[DaChris]

Hi,

I want to test a new curvature model by using InterFoam. When I try to compile the following code I get an error, but I don't know how to fix it. I hope, someone can help me.

//Cell gradient of gamma
    volVectorField gradGamma = fvc::grad(gamma);
    // Interpolated face-gradient of gamma
    
    surfaceScalarField phiGradGamma = fvc::interpolate(gradGamma)& mesh.Sf();
     
    //curvature  
    surfaceScalarField kappa =     ((1) / mag(gradGamma))
                    * (((gradGamma)/(mag(gradGamma))) 
                    * fvc::grad(mag(gradGamma)) 
      //line.29=>              - fvc::div(phiGradGamma));

And this is the first error:

curvature.H:29: error: conversion from ‘Foam::tmp<Foam::GeometricField<Foam::Tensor<doubl e>, Foam::fvPatchField, Foam::volMesh> >’ to non-scalar type ‘Foam::surfaceScalarField’ requested

[kathrin_kissling]

Dear Chris,

the error you get tells you your problem quite clearly. You just need to check carefully.
You want to calculate a surfaceScalarField for the curvature. Obviosly there is a volTensorField somewhere inside your calculation. Because it is not possible to initialize a surfaceScalarField by a volTensorField you get an error.
Go carefully through your expression and you will find

//curvature
surfaceScalarField kappa = ((1) / mag(gradGamma))
* (((gradGamma)/(mag(gradGamma)))
* fvc::grad(mag(gradGamma))
//line.29=> - fvc::div(phiGradGamma));(1)/mag(gradGamma) gives you a volScalarField (remember you want to have a surfaceScalarField, at least you seam to initialize it that way)

you multiply it by the volVectorField (gradGamma)/mag(gradGamma)
now you have a volVectorField

now you perform another multiplication and I'm not sure what you inted to do. you multiply it by another volVectorField. The * operator gives you the outer product of two vectors and produces a tensor. Now we have your volTensorField. In addition you now want to subtract the divergence of a scalar? What is that?

In summary:

1. you are not allowed to mix fields defined on the faces and on the volumes.

2. you should go over your mathematics, I think theres a bug inside your implementation or inside the equation you are trying to implement. If you need help on that, we would need the equation

Hope this helps
Best

Kathrin

[DaChris]

Dear Kathrin,

thank you for the hints. I think my implementation is blemished. I'll go through my implementation and try to correct it. If this doesn't work, I would post the equation.


Best

Chris

[DaChris]

Hi,

I did it and compiled the solver, but a new problem appears.

Here is the equation:

volVectorField gradGamma = fvc::grad(gamma);

volScalarField kappa =     ((1) / mag(gradGamma))
                    *((((gradGamma)/(mag(gradGamma)))  
                    & fvc::grad(mag(gradGamma)))
                     - (fvc::div(gradGamma)
                    ));

Further the undefined keyword is caused by (fvc::div(gradGamma)).

keyword div(grad(gamma)) is undefined in dictionary "~/case/yTestCase2/system/fvSchemes::divSchemes"

file: ~/case/yTestCase2/system/fvSchemes::divSchemes from line 33 to line 40.

From function dictionary::lookupEntry(const word& keyword) const
in file db/dictionary/dictionary.C at line 213.

FOAM exiting

When I define the keyword in fvSchemes, I get an EOF error for Gauss upwind e.g and when I try Gauss linear, I get a floating Point exception.

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/caelinux/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/caelinux/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) in "/home/caelinux/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(Foam::dimensioned<double> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) in "/home/caelinux/OpenFOAM/caelinux-1.5/applications/bin/linux64GccDPOpt/myFoam"
#5 main in "/home/caelinux/OpenFOAM/caelinux-1.5/applications/bin/linux64GccDPOpt/myFoam"
#6 __libc_start_main in "/lib/libc.so.6"
#7 Foam::regIOobject::readIfModified() in "/home/caelinux/OpenFOAM/caelinux-1.5/applications/bin/linux64GccDPOpt/myFoam"
Floating point exception

[kathrin_kissling]

Hi Chris,

what you yre trying to do is applying a laplacian. So you should do something like

fvc::laplacian(gamma)

instead of

fvc::div(gradGamma)

be very carefull with the mathematics!

of course, then you need to specify a laplacian scheme.

You can also go


fvc::laplacian(gamma, nameOfYourDesiredScheme)

then the scheme is hardcoded and cannot be changed from fvSchemes.

Check on src/finiteVolume/finiteVolume/fvc/fvcLaplacian.H/.C
for details.

Hope this helps

Kathrin

[DaChris]

Hi kathrin,

I tried fvc::laplacian(gamma) with Gauss linear corrected, running the case and I get a floating point exception.

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/caelinux/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/caelinux/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) in "/home/caelinux/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(Foam::dimensioned<double> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) in "/home/caelinux/OpenFOAM/caelinux-1.5/applications/bin/linux64GccDPOpt/cstFoam"
#5 main in "/home/caelinux/OpenFOAM/caelinux-1.5/applications/bin/linux64GccDPOpt/myFoam"
#6 __libc_start_main in "/lib/libc.so.6"
#7 Foam::regIOobject::readIfModified() in "/home/caelinux/OpenFOAM/caelinux-1.5/applications/bin/linux64GccDPOpt/myFoam"
Floating point exception

Unfortunately, my OpenFoam skills are too low to interpret this error.

[kathrin_kissling]

Could you do me a favour?

Get rid of the laplacian term for a second, and check whether the problem really is in that one.

If this is not the point.

Maybe your dividing by zero somewhere.
Try

1/(mag(gradGamma)+SMALL)
where SMALL is a small number rescueing you from dividing by zero, which will definitly give you a floating point exeption.

Best

Kathrin

[DaChris]

Hi Kathrin,

I tried +SMALL, but it seems there are more divisions by zero. I think this division makes problems:

gradGamma/mag(gradGamma)

When I look into interfaceProperties, I find this:
surfaceVectorField nHatfv = gradGammaf/(mag(gradGammaf) + deltaN_)

I'm not sure, but I think that this missing deltaN_ causes the floating point exceptions.

deltaN_ ( "deltaN" 1e-8/pow(average(gamma.mesh().V()), 1.0/3.0) )


Edit:
I fixed the floating point exception. The problem was a couple of division by zero. Thank you very much Kathrin for the hint. But now, there is a dimension problem.

Best

Chris

[duongquaphim]

Hi Chris,

I am doing Taylor bubble simulation with OF. I also have some problems with curvature since it is very important in my flow.

Do you get a better result with your model of calculating curvature? Can you share some of your tests?

Regards,

Duong

[Andrea_85]

Hi,

I also try to define the curvature of the interface for my simulation using interFoam. Has anyone found a good way to get it?? because with the classical definition in interfaceProperties.C i get strange results.

Thanks
andrea

[idefix]

Hi,

I am a little confused of how the interface in a cell is modeled in the interFoam-solver. I´ve got difficulties to imagine one step.

If I am right, the following steps are repeated:
- alpha1 is calculated
- interface unit normal vector is calculated (PhD Rusche eq(4.17))
- the curvature is calculated with this normal vector.

I can´t really understand how I get the interface from the curvature.

Can somebody help me please?

Thanks a lot
Idefix

[vigneshTG]

Hi all !!

I am also trying to model the surface tension force with a new formulation :

I have modified some of the lines (in bold letters) in PEqn.H file in interfoam solver directory to model the force.

volScalarField lapalpha(fvc::laplacian(alpha1));
surfaceScalarField phig
    (
        (

                 fvc::interpolate(lapalpha)*interface.sigma()*interface.nHatf()
           - ghf*fvc::snGrad(rho)
        )*rAUf*mesh.magSf()
    );

I was able to compile the solver but, when i run a test case, i get floating point exception (core dumped) error. Can someone help me with this ?
Also, I want to know whether i have coded correctly ?

I am new to Openfoam !!

Thanks and Regards
Vignesh TG

[Martin_K_lalelu]

Hi Vignesh,

curvature calculation seems to be crucial in interfoam/CSF, did you make any progress with this approach?


best regards

Martin

[vigneshTG]

Hi Martin,

I implemented the above formulation but it doesn't work properly. I suggest you to give a try to the code interfoamssf posted in this thread !! There is also a paper by the same person regarding its formulation.

also this thread how is parasitic currents now ?

[Martin_K_lalelu]

Thanks a lot for your answer, I will have a look!

[Z.Q. Niu]

Dear Martin,
Have you got any new idea about the curvature model for interFoam ?