[Hgholami]

Dear
I try to solve FSI problem with two or more elastic beams in flow channel. First, I generate mesh with ansys mechanical and import to openFoam-ext4.0, then checkMesh and it OK. uses createPatch to merge some boundary and still mesh OK. after running after some timesteps, appear errors "Floating point exception (core dumped)". I checkMesh and found "Failed 1 mesh checks" with this statement
Checking geometry...
This is a 2-D mesh
Overall domain bounding box (-0.3 -0.025 0) (0.5 0.025 0.0002)
Mesh (non-empty, non-wedge) directions (1 1 0)
Mesh (non-empty) directions (1 1 0)
Mesh (non-empty, non-wedge) dimensions 2
***Number of edges not aligned with or perpendicular to non-empty directions: 153
Writing 306 points on non-aligned edges to set nonAlignedEdges
Boundary openness (1.17707e-20 7.90055e-19 7.14214e-19) Threshold = 1e-06 OK.
Max cell openness = 2.04795e-16 OK.
Max aspect ratio = 170.202 OK.
Minumum face area = 1.29252e-08. Maximum face area = 6.80809e-05. Face area magnitudes OK.
Min volume = 2.58504e-12. Max volume = 1.36162e-08. Total volume = 7.88827e-06. Cell volumes OK.
Mesh non-orthogonality Max: 50.0436 average: 12.3892 Threshold = 70
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 2.49004 OK.

Failed 1 mesh checks.
--------
Maybe it's due to dynamicMesh. My dynamicMeshDict is as:
dynamicFvMesh dynamicMotionSolverFvMesh;

twoDMotion yes;

solver refVelocityLaplacian;

diffusivity quadratic inverseDistance 2(elastic fix);

nNonOrthogonalCorrectors 2;
leastSquaresVolPoint yes;
----
I can't recognize why the error appear? Anyone Can help me? thanks a lot.

[simrego]

Hi!


I'm not so familiar with icoFsiElasticNonLinULSolidFoam, but based on your description it is seems like you have a 2D mesh, and i think the structure is moving out of the plane. ("***Number of edges not aligned with or perpendicular to non-empty directions: 153")
Try to constrain it in order to stay in the plane.
And you can visualize the bad points in paraview ("Writing 306 points on non-aligned edges to set nonAlignedEdges"), so you can check the location of the error.
And try to use planeStrain to avoid the Poisson effect. (Maybe this won't be a good modelling approach for you but you can try to find the problem)

[Hgholami]

Dear simrego
I use flattenMesh to fix the problem. again I run the solver, but in first time step after some iteration give error. Now the checkMesh is OK.
Time = 0.0001, iteration: 5
Maximal accumulated displacement of interface points: 0.00229892
Courant Number mean: 0.00785269 max: 4.97262 velocity magnitude: 14.1465
BiCGStab: Solving for Ux, Initial residual = 0.00175064, Final residual = 1.186e-07, No Iterations 3
BiCGStab: Solving for Uy, Initial residual = 0.00818076, Final residual = 7.47515e-07, No Iterations 3
Floating point exception (core dumped)
----------
is Anybody fix this error?

[Hgholami]

I change the parameters of fvscheme and the problem solved.

[wulonglong]

May i ask a question,

what is the difference between icoFsiElasticNonLinULSolidFoam and fsiFoam?

[Hgholami]

Dear wulonglong
I thinks the two solver have the same algorithm to solve FSI problem. The only reason that I use icoFsiElasticNonLinULSolidFoam, is due to separated files in the solver. I want to modify the fluid solver to add thermal equation. In my opinion, icoFsiElasticNonLinULSolidFoam is understandable than fsiFoam and easily we can add extra equation to it.

[popa]

Originally Posted by Hgholami

I change the parameters of fvscheme and the problem solved.

Could you explain the specific details?Here i need the parameters to continue the case,once i run the case and it stopped without other reminds but "Floating point exception (core dumped)".
Thank you in advance.

[popa]

Originally Posted by Nexfast

Hi everybody ,

I set openfoam extended to try HronTurek's tutorial with the solver icoFsiElasticNonLinULSolidFoam. Also, i used Openfoam4.1 and no problem to use icoFoam or pisoFoam solver, it works very well !

My problem is about openfoam extended : i have sourced the bashrc and did allwmake.firstinstall, it looks works but when I do ./Allrun in HronTurek tutorial, it makes empty log file in solid and fluid repository and in this log file it is written "./Allrun: 55: ./Allrun: icoFsiElasticNonLinULSolidFoam: not found" for log.icoFsiElasticNonLinULSolidFoam. All others log.file are empty.

If i source with the bashrc of Openfoam4.1, log.file in openfoamextended are well computed except the log.icoFsiElasticNonLinULSolidFoam because i think the bashrc doesn't active the icoFsiElasticNonLinULSolidFoam solver.

I work on a virtual toolbox. Openfoam4.1 are set in /opt/... (i often have to use "sudo command") and i set openfoam extended 4.0 in my home directory .... I don't know what is the problem. I work on that for 2 days yet whithout solving this problem

I would be very grateful if somebody could help me !!!
NewFast.

Also, i used Openfoam4.1 and i run the same case.But i can't see the solid to swing up and down,so i change the E of the solid,but it went wrong ,and give the information "Floating point exception (core dumped)".
Can you explain the ways to tun the case in detail?I have spent much time in this problem,thank you in advance.

[Hgholami]

check this first fvscheme

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | foam-extend: Open Source CFD |
| \\ / O peration | Version: 4.0 |
| \\ / A nd | Web: http://www.foam-extend.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default backward;
}

gradSchemes
{
default Gauss linear;

}

divSchemes
{
default none;
div(phi,U) Gauss skewCorrected linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}


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

and fvsolution

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | foam-extend: Open Source CFD |
| \\ / O peration | Version: 4.0 |
| \\ / A nd | Web: http://www.foam-extend.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
// p PCG
// {
// preconditioner DIC;
// tolerance 1e-06;
// relTol 0;
// };
p
{
solver GAMG;
tolerance 1e-06;
relTol 0;
minIter 1;
maxIter 1000;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;
scaleCorrection true;
directSolveCoarsest false;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
};

cellMotionU
{
solver GAMG;
tolerance 1e-6;
relTol 1e-3;
minIter 1;
maxIter 1000;

smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;

scaleCorrection true;
directSolveCoarsest false;

cacheAgglomeration true;

nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
};

U
{
solver BiCGStab;
preconditioner DILU;
tolerance 1e-06;
relTol 0;
};
}

PISO
{
nCorrectors 5;
nNonOrthogonalCorrectors 5;
nOuterCorrectors 50;
ddtPhiCorr yes;
}

relaxationFactors
{

fields
{
p 0.5;
}
equations
{
U 0.3;
}
}
// ************************************************** *********************** //

and couplingProperties

solidPatch plate;
solidZone plateZone;

fluidPatch plate;
fluidZone plateZone;

fsiRelaxationFactor 0.001;

interfaceDeformationLimit 0.05;

outerCorrTolerance 1e-3;

couplingScheme FixedRelaxation;

fsi yes;

maybe you need to use this trick, in first 2 second times, the fsi should off and then during the solution, you on it. In tutorial of fsiFoam, this trick used with object function

[popa]

Originally Posted by Hgholami

check this first fvscheme

and fvsolution

and couplingProperties

maybe you need to use this trick, in first 2 second times, the fsi should off and then during the solution, you on it. In tutorial of fsiFoam, this trick used with object function

Except this,did you change some other parameters,such as the E of the solid (compare to the basic case,because in another thread,you also saied you use some tools and use the solver of fsiFoam,then get the result.)

Thank you in advance.

[Hgholami]

which solver do you want to use? fsiFoam or icoFsiElasticNonLinULSolidFoam

[popa]

Originally Posted by Hgholami

which solver do you want to use? fsiFoam or icoFsiElasticNonLinULSolidFoam

icoFsiElasticNonLinULSolidFoa,because i use form-extend4.0

[Hgholami]

you can also use fsiFoam by installing FSI toolkits.
my configuration in icoFsiElasticNonLinULSolidFoam was

planeStress no;

rheology
{
type linearElastic;
rho rho [1 -3 0 0 0 0 0] 10000;
E E [1 -1 -2 0 0 0 0] 5.0e5;
nu nu [0 0 0 0 0 0 0] 0.4;
}

[popa]

Originally Posted by Hgholami

you can also use fsiFoam by installing FSI toolkits.
my configuration in icoFsiElasticNonLinULSolidFoam was

Thank you for your answer,you are patient and warmhearted .I will try it,thank you again.

[DouglasFreds]

Hi, Looks ok in my current ElmerGUI version. Maybe you have quite on old ElmerGUI? You could also try to translate it manually ElmerGrid 14 2 mymesh.msh -autoclean and the open the mesh in ElmerGUI. -Peter