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

'''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 Objectives'''
|| 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''' Operating System 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 metre 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 the '''Fourier’s Law''', we expect the flow of heat 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''' and '''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''' plus '''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 '''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 two boundaries '''left''' and '''right''' are defined as '''type wall'''.

The boundaries '''topAndBottom''' and '''frontAndBack''' are 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'''  and  ''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 will 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: 

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

'''ls constant'''
|| Let’s now see the content 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''' drop down 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 drop down.

|- 
|| [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 or 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.
|-
|}