CFD Online Discussion Forums - [OpenFOAM] Plot over line average magnitude of particle velocity in paraview

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- ParaView (https://www.cfd-online.com/Forums/paraview/)

- - [OpenFOAM] Plot over line average magnitude of particle velocity in paraview (https://www.cfd-online.com/Forums/paraview/137282-plot-over-line-average-magnitude-particle-velocity-paraview.html)

maysmech

June 12, 2014 03:41

Plot over line average magnitude of particle velocity in paraview

Hi all,
How can I plot over line the particle velocity in a lagrangian solver?
"plot over line" plots the continuous phase variables only and can not plot lagrangian variables.
Any idea?

mechem

June 13, 2014 02:42

Plot over line average magnitude of particle velocity in paraview

Hello,
How is possible to plot over line the velocity of particles in lagrangian solvers like MPPICFoam?
How can we find the average magnitude of particle velocity in a two-horizontal lines?
Thanks in advance

wyldckat

June 14, 2014 08:40

Greetings to all!

@Maysam: There is a filter named "Plot data" which will plot any dataset. So essentially it depends on whether you can prepare the Lagrangian data in a way that it's ready to be plotted.

Best regards,
Bruno

maysmech

June 14, 2014 10:24

Quote:

Originally Posted by wyldckat (Post 497022)

Thanks a lot Bruno,
I couldn't use this filter. What we need is plotting average of particle velocities in a line. Because the particles are not in a horizontal line and there is some vertical distances, I think we should use averaging in each cell (like calculation of betta in drag force source term) then possible to plot a discrete lagrangian variable over a line. Running tutorials in Lagrangian solvers like MPPICFoam creates Lagrangian velocities (U) in timeFolder/lagrangian/kinematicCloud directory. The problem is they are sorted by their particle ID, not mesh cell number. What do you think about plotting these discrete variables over line using "Plot Data" filter?
Regards,

wyldckat

June 15, 2014 08:13

Greetings Charlie and Maysam,

Since both your questions are related, I've moved all posts into a single thread.

If I understand your questions correctly, you want to:

First re-sample the velocity data that comes from the particles onto the mesh. Essentially, create the field "U.particles".
Then do a time average of that field "U.particles".
Then plot this field "U.particles.avg" over a line.

I've done some attempts just now on this topic and I have not managed to figure out the solution, if at all possible to be done directly in ParaView. The best I can figure out is that the "Programmable filter" would have to be used for this, because this kind of calculation isn't very usual.

It looks like that for this particular objective, you will have to create a dedicated OpenFOAM utility or Python filter for ParaView.

Problem is that the more I think about this, the less sense it makes to me. Because the problem is that this approach implies binning (placing in bins ;)) into each mesh cell the average speed of all particles inside that cell. In other words, the plot you'll get will be more of a spacial histogram of the particle velocity along a line.

Thinking even further, it seems that you want to calculate the average velocity of particles that are at a certain distance of a line, perhaps using a weighted distance average...

OK, the more I think about this, the more questions I end up with. So, what is the specific sampling criteria do you want to use?
I ask this because the particles are solved almost separately from the mesh, therefore it doesn't make much sense to plot particle speeds over a line, since very rarely will particles will cross over that line.

Best regards,
Bruno

maysmech

June 15, 2014 08:40

Quote:

Originally Posted by wyldckat (Post 497101)

If I understand your questions correctly, you want to:

First re-sample the velocity data that comes from the particles onto the mesh. Essentially, create the field "U.particles".
Then do a time average of that field "U.particles".
Then plot this field "U.particles.avg" over a line.

Thanks Bruno and Charlie!
Yes I meant these steps exactly. I need particle flux for each grid cell using this equation:
particle flux (kg/m2.s)=(1-alpha.air)*rho_p*U_p
This is the flux of particles in each time. Averaging this term leads to the flux of particles in a desired line.

wyldckat

June 15, 2014 11:30

Hi Maysam,

The most I can do is to suggest that you study the source code that is in the folders indicated by the following commands:

Code:

echo $FOAM_UTILITIES/postProcessing/lagrangian/particleTracks

echo $FOAM_SOLVERS/lagrangian/DPMFoam

and to try to develop your own utility for performing that calculation.

In addition, have a look into this wiki page for more ideas: http://openfoamwiki.net/index.php/Ho..._based_methods

Good luck! Best regards,
Bruno

maysmech

June 15, 2014 11:48

Thanks Bruno for your suggestions.
I will work on the source code and will return here.
Regards,

mneben

July 24, 2014 07:55

Hello Maysam,

did you find a appropriate solution?

I had the same problem and therefore I changed the DPMFoam source code:

in createFields I wrote

Code:

    

    Info<< "Creating field particleFlux\n" << endl;

    // mass Flux of the lagrangian particle [kg/(m^2*s)]

    volVectorField particleFluxByA

    (

        IOobject

        (

            "particleFluxByA",

            runTime.timeName(),

            mesh,

            IOobject::NO_READ,

            IOobject::AUTO_WRITE

        ),

        mesh,

        dimensionedVector("zero", dimVelocity*dimMass/dimVolume, vector::zero)

    );

In DPFMFoam.C above main function

Code:

typedef typename basicKinematicTypeCloud::particleType parcelType;

...and before the evolving of the particles I added the following lines:

Code:

    forAll(particleFluxByA,i)

    {

        particleFluxByA[i] = vector(0.0,0.0,0.0);

    }

    forAllConstIter(typename basicKinematicTypeCloud, kinematicCloud, iter)

    {

        const parcelType& p = iter();

        const label cellI = p.cell();

        particleFluxByA[cellI]+=p.nParticle()*p.mass()*p.U();

    }

    forAll(mesh.V(),i)

    {

        particleFluxByA[i]/=mesh.V()[i];

    }

The idea behind it is that the flux f = (1-alpha.air)*rho_p*U_p =rho_bulk*U_p whereas U_p is the mean value.
The mass averaged mean value can be calculated with Up=sum(vi*mi*ni)/mtotal

mtotal =(total) mass of all parcels in a cell; mi, ni and vi are the values of the individual parcels
mtotal=rho_bulk*Vcell

--> f=rho_bulk*sum(vi*mi*ni)/(rho_bulk*Vcell) =sum(vi*mi*ni)/Vcell

Kind regards

Matthias

maysmech

July 24, 2014 11:46

Quote:

Originally Posted by mneben (Post 502968)

Hello Maysam,

did you find a appropriate solution?

I had the same problem and therefore I changed the DPMFoam source code:

in createFields I wrote

Code:

    

    Info<< "Creating field particleFlux\n" << endl;

    // mass Flux of the lagrangian particle [kg/(m^2*s)]

    volVectorField particleFluxByA

    (

        IOobject

        (

            "particleFluxByA",

            runTime.timeName(),

            mesh,

            IOobject::NO_READ,

            IOobject::AUTO_WRITE

        ),

        mesh,

        dimensionedVector("zero", dimVelocity*dimMass/dimVolume, vector::zero)

    );

In DPFMFoam.C above main function

Code:

typedef typename basicKinematicTypeCloud::particleType parcelType;

...and before the evolving of the particles I added the following lines:

Code:

    forAll(particleFluxByA,i)

    {

        particleFluxByA[i] = vector(0.0,0.0,0.0);

    }

    forAllConstIter(typename basicKinematicTypeCloud, kinematicCloud, iter)

    {

        const parcelType& p = iter();

        const label cellI = p.cell();

        particleFluxByA[cellI]+=p.nParticle()*p.mass()*p.U();

    }

    forAll(mesh.V(),i)

    {

        particleFluxByA[i]/=mesh.V()[i];

    }

Hi Matthias
I wrote a Fortran code to do postprocessing the results. Your work in changing the source code seems nice. I try yours too and compare it with mine. Regards,

wenxu

October 31, 2014 21:18

Quote:

Originally Posted by mneben (Post 502968)

Hello Maysam,

did you find a appropriate solution?

I had the same problem and therefore I changed the DPMFoam source code:

[...]

Kind regards

Matthias

hello,Matthias Neben,

how can i get the particle's mean velocity and RMS along a line (a distance tolerance ), i'm really new to OF, any suggestion will be helpful!!

regards,
wen

Quote:

Originally Posted by mechem (Post 496868)

HI,Charlie.
Have you solved your problem? please give me some suggestion, thank you !

regards
wen

surajkvs

June 28, 2017 09:25

Quote:

Originally Posted by wyldckat (Post 497022)

hey,
I am able to plot data but how will I get the particle velocity over line.
I am new on openFoam and I am doing the fluidised bed case.name Goldscmidt.
so,is there anybody who was able to solve.than please suggest me the solution.

wangchengan2003

August 5, 2022 21:42

Hello Maysam,
I have output the data of water spray. Such as

https://s2.loli.net/2022/08/06/2opzbEqIHhAcgTm.png

I want to plot a ling of variation of the average diameter along the axis of each spray. It means that I should calculate the average diameter at any plane perpendicular to the axis. Could you give me some suggestions?

Best regards,
Chengan

Thiago800

August 12, 2022 11:46

Hello wangchengan2003,

how did you output the data of this spray like that in paraview?
I am also doing a spray simulation, and I am searching a way to plot the particle like you did.
How did you do that?

Thank you:)

All times are GMT -4. The time now is 22:38.