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

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.

Contributors and Content Editors

Biraj, Omkar