[Redrakham]

Hi,
I am new in openFoam. I am solving sixdofrigidbodymotion for tandem arrangement of cylinder. I created the cylinders in gmsh and others in blockMessh. But when I try to setFields and setting topology only happens for one cylinder. I have tried everything but got nothing. Please help!!!
I am attaching my case here.

[mAlletto]

Can you describe the Problem in order that one does not have to download the files, run and look at the results?

This is a bit of work and probably this is the reason you did not get any answer yet

If you can pose your Problem in a way that one understands quickly what is going wrong the probabilty to get an answer is much higher than in the way you did it.

[Redrakham]

I am doing an OpenFoam case with two cylinders in tandem arrangement with overset mesh- a background mesh, one refinement zone and two cylinder mesh. I am using overPimpleDyMFoam but got this error: Attempt to cast type dynamicOversetFvMesh to type dynamicMotionSolverFvMesh.

This is my dynamicMeshDict:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: plus-overset |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

motionSolverLibs ("libsixDoFRigidBodyMotion.so");
dynamicFvMesh dynamicOversetFvMesh;
/*
dynamicOversetFvMeshCoeffs
{
// layerRelax 0.3;
}
*/

//motionSolverLibs ( "libfvMotionSolvers.so" );
//
//solver displacementLaplacian;
//
//displacementLaplacianCoeffs
//{
// diffusivity uniform 1;
//}


solver sixDoFRigidBodyMotion;

sixDoFRigidBodyMotionCoeffs
{
patches (cyl);

innerDistance 100.0;
outerDistance 101.0;

mass 1.5707963;
centreOfMass (0 0 0);
momentOfInertia (1 1 1);
orientation
(
1 0 0
0 1 0
0 0 1
);
velocity (0 0 0);
acceleration (0 0 0);
angularMomentum (0 0 0);
torque (0 0 0);

g (0 0 0);
rho rhoInf;
rhoInf 1;
accelerationRelaxation 0.9;
accelerationDamping 0.95;
report on;
reportToFile on;
solver
{
type Newmark;
}

constraints
{
yLine_1
{
sixDoFRigidBodyMotionConstraint line;
direction (0 1 0);
}

noAxis_1
{
sixDoFRigidBodyMotionConstraint orientation;
}
}

restraints
{
verticalSpring_1
{
sixDoFRigidBodyMotionRestraint linearSpring;

anchor (0 2 0);
refAttachmentPt (0 0 0);
stiffness 1.72257;
damping 0;
restLength 2;
}
}

}
************************************************** *********************** //

[mAlletto]

Can you sketch the case you are trying to solve

[mAlletto]

Did you have a look at this tutorial. There are two zones specified
https://develop.openfoam.com/Develop...woSimpleRotors

[Redrakham]

Here is the geometry.

[Redrakham]

I tried all the things but no hope.

[mAlletto]

Are the cylinders suposed to move independently from each other

[Redrakham]

No, they are rigidly connected.

[mAlletto]

Can you provide a zipped file which contains your case together with an allrun script to reproduce the error

[Redrakham]

It is the same case. Only I made two cylinders separately with blockMesh.

[mAlletto]

Hello what kind of OF version are you using?


I try to run the scripts with OF2012 and there are a lot of errors thrown. Like in all/ the system/blockMeshDict is missing ...
you run in the file run_mesh.sh the command blockMesh in the folder all and no blockMesh dict is present...




So I'm wondering if you have checked the script before you submitted it...

[Redrakham]

I have the same version of OpenFoam. I have not encountered the blockMeshDict problem. I run the command: "sh run_all.sh" in the moving cylinder directory not inside the all directory.

[mAlletto]

Which version do you have?

[Redrakham]

OpenFoam v2012.

[Redrakham]

My version is 2012. You can see it in the screenshot.

[mAlletto]

my version is the same





I'm wounder in your shell script run_meh.sh you have:

foamCleanTutorials

cd cylinder1
blockMesh | tee log.blockMesh
cd ..

cd cylinder2
blockMesh | tee log.blockMesh
cd ..

cd refinementZone
blockMesh | tee log.blockMesh
cd ..

cd all
blockMesh | tee log.blockMesh

so you run blockMesh in the directory all. But if no blockMeshDict is in all/system how it is possible you do not get any error.

[Redrakham]

Ooops!! My bad. I think some my files have gone missing while downloading. I will re-upload the case.

[Redrakham]

Here is the case file. I hope this time there will be no problem.

[mAlletto]

If you comment out the function object

sixDoFRigidBodyState
    {
        type           sixDoFRigidBodyState;
        libs           ("libsixDoFRigidBodyState.so");
        angleFormat    degrees;
    }

the simulation runs.


The problem is that the sixDoFRigidBodyState tries a dynamic cast in the write() function:

const dynamicMotionSolverFvMesh& mesh =
 
         refCast<const dynamicMotionSolverFvMesh>(obr_);

I.E. it tries to cast a dynamicOversetFvMesh to a dynamicMotionSolverFvMesh.



dynamicMotionSolverFvMesh is derived from dynamicFvMesh


dynamicOversetFvMesh is derived from dynamicMotionSolverListFvMesh


dynamicMotionSolverListFvMesh is derived from dynamicFvMesh


apparently this side cast does not work