OpenFOAM-version-7/C2/Grid-Resolution-and-Convergence-in-OpenFOAM/English

Title of the script: Grid Resolution and Convergence in OpenFOAM

Author: Ashley Melvin

Keywords: OpenFOAM, ParaView, blockMesh, meshing, mesh refinement, coarse mesh, medium mesh, fine mesh, grid independence study, Courant number, lid-driven cavity, video tutorial

Visual Cue	Narration
Slide: Opening Slide	Welcome to this tutorial on Grid Resolution and Convergence in OpenFOAM.
Slide: Learning Objectives	In this tutorial, we will learn to: Refine a mesh using blockMeshDict Change the time step to achieve numerical stability, and Perform a grid independence study
Slide: System Specifications	To record this tutorial, I am using, Ubuntu Linux OS version 18.04 OpenFOAM version 7 ParaView version 5.6.0, and gedit Text editor However, you may use any other text editor of your choice.
Slide: Prerequisites	As a prerequisite: You should be familiar with setting up a case and creating a mesh in OpenFOAM. You should also be familiar with basic post-processing using ParaView. If not, please go through the prerequisite OpenFOAM tutorials on this website.
Slide: Lid Driven Cavity	We will use the lid driven cavity case in this tutorial. This is the diagram of Lid Driven Cavity Flow.
CTRL + ALT + T	Open the terminal by pressing Ctrl, Alt & T keys.
Only Narration	Here onwards please remember to press the Enter key after typing each command.
[Terminal] Type: cd $FOAM_RUN	Type the following command to move into the RUN directory.
[Terminal] Type: cp -r $FOAM_TUTORIALS/incompressible/icoFoam/cavity/cavity .	Let us copy the Lid driven cavity case from the TUTORIALS directory into the RUN directory. Type the following command to do so.
[Terminal] Type: cd cavity	Now let us go into the Lid Driven Cavity case folder using the cd command.
[Terminal] Type: gedit system/blockMeshDict	Let’s open the blockMeshDict file in a text editor.
[gedit - blockMeshDict] Highlight (20 20 1)	This is a 2 dimensional mesh having 20 cells along both x and y directions.
[gedit - blockMeshDict] Close Text Editor	Close the blockMeshDict file.
[Terminal] Type: gedit system/controlDict	Now, let’s open the controlDict file in a text editor.
[gedit - controlDict] Highlight: deltaT	The time step for the simulation is specified using the keyword delta T. When running the simulation, temporal accuracy and numerical stability needs to be achieved. The Courant number is required to be less than 1 to achieve this. Please refer to the Additional Reading Material on this tutorial page for details. It mentions the steps used to calculate the time-step.
[gedit - controlDict] Highlight: 0.005	We have calculated the time step for this simulation to be 0.005 seconds. So, this will be the value of delta T.
[gedit - controlDict] Close Text Editor	Close the controlDict file.
[Terminal] Type: blockMesh	Let us mesh the geometry now using the blockMesh command on the terminal.
[Terminal] Type: icoFoam	We will be using the icoFoam solver to simulate the case. Type the following command on the terminal to start the simulation.
[Terminal] Highlight: End	The iterations are now complete.
[Terminal] Type: paraFoam	Let us view the simulated results in ParaView using the paraFoam command.
[ParaView] Properties Tab Click on Apply	Click on the Apply button in the Properties tab to view the geometry.
[ParaView] Active Variable Controls Click on vtkBlockColors >> Click on p	Next, let’s view the pressure contours for the simulation. Click on the vtkBlockColors dropdown in the Active Variable Controls and select p.
[ParaView] VCR Controls Click on Last Frame	Now, let us view the contours at the end of the simulation. Click on the Last Frame button in the VCR Controls.
[ParaView] Data Analysis Click on Probe Location	Next, let’s see the values of pressure and velocity at the centre of the domain. To do so, click on the Probe Location button in the Data Analysis section.
Slide: Probe Location	Probe Location filter shows the details of the points within an arbitrary sphere. By default, this sphere is centered at the center of the domain and has zero radius. Changing these parameters will change the probe location or the range of the probe.
[ParaView] Properties Tab Click on Apply	We need the values at the centre of the domain. Therefore, we stick with the default Sphere Parameters in the Properties Tab. Click on the Apply button.
[ParaView] SpreadSheetView	We can now see the velocity and pressure values in the SpreadSheetView. Note down the value of pressure as we will be using this later.
[ParaView] Close the Window	Then close the ParaView window.
Only Narration	Now, let us increase the number of cells in the x and y direction to 40 cells.
Slide: Mesh Refinement	This process of dividing the existing cells is called mesh refinement. Mesh refinement changes a coarse mesh into a finer mesh.
[Terminal] Type: gedit system/blockMeshDict	Let us open the blockMeshDict file in a text editor.
[gedit - blockMeshDict] Highlight: 40 40	Change the number of cells in x and y direction as shown.
[gedit - blockMeshDict] Save >> Close the window	Save and close the file.
Only Narration	Since we have changed the number of cells, we need to update the time step. This is to ensure that the Courant number is less than 1.
[Terminal] Type: gedit system/controlDict	Let’s open the controlDict file in a text editor.
[gedit - controlDict] Highlight: 0.0025	For the refined mesh, the calculated time-step is 0.0025 seconds. Update delta T as shown.
[gedit - controlDict] Save >> Close the window	Save and close the file.
[Terminal] Type: blockMesh	Since we have changed the meshing parameters, we need to mesh the geometry again. On the terminal, type the command as shown.
[Terminal] Type: ls	Let us view the contents of the cavity folder. Type ls in the terminal.
[Terminal] Highlight: 0.1 0.2 0.3 0.4 0.5	We can see that the files from the previous run exist in the cavity folder.
[Terminal] Type: foamListTimes -rm	Let’s remove these files by typing this command.
[Terminal] Type: icoFoam	Let’s run the icoFoam solver.
[Terminal] Type: paraFoam	And view the results in ParaView by typing paraFoam.
[ParaView] Click Apply >> Click on vtkBlockColors >> Click on p >> Click on Last Frame >> Click on Probe Location >> Click Apply	Let us find the value of the pressure field at the centre of the domain at the final time step. As explained earlier, we use the Last Frame option to move to the final time step. And, we use the Probe Location filter to find the data at the centre of the domain.
[ParaView] SpreadSheetView	We can see the value of the pressure field at the centre of the domain.
[ParaView] Close the Window	Close the ParaView window.
Only Narration	Similarly, we can find the pressure at the centre for more number of cells. Note that the time step is changed for each run depending on the cell size.
Slide: Pressure at the Centre	The following table shows the pressure values for various numbers of cells.
Slide: Pressure at the Centre	This is the Pressure versus number of cells plot based on the data. Let’s consider that values within the order of 10-3 (10 to the power minus 3) are acceptable. We can see that the pressure values at 6400 and 25600 cells differ only by an order of 10-4 (10 to the power minus 4). Any more refinement than 6400 cells, will only give us results that differ by less than 10-3 (10 to the power minus 3). Therefore, the results from a mesh having 6400 cells or more, surely gives acceptable results. In other words, the results become independent of the mesh, if it has more than 6400 cells. What we have just performed is called a grid independence study.
Only Narration	The Additional Reading Material has more details on grid independence study. Please refer to it.
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: Refine a mesh using blockMeshDict Change the time step to achieve numerical stability, and Perform a grid independence study
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	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: Spoken Tutorial	The Spoken Tutorial project is supported by MHRD, Govt. of India. The script for this tutorial is contributed by Ashley Melvin. And this is Swetha Sridhar from IIT Bombay signing off. Thank you for joining.

Contributors and Content Editors

Ashleymelvin, Nancyvarkey