[last_jedi]

Hi guys, i am quite new in OpenFoam. I have been trying to setup a RANS k-Omega simulation in OpenFoam. My mesh is exported from Pointwise in OpenFoam format and is a realistic car model created with T-Rex tool.

I have followed some tutorials in order to set-up my case in OpenFoam but i get the following Error. Any help pls..???


kOmegaSSTCoeffs
{
alphaK1 0.85;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.856;
gamma1 0.555556;
gamma2 0.44;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
b1 1;
c1 10;
F3 false;
}

No MRF models present

No finite volume options present


Starting time loop

Time = 0.001

smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.00741547, No Iterations 1
smoothSolver: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0
#0 Foam::error:rintStack(Foam::Ostream&) in "/apps/OpenFOAM+/OpenFOAM-v1612+/platforms/linux64IccDPInt32Opt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/apps/OpenFOAM+/OpenFOAM-v1612+/platforms/linux64IccDPInt32Opt/lib/libOpenFOAM.so"
#2 ? in "/lib64/libc.so.6"
#3 double Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) in "/apps/OpenFOAM+/OpenFOAM-v1612+/platforms/linux64IccDPInt32Opt/lib/libOpenFOAM.so"
#4 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/apps/OpenFOAM+/OpenFOAM-v1612+/platforms/linux64IccDPInt32Opt/lib/libOpenFOAM.so"
#5 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<d ouble>&, Foam::Field<double> const&) const in "/apps/OpenFOAM+/OpenFOAM-v1612+/platforms/linux64IccDPInt32Opt/lib/libOpenFOAM.so"
#6 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/apps/OpenFOAM+/OpenFOAM-v1612+/platforms/linux64IccDPInt32Opt/lib/libOpenFOAM.so"
#7 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/apps/OpenFOAM+/OpenFOAM-v1612+/platforms/linux64IccDPInt32Opt/lib/libOpenFOAM.so"
#8 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) in "/apps/OpenFOAM+/OpenFOAM-v1612+/platforms/linux64IccDPInt32Opt/lib/libfiniteVolume.so"
#9 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/apps/OpenFOAM+/OpenFOAM-v1612+/platforms/linux64IccDPInt32Opt/bin/simpleFoam"
#10 ? in "/apps/OpenFOAM+/OpenFOAM-v1612+/platforms/linux64IccDPInt32Opt/bin/simpleFoam"
#11 __libc_start_main in "/lib64/libc.so.6"
#12 ? in "/apps/OpenFOAM+/OpenFOAM-v1612+/platforms/linux64IccDPInt32Opt/bin/simpleFoam"
Floating point exception (core dumped)
s258761@ssw7228f-li [112] 06:41 PM [motorbike2]

[Kina]

please post fvSolution, fvSchemes and controlDict as code.
Why is your timestep 0.001 (looks transient) but your solver seems to be simpleFoam (steady)?

cheers
alex

[BlnPhoenix]

Have you tried "laminar" first? Is your case running succesfully with laminar?

From the error code alone it's not clear where the error sits in your setup.

[last_jedi]

Originally Posted by Kina

please post fvSolution, fvSchemes and controlDict as code.
Why is your timestep 0.001 (looks transient) but your solver seems to be simpleFoam (steady)?

cheers
alex

My timestep was initially 1, but i tried a smaller timestep to see if it could give any better results. My fvSolution, fvSchemes and controlDict are the following:

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
p
{
solver GAMG;
smoother GaussSeidel;
tolerance 1e-7;
relTol 0.01;
}

Phi
{
$p;
}


U
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

k
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

omega
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}
}

SIMPLE
{
nNonOrthogonalCorrectors 0;
consistent yes;

residualControl
{
p 0.001;
U 0.001;
k 0.001;
omega 0.001;
}
}

potentialFlow
{
nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
equations
{
U 0.3;
k 0.3;
omega 0.3;
}
}

cache
{
grad(U);
}

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



FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default cellLimited leastSquares 1.0;
}

divSchemes
{
default none;
div(phi,U) bounded Gauss linearUpwindV grad(U);
div(phi,k) bounded Gauss upwind;
div(phi,omega) bounded Gauss upwind;
div((nuEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default limited corrected 0.5;
}

wallDist
{
method meshWave;
}


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


FoamFile
{
version 2.0;
format ascii;
class dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application simpleFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 100;

deltaT 1;

writeControl timeStep;

writeInterval 100;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression uncompressed;

timeFormat general;

timePrecision 6;

runTimeModifiable true;

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

[Kina]

Why are you using such fancy schemes?
for grad, I would start with "default linear"
for snGrad, I would stay with "default corrected"
for div(phi,U), I would start with "bounded Gauss upwind" and then change it to "bounded Gauss linear" later.

From my experience, the rather fancy schemes in of really have to fit the problem. Otherwise, you are just making it worse.

One more thing: your smoothSolver says, it's solving only in X-direction. For y and z it shows 0 iterations. What's your checkMesh?

Timestep for simpleFoam is irrelevant since it doesn't have a time scheme. So 1 is ok and reasonable

Cheers
Alex

[last_jedi]

Originally Posted by Kina

Why are you using such fancy schemes?
for grad, I would start with "default linear"
for snGrad, I would stay with "default corrected"
for div(phi,U), I would start with "bounded Gauss upwind" and then change it to "bounded Gauss linear" later.

From my experience, the rather fancy schemes in of really have to fit the problem. Otherwise, you are just making it worse.

One more thing: your smoothSolver says, it's solving only in X-direction. For y and z it shows 0 iterations. What's your checkMesh?

Timestep for simpleFoam is irrelevant since it doesn't have a time scheme. So 1 is ok and reasonable

Cheers
Alex

Thank you for your advises. In the beginning my mesh check failed. But now its okk, after some changes in my initial mesh. Even though i followed your proposals i still get the same error. The only difference now is that in X-Direction it solves for 1000 it. and in y and z only 1 i.

[Kina]

Can you post the checkMesh output? Also, I would go for maxIter 100 on the velocity solver.

[last_jedi]

Originally Posted by Kina

Can you post the checkMesh output? Also, I would go for maxIter 100 on the velocity solver.

Where can i change max. iterations for velocity solver? My checkMesh screenshot is the following:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time


Create polyMesh for time = 0

Time = 0

Mesh stats
points: 1607575
faces: 17960892
internal faces: 17441560
cells: 8850613
faces per cell: 4
boundary patches: 7
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 0
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 8850613
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
car 436892 218448 ok (closed singly connected)
ceiling 5908 3043 ok (non-closed singly connected)
floor 71486 35832 ok (non-closed singly connected)
inlet_main 1076 586 ok (non-closed singly connected)
inlet_secondary 1452 788 ok (non-closed singly connected)
outflow_main 1072 584 ok (non-closed singly connected)
outflow_secondary 1446 785 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-13.839 -18.452 0) (36.904 18.452 9.226)
Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)
Boundary openness (2.18482e-18 -3.17211e-16 1.7067e-15) OK.
Max cell openness = 3.12272e-16 OK.
Max aspect ratio = 11.4276 OK.
Minimum face area = 3.29743e-07. Maximum face area = 1.39245. Face area magnitudes OK.
Min volume = 8.22926e-11. Max volume = 0.505525. Total volume = 17269.7. Cell volumes OK.
Mesh non-orthogonality Max: 61.7408 average: 19.6088
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.958172 OK.
Coupled point location match (average 0) OK.

Mesh OK.

End

[Kina]

In fvSolution, put for p:

solver GAMG;
smoother GaussSeidel;
tolerance 1e-7;
relTol 0.01;
maxIter 100;

The rest looks fine. Of course, your skewness and non-orthogonality are pretty high but that should not be the problem.
My final guess is that you could have messed something up with the boundary conditions. Can you post these?

[last_jedi]

I tried what you proposed for "p" in fvSolution but unfortunately doesn't change anything. My boundary file can be seen below. "Inlet secondary" and "outflow secondary" are just side walls of the outer box domain which i will use later in order to implement sidewind velocity. So at the moment i am using them as side walls and declared them as symmetry planes.


FoamFile
{
version 2.0;
format ascii;
class polyBoundaryMesh;
location "constant/polyMesh";
object boundary;
}

7
(
car
{
type wall;
nFaces 436892;
startFace 17441560;
}
ceiling
{
type symmetryPlane;
nFaces 5908;
startFace 17878452;
}
floor
{
type wall;
nFaces 71486;
startFace 17884360;
}
inlet_main
{
type patch;
nFaces 1076;
startFace 17955846;
}
inlet_secondary
{
type symmetryPlane;
nFaces 1452;
startFace 17956922;
}
outflow_main
{
type patch;
nFaces 1072;
startFace 17958374;
}
outflow_secondary
{
type symmetryPlane;
nFaces 1446;
startFace 17959446;
}
)

[Kina]

The maxIter stuff doesn't solve a problem. It's not supposed to. I'm just saying that if your solver takes more than 100 iterations to solve the matrix, there's something wrong with your setup.

I didn't mean the boundary file, but the boundary conditions:
0/p
0/U
0/k
0/omega

[last_jedi]

My boundary condition files are the following:


U:

FoamFile
{
version 2.0;
format ascii;
class volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

flowVelocity ( 16 0 0 );

pressure 0;

turbulentKE 0.1536;

turbulentOmega 0.155;

dimensions [ 0 1 -1 0 0 0 0 ];

internalField uniform ( 16 0 0 );


boundaryField
{

outflow_main
{
type inletOutlet;
inletValue uniform ( 0 0 0 );
value uniform ( 16 0 0 );
}

floor
{
type fixedValue;
value uniform (16 0 0);
}

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

ceiling
{
type symmetryPlane;

}

outflow_secondary
{
type symmetryPlane;
}

inlet_secondary
{
type symmetryPlane;

}

inlet_main
{
type fixedValue;
value uniform (16 0 0);
}

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

P:


FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0;

boundaryField
{

inlet_main
{
type zeroGradient;
}

outflow_main
{
type fixedValue;
value uniform 0;
}

floor
{
type zeroGradient;
}

car
{
type zeroGradient;
}

inlet_secondary
{
type symmetryPlane;
}


outflow_secondary
{
type symmetryPlane;
}

ceiling
{
type symmetryPlane;
}

}

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

K:


FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0.1536;

boundaryField
{

outflow_main
{
type inletOutlet;
inletValue uniform 0.1536;
value uniform 0.1536;
}

floor
{
type kqRWallFunction;
value uniform 0.1536;
}

car
{
type kqRWallFunction;
value uniform 0.1536;
}

outflow_secondary
{
type symmetryPlane;
}

inlet_secondary
{
type symmetryPlane;

}

ceiling
{
type symmetryPlane;
}

inlet_main
{
type fixedValue;
value uniform 0.1536;
}

}


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

omega:

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


dimensions [0 0 -1 0 0 0 0];

internalField uniform 0.155;

boundaryField
{
outflow_main
{
type inletOutlet;
inletValue uniform 0.155;
value uniform 0.155;
}

floor
{
type omegaWallFunction;
value uniform 0.155;
}

car
{
type omegaWallFunction;
value uniform 0.155;
}

ceiling
{
type symmetryPlane;
}

outflow_secondary
{
type symmetryPlane;
}

inlet_secondary
{
type symmetryPlane;
}

inlet_main
{
type fixedValue;
value uniform 0.155;
}

}


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

[Kina]

Without seeing a picture of your setup, I'd suggest the following:

Originally Posted by last_jedi

U:

FoamFile
{
version 2.0;
format ascii;
class volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

flowVelocity ( 16 0 0 );

pressure 0;

turbulentKE 0.1536;

turbulentOmega 0.155;

dimensions [ 0 1 -1 0 0 0 0 ];

internalField uniform ( 16 0 0 );


boundaryField
{

outflow_main
{
type zeroGradient;
}

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

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

ceiling
{
type symmetryPlane;
}

outflow_secondary
{
type symmetryPlane;
}

inlet_secondary
{
type symmetryPlane;

}

inlet_main
{
type fixedValue;
value uniform (16 0 0);
}

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

P:


FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0;

boundaryField
{

inlet_main
{
type zeroGradient;
}

outflow_main
{
type fixedValue;
value uniform 0;
}

floor
{
type zeroGradient;
}

car
{
type zeroGradient;
}

inlet_secondary
{
type symmetryPlane;
}


outflow_secondary
{
type symmetryPlane;
}

ceiling
{
type symmetryPlane;
}

}

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

K:


FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0.1536;

boundaryField
{

outflow_main
{
type zeroGradient;
}

floor
{
type kqRWallFunction;
value uniform 1e-8;
}

car
{
type kqRWallFunction;
value uniform 1e-8;
}

outflow_secondary
{
type symmetryPlane;
}

inlet_secondary
{
type symmetryPlane;

}

ceiling
{
type symmetryPlane;
}

inlet_main
{
type fixedValue;
value uniform 0.1536;
}

}


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

omega:

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


dimensions [0 0 -1 0 0 0 0];

internalField uniform 0.155;

boundaryField
{
outflow_main
{
type zeroGradient;
}

floor
{
type omegaWallFunction;
value uniform 1e7;
}

car
{
type omegaWallFunction;
value uniform 1e7;
}

ceiling
{
type symmetryPlane;
}

outflow_secondary
{
type symmetryPlane;
}

inlet_secondary
{
type symmetryPlane;
}

inlet_main
{
type fixedValue;
value uniform 0.155;
}

}


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

In summary: your BCs don't make much sense
- You are specifying pressure and velocity outlet
- you are specifying k and omega at outlet
- you are fixing a velocity on a wall patch

If you want the floor wall to be no slip which is not physical, then set the velocity to zerogradient. But never fix a velocity on a wall patch other than (0 0 0), that will blow up every case.

I have updated the new BCs in the Quote.
One more thing: why are you setting the ceiling to symmetry? I'd go for a patch or wall with zeroGradient BCs.

Cheers
Alex

[last_jedi]

First of all, thank you Alex so much for your immediate responses. I tried your updated modified files but still the problem seems to insist. I forgot to upload the nut file, maybe this needs some modification too. Finally as far as the ceiling concerns i am using symmetry plane in order to relief a bit the simulation load.

nut:

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -1 0 0 0 0];

internalField uniform 0;

boundaryField
{
inlet_secondary
{
type symmetryPlane;
}

inlet_main
{
type calculated;
value uniform 0;
}

outflow_main
{
type zeroGradient;
}

floor
{ type nutkWallFunction;
value uniform 0;
}

ceiling
{
type symmetryPlane;
}

car
{
type nutkWallFunction;
value uniform 0;
}

outflow_secondary
{
type symmetryPlane;
}

}


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

[Kina]

Should be ok with the nut. Depending if you're using LowRe SST, you can set the nut for wall to type calculated; value 0;
In case you are allowed to share the case files, I'd be willing to have a look into it since we have captured most of the sources for those errors so far. As I don't know what your mesh or setup looks like, I can only make certain guesses.
You can also upload the case and send a private message.

Cheers,
Alex

[hokhay]

Have you tried altering relTol and residualControl value. I usually use 0.01 for relTol and 1e-5 for residuals. Use potentialFoam to initialize the solution and check if something wrong with the boundary conditions.

Sent from my LG-H818 using CFD Online Forum mobile app

[Kina]

One more thing you can try to see if the solver at least takes more iterations to blow up:

in the fvSolution, change the underrelaxation to:

relaxationFactors
{
   fields
   {
     p     0.3;
   }
       equations
       {
             U                  0.3;
             k                  0.3;
             omega               0.3;
       }
}

Just to check if it's the initially large change in pressure causing the solver to crash.