Nancyvarkey at 07:44, 23 July 2020

2020-07-23T07:44:20Z

Ashleymelvin: Created page with "'''Title of the script''': Grid Resolution and Convergence in OpenFOAM '''Author''': Ashley Melvin '''Keywords''': OpenFOAM, ParaView, blockMesh, meshing, mesh refinement, c..."

2020-07-22T10:45:33Z

Created page with "'''Title of the script''': Grid Resolution and Convergence in OpenFOAM '''Author''': Ashley Melvin '''Keywords''': OpenFOAM, ParaView, blockMesh, meshing, mesh refinement, c..."

New page

'''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

{| border = "1"
|-
|| '''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 '''tutorial 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 deltaT'''.

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 s'''.

So, this will be the value of '''deltaT'''.
|-
|| [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 '''0''' 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 s'''.

Update '''deltaT''' 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''' are acceptable.

We can see that the pressure values at '''6400''' and '''25600 cells''' differ only by an order of '''10-4'''.

Any more '''refinement''' than '''6400 cells,''' will only give us results that differ by less than '''10-3'''.

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.
|-
|}

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

Nancyvarkey at 07:44, 23 July 2020

Ashleymelvin: Created page with "'''Title of the script''': Grid Resolution and Convergence in OpenFOAM '''Author''': Ashley Melvin '''Keywords''': OpenFOAM, ParaView, blockMesh, meshing, mesh refinement, c..."