[Mat_fr]

Dear Eelco,

Why did you add the lift force as a non-coupled contribution ? Shouldn't it be coupled ?

Best,

Mat

[mohsen472]

Originally Posted by Mat_fr

Dear eelcovv,

It was indeed a problem of version. I'm looking forward to postprocess the results.
Thanks for this solver
I think, I will add also a Saffman lift force for the particles, which is significant in most of the cases.

Best,

Mathieu

i have the same problem, should i change my OF Version? idont know how should i compile this

[Mat_fr]

You should compile the library of Eelco inside the version 2.1 of OpenFOAM.

Here, the information to install and compile this version:
http://www.openfoam.org/download/git.php

Best,

Mat

[eelcovv]

Hi Mat,

Explicite Lift is most straight forward. I do get good agreement with measurements of bubble plumes so for me it is good enough.

How would you suggest to implement the lift force ?

Regards
Eelco

[Mat_fr]

Hello Eelco,

I implemented implicitely the lift force and it also gives correct agreement with my experimental reference. I thought it was better for the stabilization and also that it could have an influence in two-way coupling. But I don't think it is so important.

Best,

Mat

[eelcovv]

Well, any improvements are appreciated, that's why I posted my version of the LPT in incompressible flows. By the way, in my lift force with the Tomiyama model was a small error which explained by my plume stayed bit to narrow. Should be replaced by in the file LiftForce.C

    
// Drag relation based on Tomiyama etal (1995), in advance in multiphase flows
scalar CL;
    scalar E=1/(1+0.163*pow(Eo,0.757));
    scalar EoD=Eo/pow(E,2/3.);
    if(EoD>10)
    {
      // note: in the Tomiyama model this is -0.29, however this give a discontinuity for the CL~Eo relation
      // at Eo=10. -0.27 keeps this relation continuous
       CL=-0.27;
    }
    else
    {
       scalar fEoD=0.00105*pow(EoD,3)-0.0159*pow(EoD,2)-0.0204*EoD+0.474;
       if(EoD<4)
       {
         CL=min(0.288*tanh(0.121*Re),fEoD);
       }
       else
       {
         CL=fEoD;
       }
    }
    return CL;

With this correction I get the plume on top of the experiments.

Furthermore, I have implemented a cloudfunctionobject (just like VoidFraction) in order to gather the statistics of the dispersed phase (dispersed phase velocity and rms values). If you are interested let me know. I would appreciate your implementation of the lift force as well of course:-)


Regards
Eelco

[wellDone]

Hello everyone.

This solvers looks really nice eelcovv. Unfortunately I can't compile it yet, I have installed a fresh version of OpenFOAM from the git.

I can compile the library (libincompressibleLagrangianIntermediate.so) without errors. (see wmake.log). But when I try to compile the solver I obtain the next error (complete log Allwmake.log):

/home/wellDone/OpenFOAM/wellDone-2.1.x/platforms/linux64GccDPOpt/bin/pimpleLPTBubbleFoam
/home/wellDone/OpenFOAM/wellDone-2.1.x/platforms/linux64GccDPOpt/lib/libincompressibleLagrangianIntermediate.so: undefined reference to `Foam::BubbleLookupTableInjection<Foam::BubbleCloud<Foam::Cloud<Foam::CollidingParcel<Foam::BubbleParcel<Foam::particle> > > > >::BubbleLookupTableInjection(Foam::dictionary const&, Foam::BubbleCloud<Foam::Cloud<Foam::CollidingParcel<Foam::BubbleParcel<Foam::particle> > > >&)'
/home/wellDone/OpenFOAM/wellDone-2.1.x/platforms/linux64GccDPOpt/lib/libincompressibleLagrangianIntermediate.so: undefined reference to `Foam::BubbleLookupTableInjection<Foam::BubbleCloud<Foam::Cloud<Foam::BubbleParcel<Foam::particle> > > >::BubbleLookupTableInjection(Foam::dictionary const&, Foam::BubbleCloud<Foam::Cloud<Foam::BubbleParcel<Foam::particle> > >&)'
collect2: ld returned 1 exit status
make: *** [/home/wellDone/OpenFOAM/wellDone-2.1.x/platforms/linux64GccDPOpt/bin/pimpleLPTBubbleFoam] Error 1

So if I make ldd on the issued library, the above undefined reference is shown. I think that I'm not missing any steps to insttall it so I would appreciate your help.

Thanks.

[wellDone]

Hi,

I delved a little deeper into the error and I realized that the file BubbleLookupTableInjection.C present in the folder:

$FOAM_USER_SRC/lagrangian/intermediate/submodels/Bubble/InjectionModel/KinematicLookupTableInjection/

is empty. I have assumed that that code has been replaced with a new version in:

$FOAM_USER_SRC/lagrangian/intermediate/submodels/Bubble/InjectionModel/BubbleLookupTableInjection/

so I have deleted the KinematicLookupTableInjection folder and everything works now compiling pimpleLPTBubbleFoam.

Finally to be able to run the updated case bubcol3d_DES_yeLift_start1_clear could be required to change the boundary condition in nuTilda and nuSgs from nuSgsUSpaldingWallFunction to nutUSpaldingWallFunction as in a new commit they "Added support for variable density incompressible divDevReff for VoF solvers
Generalised wall-functions between RAS and LES/DES modelling" and nuSgsUSpaldingWallFunction is obsolete.

Regards

[eelcovv]

Hi wellDone,

Thanks for the comments. Yes, probably you need to tweak a bit to get the library compiled, I just compiled it too the latest 2.1.x version, but I don't keep up the versions unless I need to my self. I will have a look to the new wall function you mention.

I just got a request to share the particle statistics cloud function object. I am only attaching this because of the limited upload space (only 100kb). You should add this too the CloudFunctionObjects directory and add the following in the intermediate/parcles/include/cloudfumakeParcelCloudFunctionObjects.H file

#include "ParticleStatistics.H"

and lower

makeCloudFunctionObjectType(ParticleStatistics, CloudType);

Now you can add to the bubbleCloudProperties the following lines.

cloudFunctions
{
   voidFraction;

   particleStatistics
   {
      resetFields    true;
      prime2Mean     true;
      writeBubblePDF true;
      timeStart      100;
      timeEnd        1e10;
   }
}

The voidFraction is cloudfunction only give you the void fraction of the bubbles, but the particlestatistics also give you the particlevelocity and its rms vales, as will as the PDF of the particle distribution. Very handy, I can assure you (it is the only way to obtain mean profiles of the gas velocity)

Cheers
Eelco

[alquimista]

Thank you very much for the contribution! This cloud function object is useful

Note to remove the following lines in "makeParcelCloudFunctionObjects.H" to compile it.

    
#include "DispersedPhaseVelocity.H"
makeCloudFunctionObjectType(DispersedPhaseVelocity, CloudType);           \

[jiejie]

Originally Posted by eelcovv

Hi wellDone,

cloudFunctions
{
   voidFraction;

}

Eelco

Hi eelcovv

Could I ask how come my kinematicCloudTheta is like the following after I add the voidFraction in the kinematicCloudProperties with the cavityMassPartUncoupledSD_clear case?

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    movingWall
    {
        type            calculated;
        value           uniform 0;
    }
    walls
    {
        type            calculated;
        value           uniform 0;
    }
}

Thank you very much.

Jie

[eelcovv]

Not sure why it stays zero. Are you tracking particles ? I should work, it comes with the standard OF distrubution. Try it in one of the LPT tutorial cases to see if you can get it running.

Cheers
Eelco

[jiejie]

Hi eelcovv

I found that Void Fraction only works with the basicKinematicCloud class but doesn't work with basicKinematicColliding class. The basicKinematicColliding class is the basicKinematicCloud class plus the colliding. However, the void fraction object function keeps outputting zero with the basicKinematicColliding class, but the basicKinematicCloud class did output the right void fraction.

jiejie

[alquimista]

The function move in Colliding class overrides the function move of the Kinematic class. The function to call the void fraction calculation is not including in this class. You can fix it adding the following line in the file

*/lagrangian/intermediate/parcels/Templates/CollidingParcel/CollidingParcel.C

                if (p.onBoundary() && td.keepParticle)
                {
                    if (isA<processorPolyPatch>(pbMesh[p.patch(p.face())]))
                    {
                        td.switchProcessor = true;
                    }
                }

                p.age() += dt;

                td.cloud().functions().postMove(p, cellI, dt);

            }

Originally Posted by jiejie

Hi eelcovv

I found that Void Fraction only works with the basicKinematicCloud class but doesn't work with basicKinematicColliding class. The basicKinematicColliding class is the basicKinematicCloud class plus the colliding. However, the void fraction object function keeps outputting zero with the basicKinematicColliding class, but the basicKinematicCloud class did output the right void fraction.

jiejie

[vonboett]

...take a look at CFDEM/LIGGGHTS coupling openFOAM to LAMMMPS Lagrangian Particle Code in resolved and unresolved way. For treating the turbulence interaction, a coupling between LIGGGHTS particle code and PALABOS Lattice Boltzmann code is in developement, and its embedding in OpenFOAM will be the next challenge to get a full coupled cascade of turbulent particle laden flow

[koulis]

thanks solved it;#

[baila12]

Thank you for posting this solver! I am very interested in using it and am wondering if you have any advice for how to compile it using version 2.2.

[Dommy]

First - thanks eelcovv for this wonderful working solver - pretty much what I needed in advance to the existing solvers in OF!

In case of errors while compiling the solver I changed

-I$(FOAM_USER_SRC)/lagrangian/incompressible/intermediate/lnInclude \

to the absolute path - e.g.

-I/disk701/home/Dommy/OpenFOAM/Dommy-2.1.x/userPrograms/lagrangian/incompressible/intermediate/lnInclude \

(just where lnInclude of the new langrangian lib is located)

I´m thinking about adding a collision model (such as implemented in icoUncoupledParcelFoam) to that solver. It would make it more accurate for high mass loaddings. Any experiences with that?

Speaking of high mass loadings - at the moment I try to validate the solver (with other Euler-Langrange solvers in OF21x) for some test cases.

In order to reach significant mass loadings (22 - 100%) one has unite particles to parcels. The solver seams to have problems with a large number of particles per parcel.

It crashs from one time step to another with exploding time step continuity errors. By reducing the particles per parcel it works fine again but more parcels have to be calculated - somebody has experienced the same?

Regards,
Tom

[mayank.dce2k7]

Hi Eelcov,

Thanks for the wonderful solver. I was looking for two way coupled Lagrangian solver and your solver works great!

I am simulating a case were one tube having one inlet bifurcates into two branches having one outlet each.

The problem is I want a steady state Lagrangian solver. Now, I started studying your solver and in a similar way I tried to modify 'bouyantBousinessqSimpleFoam' as your solver was based on 'bouyantBousinessqPimpleFoam' and I compiled the solver succesfully but when I am running on a test case I am getting following errors:

--> FOAM FATAL ERROR:
temporary deallocated

From function T& Foam::tmp<T>:perator()()
in file /opt/openfoam211/src/OpenFOAM/lnInclude/tmpI.H at line 158.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2
in "/home/mayank/OpenFOAM/mayank-2.1.1/platforms/linux64GccDPOpt/bin/simpleCoupledKinematicParcelFoam"
#3 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#4
in "/home/mayank/OpenFOAM/mayank-2.1.1/platforms/linux64GccDPOpt/bin/simpleCoupledKinematicParcelFoam"
Aborted (core dumped)

I don't understand where to remove this error. I checked I removed field 'T' from everywhere within the solver. I have also attached a copy of modified steady state Lagrangian solver.

Please advice me.

Regards,
Mayank

[mayank.dce2k7]

I removed the above error....I made a mistake while editing the solver.

Thanks again for transient two way coupled solver.