heat source''', a '''mass source''', a '''damping source''' etc.</p></blockquote></li>
<li><blockquote><p>Here, the '''fvModels''' file is used to add a heat source</p></blockquote></li></ul>
|-
| [Terminal] Type: '''gedit constant/fvModels'''
| Let’s open the '''fvModels''' file
|-
|
[gedit - '''fvModels'''] Highlight:

'''source''' [https://i.imgur.com/o4Ey8mm.png <span class="underline">Link</span>]
|
<ul>
<li><blockquote><p>'''heatSource''' is the type of the source term</p></blockquote></li>
<li><blockquote><p>'''addedHeatSources''' is the cellSet previously assigned in '''topoSetDict'''</p></blockquote></li>
<li><blockquote><p>The magnitude of '''Q''' is '''100 Watts'''</p></blockquote></li></ul>
|-
| [gedit - '''fvModels'''] Close the window
| Close the '''fvModels''' file
|-
| [Terminal] Type: '''gedit constant/g'''
| Let’s open the '''g''' file
|-
|
[gedit - '''g'''] Highlight:

'''value (0 -10 0)''' [https://imgur.com/D0nNzya.png <span class="underline">Link</span>]
|
Since '''g''' is a '''vector''', its '''velocity''' and '''magnitude''' have to be specified

In this case, the '''magnitude''' of '''g''' is '''10''' '''m/s<sup>2</sup>'''

Its direction is in the '''negative y-direction'''
|-
| [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''' [https://imgur.com/xwMHcng.png <span class="underline">Link</span>]
| 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
|-
| Only Narration
|
In this file, '''properties''' of the '''fluid''' used in our '''simulation''' are specified

We’ll be '''simulating''' the '''flow''' inside the '''cavity'''
|-
| [gedit - '''thermophysicalProperties'''] Highlight: '''thermoType''' field [https://imgur.com/HuO1iqI.png <span class="underline">Link</span>]
|
'''OpenFOAM''' contains various '''thermophysical''' modeling packages

The '''thermoType''' assembles the various '''thermophysical''' modeling packages
|-
| Only Narration
|
The '''additional reading material''' has more details on the '''thermophysical''' modeling 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''' [https://imgur.com/iV7ahAQ.png <span class="underline">Link</span>]
| We will be using the '''Boussinesq approximation''' for the '''equation of state'''
|-
| [gedit - '''thermophysicalProperties'''] Highlight: '''molWeight 28.9''' [https://imgur.com/ipqEFKC.png <span class="underline">Link</span>]
| The '''molecular weight''' of the fluid is specified as '''28.9 g/mol'''
|-
| Only Narration
| '''Reference density''' and '''coefficient of volumetric expansion''' are fluid properties
|-
|
'''Slide:'''

'''Reference Temperature'''
|
The '''reference temperature''' depends on the problem being solved

In our case, it is taken as 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: '''rho0 1;'''

'''T0 0.5;''' [https://imgur.com/k74Qbpk.png <span class="underline">Link</span>]
|
For the fluid in our '''simulation''', '''reference density''' is specified as '''1 kg/m<sup>3</sup>'''

This is the '''reference density''' at a '''reference temperature''' of '''0.5 K'''
|-
| [gedit - '''thermophysicalProperties'''] Close the window
| Close the '''thermophysicalProperties''' file
|-
| [Terminal] Type: '''blockMesh'''
| Let’s '''mesh''' the geometry using the '''blockMesh''' '''command'''
|-
| [Terminal] Type: '''topoSet'''
| Let’s create the '''heat source cell set''' using the '''topoSet''' '''command'''
|-
| [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''' &gt;&gt; Click on '''T''' [https://imgur.com/VsCcHFW.png <span class="underline">Link</span>]
|
Let’s view the '''temperature contours''' for the simulation

Click the '''vtkBlockColors''' dropdown in the '''Active Variable Controls''' and select '''T'''
|-
|
[ParaView] '''VCR Controls'''

Click on '''Last Frame''' [https://imgur.com/4Hto0ab.png <span class="underline">Link</span>]
|
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''' [https://imgur.com/LoR0dmo.png <span class="underline">Link</span>]
| Click on '''Rescale to Visible Data Range'''
|-
|
[ParaView] '''Active Variable Controls'''

Click on '''vtkBlockColors''' &gt;&gt; Click on '''U''' [https://imgur.com/VsCcHFW.png <span class="underline">Link</span>]
|
Let’s view the '''velocity contours''' for the simulation

Click the '''vtkBlockColors''' dropdown in the '''Active Variable Controls''' and select '''U'''

Ensure that you click on '''U''' option with a '''point icon''' and not the '''box icon'''
|-
|
[ParaView] '''Layout Window'''

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

<ul>
<li><blockquote><p>Set up a case of '''heat transfer''' in '''OpenFOAM'''</p></blockquote></li>
<li><blockquote><p>Simulate a '''buoyancy-driven flow''' with a heat source, and</p></blockquote></li>
<li><blockquote><p>Set up '''topoSetDict''' and '''fvModels''' in '''OpenFOAM'''</p></blockquote></li></ul>
|-
|
'''Slide:'''

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

<ul>
<li><blockquote><p>Increase the '''length''' of the '''cavity''' in the '''x-direction''' to '''2 m'''</p></blockquote></li>
<li><blockquote><p>Change the magnitude of '''heat source''' to '''200 Watts'''</p></blockquote></li>
<li><blockquote><p>'''Simulate''' the '''buoyancy driven''' '''flow''' in a '''rectangular cavity'''</p></blockquote></li></ul>
|-
|
'''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'''
|
<ul>
<li><blockquote><p>Do you have any general/technical questions?</p></blockquote></li>
<li><blockquote><p>Please visit the forum given in the link</p></blockquote></li></ul>
|-
|
'''Slide:'''

'''FOSSEE Case Study Project'''
|
<ul>
<li><blockquote><p>The FOSSEE team coordinates solving feasible CFD problems of reasonable complexity using OpenFOAM</p></blockquote></li>
<li><blockquote><p>We give honorarium and certificates to those who do this</p></blockquote></li>
<li><blockquote><p>For more details, please visit these sites</p></blockquote></li></ul>
|-
|
'''Slide:'''

'''Acknowledgements'''
| The Spoken Tutorial Project was established by the Ministry of Education, Govt. of India
|-
| Only Narration
| This tutorial is contributed by Mano Prithvi Raj, Binayak Lohani, Biraj Khadka and Payel Mukherjee from IIT Bombay Thanks for joining
|}