Script | Spoken-Tutorial - User contributions [en]

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

2023-10-13T10:17:19Z

Omkar: Created page with "'''Title of the script''': Simulating 1-D Conduction through a Bar '''Author''': Mano Prithvi Raj '''Keywords''': OpenFOAM, ParaView, CFD, computational fluid dynamics, bloc..."

'''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 Kelvin''',
* The '''right face''' is maintained at '''273 Kelvin''', 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 Kelvin'''.
|-
|| [gedit - '''T'''] Highlight:

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

'''top '''boundary condition
|| The '''right face''' is maintained at a '''temperature''' of '''273 Kelvin'''.
|-
|| [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.
|-
|}

OpenFOAM-version-7/C3/Simulating-Flow-using-Cyclic-Conditions/English

2023-10-13T10:12:31Z

Omkar: Created page with "Title of the script: Simulating flow using cyclic conditions Author: Divyesh Variya, Abhushan Regmi Keywords: OpenFOAM, Channel flow, Cyclic condition, Paraview, Video-Tut..."

Title of the script: Simulating flow using cyclic conditions

Author: Divyesh Variya, Abhushan Regmi

Keywords: OpenFOAM, Channel flow, Cyclic condition, Paraview, Video-Tutorial.

{| border =1
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
||Slide: '''Opening Slide'''
||Welcome to this tutorial on '''Simulating flow using cyclic conditions'''.
|-
|| Slide: '''Learning Objectives'''
|| In this tutorial, we will learn to,

* Setup ''' mesh ''' for a '''cyclic flow'''
* Setup ''' boundary conditions ''' for a '''cyclic flow'''
* Add ''' momentum source'''
* '''Simulate''' the case using '''pimpleFoam 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 text editor of your choice.
|-
||'''Slide''':

'''Prerequisites'''

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

||To practise, this tutorial learner should have knowledge of,

* Basic Linux commands, and
* Basic knowledge of '''OpenFOAM ''' software
* If not, please go through the prerequisite '''OpenFOAM '''tutorials on this website.

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

'''Cyclic Conditions'''
||'''Cyclic condition''' is a special '''periodic boundary condition'''.

It is often used in '''CFD''' when we have repetitive geometry for larger '''domains'''.

Here we consider that both the ends of the geometry are connected.

Mainly two types of repetitive conditions can be seen.

# '''Rotational''' and
# '''Transitional'''

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

'''Cyclic Conditions'''
||'''Rotational cyclic condition''' is helpful in '''turbomachinery''' applications.

'''Transitional cyclic conditions '''are helpful in simulating''' long pipes.'''

'''Cyclic conditions '''can help to save the '''computational time''' and ''' resources'''.
|-
||'''Slide''':

'''Problem Statement'''
||As you can see, we have a '''2D channel geometry''' on the screen.

Dimensions are 2 '''meter'''s in height and 4 '''mete'''rs in length.

'''Reynolds number''' will be '''100''', so the case will be '''laminar'''.

In this case we will simulate '''cyclic conditions'''.

And compare '''computational time''' with '''traditional inlet-outlet''' condition cases.
|-
||'''Slide''':

'''Analytical Solution'''
||From the input data, we can analytically calculate:

'''Entrance length''',

'''Maximum velocity ''', and

'''Pressure gradient'''.
|-
||'''Slide''':

'''Solver & Base Tutorial'''
||We know that when we install '''OpenFOAM ''' some ''' benchmark cases''' come as '''tutorials'''.

For a '''cyclic condition''', we have '''channel395''' case in '''pimpleFoam/LES''' location.

'''pimpleFoam''' solver is a '''Transient ''' solver for:
* '''Incompressible fluid'''
* '''Turbulent flow''' on a '''moving mesh'''.

But it can also be used for ''' laminar flow''' with '''static mesh'''.
|-
||'''Slide''':

'''Source Term'''
||When we use '''cyclic conditions''', two ends of the geometry are connected.

To keep the fluid flowing, adding a constant force in the domain is necessary.

This '''force''' can be applied using '''source terms''' in '''OpenFOAM'''.

We can give the '''mean velocity source''' in the '''fvConstraints''' file.

'''Syntax''' of the '''code''' is given in the slide for reference.

We shall explain the code later.
|-
||Only Narration
||Let’s copy the '''base case''' from the '''pimpleFoam tutorial''' to our local directory '''FOAM_RUN'''.
|-
||CTRL + ALT + T
||Open the '''terminal '''by pressing '''Ctrl''',''' Alt ''' and ''' T''' keys.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''

'''cp -r $FOAM_TUTORIALS/incompressible/pimpleFoam/LES/channel395 $FOAM_RUN'''
|| Type these '''commands '''to go to the '''run''' folder and then copy the '''base case'''.
|-
|| [Terminal] Type:

'''cd channel395'''
||Go to the '''channel395 '''directory.
|-
|| [Terminal] Type:

'''rm -r 0 0.orig/k 0.orig/nu*'''
||The '''tutorial case''' we used is made for '''LES '''simulations.

There are a few unnecessary files to simulate a '''laminar '''case.

Hence, type this command to delete those files.
|-
||Only Narration
||Let’s first look at the '''blockMeshDict '''file.

Then setup '''geometry''' and '''mesh '''for our '''problem statement'''.
|-
|| [Terminal] Type:

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

Here you need to mention from which number the changes have to be made.(0 0 '''2''') => (0 0 '''0.2''')

(4 0 '''2''') => (4 0 '''0.2''')

(0 1 '''2''') => (0 1 '''0.2''')

(4 1 '''2''') => (4 1 '''0.2''')

(0 2 '''2''') => (0 2 '''0.2''')

(4 2 '''2''') => (4 2 '''0.2''')

(40 25 '''30''') => (40 25 '''1''')

(40 25 '''30''') => (40 25 '''1''')
||As we can see, the entire geometry is made of '''2 blocks''' and it is '''3D geometry'''.

To convert it into 2D, we can simply change '''z-coordinates '''with '''0.2'''.

Also, don’t forget to make the '''number of cells''' in the '''z-direction''' '''<nowiki>= 1</nowiki>'''.

|-
||Point to the expansion ratio.
||By default, some '''expansion ratio''' is used to '''refine''' the '''mesh '''near the '''wall'''.

We will keep it as it is.
|-
||Point to the Top and Bottom walls part in the text editor.
||Here, our main focus is the '''boundary '''section.

As we can see, '''top''' and '''bottom walls '''were taken as '''wall '''types.
|-
||Point to the cyclic patches in the file.
||The '''cyclic patches''' can be defined as shown on the screen.

The type of the '''cyclic patch''' can be given as “'''cyclic'''.”

An additional entry needs to be added to define the '''neighbor patch'''.
|-
||Click on Save and Click on Close.
||Save the file and close it.
|-
||Only Narration
||To define '''boundary conditions''', we can go to the '''0.orig''' folder and modify the fields file.
|-
|| [Terminal] Type:

'''gedit 0.orig/U'''
||Let’s open the velocity file first.
|-
|| [gedit] Change:

internalField uniform ('''0.1335''' 0 0); '''<nowiki>=></nowiki>''' internalField uniform ('''1''' 0 0);

Click on Save and Click on Close.
||Set up '''1 m/s velocity''' in the '''internal field''' to initialize the simulation.

The other boundary conditions will be '''cyclic'''.

Save the file and close it.
|-
|| [Terminal] Type:

'''gedit 0.orig/p'''

Click on Close

||In the same way, we have initialized the field with '''0 kinematic pressure''' in the '''p''' file.

The boundary conditions for other''' '''patches will be '''cyclic''' similar to that of '''U'''

Close the file.
|-
|| [Terminal] Type:

'''cp -r 0.orig 0'''
||Type the following command to make a clone of the 0.orig file with 0 name.
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
||Now, we can set up '''kinematic viscosity''' in the '''transportProperties '''file from the '''constant''' folder.
|-
|| [gedit] Change:

'''nu 2e-05 => 0.02'''

'''Ubar 0.1335 => 1 '''

Click on Save and Click on Close
||Also, set the '''Ubar''' value in the x-direction to

'''1 m/s'''.

Save and close the file.
|-
|| [Terminal] Type:

'''gedit constant/momentumTransport'''

simulationType''' LES; => '''simulationType''' laminar; '''

Click on Save and Click on Close.

||In the''' momentumTransport '''file, we need to specify '''laminar''' type flow.

Save and close the file
|-
|| [Terminal] Type:

'''gedit system/controlDict '''

endTime''' 1000 => 15'''

deltaT''' 0.2 => 0.1'''

writeInterval''' 200 => 10'''

Click on Save and Click on Close

|| In the '''controlDict '''file, let's set '''endTime '''equal''' to 15 seconds'''.

Also, set '''deltaT '''equals '''0.1 '''and''' writeInterval 10'''.

Save and close the file.

|-
|| [Terminal]:

Only Narration
||Our case setup is almost ready.

But here, we haven't specified any '''force''' to drive fluid in our system.

It is necessary to provide an '''external force''' in our system to keep''' fluid flowing'''.

To add a specific type of '''external force''', we can use the '''fvConstraints '''utility in '''OpenFOAM'''.
|-
|| [Terminal] Type:

'''gedit system/fvConstraints'''
||The '''fvConstraints '''file is located in a '''constant '''or '''system '''folder.

Here, in this '''tutorial''', it is located under the '''system '''folder.

Open it in a text editor using the following command.
|-
|| [gedit fvConstraints]:

Point to '''momentumForce'''
|| In this dictionary we are providing '''momentumSource '''as a '''Source'''
|-
|| [gedit fvConstraints]:

Point to''' type'''
||We are providing '''meanVelocityForce'''

This applies a force to maintain a user-specified '''volume-averaged mean velocity'''
|-
|| [gedit fvConstraints]:

Point to '''SelectionMode'''
||Here we are selecting all '''cells''' of the '''domain'''
|-
|| [gedit fvConstraints]:

Point to '''fields and Ubar'''
||We are providing this source term to the '''field''' '''velocity'''.

We will provide mean velocity of '''1m/s '''in the x-direction.

Also, we will get a '''parabolic velocity profile''' in the domain.
|-
|| [gedit] Change:

Ubar ('''0.1335 '''0 0); '''<nowiki>=> </nowiki>'''

Ubar ('''1''' 0 0);

Click on Save and Click on Close.
||Change '''Ubar''' value from '''0.1335 '''to '''1'''.

Save and close the file.
|-
|| [Terminal] Type:

'''blockMesh'''

'''pimpleFoam'''
||Let us run simulation commands.

First type '''blockMesh '''for '''meshing '''and then '''pimpleFoam '''to run the '''simulation'''.
|-
|| [Terminal] Type:

'''paraFoam'''
|| In just a few seconds, the simulation is finished.

Let us open our case in '''ParaView '''using the '''paraFoam '''command.
|-
|| [ParaView] '''Properties''' '''Tab'''

Click on '''Apply''' button
||Click on the '''apply '''button and see the '''velocity field'''.
|-
|| [ParaView]

'''VCR Controls''' '''<nowiki>=></nowiki>''' Click on '''Last Frame '''

'''&&'''

'''Active Variable Controls => '''Click on''' vtkBlockColors ==> Click on''' a''' box icon'''

||On the top of the screen, click on the '''last frame''' as shown.

Click on''' vtkBlockColors '''on the top-left and from the drop down menu select''' U''' with '''box icon'''

|-
|| [ParaView]

Showing Velocity Contour

||As you can see, we have the same '''profile '''or '''velocity distribution '''all over the domain.
|-
|| [ParaView]

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

||Now, let us check the '''velocity profile '''over '''radial distance'''.

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

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

'''&&'''

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

As we can see, it is parabolic.

The''' maximum velocity''' is '''1.5 m/s'''.
|-
||where is the analytic solution?

Point to it, instead writing only Narration.Only Narration
||Now, let us compare our result with the '''analytical solution'''.
|-
|| Slide: '''Result Comparison'''
|| From the comparison we can find the following.

'''Cyclic condition''' results exactly match the '''analytical solution''' and '''full-length channel case'''.

The ''' time consumed''' to simulate '''cyclic cases''' is less than the '''entire domain case'''.
|-
|| '''Slide''':

'''Summary'''
|| In this tutorial, we have learned to,

* Setup''' mesh '''for''' cyclic flow'''
* Setup''' boundary conditions ''' for '''cyclic flow'''
* Add ''' momentum source'''
* '''Simulate''' the case using '''pimpleFoam solver'''.
|-
||'''Slide''':

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

* Simulate two cases using the same geometry with velocity 0.002 m/s.
* One with the '''cyclic condition''' and,
* Second without '''cyclic condition'''
* Compare both results with '''analytical solution'''
* Note time difference to run both cases

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

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

|-
||Slide: '''Spoken Tutorial '''
||The Spoken Tutorial project is supported by the Ministry of Education, Govt. of India.

This tutorial is contributed by Divyesh Varya, Aabhushan Regmi and Payel Mukherjee from IIT Bombay. Thank you for joining.
|-
|}