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

atmospheric wind study

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 14, 2011, 03:50
Default atmospheric wind study
  #1
New Member
 
chyn wey lee
Join Date: Apr 2009
Posts: 22
Rep Power: 7
djstoneage is on a distinguished road
Hi all i am tryng to model an atmospheric wind over an off shore platform with a K-Epsilon model. when i run simpleFoam im getting a pointstack error as below :_

Code:
[clee@localhost QU]$ simpleFoam
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.6.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 1.6.x
Exec   : simpleFoam
Date   : Mar 14 2011
Time   : 15:38:01
Host   : localhost.localdomain
PID    : 6519
Case   : /home/clee/Desktop/QU
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
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 kEpsilon
--> Upgrading k to employ run-time selectable wall functions
    Backup original k to k.old
    Writing updated k
--> Upgrading epsilon to employ run-time selectable wall functions
    Backup original epsilon to epsilon.old
    Writing updated epsilon
--> Creating nut to employ run-time selectable wall functions
    Writing new nut
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    sigmaEps        1.3;
}


Starting time loop

Time = 1

smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 0.05163843541, No Iterations 3
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 0.05450915783, No Iterations 3
smoothSolver:  Solving for Uz, Initial residual = 1, Final residual = 0.03639899326, No Iterations 2
#0  Foam::error::printStack(Foam::Ostream&) in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::sigFpe::sigFpeHandler(int) in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2  __restore_rt at sigaction.c:0
#3  Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#4  Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#5  Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#6  Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#7  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#8  Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#9  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::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 "/home/clee/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#10  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#11  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#12  main in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam"
#13  __libc_start_main in "/lib64/libc.so.6"
#14  Foam::regIOobject::writeObject(Foam::IOstream::streamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/clee/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam"
Floating point exception

anyone has got any idea on whats the problem
djstoneage is offline   Reply With Quote

Old   March 14, 2011, 21:23
Default
  #2
New Member
 
chyn wey lee
Join Date: Apr 2009
Posts: 22
Rep Power: 7
djstoneage is on a distinguished road
noone has an asnwer to this??
djstoneage is offline   Reply With Quote

Old   March 15, 2011, 09:00
Default atmospheric wind study
  #3
New Member
 
Goncalo Pedro
Join Date: Nov 2009
Location: Vancouver, British Columbia
Posts: 26
Rep Power: 6
gonpe is on a distinguished road
How are you specifying your boundary conditions?

Goncalo
gonpe is offline   Reply With Quote

Old   March 15, 2011, 22:49
Default
  #4
New Member
 
chyn wey lee
Join Date: Apr 2009
Posts: 22
Rep Power: 7
djstoneage is on a distinguished road
currently my boundry condition is a cylindrical control volume. ive specified the top and the sides to be an inlet the bottom of the control volume which represent the sea and my geometry(offshore plateform) to be walls.

i am trying to run a simple kepsilon turbulence model.

i need help in setting up the case, i am trying to replicate a CFX run to validate results.
djstoneage is offline   Reply With Quote

Old   March 16, 2011, 04:34
Default
  #5
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 408
Rep Power: 10
mvoss is on a distinguished road
no offense but even in CFX:
-if its a cylinder and you have one wall and 2 inlets where shall the flow go too?
-the platform is @ the axis of the cylinder?
mvoss is offline   Reply With Quote

Old   March 16, 2011, 05:28
Default
  #6
New Member
 
chyn wey lee
Join Date: Apr 2009
Posts: 22
Rep Power: 7
djstoneage is on a distinguished road
in cfx i specified it as an opening. i am trying to figure out how to replicate that. does the inletOutlet type the same as opening type in CFX?
djstoneage is offline   Reply With Quote

Old   March 16, 2011, 06:04
Default
  #7
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 408
Rep Power: 10
mvoss is on a distinguished road
Since i know that from CFX, you can cut the entire domain in half, depending on the wind dir. and specify one half as inlet and the other half as a inletOutlet (no backflow) with 0Pa rel.Pressure and the top as zeroGradient for the vel. and a desired pressure level for p.

If you really have an pressure/velocity-atmospheric profile you should think about using grovvybc to set everything depending on the height of your domain.
mvoss is offline   Reply With Quote

Old   March 17, 2011, 22:46
Default
  #8
New Member
 
chyn wey lee
Join Date: Apr 2009
Posts: 22
Rep Power: 7
djstoneage is on a distinguished road
i am trying to setup this boundary condition on my domain but cant seem to figure out a way to define it.

this is a CEL script from CFX

AirDensity = 1 [atm] / (287.06 [J kg^-1 C^-1] *AirTemperature)
AirTemperature = 10[C]
ak=0.41[]
cmu=0.090000004[]
cmuhalf=cmu^0.5
dir=0[]
dira=dir*pi180
ed1=(ustarnew^3)/(ak*(zabs-zref))
eps=30.0 *z0
pi180=pi/180
speed =(ustarnew*loge((zabs-zref)/z0)/ak)*step((z-z0)/1[m])
te1=ustarnew^2)/cmuhalf
thetaa=dira+(pi/2.0)
u1=speed*cos(thetaa)
uref=2[m s^-1]
ustarnew=al*uref/loge((zuref-zref)/z0)
v1=-speed*sin(theetaa)
w1=0.0[ms^-1]
z0=0.001[m]
zabs=abs(z+1E-007[m])
zref=0[m]
zuref=10[m]

anyone knows how to do this??
djstoneage is offline   Reply With Quote

Old   March 18, 2011, 04:12
Default
  #9
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 408
Rep Power: 10
mvoss is on a distinguished road
Did you took a look at atmBoundaryLayerInletVelocity?
mvoss is offline   Reply With Quote

Old   March 18, 2011, 04:49
Default
  #10
New Member
 
chyn wey lee
Join Date: Apr 2009
Posts: 22
Rep Power: 7
djstoneage is on a distinguished road
i just found out about its existance it openFoam1.7.1 i am installing it right now. will try it out
djstoneage is offline   Reply With Quote

Old   March 21, 2011, 01:16
Default
  #11
New Member
 
chyn wey lee
Join Date: Apr 2009
Posts: 22
Rep Power: 7
djstoneage is on a distinguished road
i am trying to use theatmBoundaryLayerInletEpsilon boundary condition but when i run potentialFoam it says its an invalid patch type.

DOMAIN
{
type atmBoundaryLayerInletEpsilon;
Ustar $Ustar;
z $zDirection;
z0 $z0;
value $internalField;
zGround $zGround;
}

this is how i've set my boundary condition.
djstoneage is offline   Reply With Quote

Old   March 21, 2011, 02:13
Default
  #12
New Member
 
chyn wey lee
Join Date: Apr 2009
Posts: 22
Rep Power: 7
djstoneage is on a distinguished road
when i run simpleFoam this is what i am getting

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 1.7.1-03e7e056c215
Exec   : simpleFoam
Date   : Mar 21 2011
Time   : 14:10:17
Host   : localhost.localdomain
PID    : 21308
Case   : /home/clee/Desktop/DPQU
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
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 kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    sigmaEps        1.3;
}


Starting time loop

Time = 1

^TsmoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 0.09952992287, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 0.09000813227, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 1, Final residual = 0.03000555398, No Iterations 2


--> FOAM FATAL ERROR: 
Continuity error cannot be removed by adjusting the outflow.
Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
Total flux              : 5.42432e+06
Specified mass inflow   : 1.37928e+06
Specified mass outflow  : 1.37925e+06
Adjustable mass outflow : 0


    From function adjustPhi(surfaceScalarField& phi, const volVectorField& U,const volScalarField& p
    in file cfdTools/general/adjustPhi/adjustPhi.C at line 115.

FOAM exiting
djstoneage is offline   Reply With Quote

Old   March 21, 2011, 07:25
Default
  #13
Member
 
inginer's Avatar
 
Ovidiu Michiu
Join Date: Apr 2010
Location: Ingolstadt, Germany
Posts: 52
Rep Power: 6
inginer is on a distinguished road
hello,

try to take a look in the tutorial of simpleWindFoam. you can find it in tutorials/incompresible/simpleWindFoam. there you have a case, which maybe close to your problem.

Best,
Ovidiu
inginer is offline   Reply With Quote

Old   March 23, 2011, 00:48
Default
  #14
New Member
 
chyn wey lee
Join Date: Apr 2009
Posts: 22
Rep Power: 7
djstoneage is on a distinguished road
I followed the tutorial but importing in myown mesh from icem. it runs perfectly without turbulence, but when i turn on turbulence it crashed out after 2 iterations as below : - please advice on the following issues

apreciate any help

thank yo

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 1.7.1-03e7e056c215
Exec   : simpleFoam -parallel
Date   : Mar 23 2011
Time   : 12:14:23
Host   : localhost.localdomain
PID    : 22423
Case   : /home/clee/Desktop/DPQU4
nProcs : 6
Slaves : 
5
(
localhost.localdomain.22424
localhost.localdomain.22425
localhost.localdomain.22426
localhost.localdomain.22427
localhost.localdomain.22428
)

Pstream initialized with:
    floatTransfer     : 0
    nProcsSimpleSum   : 0
    commsType         : nonBlocking
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
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 kEpsilon
--> FOAM Warning : 
    From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
    in file /home/quy/OpenFOAM/OpenFOAM-1.7.1/src/OpenFOAM/lnInclude/Field.C at line 262
    Reading "/home/clee/Desktop/DPQU4/processor0/0/nut::boundaryField::SEA" from line 31 to line 34
    expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.
--> FOAM Warning : 
    From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
    in file /home/quy/OpenFOAM/OpenFOAM-1.7.1/src/OpenFOAM/lnInclude/Field.C at line 262
    Reading "/home/clee/Desktop/DPQU4/processor0/0/nut::boundaryField::SEA" from line 31 to line 34
    expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              -0.33;
    sigmak          1;
    sigmaEps        1.11;
    Prt             1;
}


Starting time loop

Time = 1

smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 0.0555723564877, No Iterations 3
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 0.0550617478002, No Iterations 3
smoothSolver:  Solving for Uz, Initial residual = 1, Final residual = 0.0505116027098, No Iterations 2
smoothSolver:  Solving for p, Initial residual = 1, Final residual = 0.00998051548345, No Iterations 276
smoothSolver:  Solving for p, Initial residual = 0.110253383451, Final residual = 0.002106445285, No Iterations 300
time step continuity errors : sum local = 3.83276734343, global = -2.75858375028, cumulative = -2.75858375028
smoothSolver:  Solving for epsilon, Initial residual = 0.998076065936, Final residual = 0.0531743869439, No Iterations 4
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 0.0312753766608, No Iterations 2
bounding k, min: 0 max: 2.7152548344e-05 average: 1.38834995478e-07
ExecutionTime = 217.58 s  ClockTime = 221 s

Time = 2

smoothSolver:  Solving for Ux, Initial residual = 0.497202681096, Final residual = 0.0275293576353, No Iterations 3
smoothSolver:  Solving for Uy, Initial residual = 0.596221211389, Final residual = 0.0324851173556, No Iterations 3
smoothSolver:  Solving for Uz, Initial residual = 0.605757042665, Final residual = 0.0292697272504, No Iterations 3
smoothSolver:  Solving for p, Initial residual = 0.999999994462, Final residual = 0.0269541218382, No Iterations 300
smoothSolver:  Solving for p, Initial residual = 0.0128499408047, Final residual = 0.000832027351103, No Iterations 300
time step continuity errors : sum local = 16.0815980332, global = -3.02734777888, cumulative = -5.78593152916
[0] #0  Foam::error::printStack(Foam::Ostream&)[5] #0  Foam::error::printStack(Foam::Ostream&)[3] #0  Foam::error::printStack(Foam::Ostream&)[2] #0  Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[0] #1  Foam::sigFpe::sigFpeHandler(int)[4] #0  Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[3] #1  Foam::sigFpe::sigFpeHandler(int) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[5] #1  Foam::sigFpe::sigFpeHandler(int) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[2] #1  Foam::sigFpe::sigFpeHandler(int) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[4] #1  Foam::sigFpe::sigFpeHandler(int) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[0] #2   in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[5] #2   in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[3] #2  __restore_rt in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[4] #2   in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[2] #2   at sigaction.c:0
[0] #3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&)__restore_rt__restore_rt in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[0] #4  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&)__restore_rt__restore_rt at sigaction.c:0
[5] #3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[0] #5  Foam::incompressible::RASModels::kEpsilon::correct() at sigaction.c:0
[4] #3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[5] #4  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at sigaction.c:0
[3] #3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at sigaction.c:0
[2] #3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[4] #4  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[0] #6   in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[4] #5  Foam::incompressible::RASModels::kEpsilon::correct() in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[5] #5  Foam::incompressible::RASModels::kEpsilon::correct() in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[3] #4  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[2] #4  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[4] #6   in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[5] #6  ?? in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[2] #5  Foam::incompressible::RASModels::kEpsilon::correct() in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[3] #5  Foam::incompressible::RASModels::kEpsilon::correct() in "/opt/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/simpleFoam"
[0] #7  __libc_start_main in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[2] #6   in "/opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[3] #6   in "/lib64/libc.so.6"
[0] #8  ????Foam::regIOobject::writeObject(Foam::IOstream::streamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const?? in "/opt/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/simpleFoam"
[4] #7  __libc_start_main in "/lib64/libc.so.6"
[4] #8   in "/opt/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/simpleFoam"
[localhost:22423] *** Process received signal ***
[localhost:22423] Signal: Floating point exception (8)
[localhost:22423] Signal code:  (-6)
[localhost:22423] Failing at address: 0x1f400005797
[localhost:22423] [ 0] /lib64/libc.so.6 [0x3ae10302d0]
[localhost:22423] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x3ae1030265]
[localhost:22423] [ 2] /lib64/libc.so.6 [0x3ae10302d0]
[localhost:22423] [ 3] /opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam6divideERNS_5FieldIdEERKNS_5UListIdEES6_+0xc9) [0x2ae2ec5f60e9]
[localhost:22423] [ 4] /opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so(_ZN4FoamdvINS_12fvPatchFieldENS_7volMeshEEENS_3tmpINS_14GeometricFieldIdT_T0_EEEERKS8_RKS7_+0x2c8) [0x2ae2eacd1f28]
[localhost:22423] [ 5] /opt/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleRASModels.so(_ZN4Foam14incompressible9RASModels8kEpsilon7correctEv+0x345) [0x2ae2eacbe795]
[localhost:22423] [ 6] simpleFoam [0x4179e3]
[localhost:22423] [ 7] /lib64/libc.so.6(__libc_start_main+0xf4) [0x3ae101d994]
[localhost:22423] [ 8] simpleFoam(_ZNK4Foam11regIOobject11writeObjectENS_8IOstream12streamFormatENS1_13versionNumberENS1_15compressionTypeE+0xc1) [0x4148e9]
[localhost:22423] *** End of error message ***
 in "/opt/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/simpleFoam"
[5] #7  __libc_start_main in "/opt/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/simpleFoam"
[2] #7  __libc_start_main in "/lib64/libc.so.6"
[5] #8  --------------------------------------------------------------------------
mpirun noticed that process rank 0 with PID 22423 on node localhost.localdomain exited on signal 8 (Floating point exception).
djstoneage is offline   Reply With Quote

Old   May 3, 2011, 03:39
Default
  #15
New Member
 
Marta Camps Santasmasas
Join Date: Feb 2010
Posts: 2
Rep Power: 0
mcamps is on a distinguished road
Hello,

Maybe the problem is in your mesh. Have you tried to run checkMesh and see if it find any problem in your mesh?
mcamps is offline   Reply With Quote

Old   May 6, 2011, 08:45
Default
  #16
New Member
 
Balakrshnan Ramakrishnan
Join Date: May 2009
Posts: 22
Rep Power: 7
Balakrshnan Ramakrishnan is on a distinguished road
I am certainly not sure this is work. But I had similar problems and I tried to give low values for relaxation factors for p,U,k,epsilon in the
system/fvSchemes like :

relaxationFactors
{
p 0.01;
U 0.02;
k 0.02;
epsilon 0.02;
}

This is because the values of k and epsilon blows up very high that they exceed machine precision like 1.5e200 etc.. This very low relaxation factor will avoid such blow up.

You may need to run more than twice the number of iterations as the convergence will be very slow, but it worked for me.

Also you can give higher number for nOrthogonal Correctors like
SIMPLE
{
nNonOrthogonalCorrectors 5;
}

This will also increase computational time but hopefully will try to get better convergence.

Let me know if this helps..

Bala
Balakrshnan Ramakrishnan 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
Are there anybody study in compute wind engineering ivanyao OpenFOAM Running, Solving & CFD 2 November 25, 2008 21:48
Rough baundary in atmospheric wind majidhojjat OpenFOAM Running, Solving & CFD 3 August 18, 2008 11:15
Virtual Wind Tunnel in FLUENT ND FLUENT 0 April 7, 2006 07:43
wind engineering problem justin Main CFD Forum 0 February 20, 2006 19:23
Atmospheric Wind Profile - Inlet Subroutine Roger CD-adapco 3 December 12, 2002 10:00


All times are GMT -4. The time now is 11:51.