CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Pre-Processing (https://www.cfd-online.com/Forums/openfoam-pre-processing/)
-   -   SaffmanMeiLiftForce (https://www.cfd-online.com/Forums/openfoam-pre-processing/124795-saffmanmeiliftforce.html)

Danath October 13, 2013 11:16

SaffmanMeiLiftForce
 
Hi

Can anyone provide an example of SaffmanMeiLiftForce dictionary ?

thanks a lot !

wyldckat October 13, 2013 14:51

Hi Evangelos,

:eek: I had no idea there was such a thing as "SaffmanMeiLiftForce" in OpenFOAM...
But if you can provide an example case, something simple based on one of OpenFOAM's tutorials, in which this dictionary can be used, then it should be pretty simple to reverse engineer it!
Actually, OpenFOAM helps with this in two ways:
Best regards,
Bruno

Danath October 13, 2013 16:00

Hello Bruno !

I try to calculate the orbit of a particle when injected into a domain without fluid motion.I use icoUncoupledKinematicFoam but i am a little bit confused!
All the solvers take into account dragforce and gravity without calculate the lift from the fluid !

In openfoam 2.2.0 particle lift is available

So in the kinematicTransportproperties/particleforces under the drag force and gravity i add particle force and the program show me the valid particle forces

There are two " lift methods " TomiyamaLift and SaffmanMeiLiftForce

http://www.cfd-online.com/Forums/ope...rce-model.html

Danath October 14, 2013 04:06

I need something like that

http://www.cfd-online.com/Forums/ope...ictionary.html

but for saffmanmeiliftforce!!!

wyldckat October 14, 2013 16:47

Hi Evangelos,

Do you mean "icoUncoupledKinematicParcelFoam"?

Do you think that the tutorial "lagrangian/icoUncoupledKinematicParcelFoam/hopper" can be used to test this dictionary you are asking about? If so, I can give it a try next weekend.

Best regards,
Bruno

maysmech October 4, 2014 23:34

Hi all,
Do you find any dictionary for saffmanMeiLiftForce?

wyldckat October 5, 2014 04:20

Greetings Maysam,

Quote:

Originally Posted by maysmech (Post 512927)
Do you find any dictionary for saffmanMeiLiftForce?

At least I haven't, because Evangelos didn't answer back :(

Therefore my questions and offer still stand:
Quote:

Originally Posted by wyldckat (Post 456930)
Do you mean "icoUncoupledKinematicParcelFoam"?

Do you think that the tutorial "lagrangian/icoUncoupledKinematicParcelFoam/hopper" can be used to test this dictionary you are asking about? If so, I can give it a try next weekend.

Best regards,
Bruno

maysmech October 5, 2014 04:33

For example for DPMFoam

wyldckat October 5, 2014 06:58

OK, so as I mentioned in one of the posts above, having an example case as a basis and using the "banana" trick, here's what I've done (used OpenFOAM 2.3.x for this example):
  1. Made a copy of the tutorial "lagrangian/DPMFoam/Goldschmidt" and ran the utility blockMesh.
  2. Then I had to look at which file needed to modified. All pointed to the file "constant/kinematicCloudProperties".
  3. Now I had to figure out where the Lift comes in. After going around looking at the other tutorials and a few threads, the conclusion was that this block of dictionary is where we can stack up the various forces at work:
    Code:

        particleForces
        {
            ErgunWenYuDrag
            {
                alphac alpha.air;
            }
            gravity;
        }

  4. And here's where the "banana" comes in:
    Code:

        particleForces
        {
            ErgunWenYuDrag
            {
                alphac alpha.air;
            }
            gravity;
            banana;
        }

  5. As soon as I run DPMFoam, it complains about "banana" not being valid:
    Code:

    --> FOAM FATAL ERROR:
    Unknown particle force type banana, constructor not in hash table

        Valid particle force types are:

    13
    (
    ErgunWenYuDrag
    PlessisMasliyahDrag
    SRF
    SaffmanMeiLiftForce
    TomiyamaLift
    WenYuDrag
    gravity
    nonInertialFrame
    nonSphereDrag
    paramagnetic
    pressureGradient
    sphereDrag
    virtualMass
    )

    There's our pretty lift model "SaffmanMeiLiftForce".
  6. OK, rename "banana" to "SaffmanMeiLiftForce" and added brackets with a "banana" inside :rolleyes::
    Code:

        particleForces
        {
            ErgunWenYuDrag
            {
                alphac alpha.air;
            }
            gravity;
            SaffmanMeiLiftForce
            {
                banana;
            }
        }

    mmm... the solver crashed. So much for the "banana".
  7. OK, if we look at the source code for this model:
    Code:

    template<class CloudType>
    Foam::SaffmanMeiLiftForce<CloudType>::SaffmanMeiLiftForce
    (
        CloudType& owner,
        const fvMesh& mesh,
        const dictionary& dict,
        const word& forceType
    )
    :
        LiftForce<CloudType>(owner, mesh, dict, forceType)
    {}

    there is no coefficient necessary.
  8. Therefore, this should be enough:
    Code:

        particleForces
        {
            ErgunWenYuDrag
            {
                alphac alpha.air;
            }
            gravity;
            SaffmanMeiLiftForce;
        }

  9. Er, nope... it complains it should be a dictionary itself. Then back to this:
    Code:

        particleForces
        {
            ErgunWenYuDrag
            {
                alphac alpha.air;
            }
            gravity;
            SaffmanMeiLiftForce
            {
            }
        }

  10. So we go back to the crash. The error given is this:
    Code:

    --> FOAM FATAL ERROR:

        request for volVectorField U from objectRegistry region0 failed
        available objects of type volVectorField are
    1(U.air)

    OK, it's looking for the "U" field and it only found "U.air". So, either the model is just wrong, or something else is missing.
  11. Looking at the class from which this model derives, the constructor has a vital clue to what's missing:
    Code:

    template<class CloudType>
    Foam::LiftForce<CloudType>::LiftForce
    (
        CloudType& owner,
        const fvMesh& mesh,
        const dictionary& dict,
        const word& forceType
    )
    :
        ParticleForce<CloudType>(owner, mesh, dict, forceType, true),
        UName_(this->coeffs().template lookupOrDefault<word>("U", "U")),
        curlUcInterpPtr_(NULL)
    {}

    It's looking for a new name for "U", something like:
    Code:

    U U.air;
  12. So let's try this:
    Code:

        particleForces
        {
            ErgunWenYuDrag
            {
                alphac alpha.air;
            }
            gravity;
            SaffmanMeiLiftForce
            {
                U U.air;
            }
        }

    Side note: curiously enough, Maysam got a similar answer a few minutes ago in post #4 at http://www.cfd-online.com/Forums/ope...tml#post512965
  13. Running DPMFoam once again gives this error message:
    Code:

    --> FOAM FATAL IO ERROR:
    keyword curlUcDt is undefined in dictionary "/home/ofuser/OpenFOAM/ofuser-2.3.x/run/tutorials/lagrangian/DPMFoam/Goldschmidt/constant/kinematicCloudProperties.solution.interpolationSchemes"

    file: /home/ofuser/OpenFOAM/ofuser-2.3.x/run/tutorials/lagrangian/DPMFoam/Goldschmidt/constant/kinematicCloudProperties.solution.interpolationSchemes from line 27 to line 29.

    OK, we need to look at this this block of dictionary:
    Code:

    solution
    {
        active          true;
        coupled        true;
        transient      yes;
        cellValueSourceCorrection off;

        interpolationSchemes
        {
            rho.air        cell;
            U.air          cellPoint;
            mu.air          cell;
        }

        integrationSchemes
        {
            U              Euler;
        }

        sourceTerms
        {
            schemes
            {
                U semiImplicit 1;
            }
        }
    }

  14. Let's try:
    Code:

        interpolationSchemes
        {
            rho.air        cell;
            U.air          cellPoint;
            mu.air          cell;
            curlUcDt        banana;
        }

    The error message stated by DPMFoam:
    Code:

    --> FOAM FATAL ERROR:
    Unknown interpolation type banana for field curlUcDt

    Valid interpolation types :

    6
    (
    cell
    cellPatchConstrained
    cellPoint
    cellPointFace
    cellPointWallModified
    pointMVC
    )

  15. :confused: I have no idea. Let's try the most conservative/complex one "cellPointFace"... nope, it crashes. Let's try all others... nope, all of them crash.
  16. The error message of the crash is something like this:
    Code:

    Solving 3-D cloud kinematicCloud
    #0  Foam::error::printStack(Foam::Ostream&) in "/home/ofuser/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
    #1  Foam::sigFpe::sigHandler(int) in "/home/ofuser/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
    #2  in "/lib/x86_64-linux-gnu/libc.so.6"
    #3  Foam::SaffmanMeiLiftForce<Foam::KinematicCloud<Foam::Cloud<Foam::CollidingParcel<Foam::KinematicParcel<Foam::particle> > > > >::Cl(Foam::CollidingParcel<Foam::KinematicParcel<Foam::particle> > const&, Foam::Vector<double> const&, double, double) const in "/home/ofuser/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/liblagrangianIntermediate.so"
    #4  Foam::LiftForce<Foam::KinematicCloud<Foam::Cloud<Foam::CollidingParcel<Foam::KinematicParcel<Foam::particle> > > > >::calcCoupled(Foam::CollidingParcel<Foam::KinematicParcel<Foam::particle> > const&, double, double, double, double) const in "/home/ofuser/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/liblagrangianIntermediate.so"
    #5 
     in "/home/ofuser/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/DPMFoam"
    #6

    and it continues with more information, but doesn't help much more...
    So there was a "sigFpe", hence division by zero or infinite or something like that, in the method "::Cl" (it's in line #3).
  17. OK, looking at the source code for this method:
    Quote:

    https://github.com/OpenFOAM/OpenFOAM...MeiLiftForce.C
    Code:

    template<class CloudType>
    Foam::scalar Foam::SaffmanMeiLiftForce<CloudType>::SaffmanMeiLiftForce::Cl
    (
        const typename CloudType::parcelType& p,
        const vector& curlUc,
        const scalar Re,
        const scalar muc
    ) const
    {
        scalar Rew = p.rhoc()*mag(curlUc)*sqr(p.d())/(muc + ROOTVSMALL);
        scalar beta = 0.5*(Rew/(Re + ROOTVSMALL));
        scalar alpha = 0.3314*sqrt(beta);
        scalar f = (1.0 - alpha)*exp(-0.1*Re) + alpha;

        scalar Cld = 0.0;
        if (Re < 40)
        {
            Cld = 6.46*f;
        }
        else
        {
            Cld = 6.46*0.0524*sqrt(beta*Re);
        }

        return 3.0/(mathematical::twoPi*sqrt(Rew))*Cld;
    }


    :eek: there are a few possible locations where it might have broken.
  18. OK, let's go old-school debugging:
    Code:

    template<class CloudType>
    Foam::scalar Foam::SaffmanMeiLiftForce<CloudType>::SaffmanMeiLiftForce::Cl
    (
        const typename CloudType::parcelType& p,
        const vector& curlUc,
        const scalar Re,
        const scalar muc
    ) const
    {
        scalar Rew = p.rhoc()*mag(curlUc)*sqr(p.d())/(muc + ROOTVSMALL);
        Info << "Rew: " << Rew << endl;
       
        scalar beta = 0.5*(Rew/(Re + ROOTVSMALL));
        Info << "Re: " << Re << endl;
        Info << "beta: " << beta << endl;

        scalar alpha = 0.3314*sqrt(beta);
        Info << "alpha: " << alpha << endl;

        scalar f = (1.0 - alpha)*exp(-0.1*Re) + alpha;
        Info << "f: " << f << endl;

        scalar Cld = 0.0;
        if (Re < 40)
        {
            Cld = 6.46*f;
        }
        else
        {
            Cld = 6.46*0.0524*sqrt(beta*Re);
        }

        Info << "Cld: " << Cld << endl;

        return 3.0/(mathematical::twoPi*sqrt(Rew))*Cld;
    }

    we print out everything so that we can have a look at each value. It's good to know what's happening under-the-hood, instead of having to guess: http://openfoamwiki.net/index.php/HowTo_debugging
  19. And we have to build the modified library "src/lagrangian/intermediate":
    Code:

    wmake libso $FOAM_SRC/lagrangian/intermediate
  20. Let's have another go with DPMFoam... the output we now get:
    Code:

    Solving 3-D cloud kinematicCloud
    Rew: 0
    Re: 71.5702
    beta: 0
    alpha: 0
    f: 0.00077937
    Cld: 0

    :eek: that's waaaay too many zeros... this leads to this expression to go haywire:
    Code:

    return 3.0/(mathematical::twoPi*sqrt(Rew))*Cld;
    Because it becomes:
    Code:

    3.0/(2*Pi*sqrt(0.0))*0.0
    where it divides by zero.
  21. OK, we can try and insert a division protection like it's done for the others:
    Code:

    return 3.0/(mathematical::twoPi*sqrt(Rew+SMALL))*Cld;
  22. Build the library again and gave DPMFoam another run... didn't crash, but gave a lot of junk output. So I Ctrl+C to cancel the run and went back to the code and removed the "Info" lines I had added. And built the library again.
  23. Another run with DPMFoam and... and it's finally working! As to whether it's giving good or bad values, I have no idea.
In the meantime I'll report this bug, although I'm not sure if the fix I presented is correct or not :(.

-------------------
edit: Bug reported here: http://www.openfoam.org/mantisbt/view.php?id=1408

Additional note: Letting the case run first without any particles should initialize the "U.air" field, should no longer require you to modify the source code, since the flow field would all not be zero.
-------------------

Best regards,
Bruno

maysmech October 5, 2014 20:25

Thank you very much Bruno. I used a lot from your step by step debugging.
Especially Banana and Old-School debugging were fantastic.
This problem is for other forces too such as pressure gradient force.
However thanks for submit of the bug.

wyldckat October 18, 2014 13:38

FYI: Bug has been fixed: http://www.openfoam.org/mantisbt/view.php?id=1408
The official fix can be seen here: https://github.com/OpenFOAM/OpenFOAM...1d371bd9be3000

lithos November 21, 2014 07:54

Quote:

Originally Posted by wyldckat (Post 514974)

Dear Bruno, you made my day. Thank you very much for this little detail, explained very understandable. Cheers, Michael

P.S.: I used this with 2.2.x.

AJAY BHANDARI June 27, 2018 02:05

Brownian motion force not running when using uncoupledKinematicParcelFoam
 
Hi all,

I think my post best suits here.

Basically i am solving a steady state continuity and darcy equation to get steady state pressure and velocity fields, which go into a transient convection diffusion equation to solve time dependent concentration of a species in a computational domain. Now i want to couple my developed eulerain solver with lagrangian one.

For that i am using uncoupledKinematicParcelFoam and coupling it with my eulerian solver. The solver is compiled succesfully. But when i am running the case it is giving following error.
Code:

Constructing kinematicCloud kinematicCloud
--> FOAM Warning :
    From function entry::getKeyword(keyType&, Istream&)
    in file db/dictionary/entry/entryIO.C at line 80
    Reading /home/ajay/OpenFOAM/ajay-4.1/run/mytutorials/srmparticlenew/constant/kinematicCloudProperties
    found on line 64 the punctuation token '{'
    expected either } or EOF
Constructing particle forces
    Selecting particle force sphereDrag
    Selecting particle force gravity
    Selecting particle force BrownianMotion


--> FOAM FATAL ERROR:
Unknown particle force type BrownianMotion, constructor not in hash table

    Valid particle force types are:

13
(
ErgunWenYuDrag
PlessisMasliyahDrag
SRF
SaffmanMeiLiftForce
TomiyamaLift
WenYuDrag
gravity
nonInertialFrame
nonSphereDrag
paramagnetic
pressureGradient
sphereDrag
virtualMass
)


    From function static  Foam::autoPtr<Foam::ParticleForce<CloudType> >  Foam::ParticleForce<CloudType>::New(CloudType&, const  Foam::fvMesh&, const Foam::dictionary&, const Foam::word&)  [with CloudType =  Foam::KinematicCloud<Foam::Cloud<Foam::CollidingPa  rcel<Foam::KinematicParcel<Foam::particle> > > >]
    in file lagrangian/intermediate/lnInclude/ParticleForceNew.C at line 47.

FOAM exiting

I know the error is coming because of addition of Brownian motion force in the case.

Can anybody please help why the brownian motion force is not running for the case or where i am doing the mistake.

I have compiled the Lagrangian library properly. But in that there is no Brownian motion force in that. Brownian motion force is situated in different folder named turbulence. I compiled it as well but not running.

Any help will be appreciated.

Thanks
Ajay

wyldckat August 22, 2018 09:30

Greetings Ajay,


Sorry for the late reply, but I only managed to look into this now. Here is a quick notes answer:

  1. That force is deployed with this macro: https://github.com/OpenFOAM/OpenFOAM...ulenceForces.H
  2. That macro is only used in a few cloud types: https://github.com/OpenFOAM/OpenFOAM...rbulenceForces
  3. Essentially if your clouds are not of type spray, reactive nor thermal, then you cannot use that force, given that it depends on thermodynamic characteristics of the fluid(s).
  4. From your description, it's not clear if there is even temperature being used in your fluid transport, therefore this force may very likely not be usable in the first place.
  5. The warning given above the error message is of some concern, because a misplaced bracket pair "{ }" is enough to break the way the dictionary is read...
Best regards,
Bruno


All times are GMT -4. The time now is 00:57.