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

Title of the script: Heat source addition to buoyantSimpleFoam

Author: Mano Prithvi Raj, Binayak Lohani, Biraj Khadka

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

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: Set up a case of heat transfer in OpenFOAM Simulate a buoyancy-driven flow with a heat source, and Set up topoSetDict and fvModels in OpenFOAM
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-tutorialorg	As a prerequisite: You should have basic knowledge of convective heat transfer You should be familiar with setting up a case in OpenFOAM If not, please go through the prerequisite OpenFOAM tutorials on this website
Slide: Code Files	The files used in this tutorial are available in the Code Files link on this tutorial page Please download and extract them Make a copy and then use them while practicing
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	Bottom wall is maintained at a higher temperature compared to the top wall The side walls are adiabatic
Slide: Problem Statement	A 2D rectangular heat source of 100 Watts is added in the middle of the cavity
Slide: Problem Statement	Gravity is acting downwards, in the negative y-direction Inside the cavity, the fluid close to the hot wall at the bottom is lighter Fluid close to the cold wall on the top is heavier Moving top wall creates circulation in cavity due to density and shear flow difference The addition of heat source and its magnitude affects the circulation of fluid
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	In this simulation, we consider a square cavity with an edge length of 1 m There will be a heat source in the middle of the square cavity The magnitude of power Q is 100 Watts
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 Link	The domain is initialised with 1 K
[gedit - T] Highlight: Link bottom boundary condition	The bottom wall is maintained at a constant temperature of 1 K
[gedit - T] Highlight: Link top boundary condition	The top wall is maintained at a temperature of 0 K
[gedit - T] Highlight: 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: Link all walls boundary condition	All 4 walls have been assigned the fixedFluxPressure boundary condition
[gedit - p_rgh] Highlight: 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: 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: 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	topoSetDict is used to select cells, faces or points in the computational domain topoSetDict is used to select a set of cells to define the location of heat source
[Terminal] Type: gedit system/topoSetDict	Let’s open the topoSetDict file
[gedit - topoSetDict] Highlight: Actions Link	addedHeatSource is the name of the cellSet The dimensions of the box for the boxToCell option are defined under sourceInfo Let’s see how the box dimensions are defined
Slide: boxToCell	Here, we can see the domain, and the region where heat source is to be applied boxToCell option chooses all the cells inside the box region for the cellSet
Slide: boxToCell	Box is defined as below Smallest coordinates are mentioned first followed by the greatest coordinates
[gedit - topoSetDict] Highlight: actions Link	In our case, the coordinates would be (0.4 0.4 -0.1) followed by (0.6 0.6 0.1)
[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	fvModels file contains the source term type and magnitude The g file contains the details of the gravitational force The momentumTransport file contains the details of turbulence properties The thermophysicalProperties file contains the properties of the fluid used
Slide: fvModels	fvModels file is used to add source terms to the governing equations of solvers The source term can be a heat source, a mass source, a damping source etc. Here, the fvModels file is used to add a heat source
[Terminal] Type: gedit constant/fvModels	Let’s open the fvModels file
[gedit - fvModels] Highlight: source Link	heatSource is the type of the source term addedHeatSources is the cellSet previously assigned in topoSetDict The magnitude of Q is 100 Watts
[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) 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 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 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 Link	We will be using the Boussinesq approximation for the equation of state
[gedit - thermophysicalProperties] Highlight: molWeight 28.9 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; 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 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 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 Link	Click on Rescale to Visible Data Range
[ParaView] Active Variable Controls Click on vtkBlockColors >> Click on U 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: Set up a case of heat transfer in OpenFOAM Simulate a buoyancy-driven flow with a heat source, and Set up topoSetDict and fvModels in OpenFOAM
Slide: Assignment	As an assignment: Increase the length of the cavity in the x-direction to 2 m Change the magnitude of heat source to 200 Watts Simulate the buoyancy driven flow in a rectangular cavity
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, Binayak Lohani, Biraj Khadka and Payel Mukherjee from IIT Bombay Thanks for joining

Contributors and Content Editors

Biraj