[fedvasu]

Hi Foamers,

I have the case of rotating fan, which I simulated using cyclicAMI(cylinder) around the fan and motion of the cyclicAMI was moving with respect to the domain
like propeller tutorial I was not able to predict forces accurately (other parameters were match with experiments).


so I am trying another approach I am using dynamicMotionSolverFvMesh my pointDisplacement file. I am getting FPE, when I did unset FOAM_SIGFPE and started the solver after a while forces on my patch "Imperial.*" keep decreasing and /0 happens.
I presume the diffusivity solver should take care of the mesh motion but it isn't

I have kept Courant number 0.2 (for the AMI case Courant number 1-2 was used)

Any help would be appreciated

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       pointVectorField;
    location    "0.01";
    object      pointDisplacement;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 0 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    "ImperialBlade.*"
    {
      type            solidBodyMotionDisplacement;
      solidBodyMotionFunction axisRotationMotion;
      axisRotationMotionCoeffs {
	origin   (0 0 0);
	radialVelocity (0 -37.7 0);
      }
    }

    front
    {
      type            fixedValue;
      value           uniform (0 0 0);
    }

    back
    {
      type            fixedValue;
      value           uniform (0 0 0);
    }

     outerCylinder
     {
         type            fixedValue;
         value           uniform (0 0 0);
     }
}


// ************************************************************************* //

My dynamicMeshDict

/*--------------------------------*- C++ -*----------------------------------*\                                                                       
| =========                 |                                                 |                                                                       
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |                                                                       
|  \\    /   O peration     | Version:  2.2.1                                 |                                                                       
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |                                                                       
|    \\/     M anipulation  |                                                 |                                                                       
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //                                                                       

dynamicFvMesh   dynamicMotionSolverFvMesh;

motionSolverLibs ( "libfvMotionSolvers.so" );

solver displacementSBRStress;

displacementSBRStressCoeffs
{
  //diffusivity  uniform;                                                                                                                             
  // diffusivity  directional (1 200 0);                                                                                                              
  // diffusivity  motionDirectional (1 1000 0);                                                                                                       
  // diffusivity  file motionDiffusivity;                                                                                                             
  diffusivity  quadratic inverseDistance 1("ImperialBlade.*");
}

my FPE error

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::solidBodyMotionFunctions::axisRotationMotion::transformation() const in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libdynamicFvMesh.so"
#4  Foam::solidBodyMotionDisplacementPointPatchVectorField::solidBodyMotionDisplacementPointPatchVectorField(Foam::pointPatch const&, Foam::DimensionedField<Foam::Vector<double>, Foam::pointMesh> const&, Foam::dictionary const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libdynamicFvMesh.so"
#5  Foam::pointPatchField<Foam::Vector<double> >::adddictionaryConstructorToTable<Foam::solidBodyMotionDisplacementPointPatchVectorField>::New(Foam::pointPatch const&, Foam::DimensionedField<Foam::Vector<double>, Foam::pointMesh> const&, Foam::dictionary const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libdynamicFvMesh.so"
#6  Foam::pointPatchField<Foam::Vector<double> >::New(Foam::pointPatch const&, Foam::DimensionedField<Foam::Vector<double>, Foam::pointMesh> const&, Foam::dictionary const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#7  Foam::GeometricField<Foam::Vector<double>, Foam::pointPatchField, Foam::pointMesh>::GeometricBoundaryField::readField(Foam::DimensionedField<Foam::Vector<double>, Foam::pointMesh> const&, Foam::dictionary const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#8  Foam::GeometricField<Foam::Vector<double>, Foam::pointPatchField, Foam::pointMesh>::readFields(Foam::dictionary const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#9  Foam::GeometricField<Foam::Vector<double>, Foam::pointPatchField, Foam::pointMesh>::readFields() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#10   at displacementMotionSolver.C:0
#11  Foam::displacementMotionSolver::displacementMotionSolver(Foam::polyMesh const&, Foam::IOdictionary const&, Foam::word const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libdynamicMesh.so"
#12  Foam::displacementSBRStressFvMotionSolver::displacementSBRStressFvMotionSolver(Foam::polyMesh const&, Foam::IOdictionary const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libfvMotionSolvers.so"
#13  Foam::motionSolver::adddictionaryConstructorToTable<Foam::displacementSBRStressFvMotionSolver>::New(Foam::polyMesh const&, Foam::IOdictionary const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libfvMotionSolvers.so"
#14  Foam::motionSolver::New(Foam::polyMesh const&, Foam::IOdictionary const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libdynamicMesh.so"
#15  Foam::motionSolver::New(Foam::polyMesh const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libdynamicMesh.so"
#16  Foam::dynamicMotionSolverFvMesh::dynamicMotionSolverFvMesh(Foam::IOobject const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libdynamicFvMesh.so"
#17  Foam::dynamicFvMesh::addIOobjectConstructorToTable<Foam::dynamicMotionSolverFvMesh>::New(Foam::IOobject const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libdynamicFvMesh.so"
#18  Foam::dynamicFvMesh::New(Foam::IOobject const&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libdynamicFvMesh.so"
#19  
 in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/pimpleDyMFoam"
#20  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#21  
 in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/pimpleDyMFoam"
Floating point exception (core dumped)

[fedvasu]

when i unset FOAM_SIGFPE variable and run pimpleDyMFoam

I found this line

solidBodyMotionFunctions::axisRotationMotion::transformation(): Time = 0 transformation: ((nan nan -nan) (-nan (-nan -nan -nan)))

I am not sure why nan's are passed , do I have to make my blade an AMI?

[vasava]

Did you manage to solve your problem?

[fedvasu]

Originally Posted by vasava

Did you manage to solve your problem?

Hi Vasava,

yeah, If you unset FOAM_SIGFPE you'll notice that, omega*t is happening at 0 time as well.

Anyway I changed my dynamicMeshDict to use solidbody rotation and made my pointDisplacement as follows

pointDsiplacement

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       pointVectorField;
    location    "0.00001";
    object      pointDisplacement;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 0 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    "ImperialBlade.*"
    {
      type           calculated;
      uniform        (0 0 0);
    }

    front
    {
      type            fixedValue;
      value           uniform (0 0 0);
    }

    back
    {
      type            fixedValue;
      value           uniform (0 0 0);
    }

     outerCylinder
     {
         type            fixedValue;
         value           uniform (0 0 0);
     }
}
// ************************************************************************* //

dynamicMeshDict

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dynamicFvMesh   solidBodyMotionFvMesh;

motionSolverLibs ( "libFvMotionSolvers.so" );


solidBodyMotionFvMeshCoeffs
{
  solidBodyMotionFunction axisRotationMotion;
  axisRotationMotionCoeffs {
    patches   ("ImperialBlade.*");
    origin (0 0 0);
    radialVelocity (0 -2160 0);
  }

}

// ************************************************************************* //

my patch("ImperialBlade.*") moves just fine, but the forces are still over-predicting (Same as cyclicAMI case) and mass flow was way-off, way worse than cyclicAMI case (mayn't be due to mesh)

I will update if manage to get reasonable mass-flow and forces.

[vasava]

Ok. I was just curious about your dynamicMeshDict file. I am simulating objects thrown in to the air (like football) and am looking for help about mesh modifying with each time.

[fedvasu]

Originally Posted by vasava

Ok. I was just curious about your dynamicMeshDict file. I am simulating objects thrown in to the air (like football) and am looking for help about mesh modifying with each time.

if you know mass of your body, there is a provision to do 6-DOF mesh motion. checkout the wingMotion2D tutorial, I haven't tried but I was getting many results about 6-DOF while I was searching for this problem.

[vasava]

I have tried some of the 6dof tutorial successfully and even modified some tutorial to my needs. But these tutorials are good for cases where the final position of the moving object is not far from the original position.

I am looking for rather adaptive mesh. Currently I am reading about dynamicTopoFvMesh which seems promising to me.

Do you have any idea about adaptive mesh with openfoam??

[fedvasu]

Originally Posted by vasava

I have tried some of the 6dof tutorial successfully and even modified some tutorial to my needs. But these tutorials are good for cases where the final position of the moving object is not far from the original position.

I am looking for rather adaptive mesh. Currently I am reading about dynamicTopoFvMesh which seems promising to me.

Do you have any idea about adaptive mesh with openfoam??

Agreed 6DOF is great only if the motion is oscillatory or displacement isn't far from equilibrium point. I am not sure about the adaptive mesh techniques, I couldn't figure out how to use rawtopochangerfvMesh.

Anyway, if it is possible for you, please post the dynamicMeshDict and pointDisplacement (if applicable) or any other dict important for the set-up.

[vasava]

While looking for help I realized that the solver dynamicTopoFvMesh may do the trick. I have started a thread and Sandeep Menon who has developed this tool is guiding on how to make it work with openFoam 2.2.0.

[vasava]

Here is the pointDiplacement file. This is the file I modified from the floatingObject tutorial.