Script | Spoken-Tutorial - User contributions [en]

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

2024-01-08T10:50:08Z

Biraj: Created page with "'''Title of the script''': Heat source addition to buoyantSimpleFoam '''Author''': Mano Prithvi Raj, Binayak Lohani, Biraj Khadka '''Keywords''': OpenFOAM, ParaView, CFD, co..."

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

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

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

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

'''Prerequisites'''

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

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

'''Code Files'''
|
<ul>
<li><blockquote>The files used in this tutorial are available in the '''Code''' '''Files''' link on this tutorial page</blockquote></li>
<li><blockquote>Please download and extract them</blockquote></li>
<li><blockquote>Make a copy and then use them while practicing</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>'''Bottom wall''' is maintained at a higher temperature compared to the '''top wall'''</blockquote></li>
<li><blockquote>The '''side walls''' are '''adiabatic'''</blockquote></li></ul>
|-
|
'''Slide:'''

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

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

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

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

<ul>
<li><blockquote>Moving '''top wall''' creates '''circulation''' in '''cavity''' due to '''density''' and '''shear flow''' difference</blockquote></li>
<li><blockquote>The addition of '''heat source''' and its magnitude affects the '''circulation''' of fluid</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>In this '''simulation''', we consider a '''square cavity''' with an '''edge length''' of '''1 m'''</blockquote></li>
<li><blockquote>There will be a '''heat source''' in the middle of the '''square cavity'''</blockquote></li>
<li><blockquote>The magnitude of '''power Q''' is '''100 Watts'''</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 Link]
| The '''domain''' is '''initialised''' with '''1 K'''
|-
|
[gedit - '''T'''] Highlight: [https://imgur.com/J0KUmot.png Link]

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

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

'''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: [https://imgur.com/kp8xjSs.png Link]

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

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 Link]

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 Link]

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

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

'''boxToCell'''
|
<ul>
<li><blockquote>Here, we can see the domain, and the region where heat source is to be applied</blockquote></li>
<li><blockquote>'''boxToCell''' option chooses all the cells inside the box region for the '''cellSet'''</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 Link]
|
<ul>
<li><blockquote>In our case, the coordinates would be '''(0.4 0.4 -0.1''') followed by '''(0.6 0.6 0.1)'''</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>'''fvModels''' file contains the '''source term''' type and magnitude</blockquote></li>
<li><blockquote>The '''g''' file contains the details of the '''gravitational force'''</blockquote></li>
<li><blockquote>The '''momentumTransport''' file contains the details of '''turbulence properties'''</blockquote></li>
<li><blockquote>The '''thermophysicalProperties''' file contains the '''properties''' of the '''fluid''' used</blockquote></li></ul>
|-
|
'''Slide:'''

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

'''source''' [https://i.imgur.com/o4Ey8mm.png Link]
|
<ul>
<li><blockquote>'''heatSource''' is the type of the source term</blockquote></li>
<li><blockquote>'''addedHeatSources''' is the cellSet previously assigned in '''topoSetDict'''</blockquote></li>
<li><blockquote>The magnitude of '''Q''' is '''100 Watts'''</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 Link]
|
Since '''g''' is a '''vector''', its '''velocity''' and '''magnitude''' have to be specified

In this case, the '''magnitude''' of '''g''' is '''10''' '''m/s2'''

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 Link]
| 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 Link]
|
'''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 Link]
| We will be using the '''Boussinesq approximation''' for the '''equation of state'''
|-
| [gedit - '''thermophysicalProperties'''] Highlight: '''molWeight 28.9''' [https://imgur.com/ipqEFKC.png Link]
| 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 Link]
|
For the fluid in our '''simulation''', '''reference density''' is specified as '''1 kg/m3'''

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''' >> Click on '''T''' [https://imgur.com/VsCcHFW.png Link]
|
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 Link]
|
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 Link]
| Click on '''Rescale to Visible Data Range'''
|-
|
[ParaView] '''Active Variable Controls'''

Click on '''vtkBlockColors''' >> Click on '''U''' [https://imgur.com/VsCcHFW.png Link]
|
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>Set up a case of '''heat transfer''' in '''OpenFOAM'''</blockquote></li>
<li><blockquote>Simulate a '''buoyancy-driven flow''' with a heat source, and</blockquote></li>
<li><blockquote>Set up '''topoSetDict''' and '''fvModels''' in '''OpenFOAM'''</blockquote></li></ul>
|-
|
'''Slide:'''

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

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

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

OpenFOAM-version-7/C3/Flow-in-a-Convergent-Divergent-Nozzle/English

2023-12-15T09:29:37Z

Biraj:

'''Title of the script''': Flow in a Convergent-Divergent Nozzle

'''Author''': Ashley Melvin, Biraj Khadka

'''Keywords''': OpenFOAM, ParaView, CFD, computational fluid dynamics, blockMesh, axi-symmetry, wedge geometry, spline, compressible flow, inviscid, convergent-divergent nozzle, rhoCentralFoam, shock, FOSSEE, spoken tutorial, video tutorial

{| border=1
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| '''Slide''':
'''Opening Slide'''
| Welcome to the spoken tutorial on '''Flow in a Convergent-Divergent Nozzle'''.
|-
|
'''Slide:'''

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

<ul>
<li><blockquote>Create an '''axi-symmetric''' geometry using '''blockMesh'''</blockquote></li>
<li><blockquote>Create '''spline''' curved edge using '''blockMesh''', and</blockquote></li>
<li><blockquote>Set up and run a case of '''compressible flow'''</blockquote></li></ul>
|-
|
'''Slide:'''

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

<ul>
<li><blockquote>'''Ubuntu Linux''' OS version 22.04</blockquote></li>
<li><blockquote>'''OpenFOAM''' version 9</blockquote></li>
<li><blockquote>'''ParaView''' version 5.6.3, and</blockquote></li>
<li><blockquote>'''gedit''' Text editor</blockquote></li></ul>
|-
|
'''Slide:'''

'''Prerequisites'''

'''https://spoken-tutorial.org'''
|
As a prerequisite:

<ul>
<li><blockquote>You should have basic knowledge of '''compressible flows''' and '''gas dynamics'''.</blockquote></li>
<li><blockquote>You should be familiar with '''setting up a case''' and '''creating a mesh''' in '''OpenFOAM'''.</blockquote></li>
<li><blockquote>If not, please go through the prerequisite '''OpenFOAM''' tutorials on this website.</blockquote></li></ul>
|-
|
'''Slide:'''

'''Code Files'''
|
The files used in this tutorial are available in the '''Code''' '''Files''' link on the tutorial page

Please download and extract them

Make a copy and then use them while practising.
|-
|
'''Slide:'''

'''Convergent-Divergent Nozzle'''
|
We will be solving flow through a '''convergent-divergent nozzle'''.

Note that:

<ul>
<li><blockquote>at the '''inlet''', '''total pressure''' is specified, and</blockquote></li>
<li><blockquote>at the '''outlet''', '''static pressure''' is specified.</blockquote></li></ul>
|-
|
'''Slide:'''

'''Convergent-Divergent Nozzle'''
| The geometry is a '''converging-diverging''' duct.
|-
|
'''Slide:'''

'''Convergent-Divergent Nozzle'''
| Variation of the cross-sectional area is given by this '''cosine''' function along the length.
|-
| Press CTRL + ALT + T keys.
| Open the '''terminal''' by pressing '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|
[Terminal] Type:

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

'''cp -r ~/Downloads/Nozzle .'''
|
We have downloaded and extracted the case folder.

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

'''cd Nozzle'''
| Let’s move into the case folder using the '''cd''' '''command'''.
|-
|
[Terminal] Type:

'''gedit system/blockMeshDict'''
| Let’s open the '''blockMeshDict''' file in a text editor.
|-
|
'''Slide:'''

'''Axi-symmetric Geometry'''
|
<ul>
<li><blockquote>'''Axi-symmetric''' geometry can be created in '''OpenFOAM''' using the '''wedge''' patch type.</blockquote></li>
<li><blockquote>The geometry is a '''wedge''' of a small angle, usually less than '''5o'''.</blockquote></li>
<li><blockquote>It has '''1 cell''' normal to the '''planes of symmetry'''.</blockquote></li></ul>
|-
|
'''Slide:'''

'''Axi-symmetric Geometry'''
| A typical '''wedge''' geometry is shown in the figure.
|-
|
'''Slide:'''

'''Axi-symmetric Geometry'''
| The '''wedge''' geometry used for the '''convergent-divergent nozzle''' is shown in the figure.
|-
|
'''Slide:'''

'''Vertices'''
|
The geometry has '''6 vertices'''.

The '''vertices''' of the geometry are numbered as shown.
|-
|
'''Slide:'''

'''Vertex Coordinates'''
| Let us consider the '''inlet''' plane.
|-
|
'''Slide:'''

'''Vertex Coordinates-Inlet'''
|
<ul>
<li><blockquote>The '''inlet''' is along the '''y-z-plane''' at '''x = 0'''.</blockquote></li>
<li><blockquote>'''Vertex 0''' is at the '''origin'''.</blockquote></li>
<li><blockquote>The cross-sectional area at the '''inlet''' is '''2.5 m2'''.</blockquote></li>
<li><blockquote>The radius at the '''inlet''' is therefore, '''0.892 m'''.</blockquote></li>
<li><blockquote>The '''y''' and '''z coordinates''' of '''vertex 1''' are as indicated in the diagram.</blockquote></li>
<li><blockquote>Similarly, the coordinates of '''vertex 2''' are evaluated.</blockquote></li></ul>
|-
|
'''Slide:'''

'''Vertex Coordinates-Outlet'''
|
The '''outlet''' is along the '''yz-plane''' at '''x = 10''' and its cross-sectional area is '''2.5 m2'''.

The '''vertices''' of the '''outlet''' plane are indicated in the diagram.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

Vertices List [https://imgur.com/w77RPX6 Link]
| The '''6 vertices''' are entered in the ascending order of their '''vertex numbers''' as shown.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''0 3 5 2''' [https://imgur.com/pPDfXQ5 Link]
|
Let’s define the '''block'''.

We first enter the '''vertices''' of the lower '''xy-plane'''.

In this case, that would be the lower plane, when viewed along the '''negative z direction'''.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''0 3 4 1''' [https://imgur.com/UegK4aR Link]
| Similarly, the '''vertices''' of the '''front''' plane are ordered as shown.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''100 20''' [https://imgur.com/undefined Link]
|
The '''axis''' of the '''nozzle''' is along the '''x direction'''.

There are '''100 cells''' along the '''x direction''' and '''20 cells''' along the '''y direction'''.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''1''' [https://imgur.com/WVkOqWV Link]
|
The '''z direction''' is normal to the '''plane of symmetry''', also known as the '''azimuthal direction'''.

There is only '''1 cell''' along the '''z axis'''.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''edges''' [https://imgur.com/q3hgXOI Link]
|
We have '''curved edges''' that define the '''nozzle'''.

We need to specify these '''edges'''.
|-
| Slide: '''Spline'''
|
'''Spline''' curves can be created in '''blockMesh''' using the keyword '''spline'''.

It requires:

<ul>
<li><blockquote>The '''2 vertices''' that '''edge''' connects, and</blockquote></li>
<li><blockquote>The '''interpolation points''' through which '''edge''' passes</blockquote></li></ul>
|-
| Slide: '''Front Edge'''
|
Let’s look at the '''front edge''' of the '''nozzle'''.

'''Front edge''' connects the '''vertices 1''' and '''4'''.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''spline 1 4''' [https://imgur.com/3eURiww Link]
| We have used the keyword '''spline''' to indicate that a '''spline''' curve connects the '''vertices 1''' and '''4'''.
|-
| Slide: '''Interpolation Points'''
|
Let us calculate the '''interpolation points''' for the '''front edge''':

<ul>
<li><blockquote>Let us calculate the coordinates of a point on the '''edge''' at '''x = 1'''.</blockquote></li>
<li><blockquote>From the '''cosine''' relation, at '''x = 1''', the cross-sectional area is '''2.357 m2'''.</blockquote></li>
<li><blockquote>The radius of the '''nozzle''' is therefore '''0.866 m'''.</blockquote></li>
<li><blockquote>We follow the same procedure as calculating the '''vertex''' coordinates earlier.</blockquote></li></ul>

<ul>
<li><blockquote>The '''y''' and '''z coordinates''' are found to be '''0.865''' and '''0.0378'''.</blockquote></li></ul>
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''spline 2 5''' [https://imgur.com/s1iuZPN Link]
| Using the same procedure, we define the '''spline edge''' connecting '''vertices 2''' and '''5'''.
|-
| Slide: '''Boundary'''
|
The '''boundaries''' of the geometry are:

<ul>
<li><blockquote>'''inlet''' and '''outlet'''</blockquote></li>
<li><blockquote>'''nozzle'''</blockquote></li>
<li><blockquote>'''back''', and</blockquote></li>
<li><blockquote>'''front'''</blockquote></li></ul>
|-
|
[gedit - '''blockMeshDict'''] Highlight:

Boundaries List [https://i.imgur.com/sRRBRAj.png Link]
| We define the '''5 boundaries''' as shown.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

wedge >> wedge [https://i.imgur.com/gG8r6RO.png Link]
|
Note that the '''back''' and '''front faces''' are of the type '''wedge'''.

This indicates that the '''front''' and '''back faces''' are '''axi-symmetric wedge planes'''.
|-
|
[gedit - '''blockMeshDict''']

Close the window
| Close the '''blockMeshDict''' file.
|-
| [Terminal] Type: '''gedit 0/p'''
| Let’s view the initial and '''boundary''' '''values''' of '''pressure'''.
|-
|
[gedit - '''p'''] Highlight:

'''internalField uniform 10000''' [https://i.imgur.com/EhEocHs.png Link]
| The '''domain''' is '''initialized''' with 10,000 '''Pa'''.
|-
|
[gedit - '''p'''] Highlight:

'''type totalPressure''' [https://i.imgur.com/RBvQXkt.png Link]
| At the '''inlet''', we have the '''total pressure''' condition.
|-
|
[gedit - '''p'''] Highlight:

'''gamma 1.4''' [https://i.imgur.com/hF1Cnr9.png Link]
|
Since the flow is compressible, we need to specify the '''ratio of specific heats'''.

We consider the fluid to be '''air''' in this simulation.

The '''ratio of specific heats''', '''gamma''', of '''air''' is '''1.4'''.
|-
|
[gedit - '''p'''] Highlight:

'''p0 uniform 10000''' [https://i.imgur.com/qMpO2T2.png Link]
| The '''total pressure''' at the '''inlet''' is set to 10,000 '''Pa'''.
|-
|
[gedit - '''p'''] Highlight:

'''value uniform 10000''' [https://i.imgur.com/sxEMkAv.png Link]
| For the '''type totalPressure''', '''value''' is just a '''placeholder''' for the first '''time-step'''.
|-
|
[gedit - '''p'''] Highlight:

back and front BC [https://i.imgur.com/41FTbr3.png Link]
|
The '''back''' and '''front faces''' are the '''axi-symmetric wedge planes'''.

Therefore, the '''wedge''' '''boundary condition''' is used.
|-
| [gedit - '''p'''] Close the window
| Close the '''p''' file.
|-
| Slide: '''Boundary Conditions'''
|
Let’s now look at the '''boundary values''' of '''temperature''' and '''velocity'''.

<ul>
<li><blockquote>They are tabulated as shown.</blockquote></li></ul>
|-
|
Slide: Boundary Conditions

Highlight: '''slip''' [https://i.imgur.com/N48sg9z.png Link]
| Note that '''slip''' condition is imposed at the '''nozzle wall''' as the flow is '''inviscid'''.
|-
| Slide: '''Thermophysical Properties'''
|
<ul>
<li><blockquote>The '''molecular weight''' of '''air''' is '''29 g/mol'''.</blockquote></li>
<li><blockquote>The '''specific heat at constant pressure''' ('''cp''') is '''1005 J/kg-K'''.</blockquote></li>
<li><blockquote>Since we don’t consider any '''phase change''', the '''heat of fusion''' ('''Hf''') can be taken as '''0'''.</blockquote></li></ul>
|-
| Slide: '''Transport Properties'''
|
Since the flow is '''inviscid''', '''viscosity''' and '''thermal conductivity''' effects are ignored.

<ul>
<li><blockquote>'''Viscosity''' ('''μ''') can be taken as '''0''', and</blockquote></li>
<li><blockquote>The '''Prandtl number''' ('''Pr''') can be taken as '''1'''.</blockquote></li></ul>

You may assign any other '''non-zero''' value for the '''Prandtl number'''.
|-
| [Terminal] Type: '''gedit constant/thermophysicalProperties'''
| Now, let’s view the '''thermophysicalProperties''' file.
|-
| [gedit - '''thermophysicalProperties'''] Highlight: Properties values [https://i.imgur.com/64PTynu.png Link]
| The '''thermophysical properties''' are entered as shown.
|-
|
[gedit - '''thermophysicalProperties''']

Close the window
| Close the '''thermophysicalProperties''' file.
|-
|
[Terminal] Type:

'''gedit system/controlDict'''
| Let’s open the '''controlDict''' file.
|-
|
[gedit - '''controlDict'''] Highlight:

'''adjustTimeStep yes''' [https://i.imgur.com/gMwalLV.png Link]
|
We have enabled the '''adjustTimeStep'''.

It calculates '''time step''' after every iteration based on the specified '''maximum Courant number'''.
|-
|
[gedit - '''controlDict'''] Highlight:

'''maxCo 0.9''' [https://i.imgur.com/blWSJNN.png Link]
| The '''maximum Courant number''' is set as '''0.9'''.
|-
|
[gedit - '''controlDict'''] Highlight:

'''maxDeltaT 1''' [https://i.imgur.com/oTWQKiS.png Link]
| The '''maximum time step''' is set as '''1'''.
|-
|
[gedit - '''controlDict'''] Highlight:

'''writeControl adjustableRunTime''' [https://i.imgur.com/UFZqUOt.png Link]
| Since the '''time step''' is not constant, the '''write control''' is also made adjustable.
|-
|
[gedit - '''controlDict'''] Highlight:

'''deltaT 1e-6''' [https://i.imgur.com/CVmHtlG.png Link]
|
The first '''time step''' is '''1 micro second'''.

Value is chosen such that the '''Courant number''' is less than '''0.9''' for the first '''time step'''.
|-
|
[gedit - '''controlDict''']

Close the window
| Close the '''controlDict''' file.
|-
| [Terminal] Type: '''blockMesh'''
| Let’s '''mesh''' the geometry using the '''blockMesh''' '''command'''.
|-
| Slide: '''rhoCentralFoam'''
|
We will be using the '''rhoCentralFoam''' solver in this simulation.

It is:

<ul>
<li><blockquote>A '''density-based''' '''compressible flow''' solver</blockquote></li>
<li><blockquote>Based on '''central-upwind schemes''' of '''Kurganov''' and '''Tadmor'''</blockquote></li></ul>
|-
| [Terminal] Type: '''rhoCentralFoam'''
| Let’s start the simulation using the following '''command'''.
|-
| Cursor in the terminal.
| 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'''.

Type '''paraFoam''' at the prompt.
|-
|
[ParaView] '''Properties''' '''Tab'''

Click on '''Apply'''
| Click on the '''Apply''' button to view the geometry.
|-
|
[ParaView] '''Active Variable Controls'''

Click on '''vtkBlockColors''' >> Click on '''p'''
|
Let’s view the '''pressure contours''' for the simulation.

Click on the '''vtkBlockColors''' dropdown in the '''Active Variable Controls''' and select '''p'''.

Click on the '''p''' option with a '''point icon''' and not the '''box icon''', in the dropdown.
|-
|
[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'''.

You can now see the '''steady-state pressure contour'''.
|-
|
[ParaView] '''Active Variable Controls'''

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

Point to Shock
|
Notice the sudden jump in '''pressure''' in the '''diverging section''' of the '''nozzle'''.

This jump indicates the presence of '''normal shock''' in the '''nozzle'''.
|-
| [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>Create an '''axi-symmetric''' geometry using '''blockMesh'''</blockquote></li>
<li><blockquote>Create '''spline''' curved edge using '''blockMesh''', and</blockquote></li>
<li><blockquote>Set up and run a case of '''compressible flow'''</blockquote></li></ul>
|-
| Slide: '''Assignment'''
|
As an assignment:

<ul>
<li><blockquote>Change the '''outlet pressure''' to '''8900 Pa'''.</blockquote></li>
<li><blockquote>Keep all the other parameters the same and run the simulation.</blockquote></li>
<li><blockquote>View the '''steady-state pressure contour''' in '''ParaView'''</blockquote></li></ul>
|-
| 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'''
|
<ul>
<li><blockquote>Do you have any general/technical questions?</blockquote></li>
<li><blockquote>Please visit the forum given in the link.</blockquote></li></ul>
|-
| Slide: '''FOSSEE Case Study Project'''
|
<ul>
<li><blockquote>The FOSSEE team coordinates solving feasible CFD problems of reasonable complexity using OpenFOAM.</blockquote></li>
<li><blockquote>We give honorarium and certificates to those who do this.</blockquote></li>
<li><blockquote>For more details, please visit these sites.</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 Ashutosh P. Shridhar, Binayak Lohani, Biraj Khadka and Payel Mukherjee from IIT Bombay. Thanks for joining.
|}

OpenFOAM-version-7/C3/Flow-in-a-Convergent-Divergent-Nozzle/English

2023-12-15T09:13:12Z

Biraj: Created page with "'''Title of the script''': Flow in a Convergent-Divergent Nozzle '''Author''': Ashley Melvin, Biraj Khadka '''Keywords''': OpenFOAM, ParaView, CFD, computational fluid dynam..."

'''Title of the script''': Flow in a Convergent-Divergent Nozzle

'''Author''': Ashley Melvin, Biraj Khadka

'''Keywords''': OpenFOAM, ParaView, CFD, computational fluid dynamics, blockMesh, axi-symmetry, wedge geometry, spline, compressible flow, inviscid, convergent-divergent nozzle, rhoCentralFoam, shock, FOSSEE, spoken tutorial, video tutorial

{|
!width="50%"| '''Visual Cue'''
!width="50%"| '''Narration'''
|-
|
'''Slide:'''

'''Opening Slide'''
| Welcome to the spoken tutorial on '''Flow in a Convergent-Divergent Nozzle'''.
|-
|
'''Slide:'''

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

<ul>
<li><blockquote>Create an '''axi-symmetric''' geometry using '''blockMesh'''</blockquote></li>
<li><blockquote>Create '''spline''' curved edge using '''blockMesh''', and</blockquote></li>
<li><blockquote>Set up and run a case of '''compressible flow'''</blockquote></li></ul>
|-
|
'''Slide:'''

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

<ul>
<li><blockquote>'''Ubuntu Linux''' OS version 22.04</blockquote></li>
<li><blockquote>'''OpenFOAM''' version 9</blockquote></li>
<li><blockquote>'''ParaView''' version 5.6.3, and</blockquote></li>
<li><blockquote>'''gedit''' Text editor</blockquote></li></ul>
|-
|
'''Slide:'''

'''Prerequisites'''

'''https://spoken-tutorial.org'''
|
As a prerequisite:

<ul>
<li><blockquote>You should have basic knowledge of '''compressible flows''' and '''gas dynamics'''.</blockquote></li>
<li><blockquote>You should be familiar with '''setting up a case''' and '''creating a mesh''' in '''OpenFOAM'''.</blockquote></li>
<li><blockquote>If not, please go through the prerequisite '''OpenFOAM''' tutorials on this website.</blockquote></li></ul>
|-
|
'''Slide:'''

'''Code Files'''
|
The files used in this tutorial are available in the '''Code''' '''Files''' link on the tutorial page

Please download and extract them

Make a copy and then use them while practising.
|-
|
'''Slide:'''

'''Convergent-Divergent Nozzle'''
|
We will be solving flow through a '''convergent-divergent nozzle'''.

Note that:

<ul>
<li><blockquote>at the '''inlet''', '''total pressure''' is specified, and</blockquote></li>
<li><blockquote>at the '''outlet''', '''static pressure''' is specified.</blockquote></li></ul>
|-
|
'''Slide:'''

'''Convergent-Divergent Nozzle'''
| The geometry is a '''converging-diverging''' duct.
|-
|
'''Slide:'''

'''Convergent-Divergent Nozzle'''
| Variation of the cross-sectional area is given by this '''cosine''' function along the length.
|-
| Press CTRL + ALT + T keys.
| Open the '''terminal''' by pressing '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|
[Terminal] Type:

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

'''cp -r ~/Downloads/Nozzle .'''
|
We have downloaded and extracted the case folder.

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

'''cd Nozzle'''
| Let’s move into the case folder using the '''cd''' '''command'''.
|-
|
[Terminal] Type:

'''gedit system/blockMeshDict'''
| Let’s open the '''blockMeshDict''' file in a text editor.
|-
|
'''Slide:'''

'''Axi-symmetric Geometry'''
|
<ul>
<li><blockquote>'''Axi-symmetric''' geometry can be created in '''OpenFOAM''' using the '''wedge''' patch type.</blockquote></li>
<li><blockquote>The geometry is a '''wedge''' of a small angle, usually less than '''5o'''.</blockquote></li>
<li><blockquote>It has '''1 cell''' normal to the '''planes of symmetry'''.</blockquote></li></ul>
|-
|
'''Slide:'''

'''Axi-symmetric Geometry'''
| A typical '''wedge''' geometry is shown in the figure.
|-
|
'''Slide:'''

'''Axi-symmetric Geometry'''
| The '''wedge''' geometry used for the '''convergent-divergent nozzle''' is shown in the figure.
|-
|
'''Slide:'''

'''Vertices'''
|
The geometry has '''6 vertices'''.

The '''vertices''' of the geometry are numbered as shown.
|-
|
'''Slide:'''

'''Vertex Coordinates'''
| Let us consider the '''inlet''' plane.
|-
|
'''Slide:'''

'''Vertex Coordinates-Inlet'''
|
<ul>
<li><blockquote>The '''inlet''' is along the '''y-z-plane''' at '''x = 0'''.</blockquote></li>
<li><blockquote>'''Vertex 0''' is at the '''origin'''.</blockquote></li>
<li><blockquote>The cross-sectional area at the '''inlet''' is '''2.5 m2'''.</blockquote></li>
<li><blockquote>The radius at the '''inlet''' is therefore, '''0.892 m'''.</blockquote></li>
<li><blockquote>The '''y''' and '''z coordinates''' of '''vertex 1''' are as indicated in the diagram.</blockquote></li>
<li><blockquote>Similarly, the coordinates of '''vertex 2''' are evaluated.</blockquote></li></ul>
|-
|
'''Slide:'''

'''Vertex Coordinates-Outlet'''
|
The '''outlet''' is along the '''yz-plane''' at '''x = 10''' and its cross-sectional area is '''2.5 m2'''.

The '''vertices''' of the '''outlet''' plane are indicated in the diagram.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

Vertices List [https://imgur.com/w77RPX6 Link]
| The '''6 vertices''' are entered in the ascending order of their '''vertex numbers''' as shown.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''0 3 5 2''' [https://imgur.com/pPDfXQ5 Link]
|
Let’s define the '''block'''.

We first enter the '''vertices''' of the lower '''xy-plane'''.

In this case, that would be the lower plane, when viewed along the '''negative z direction'''.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''0 3 4 1''' [https://imgur.com/UegK4aR Link]
| Similarly, the '''vertices''' of the '''front''' plane are ordered as shown.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''100 20''' [https://imgur.com/undefined Link]
|
The '''axis''' of the '''nozzle''' is along the '''x direction'''.

There are '''100 cells''' along the '''x direction''' and '''20 cells''' along the '''y direction'''.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''1''' [https://imgur.com/WVkOqWV Link]
|
The '''z direction''' is normal to the '''plane of symmetry''', also known as the '''azimuthal direction'''.

There is only '''1 cell''' along the '''z axis'''.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''edges''' [https://imgur.com/q3hgXOI Link]
|
We have '''curved edges''' that define the '''nozzle'''.

We need to specify these '''edges'''.
|-
| Slide: '''Spline'''
|
'''Spline''' curves can be created in '''blockMesh''' using the keyword '''spline'''.

It requires:

<ul>
<li><blockquote>The '''2 vertices''' that '''edge''' connects, and</blockquote></li>
<li><blockquote>The '''interpolation points''' through which '''edge''' passes</blockquote></li></ul>
|-
| Slide: '''Front Edge'''
|
Let’s look at the '''front edge''' of the '''nozzle'''.

'''Front edge''' connects the '''vertices 1''' and '''4'''.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''spline 1 4''' [https://imgur.com/3eURiww Link]
| We have used the keyword '''spline''' to indicate that a '''spline''' curve connects the '''vertices 1''' and '''4'''.
|-
| Slide: '''Interpolation Points'''
|
Let us calculate the '''interpolation points''' for the '''front edge''':

<ul>
<li><blockquote>Let us calculate the coordinates of a point on the '''edge''' at '''x = 1'''.</blockquote></li>
<li><blockquote>From the '''cosine''' relation, at '''x = 1''', the cross-sectional area is '''2.357 m2'''.</blockquote></li>
<li><blockquote>The radius of the '''nozzle''' is therefore '''0.866 m'''.</blockquote></li>
<li><blockquote>We follow the same procedure as calculating the '''vertex''' coordinates earlier.</blockquote></li></ul>

<ul>
<li><blockquote>The '''y''' and '''z coordinates''' are found to be '''0.865''' and '''0.0378'''.</blockquote></li></ul>
|-
|
[gedit - '''blockMeshDict'''] Highlight:

'''spline 2 5''' [https://imgur.com/s1iuZPN Link]
| Using the same procedure, we define the '''spline edge''' connecting '''vertices 2''' and '''5'''.
|-
| Slide: '''Boundary'''
|
The '''boundaries''' of the geometry are:

<ul>
<li><blockquote>'''inlet''' and '''outlet'''</blockquote></li>
<li><blockquote>'''nozzle'''</blockquote></li>
<li><blockquote>'''back''', and</blockquote></li>
<li><blockquote>'''front'''</blockquote></li></ul>
|-
|
[gedit - '''blockMeshDict'''] Highlight:

Boundaries List [https://i.imgur.com/sRRBRAj.png Link]
| We define the '''5 boundaries''' as shown.
|-
|
[gedit - '''blockMeshDict'''] Highlight:

wedge >> wedge [https://i.imgur.com/gG8r6RO.png Link]
|
Note that the '''back''' and '''front faces''' are of the type '''wedge'''.

This indicates that the '''front''' and '''back faces''' are '''axi-symmetric wedge planes'''.
|-
|
[gedit - '''blockMeshDict''']

Close the window
| Close the '''blockMeshDict''' file.
|-
| [Terminal] Type: '''gedit 0/p'''
| Let’s view the initial and '''boundary''' '''values''' of '''pressure'''.
|-
|
[gedit - '''p'''] Highlight:

'''internalField uniform 10000''' [https://i.imgur.com/EhEocHs.png Link]
| The '''domain''' is '''initialized''' with 10,000 '''Pa'''.
|-
|
[gedit - '''p'''] Highlight:

'''type totalPressure''' [https://i.imgur.com/RBvQXkt.png Link]
| At the '''inlet''', we have the '''total pressure''' condition.
|-
|
[gedit - '''p'''] Highlight:

'''gamma 1.4''' [https://i.imgur.com/hF1Cnr9.png Link]
|
Since the flow is compressible, we need to specify the '''ratio of specific heats'''.

We consider the fluid to be '''air''' in this simulation.

The '''ratio of specific heats''', '''gamma''', of '''air''' is '''1.4'''.
|-
|
[gedit - '''p'''] Highlight:

'''p0 uniform 10000''' [https://i.imgur.com/qMpO2T2.png Link]
| The '''total pressure''' at the '''inlet''' is set to 10,000 '''Pa'''.
|-
|
[gedit - '''p'''] Highlight:

'''value uniform 10000''' [https://i.imgur.com/sxEMkAv.png Link]
| For the '''type totalPressure''', '''value''' is just a '''placeholder''' for the first '''time-step'''.
|-
|
[gedit - '''p'''] Highlight:

back and front BC [https://i.imgur.com/41FTbr3.png Link]
|
The '''back''' and '''front faces''' are the '''axi-symmetric wedge planes'''.

Therefore, the '''wedge''' '''boundary condition''' is used.
|-
| [gedit - '''p'''] Close the window
| Close the '''p''' file.
|-
| Slide: '''Boundary Conditions'''
|
Let’s now look at the '''boundary values''' of '''temperature''' and '''velocity'''.

<ul>
<li><blockquote>They are tabulated as shown.</blockquote></li></ul>
|-
|
Slide: Boundary Conditions

Highlight: '''slip''' [https://i.imgur.com/N48sg9z.png Link]
| Note that '''slip''' condition is imposed at the '''nozzle wall''' as the flow is '''inviscid'''.
|-
| Slide: '''Thermophysical Properties'''
|
<ul>
<li><blockquote>The '''molecular weight''' of '''air''' is '''29 g/mol'''.</blockquote></li>
<li><blockquote>The '''specific heat at constant pressure''' ('''cp''') is '''1005 J/kg-K'''.</blockquote></li>
<li><blockquote>Since we don’t consider any '''phase change''', the '''heat of fusion''' ('''Hf''') can be taken as '''0'''.</blockquote></li></ul>
|-
| Slide: '''Transport Properties'''
|
Since the flow is '''inviscid''', '''viscosity''' and '''thermal conductivity''' effects are ignored.

<ul>
<li><blockquote>'''Viscosity''' ('''μ''') can be taken as '''0''', and</blockquote></li>
<li><blockquote>The '''Prandtl number''' ('''Pr''') can be taken as '''1'''.</blockquote></li></ul>

You may assign any other '''non-zero''' value for the '''Prandtl number'''.
|-
| [Terminal] Type: '''gedit constant/thermophysicalProperties'''
| Now, let’s view the '''thermophysicalProperties''' file.
|-
| [gedit - '''thermophysicalProperties'''] Highlight: Properties values [https://i.imgur.com/64PTynu.png Link]
| The '''thermophysical properties''' are entered as shown.
|-
|
[gedit - '''thermophysicalProperties''']

Close the window
| Close the '''thermophysicalProperties''' file.
|-
|
[Terminal] Type:

'''gedit system/controlDict'''
| Let’s open the '''controlDict''' file.
|-
|
[gedit - '''controlDict'''] Highlight:

'''adjustTimeStep yes''' [https://i.imgur.com/gMwalLV.png Link]
|
We have enabled the '''adjustTimeStep'''.

It calculates '''time step''' after every iteration based on the specified '''maximum Courant number'''.
|-
|
[gedit - '''controlDict'''] Highlight:

'''maxCo 0.9''' [https://i.imgur.com/blWSJNN.png Link]
| The '''maximum Courant number''' is set as '''0.9'''.
|-
|
[gedit - '''controlDict'''] Highlight:

'''maxDeltaT 1''' [https://i.imgur.com/oTWQKiS.png Link]
| The '''maximum time step''' is set as '''1'''.
|-
|
[gedit - '''controlDict'''] Highlight:

'''writeControl adjustableRunTime''' [https://i.imgur.com/UFZqUOt.png Link]
| Since the '''time step''' is not constant, the '''write control''' is also made adjustable.
|-
|
[gedit - '''controlDict'''] Highlight:

'''deltaT 1e-6''' [https://i.imgur.com/CVmHtlG.png Link]
|
The first '''time step''' is '''1 micro second'''.

Value is chosen such that the '''Courant number''' is less than '''0.9''' for the first '''time step'''.
|-
|
[gedit - '''controlDict''']

Close the window
| Close the '''controlDict''' file.
|-
| [Terminal] Type: '''blockMesh'''
| Let’s '''mesh''' the geometry using the '''blockMesh''' '''command'''.
|-
| Slide: '''rhoCentralFoam'''
|
We will be using the '''rhoCentralFoam''' solver in this simulation.

It is:

<ul>
<li><blockquote>A '''density-based''' '''compressible flow''' solver</blockquote></li>
<li><blockquote>Based on '''central-upwind schemes''' of '''Kurganov''' and '''Tadmor'''</blockquote></li></ul>
|-
| [Terminal] Type: '''rhoCentralFoam'''
| Let’s start the simulation using the following '''command'''.
|-
| Cursor in the terminal.
| 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'''.

Type '''paraFoam''' at the prompt.
|-
|
[ParaView] '''Properties''' '''Tab'''

Click on '''Apply'''
| Click on the '''Apply''' button to view the geometry.
|-
|
[ParaView] '''Active Variable Controls'''

Click on '''vtkBlockColors''' >> Click on '''p'''
|
Let’s view the '''pressure contours''' for the simulation.

Click on the '''vtkBlockColors''' dropdown in the '''Active Variable Controls''' and select '''p'''.

Click on the '''p''' option with a '''point icon''' and not the '''box icon''', in the dropdown.
|-
|
[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'''.

You can now see the '''steady-state pressure contour'''.
|-
|
[ParaView] '''Active Variable Controls'''

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

Point to Shock
|
Notice the sudden jump in '''pressure''' in the '''diverging section''' of the '''nozzle'''.

This jump indicates the presence of '''normal shock''' in the '''nozzle'''.
|-
| [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>Create an '''axi-symmetric''' geometry using '''blockMesh'''</blockquote></li>
<li><blockquote>Create '''spline''' curved edge using '''blockMesh''', and</blockquote></li>
<li><blockquote>Set up and run a case of '''compressible flow'''</blockquote></li></ul>
|-
| Slide: '''Assignment'''
|
As an assignment:

<ul>
<li><blockquote>Change the '''outlet pressure''' to '''8900 Pa'''.</blockquote></li>
<li><blockquote>Keep all the other parameters the same and run the simulation.</blockquote></li>
<li><blockquote>View the '''steady-state pressure contour''' in '''ParaView'''</blockquote></li></ul>
|-
| 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'''
|
<ul>
<li><blockquote>Do you have any general/technical questions?</blockquote></li>
<li><blockquote>Please visit the forum given in the link.</blockquote></li></ul>
|-
| Slide: '''FOSSEE Case Study Project'''
|
<ul>
<li><blockquote>The FOSSEE team coordinates solving feasible CFD problems of reasonable complexity using OpenFOAM.</blockquote></li>
<li><blockquote>We give honorarium and certificates to those who do this.</blockquote></li>
<li><blockquote>For more details, please visit these sites.</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 Ashutosh P. Shridhar, Binayak Lohani, Biraj Khadka and Payel Mukherjee from IIT Bombay. Thanks for joining.
|}

OpenFOAM-version-7/C3/Simulating-1D-Conduction-through-a-Bar/English

2023-10-16T10:03:37Z

Biraj:

'''Title of the script''': Simulating 1-D Conduction through a Bar

'''Author''': Mano Prithvi Raj

'''Keywords''': OpenFOAM, ParaView, CFD, computational fluid dynamics, blockMesh, heat transfer, conduction, laplacianFoam, transport properties, FOSSEE, spoken tutorial, video tutorial

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

'''Opening Slide'''
|| Welcome to the spoken tutorial on '''Simulating 1D Conduction through a Bar'''.
|-
|| '''Slide''':

'''Learning Objective'''
|| In this tutorial, we will learn to:
* Set up a case of '''heat transfer''' in '''OpenFOAM'''
* Simulate a '''conduction heat transfer case '''using a''' laplacianFoam''' solver

|-
|| 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 '''conductive 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 provided in the '''Code''' '''Files''' link on this tutorial page
* Please download and extract them
* Make a copy and then use them while practising

|-
|| '''Slide''':

'''Geometry'''
|| We will be solving a '''1D Conduction Problem'''.
* The bar is '''1 meter '''long.

|-
|| Slide: '''Geometry'''
||
* The '''left face''' is maintained at a higher temperature compared to the '''right face'''.
* The '''top''' and '''bottom faces''' of the bar are '''adiabatic'''.
* According to '''Fourier’s Law''', we expect the flow of temperature from left to right.
* We will simulate this case using the '''laplacianFoam solver'''.

|-
|| Only Narration
|| Let’s look at the structure of '''laplacianFoam ''' and how its equations are modeled.
|-
|| Slide: '''laplacianFoam'''
||
* '''laplacianFoam '''is a basic '''OpenFOAM '''solver
* '''laplacianFoam''' solves simple Laplace equations
* An example of such an equation is thermal diffusion in a solid

|-
|| '''Slide''':

'''laplacianFoam'''

Highlight: '''Laplacian Equation'''
|| This is the equation implemented in '''laplacianFoam''':

where,

* '''alpha''' is the''' thermal diffusivity'''
* '''T '''is temperature

|-
|| Point to the equation.
|| Let’s see how this equation is implemented in '''OpenFOAM'''
|-
|| CTRL + ALT + T
|| Open the '''terminal''' by pressing '''Ctrl''', '''Alt''' & '''T''' keys.
|-
|| [Terminal] Type:

'''cd $FOAM_SOLVERS'''
|| Type the following '''command''' and press '''Enter''' to move into the '''solvers directory'''.
|-
|| [Terminal] Type:

'''cd basic/laplacianFoam'''
|| Type this '''command''' and press '''Enter''' to move into the''' directory '''of '''laplacianFoam'''.
|-
|| [Terminal] Type: '''ls'''
|| Type '''ls '''to view the files present in the '''laplacianFoam '''directory.
|-
|| [Terminal] Type:

'''gedit laplacianFoam.C'''
|| Type the following command to open the '''source code '''for '''laplacianFoam'''.
|-
|| [gedit '''laplacianFoam.C'''] Highlight:

Line no. 62 to 67
|| This is the code for solving the '''laplace '''equation in every timestep.
|-
|| [gedit '''laplacianFoam.C'''] Highlight:

'''fvm::ddt(T)'''
|| The first term represents the time derivative for temperature field '''T'''.
|-
|| [gedit '''laplacianFoam.C'''] Highlight:

'''fvm::laplacian(DT,T)'''
|| The second term represents the '''laplacian''' of temperature field '''T'''.

'''DT '''stands for thermal diffusivity.

|-
|| [gedit '''laplacianFoam.C'''] Highlight:

'''fvModels.source(T)'''
|| The last term is on the right hand side of the equation.

It is used to add source terms to the equation.

|-
|| Click on Close to close the gedit file.
|| Let’s move on to the simulation.

You can now close gedit.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| Type the following '''command''' and press '''Enter''' to move into the '''run directory'''.
|-
|| [Terminal]: '''Ctrl + L'''
|| Press '''Ctrl''' and '''L''' keys together to clear the screen
|-
||Only Narration
||Please remember to press '''Enter''' key after typing each '''command''' in the '''terminal'''.
|-
|| [Terminal] Type: '''cp -r ~/Downloads/conductionBar .'''
|| Copy the case folder that you had downloaded and extracted, into the '''run directory'''.
|-
|| [Terminal] Highlight:

'''Downloads/conductionBar'''
|| In my system, the case folder named '''conductionBar''' is located in the '''Downloads''' folder.

The location of the case folder may be different for you.

Please use the appropriate '''command''' while copying the folder.
|-
|| [Terminal] Type:

'''cd conductionBar'''
|| Let’s move into the case folder using the '''cd''' '''command'''.
|-
|| Slide: '''Boundaries'''
|| The '''computational domain''' has '''4 boundaries''', namely '''top''', '''bottom''', '''left''', and '''right'''.

All '''4 boundaries''' are '''fixed'''.

|-
|| [Terminal Type]:

gedit system/blockMeshDict
|| The details of the '''mesh''' can be found in the '''blockMeshDict''' file in the '''system folder'''.

Type the following command to open '''blockMeshDict '''in a text editor.

|-
|| [gedit blockMeshDict]

'''Point to vertices'''
|| These are the '''vertices''' used to make a rectangular '''domain'''.
|-
|| [gedit blockMeshDict]

'''Point to blocks'''

||We have a single block with 20 cells only in the x-direction.

|-
|| [gedit blockMeshDict]

'''Point to boundary'''
|| The four boundaries '''top, bottom, left''' and '''right''' are defined as type wall.

The boundary''' frontAndBack''' is kept empty as we are doing a '''1D simulation'''.
|-
|| [gedit blockMeshDict]

Click on Close to close the gedit file
|| Close the blockMeshDict file.
|-
|| Slide: '''Boundary Conditions'''
|| The '''boundary conditions '''used in the '''simulation''' are as shown in the table.

* The '''left face''' is maintained at '''373 K''',
* The '''right face''' is maintained at '''273 K''', and
* The '''top''' and '''bottom faces''' are '''adiabatic'''.

Therefore, they have '''zero gradient temperature boundary conditions'''.

* The '''front''' and''' back '''faces are of type empty, as we are running a '''1D''' simulation.

|-
|| Only Narration
|| Let’s see how the '''boundary conditions''' are defined in '''OpenFOAM'''.
|-
|| [Terminal] Type:

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

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

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

'''internalField uniform 273 '''
|| The '''domain''' is '''initialized''' with a temperature of '''273 K'''.
|-
|| [gedit - '''T'''] Highlight:

'''bottom '''boundary condition
|| The '''left face''' is maintained at a '''constant temperature''' of '''373 K'''.
|-
|| [gedit - '''T'''] Highlight:

'''top '''boundary condition
|| The '''right face''' is maintained at a '''temperature''' of '''273 K'''.
|-
|| [gedit - '''T'''] Highlight:

'''left '''&''' right '''boundary condition
|| The '''top''' & '''bottom''' have '''zero gradient temperature boundary condition'''.
|-
|| [gedit - '''T'''] Highlight:

'''“faces” “frontAndBack”'''
|| Since we are simulating a '''1D '''problem, '''frontAndBack '''is set to empty.
|-
|| [gedit - '''T'''] Close the window
|| Close the '''T file'''.
|-
|| [Terminal] Type:

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

'''transportProperties'''
|| We can see the '''transportProperties '''file in the '''constant''' folder.
|-
|| [Terminal] Type: '''gedit constant/transportProperties'''
|| Let’s open the '''transportProperties '''file.
|-
|| [gedit - '''transportProperties'''] Highlight:

'''“DT”'''
|| In the '''transportProperties '''file, we can see a property, '''DT'''.

'''DT''' stands for '''thermal diffusivity'''.
|-
|| [gedit - '''transportProperties'''] Close the window
|| Close the file.

|-
|| [terminal]: type '''clear'''
|| Clear the screen with the '''clear''' command.
|-
|| Only narration
|| Let’s simulate the problem in '''OpenFOAM'''.
|-
|| [Terminal] Type: '''blockMesh'''
|| First, let’s '''mesh''' the geometry using the '''blockMesh''' '''command'''.
|-
|| [Terminal] Type: '''laplacianFoam'''
|| Let’s start the '''simulation''' using the following '''command'''.

|-
|| [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 '''T '''

|| Let’s view the '''temperature contours''' for the simulation.

Click on the '''vtkBlockColors''' dropdown in the '''Active Variable Controls''' and select '''T'''.

Ensure that you click on the '''T''' option with a '''point icon''' and not the '''box icon''', in the dropdown.

|-
|| [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] '''Layout Window'''

Point to Circulation
|| We can see the dissipation of heat from the hot end of the bar to the cold end.

The temperature changes linearly as we move from left to the right of the bar.

This is indicated as the color gradually changes from red to blue from left to right.
|-
|| [ParaView]

'''Data Analysis =>''' Click on '''plot over line filter'''

||Now, let us plot the temperature''' '''along the length of the rod.

Click on the''' plot over line''' icon located on top of the screen as shown.
|-
|| [ParaView]

'''Properties''' '''Tab =>''' Click on '''x-axis'''

'''&&'''

'''Properties''' '''Tab =>''' Click on '''Apply '''
||Click on the x-axis and then click on the Apply''' button.'''

As we can see from the graph, the temperature variation is linear.
|-
|| 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:

* View how laplacian equation is implemented in OpenFoam,
* Solve heat transfer problem using OpenFoam, and
* Post-process results in paraview.

|-
|| '''Slide''':

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

* Increase the '''length''' of the '''bar''' in the '''x-direction''' to '''2 metres'''
* Change the '''DT '''value to''' 0.005'''
* Keep all the other parameters unaltered in your '''simulation'''

|-
|| '''Slide''':

'''Assignment'''

[next slide of assignment]
||
* Simulate the heat transfer through this bar
* View the temperature contours
* See how fast the temperature changes with time now.

|-
||'''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''': '''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, Aabhushan Regmi and Payel Mukherjee from IIT Bombay. Thank you for joining.
|-
|}