CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

problem with mesh after some timesteps in icoFsiElasticNonLinULSolidFoam solver

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By Hgholami
  • 1 Post By popa

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 17, 2019, 09:56
Default problem with mesh after some timesteps in icoFsiElasticNonLinULSolidFoam solver
  #1
Senior Member
 
Hojatollah Gholami
Join Date: Jan 2019
Posts: 133
Rep Power: 4
Hgholami is on a distinguished road
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.
Hgholami is offline   Reply With Quote

Old   January 17, 2019, 11:02
Default
  #2
Senior Member
 
anonymous
Join Date: Jan 2016
Posts: 405
Rep Power: 11
simrego is on a distinguished road
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)
simrego is offline   Reply With Quote

Old   January 18, 2019, 01:08
Default
  #3
Senior Member
 
Hojatollah Gholami
Join Date: Jan 2019
Posts: 133
Rep Power: 4
Hgholami is on a distinguished road
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 is offline   Reply With Quote

Old   January 18, 2019, 12:58
Default
  #4
Senior Member
 
Hojatollah Gholami
Join Date: Jan 2019
Posts: 133
Rep Power: 4
Hgholami is on a distinguished road
I change the parameters of fvscheme and the problem solved.
Hgholami is offline   Reply With Quote

Old   January 20, 2019, 23:12
Default
  #5
New Member
 
wulonglong
Join Date: Jan 2018
Posts: 7
Rep Power: 5
wulonglong is on a distinguished road
May i ask a question,

what is the difference between icoFsiElasticNonLinULSolidFoam and fsiFoam?
wulonglong is offline   Reply With Quote

Old   January 21, 2019, 01:12
Default
  #6
Senior Member
 
Hojatollah Gholami
Join Date: Jan 2019
Posts: 133
Rep Power: 4
Hgholami is on a distinguished road
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.
wulonglong likes this.
Hgholami is offline   Reply With Quote

Old   March 21, 2019, 07:45
Default Dear Hgholami
  #7
Member
 
...
Join Date: Jan 2019
Posts: 31
Rep Power: 4
popa is on a distinguished road
Quote:
Originally Posted by Hgholami View Post
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.
Goddi likes this.
popa is offline   Reply With Quote

Old   March 21, 2019, 08:10
Default Dear Nexfast
  #8
Member
 
...
Join Date: Jan 2019
Posts: 31
Rep Power: 4
popa is on a distinguished road
Quote:
Originally Posted by Nexfast View Post
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.
popa is offline   Reply With Quote

Old   March 21, 2019, 09:13
Default
  #9
Senior Member
 
Hojatollah Gholami
Join Date: Jan 2019
Posts: 133
Rep Power: 4
Hgholami is on a distinguished road
check this first fvscheme
Quote:
/*--------------------------------*- 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
Quote:
/*--------------------------------*- 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
Quote:
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
Hgholami is offline   Reply With Quote

Old   March 21, 2019, 22:56
Default Dear Hgholami
  #10
Member
 
...
Join Date: Jan 2019
Posts: 31
Rep Power: 4
popa is on a distinguished road
Quote:
Originally Posted by Hgholami View Post
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.
popa is offline   Reply With Quote

Old   March 22, 2019, 00:41
Default
  #11
Senior Member
 
Hojatollah Gholami
Join Date: Jan 2019
Posts: 133
Rep Power: 4
Hgholami is on a distinguished road
which solver do you want to use? fsiFoam or icoFsiElasticNonLinULSolidFoam
Hgholami is offline   Reply With Quote

Old   March 22, 2019, 04:11
Default Dear Hgholami
  #12
Member
 
...
Join Date: Jan 2019
Posts: 31
Rep Power: 4
popa is on a distinguished road
Quote:
Originally Posted by Hgholami View Post
which solver do you want to use? fsiFoam or icoFsiElasticNonLinULSolidFoam
icoFsiElasticNonLinULSolidFoa,because i use form-extend4.0
popa is offline   Reply With Quote

Old   March 22, 2019, 05:37
Default
  #13
Senior Member
 
Hojatollah Gholami
Join Date: Jan 2019
Posts: 133
Rep Power: 4
Hgholami is on a distinguished road
you can also use fsiFoam by installing FSI toolkits.
my configuration in icoFsiElasticNonLinULSolidFoam was
Quote:
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;
}
Hgholami is offline   Reply With Quote

Old   March 22, 2019, 06:34
Default Dear Hgholami
  #14
Member
 
...
Join Date: Jan 2019
Posts: 31
Rep Power: 4
popa is on a distinguished road
Quote:
Originally Posted by Hgholami View Post
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.
popa is offline   Reply With Quote

Old   February 2, 2020, 10:53
Default problem with mesh after some timesteps in icoFsiElasticNonLinULSolidFoam solver
  #15
New Member
 
DouglasFreds
Join Date: Jan 2020
Posts: 3
Rep Power: 3
DouglasFreds is on a distinguished road
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
DouglasFreds is offline   Reply With Quote

Reply

Tags
dynamicmeshdict, fsi, fsi 2-way

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 37 July 20, 2020 06:38
[Other] engineFoam new mesh problem ayhan515 OpenFOAM Meshing & Mesh Conversion 5 August 10, 2015 09:45
[ICEM] problem in mesh output mehrzad ANSYS Meshing & Geometry 2 December 10, 2014 19:07
[ICEM] Problem making structural mesh on a surface froztbear ANSYS Meshing & Geometry 1 November 10, 2011 09:52
A Mesh or Solver setup problem philippose OpenFOAM Running, Solving & CFD 3 November 5, 2006 15:54


All times are GMT -4. The time now is 02:16.