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

Fluent works... OF not?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 9, 2015, 06:01
Default Fluent works... OF not?
  #1
au1
New Member
 
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4
au1 is on a distinguished road
Sponsored Links
Hi everybody,
I'm studying Mechanical Engineering at Politecnico di Bari (Italy). I'm writing a thesis analyzing incompressible flow over an airfoil. (turbulence model: k-omega; flow velocity: 20 m/s; nu=10^-4 m^2/s; rho= 1 kg/m^3)

I made the mesh with Pointwise. I run it first with Fluent and it worked.

I tried to run the analysis in OpenFOAM so I adapted the "motorbike" tutorial to my case. But it doesn't work.

Quote:
Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
alphaK1 0.85034;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.85616;
gamma1 0.5532;
gamma2 0.4403;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
c1 10;
}

No field sources present


SIMPLE: no convergence criteria found. Calculations will run for 500 steps.


Starting time loop

Time = 1

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 at smoothSolver.C:0
#4 Foam::smoothSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#6
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#7
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
Floating point exception (core dumped)
Which is the problem? The smoothSolver? Boundary conditions? Mesh?

If you need any of the case files, please ask me.
au1 is offline   Reply With Quote
Sponsored Links

Old   January 9, 2015, 06:06
Default
  #2
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,688
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
Hi,

As the solver crashes during the first iteration, it can be mesh, schemes, ICs and BCs. So please post:

1. checkMesh output
2. fvSchemes file
3. 0 folder
alexeym is offline   Reply With Quote

Old   January 9, 2015, 07:06
Default
  #3
au1
New Member
 
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4
au1 is on a distinguished road
CheckMesh
Quote:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.0.1 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.0.1-51f1de99a4bc
Exec : checkMesh
Date : Jan 09 2015
Time : 11:58:32
Host : ime048
PID : 16607
Case : /home/tesisti/Togati/9-1-15/riferimento
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create polyMesh for time = 0

Time = 0

Mesh stats
points: 207080
internal points: 0
faces: 411979
internal faces: 204899
cells: 102813
boundary patches: 4
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 102813
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
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
frontAndBack 205626 207080 ok (non-closed singly connected)
inlet 797 1596 ok (non-closed singly connected)
outlet 258 518 ok (non-closed singly connected)
wall 399 798 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-8.99996 -10 0) (20.037 10 1)
Mesh (non-empty, non-wedge) directions (1 1 0)
Mesh (non-empty) directions (1 1 0)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (1.52339e-17 4.52257e-18 7.30337e-15) OK.
***High aspect ratio cells found, Max aspect ratio: 91679.8, number of cells 4620
<<Writing 4620 cells with high aspect ratio to set highAspectRatioCells
Minumum face area = 9.31926e-10. Maximum face area = 1.18331. Face area magnitudes OK.
Min volume = 9.31926e-10. Max volume = 0.755274. Total volume = 537.264. Cell volumes OK.
Mesh non-orthogonality Max: 86.8972 average: 3.26641
*Number of severely non-orthogonal faces: 49.
Non-orthogonality check OK.
<<Writing 49 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 0.693042 OK.

Failed 1 mesh checks.

End

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

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

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

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}
I attached the 0 folder.
Attached Files
File Type: zip 0.zip (3.3 KB, 3 views)
au1 is offline   Reply With Quote

Old   January 9, 2015, 09:23
Default
  #4
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,688
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
Hi,

I was not able to find errors in the settings, my suggestions will be quite generic:

1. Change smoothSolver to PBiCG. Dictionary for the solver you can find in $FOAM_TUTORIALS/heatTransfer/buoyantBoussinesqPimpleFoam/hotRoom/system/fvSolution.

2. As your mesh has highly non-orthogonal faces, consider using cellMDLimited modifications of schemes for gradients. Examples can be found in $FOAM_TUTORIALS/incompressible/pisoFoam/les/motorBike/motorBike/system/fvSchemes (though not quite sure it will be there in 2.1.1, I don't have this version installed).

3. Add bounded to divergence schemes. Example can be found in $FOAM_TUTORIALS/incompressible/simpleFoam/pitzDailyExptInlet/system/fvSchemes.
alexeym is offline   Reply With Quote

Old   January 9, 2015, 18:46
Default
  #5
Senior Member
 
anonymous
Join Date: Aug 2014
Posts: 204
Rep Power: 6
ssss is on a distinguished road
Your does seem to be the problem. Are you sure you changed frontAndBack to empty in the boundary file?
ssss is offline   Reply With Quote

Old   January 10, 2015, 08:12
Default
  #6
au1
New Member
 
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4
au1 is on a distinguished road
@alexeym

1) I changed the solver for U, k, omega from smoothSolver to PBiCG.

2) I used cellMDLimited

Quote:
gradSchemes
{
default cellMDLimited Gauss linear 1;
}
3) In fvSchemes file of pitzDailyExptInlet tutorial I found this:

Quote:
divSchemes
{
default none;
div(phi,U) Gauss upwind;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,R) Gauss upwind;
div(R) Gauss linear;
div(phi,nuTilda) Gauss upwind;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}
and when i tried to add "bounded" like this

Quote:
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*dev(T(grad(U))))) bounded Gauss linear;
}
or like this

Quote:
divSchemes
{
default bounded;
}

it gaves me an error:

Quote:
--> FOAM FATAL IO ERROR:
unknown div scheme bounded

Valid div schemes are :

1
(
Gauss
)

So I tried to run with only modifications 1 and 2.
Results:
Quote:
Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 6.09293e-05, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.000172088, No Iterations 1
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::Field<double> const&, Foam::Field<double> const&, Foam::Field<double> const&) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::lduMatrix const&, Foam::Field<double>&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 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::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#8
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
Floating point exception (core dumped)
@ssss
Yes, boundary conditions are ok.

Any more tips? Should be the problem the GAMGSolver (which is the selected solver for p)?
au1 is offline   Reply With Quote

Old   January 10, 2015, 09:27
Default
  #7
Senior Member
 
anonymous
Join Date: Aug 2014
Posts: 204
Rep Power: 6
ssss is on a distinguished road
In order to use bounded in the fvSchemes you need Openfoam2.2.0 or greater, you are using of2.1.1

Are you sure your boundary conditions are correct? Maybe there is a variable whith initial value of 0 (omega...)?
ssss is offline   Reply With Quote

Old   January 10, 2015, 09:30
Default
  #8
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,688
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
Hi,

Well, guess bounded was not implemented in 2.1.1.

According to the output, this time FPE happens in pEqn.H, so you've got two options:

1. Change solver for pressure to PCG.

2. Increase number of cell in coarsest level for GAMG solver (nCellsInCoarsestLevel). In general I set this value to nCellsInMesh^(1/3) (for 2D case it could be nCellsInMesh^(1/2), so for ~100,000 cells in your mesh the value should be around 320)

Also I've noticed this line in the output:

Code:
SIMPLE: no convergence criteria found. Calculations will run for 500 steps.
I think you should add residualControl to the SIMPLE dictionary in fvSolution file. You can find example in $FOAM_TUTORIALS/incompressible/simpleFoam/pitzDaily/system/fvSolution. Though in general final residuals should be around 1e-6 (in the example 1e-2/1e-3 were used).
alexeym is offline   Reply With Quote

Old   January 10, 2015, 12:14
Default
  #9
au1
New Member
 
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4
au1 is on a distinguished road
I'll download the 2.2 version as last option

@ssss
omega value is 1.78 everywhere. I uploaded the 0 folder in a precedent post so you can check it.

I added residualControl.

I increased the number of cell in coarsest level

Quote:
p
{
solver GAMG;
tolerance 1e-7;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration on;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 320;
mergeLevels 1;
}
but i had the same error.

So I changed the GAMG solver
Quote:
p
{
solver PCG;
preconditioner DIC;
tolerance 1e-6;
relTol 0;
}
It run. I set endTime=500 in order to monitorate the situation. When I tried to open the results in paraView i had a problem:

Quote:
created temporary '17-cfd.OpenFOAM'
Segmentation fault (core dumped)
So I couldn't visualize the results.

Looking to last outputs I think that something went wrong

Quote:
Time = 499

DILUPBiCG: Solving for Ux, Initial residual = 0.0176025, Final residual = 8.92661e-06, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.022828, Final residual = 8.31351e-06, No Iterations 1
DICPCG: Solving for p, Initial residual = 3.92221e-07, Final residual = 3.92221e-07, No Iterations 0
time step continuity errors : sum local = 2.19464e+34, global = 9.28582e+31, cumulative = 9.09985e+32
DILUPBiCG: Solving for omega, Initial residual = 0.119754, Final residual = 2.62773e-05, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.160839, Final residual = 5.17799e-05, No Iterations 1
ExecutionTime = 851.27 s ClockTime = 854 s

forceCoeffs output:
Cd = -3.43866e+69
Cl = -3.51752e+53
Cm = -1.71933e+69
Cl(f) = 1.71933e+69
Cl(r) = -1.71933e+69

Time = 500

DILUPBiCG: Solving for Ux, Initial residual = 0.0153715, Final residual = 7.43431e-06, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.0209576, Final residual = 1.01333e-05, No Iterations 1
DICPCG: Solving for p, Initial residual = 4.0874e-07, Final residual = 4.0874e-07, No Iterations 0
time step continuity errors : sum local = 2.21535e+34, global = 1.02473e+32, cumulative = 1.01246e+33
DILUPBiCG: Solving for omega, Initial residual = 0.112249, Final residual = 9.26829e-06, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.152886, Final residual = 4.04e-05, No Iterations 1
ExecutionTime = 859.41 s ClockTime = 862 s

forceCoeffs output:
Cd = -3.43851e+69
Cl = -3.51762e+53
Cm = -1.71925e+69
Cl(f) = 1.71925e+69
Cl(r) = -1.71925e+69

End
Force coefficients have impossible values. And what about the time step continuity errors?

Any more tips before updating OF in order to use the bounded divSchemes?
au1 is offline   Reply With Quote

Old   January 10, 2015, 13:59
Default
  #10
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,688
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
Hi,

"relTol 0" in pressure solver is too strict. Let it be 1e-2 or 0.1. Don't know what values of tolerance and relTol you have for velocity.

As you can see from residuals, solution is far from convergence. Increase endTime to say 25000. If solution converge earlier, it will just stop at the point of convergence.

Don't know the reason for the core dump, though as solution diverges, maybe certain values in result files lead to this behavior. Try using paraview's build-in OpenFOAM reader (paraFoam -builtin).
alexeym is offline   Reply With Quote

Old   January 10, 2015, 14:43
Default
  #11
au1
New Member
 
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4
au1 is on a distinguished road
I fixed the fvSolution file

Quote:
solvers
{
p
{
solver PCG;
preconditioner DIC;
tolerance 1e-6;
relTol 0.1;
}

U
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-6;
relTol 0.1;
}

k
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-6;
relTol 0.1;
}

omega
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-6;
relTol 0.1;
}
}

SIMPLE
{
nNonOrthogonalCorrectors 0;
}

residualControl
{
p 1e-6;
U 1e-6;
k 1e-6;
omega 1e-6
}

potentialFlow
{
nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.7;
k 0.7;
omega 0.7;
}
}

cache
{
grad(U);
}
I set endTime to 25000.

Results:

Quote:
Time = 826

DILUPBiCG: Solving for Ux, Initial residual = 0.459715, Final residual = 0.0100426, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.506025, Final residual = 0.0107321, No Iterations 1
DICPCG: Solving for p, Initial residual = 1.09289e-05, Final residual = 1.25529e-08, No Iterations 1
time step continuity errors : sum local = 4.44341e+58, global = 1.99964e+53, cumulative = 5.47876e+55
DILUPBiCG: Solving for omega, Initial residual = 0.533658, Final residual = 1.7975e-09, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.373316, Final residual = 1.61836e-07, No Iterations 1
ExecutionTime = 1028.32 s ClockTime = 1032 s

forceCoeffs output:
Cd = -1.33784e+122
Cl = -1.28579e+108
Cm = -6.68919e+121
Cl(f) = 6.68919e+121
Cl(r) = -6.68919e+121

Time = 827

DILUPBiCG: Solving for Ux, Initial residual = 0.507959, Final residual = 0.00769252, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.511595, Final residual = 0.00614268, No Iterations 1
DICPCG: Solving for p, Initial residual = 8.71646e-05, Final residual = 9.2361e-08, No Iterations 1
time step continuity errors : sum local = 4.93263e+58, global = 4.62504e+51, cumulative = 5.47922e+55
DILUPBiCG: Solving for omega, Initial residual = 0.517434, Final residual = 1.72607e-06, No Iterations 1
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#5 Foam::fvMatrix<double>::solve() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#6 Foam::incompressible::RASModels::kOmegaSST::correc t() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#7
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
Floating point exception (core dumped)
au1 is offline   Reply With Quote

Old   January 10, 2015, 14:56
Default
  #12
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,688
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
Hi,

1. Increase number of non-orthogonal correctors. nNonOrthogonalCorrectors in SIMPLE dictionary. Set it to 3-4.

2. If solution still diverges. Relax more. Set relaxation factor for velocity to 0.3.
alexeym is offline   Reply With Quote

Old   January 12, 2015, 10:55
Default
  #13
au1
New Member
 
Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4
au1 is on a distinguished road
I set the number of non-orthogonal correctors to 4.

Quote:
Time = 24999

DILUPBiCG: Solving for Ux, Initial residual = 1.57507e-05, Final residual = 2.77971e-07, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 8.88111e-05, Final residual = 3.18473e-06, No Iterations 2
DICPCG: Solving for p, Initial residual = 0.000894356, Final residual = 8.78172e-05, No Iterations 9
DICPCG: Solving for p, Initial residual = 9.23095e-05, Final residual = 9.02085e-06, No Iterations 94
DICPCG: Solving for p, Initial residual = 9.77823e-06, Final residual = 9.6372e-07, No Iterations 55
DICPCG: Solving for p, Initial residual = 1.04882e-06, Final residual = 6.18521e-07, No Iterations 1
DICPCG: Solving for p, Initial residual = 6.19302e-07, Final residual = 6.19302e-07, No Iterations 0
time step continuity errors : sum local = 4.35178e-08, global = 8.0513e-09, cumulative = 1.09825e-05
DILUPBiCG: Solving for omega, Initial residual = 8.58339e-07, Final residual = 8.58339e-07, No Iterations 0
DILUPBiCG: Solving for k, Initial residual = 1.79678e-05, Final residual = 4.7525e-07, No Iterations 1
ExecutionTime = 9546.81 s ClockTime = 9575 s

forceCoeffs output:
Cd = 0.0370108
Cl = 5.52511e-19
Cm = 0.0185054
Cl(f) = -0.0185054
Cl(r) = 0.0185054

Time = 25000

DILUPBiCG: Solving for Ux, Initial residual = 1.57509e-05, Final residual = 2.77264e-07, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 8.88113e-05, Final residual = 3.18471e-06, No Iterations 2
DICPCG: Solving for p, Initial residual = 0.000875004, Final residual = 7.37109e-05, No Iterations 10
DICPCG: Solving for p, Initial residual = 9.25738e-05, Final residual = 8.82807e-06, No Iterations 90
DICPCG: Solving for p, Initial residual = 2.34116e-05, Final residual = 2.25928e-06, No Iterations 32
DICPCG: Solving for p, Initial residual = 1.41847e-05, Final residual = 1.23549e-06, No Iterations 2
DICPCG: Solving for p, Initial residual = 1.30288e-05, Final residual = 1.02704e-06, No Iterations 1
time step continuity errors : sum local = 7.21817e-08, global = -8.91159e-09, cumulative = 1.09736e-05
DILUPBiCG: Solving for omega, Initial residual = 8.58635e-07, Final residual = 8.58635e-07, No Iterations 0
DILUPBiCG: Solving for k, Initial residual = 1.79674e-05, Final residual = 4.85255e-07, No Iterations 1
ExecutionTime = 9552.63 s ClockTime = 9581 s

forceCoeffs output:
Cd = 0.0370012
Cl = 5.52454e-19
Cm = 0.0185006
Cl(f) = -0.0185006
Cl(r) = 0.0185006

End
Why lift coefficient is so small? (Fluent result for Cl was 0.8)
au1 is offline   Reply With Quote

Old   January 12, 2015, 11:19
Default
  #14
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,688
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
Hi,

If you take a look at forceCoeffs.C:

Code:
        // lift, drag and moment
        coeffs[0] = (totForce & liftDir_)/(Aref_*pDyn);
        coeffs[1] = (totForce & dragDir_)/(Aref_*pDyn);
        coeffs[2] = (totMoment & pitchAxis_)/(Aref_*lRef_*pDyn);

        scalar Cl = sum(coeffs[0]);
        scalar Cd = sum(coeffs[1]);
        scalar Cm = sum(coeffs[2]);
If your Cd is OK, then, I guess, you've made a mistake in liftDir_ vector.
alexeym is offline   Reply With Quote

Old   January 12, 2015, 11:39
Default
  #15
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 20
RodriguezFatz will become famous soon enough
Angelo please try:
Code:
p
    {
    solver           GAMG;
        tolerance        1e-12;
        relTol           0.1;
        smoother         DICGaussSeidel;
        nPreSweeps       0;
        nPostSweeps      1;
    nFinestSweeps    2;
    scaleCorrection  true;
    directSolveCoarsestLevel false;
        cacheAgglomeration on;
        agglomerator     faceAreaPair;
        nCellsInCoarsestLevel 500;
        mergeLevels      1;
        maxIter         100;
    }
and for all others:
Code:
"(U|k|omega)"
{
        solver           smoothSolver;
    preconditioner   DILU;
        smoother         DILUGaussSeidel;
        tolerance        1e-12;
        relTol           0.1;
        nSweeps          1;
        maxIter         100;
    }
and post the log output.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   January 12, 2015, 11:40
Default
  #16
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 20
RodriguezFatz will become famous soon enough
Also one very clever person in this forum wrote you should never limit the pressure gradient.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   January 12, 2015, 12:03
Default
  #17
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,688
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
In fact it was here: http://www.openfoam.org/mantisbt/view.php?id=1410#c3246
alexeym is offline   Reply With Quote

Old   January 13, 2015, 02:18
Default
  #18
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 20
RodriguezFatz will become famous soon enough
Right there, henry... very clever.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Interesting problem: Parallel Processor VOF Fluent + Dynamic Mesh + System Coupling spaceprop FLUENT 5 September 2, 2014 09:43
The fluent stopped and errors with "Emergency: received SIGHUP signal" yuyuxuan FLUENT 0 December 3, 2013 23:56
What the differences flow equation of Fluent 6.3 and Fluent 12.1 opehterinar81 FLUENT 0 August 19, 2011 11:55
Fluent 6.3 32bit vs Fluent 12.0 64bit ibex7 FLUENT 7 April 18, 2011 02:44
How does a Fluent LICENCE works? Freeman FLUENT 4 April 14, 2006 05:58

Sponsored Links


All times are GMT -4. The time now is 07:35.