simpleFoam Validation in Urban Environment using AIJ guidelines (openCAE)

JR22 · March 20, 2013, 20:53

Hi,

I've been trying to run Case-C of the AIJ-PWEAB test cases. It consists of a model of flow of air around a simple building. The model utilizes simpleFoam to solve it. I am using openFoam-2.1.1. I got over a few hurdles to get it to work, but now that it runs, the sequence breaks at iteration #2.

The model can be found at: Case C = Simple Building Block.

This is what the terminal shows when running the Allrun script :

Code:

Running ./makeMesh on /home/admin1/AIJ-PWEAB/CaseC
Running setDiscreteFields on /home/admin1/AIJ-PWEAB/CaseC
Running simpleFoam on /home/admin1/AIJ-PWEAB/CaseC
/opt/openfoam211/bin/tools/RunFunctions: line 37:  4194 Floating point exception(core dumped) $APP_RUN $* > log.$APP_NAME 2>&1
Running foamCalc on /home/admin1/AIJ-PWEAB/CaseC
Running foamLog on /home/admin1/AIJ-PWEAB/CaseC
Running sample on /home/admin1/AIJ-PWEAB/CaseC

Here are the contents of the simpleFoam.log file:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.1-221db2718bbb
Exec   : simpleFoam
Date   : Mar 20 2013
Time   : 21:20:32
Host   : "admin1-VirtualBox"
PID    : 4194
Case   : /home/admin1/AIJ-PWEAB/CaseC
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 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;
}

No field sources present


SIMPLE: convergence criteria
    field p	 tolerance 0.001
    field "(U|k|epsilon|omega)"	 tolerance 0.0001


Starting time loop

Time = 1

DILUPBiCG:  Solving for Ux, Initial residual = 0.375188, Final residual = 0.0147972, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.0487866, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 0.0542991, No Iterations 1
GAMG:  Solving for p, Initial residual = 1, Final residual = 0.00946159, No Iterations 2
time step continuity errors : sum local = 0.429902, global = -5.28454e-17, cumulative = -5.28454e-17
DILUPBiCG:  Solving for epsilon, Initial residual = 0.0471403, Final residual = 0.000449379, No Iterations 1
DILUPBiCG:  Solving for k, Initial residual = 0.2091, Final residual = 0.00420194, No Iterations 1
ExecutionTime = 0.22 s  ClockTime = 1 s

Time = 2

DILUPBiCG:  Solving for Ux, Initial residual = 0.837893, Final residual = 0.035823, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.732454, Final residual = 0.0340259, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.726034, Final residual = 0.034602, No Iterations 1
#0  Foam::error::printStack(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::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::DICSmoother::DICSmoother(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  Foam::lduMatrix::smoother::addsymMatrixConstructorToTable<Foam::DICSmoother>::New(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::lduMatrix::smoother::New(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7  Foam::GAMGSolver::initVcycle(Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::lduMatrix::smoother>&) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#9  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#10  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#11  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#12  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"

Thank you very much in advance.

lixx · March 21, 2013, 02:18

You should check carefully the log files produced, especially the mesh part. There is a file setSet.batch missing in this directory. I copied the file from Case-A directory then everything is fine. I think the maintainer should fix this problem since I was puzzled by this problem for a long time.

Quote:

Originally Posted by JR22

Hi,

I've been trying to run Case-C of the AIJ-PWEAB test cases. It consists of a model of flow of air around a simple building. The model utilizes simpleFoam to solve it. I am using openFoam-2.1.1. I got over a few hurdles to get it to work, but now that it runs, the sequence breaks at iteration #2.

The model can be found at: Case C = Simple Building Block.

This is what the terminal shows when running the Allrun script :

Code:

Running ./makeMesh on /home/admin1/AIJ-PWEAB/CaseC
Running setDiscreteFields on /home/admin1/AIJ-PWEAB/CaseC
Running simpleFoam on /home/admin1/AIJ-PWEAB/CaseC
/opt/openfoam211/bin/tools/RunFunctions: line 37:  4194 Floating point exception(core dumped) $APP_RUN $* > log.$APP_NAME 2>&1
Running foamCalc on /home/admin1/AIJ-PWEAB/CaseC
Running foamLog on /home/admin1/AIJ-PWEAB/CaseC
Running sample on /home/admin1/AIJ-PWEAB/CaseC

Here are the contents of the simpleFoam.log file:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.1-221db2718bbb
Exec   : simpleFoam
Date   : Mar 20 2013
Time   : 21:20:32
Host   : "admin1-VirtualBox"
PID    : 4194
Case   : /home/admin1/AIJ-PWEAB/CaseC
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 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;
}

No field sources present


SIMPLE: convergence criteria
    field p	 tolerance 0.001
    field "(U|k|epsilon|omega)"	 tolerance 0.0001


Starting time loop

Time = 1

DILUPBiCG:  Solving for Ux, Initial residual = 0.375188, Final residual = 0.0147972, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.0487866, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 0.0542991, No Iterations 1
GAMG:  Solving for p, Initial residual = 1, Final residual = 0.00946159, No Iterations 2
time step continuity errors : sum local = 0.429902, global = -5.28454e-17, cumulative = -5.28454e-17
DILUPBiCG:  Solving for epsilon, Initial residual = 0.0471403, Final residual = 0.000449379, No Iterations 1
DILUPBiCG:  Solving for k, Initial residual = 0.2091, Final residual = 0.00420194, No Iterations 1
ExecutionTime = 0.22 s  ClockTime = 1 s

Time = 2

DILUPBiCG:  Solving for Ux, Initial residual = 0.837893, Final residual = 0.035823, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.732454, Final residual = 0.0340259, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.726034, Final residual = 0.034602, No Iterations 1
#0  Foam::error::printStack(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::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::DICSmoother::DICSmoother(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  Foam::lduMatrix::smoother::addsymMatrixConstructorToTable<Foam::DICSmoother>::New(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::lduMatrix::smoother::New(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7  Foam::GAMGSolver::initVcycle(Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::lduMatrix::smoother>&) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#9  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#10  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#11  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#12  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"

Thank you very much in advance.

JR22 · March 21, 2013, 06:11

It Worked !! Thanks !!

You were exactly right. The file that is missing in the "setSet.batch". The log.MakeMesh complaints about this 1/3 of the way down:

Code:

set points
end points
set face - owner - neigubour
end face - owner - neigubour
set boundary
make Mesh end
end
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.1-221db2718bbb
Exec   : insideCells constant/triSurface/building.stl building
Date   : Mar 20 2013
Time   : 21:20:24
Host   : "admin1-VirtualBox"
PID    : 4187
Case   : /home/admin1/AIJ-PWEAB/CaseC
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

Reading surface from "constant/triSurface/building.stl"
Selected 7056 of 168912 cells

Writing selected cells to cellSet building

Use this cellSet e.g. with subsetMesh : 

    subsetMesh building

End

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.1-221db2718bbb
Exec   : setSet -constant -batch setSet.batch
Date   : Mar 20 2013
Time   : 21:20:27
Host   : "admin1-VirtualBox"
PID    : 4188
Case   : /home/admin1/AIJ-PWEAB/CaseC
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 = constant

Time:constant  cells:168912  faces:516498  points:178850  patches:6  bb:(-1 -1.5 0) (1.5 1.5 1.8)
cellSets:
	building	size:7056

Time = constant
    mesh not changed.
Reading commands from file "setSet.batch"


--> FOAM FATAL ERROR: 
Cannot open file "setSet.batch"

    From function setSet
    in file setSet.C at line 890.

FOAM exiting

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.1-221db2718bbb
Exec   : subsetMesh building -overwrite
Date   : Mar 20 2013
Time   : 21:20:29
Host   : "admin1-VirtualBox"
PID    : 4189
Case   : /home/admin1/AIJ-PWEAB/CaseC
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 mesh for time = 0

Reading cell set from building

Adding exposed internal faces to a patch called "oldInternalFaces" (created if necessary)

--> FOAM Serious Error : 
    From function IOobject::readHeader(Istream&)
    in file db/IOobject/IOobjectReadHeader.C at line 89
    Reading "/home/admin1/AIJ-PWEAB/CaseC/constant/index.html" at line 1
    First token could not be read or is not the keyword 'FoamFile'

Check header is of the form:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       IOobject;
    location    "constant";
    object      index.html;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Writing subsetted mesh and fields to time 0

End

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.1-221db2718bbb
Exec   : changeDictionary
Date   : Mar 20 2013
Time   : 21:20:32
Host   : "admin1-VirtualBox"
PID    : 4190
Case   : /home/admin1/AIJ-PWEAB/CaseC
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 mesh for time = 0

Read dictionary changeDictionaryDict with replacements for dictionaries 
1
(
boundary
)

Replacing entries in dictionary boundary
Special handling of boundary as polyMesh/boundary file.
Loaded dictionary boundary with entries 
7
(
x_
_x
y_
_y
z_
_z
oldInternalFaces
)

Merging entries from 
2
(
z_
oldInternalFaces
)

fieldDict:
{
    x_
    {
        type            patch;
        nFaces          0;
        startFace       18872;
    }
    _x
    {
        type            patch;
        nFaces          0;
        startFace       18872;
    }
    y_
    {
        type            patch;
        nFaces          0;
        startFace       18872;
    }
    _y
    {
        type            patch;
        nFaces          0;
        startFace       18872;
    }
    z_
    {
        type            wall;
        nFaces          784;
        startFace       18872;
    }
    _z
    {
        type            patch;
        nFaces          0;
        startFace       19656;
    }
    oldInternalFaces
    {
        type            wall;
        nFaces          3808;
        startFace       19656;
    }
}

Writing modified fieldDict boundary

End

Here is one of the comparison graphs from the output:

JR22 · March 21, 2013, 15:49

I am now trying to run the Case B which consists of a validation of several turbulent models for wind around a single building. When you call the Allrun script, it goes through an array of values that direct it to each directory. Each Allrun script for each model contains the following code:

Code:

link ../share/Allrun

This command "link" is apparently there to save the author from repeating all the commands for each model in each script. However, it breaks and it gives me the following error message:

Code:

link: missing operand after `../share/Allrun'
Try `link --help' for more information.

The link command is expecting two operands and gets only one. I tried a couple of things, but cannot really get it to work. What do I have to change to get this "link" command to do what it is supposed to do?

The complete Case B is at the SVN repository here:
http://www.opencae.jp/svn/OpenFOAM-V...J-PWEAB/trunk/

This is the directory structure of Case B with the files highlighted:

.
├── Allclean
├── Allrun
├── index.html
├── kEpsilon
│** ├── 0
│** ├── Allclean
│** ├── Allrun
│** ├── constant
│** ├── index.html
│** └── system
├── LICENSE.GPL2
├── NonlinearKEShih
│** ├── 0
│** ├── Allclean
│** ├── Allrun
│** ├── constant
│** ├── index.html
│** └── system
├── README
├── realizableKE
│** ├── 0
│** ├── Allclean
│** ├── Allrun
│** ├── constant
│** ├── index.html
│** └── system
├── RNGkEpsilon
│** ├── 0
│** ├── Allclean
│** ├── Allrun
│** ├── constant
│** ├── index.html
│** └── system
└── share
├── 0
├── Allclean
├── Allrun <-- this one contains the juice
├── box.dat
├── caseBMesh.foam
├── constant
├── index.html
├── log.cellSet
├── log.makeMesh
├── log.setDiscreteFields
├── makeMesh
├── makeStructuredGridMesh.py
├── measured
├── org0
├── postprocess.py
├── removeCellBoxes.py
├── system
├── x.dat
├── y.dat
└── z.dat

kingjewel1 · October 9, 2013, 16:45

Did you ever work out what the problem was with B?

wyldckat · October 11, 2013, 18:39

Greetings to all!

Quote:

Originally Posted by kingjewel1

Did you ever work out what the problem was with B?

Looking back at the original problem:

Quote:

Originally Posted by JR22

When you call the Allrun script, it goes through an array of values that direct it to each directory. Each Allrun script for each model contains the following code:

Code:

link ../share/Allrun

This command "link" is apparently there to save the author from repeating all the commands for each model in each script. However, it breaks and it gives me the following error message:

Code:

link: missing operand after `../share/Allrun'
Try `link --help' for more information.

The problem is that this "link" is actually an artificial link created by the SVN mechanism. It actually means that when checking out the source code through SVN, it would automatically interpret the "Allrun" file as a symbolic link pointing to "../share/Allrun", namely this file: http://www.opencae.jp/svn/OpenFOAM-V...B/share/Allrun

To manually fix this, run from the "CaseB" folder the following block of code on the command line:

Code:

for model in kEpsilon NonlinearKEShih RNGkEpsilon realizableKE
do
    cd $model
    rm Allrun
    ln -s ../share/Allrun Allrun
done

And that's that! It's ready to be used.

Best regards,
Bruno

Alex Lee · October 18, 2013, 08:13

Dear Imano San,

I try to run the Case A from the files I download from your depository: \OpenFOAM-VandV-SIG_AIJ-PWEAB – オープンCAE学会_files

Using the ./runAll script. However, seems like there is a problem related to ¥constant/boundaryData/x_. ( File missing….. )

Could you please kindly advise what is the problem I encountered and how to resolve it ?

Thank you.

Sincerely Yours,

imano · October 18, 2013, 08:32

Dear Alex san,

Quote:

Originally Posted by Alex Lee

I try to run the Case A from the files I download from your depository: \OpenFOAM-VandV-SIG_AIJ-PWEAB – オープンCAE学会_files

Using the ./runAll script. However, seems like there is a problem related to ¥constant/boundaryData/x_. ( File missing….. )

Could you please kindly advise what is the problem I encountered and how to resolve it ?

Sorry, it appears that I have failed to add boundaryData directory...

Now I have added the missing boundaryData directory, so could you
execute "svn update" on the CaseA directory and run that again?

Code:

svn update
./Allclean
./Allrun

Ref.
http://www.opencae.jp/changeset/125/OpenFOAM-VandV-SIG

alvinsim2013 · October 21, 2013, 03:51

Hi Imano San,

I had the same problem with case A, described by Alex.

I had already added in the files you gave for the boundaryData to my constant folder. However, my 'log.sample' and 'log' files showed up error messages, as follow. May you advise me how can I best solve it?

'log' file error:
//====================================
　
--> FOAM FATAL IO ERROR:
cannot find file
file: /gpfs/home/tssim1/tssim1-2.0.1/AIJ/CaseA/constant/boundaryData/x_/points at line 0.
From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.
FOAM exiting
------------------------------------------------------------------------------

'log.sample' file error:
//======================================
Create time
Create mesh for time = 0
Reading set description:
verx_-075
verx_-050
verx_-025
verx_000
verx_050
verx_075
verx_125
verx_200
verx_325
Time = 0
　
--> FOAM FATAL IO ERROR:
cannot find file
file: /gpfs/home/tssim1/tssim1-2.0.1/AIJ/CaseA/constant/boundaryData/x_/points at line 0.
From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.
FOAM exiting

Thanks a lot.

Best Regards,
Alvin

imano · October 21, 2013, 05:50

Dear Alvin san,

Probably this is because "constant/boundaryData/x_/points" is still missing.

Please attach the result of following commands on the CaseA directory.

Code:

ls -R

If the "points" file does not exist, please confirm that "svn update" has finished correctly.

Best regards,
Masashi

alvinsim2013 · October 21, 2013, 05:58

Attached is the result of the command "ls -R"

CaseA]$ ls -R
.:
Allclean Makefile profilek.gp setSet.batch z.dat
Allrun makeStructuredGridMesh.py profileU.gp system
constant orig0 README x.dat
exp paraview.foam res.gp y.dat
./constant:
boundaryData polyMesh RASProperties transportProperties triSurface
./constant/boundaryData:
x_
./constant/boundaryData/x_:
0 points
./constant/boundaryData/x_/0:
epsilon k U
./constant/polyMesh:
boundary
./constant/triSurface:
building.stl
./exp:
resutlsHolSec0125.txt resutlsHolSec1250.txt resutlsVerSec.txt
./orig0:
epsilon include k nut p U
./orig0/include:
slipPatches
./system:
changeDictionaryDict decomposeParDict fvSolution
controlDict fvSchemes sampleDict

imano · October 21, 2013, 06:05

Dear Alvin san,

Hmm, "points" files exists...

Then how about an output of "ls -lR constant" ?

Best regards,
Masashi

alvinsim2013 · October 21, 2013, 06:29

I have a question about the case A file in trunk folder versus that in branches folder.

What are the differences between these 2 case A files?

imano · October 21, 2013, 07:08

Hi,

Quote:

Originally Posted by alvinsim2013

I have a question about the case A file in trunk folder versus that in branches folder.

What are the differences between these 2 case A files?

Branches directory is for old versions of OpenFOAM like 1.7 or 2.0,
as you see in that directory.
On the other hand trunk is a directory for relative new version of OF.

As for a structure of these kind of subversion repository,
please search "subversion" on the web.

Which version of OF do you use?

All the best,
Masashi

alvinsim2013 · October 21, 2013, 10:07

My OF is 2.0.

alvinsim2013 · October 22, 2013, 00:33

Dear Masashi-san,

I have changed to OF2.1 and included the boundaryData's points, k, U and epsilon in the constant folder.
All the log files did not show up any error messages, except 'log' file.

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.0-bd7367f93311
Exec : simpleFoam
Date : Oct 22 2013
Time : 12:22:58
Host : "hpclogin2"
PID : 16674
Case : /OpenFOAM-VandV-SIG/AIJ-PWEAB/branches/2.1/CaseA
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 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 FATAL IO ERROR:
Unknown patchField type nutkAtmRoughWallFunction for patch type wall
Valid patchField types are :
65
(
advective
atmBoundaryLayerInletEpsilon
buoyantPressure
calculated
codedFixedValue
codedMixed
cyclic
cyclicAMI
cyclicSlip
directionMixed
empty
epsilonWallFunction
fan
fanPressure
fixedFluxPressure
fixedGradient
fixedInternalValue
fixedPressureCompressibleDensity
fixedValue
freestream
freestreamPressure
inletOutlet
inletOutletTotalTemperature
kappatJayatillekeWallFunction
kqRWallFunction
mapped
mappedField
mappedFixedInternalValue
mappedFixedPushedInternalValue
mixed
nonuniformTransformCyclic
nutLowReWallFunction
nutTabulatedWallFunction
nutURoughWallFunction
nutUSpaldingWallFunction
nutUWallFunction
nutkRoughWallFunction
nutkWallFunction
omegaWallFunction
oscillatingFixedValue
outletInlet
outletMappedUniformInlet
partialSlip
processor
processorCyclic
rotatingTotalPressure
sliced
slip
symmetryPlane
syringePressure
timeVaryingMappedFixedValue
totalPressure
totalTemperature
turbulentHeatFluxTemperature
turbulentInlet
turbulentIntensityKineticEnergyInlet
turbulentMixingLengthDissipationRateInlet
turbulentMixingLengthFrequencyInlet
uniformDensityHydrostaticPressure
uniformFixedValue
uniformTotalPressure
waveSurfacePressure
waveTransmissive
wedge
zeroGradient
)
　
file: /OpenFOAM-VandV-SIG/AIJ-PWEAB/branches/2.1/CaseA/0/nut::boundaryField::z_ from line 27 to line 30.
From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&)
in file /usr/local/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 135.
FOAM exiting

Thanks a lot.

Alex Lee · October 22, 2013, 02:29

Dear all,

While running the ./Allrun script in /CaseB/ folder, there is an error associated with simpleFoam.

The error message is captured below for your reference:

*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.1-221db2718bbb
Exec : simpleFoam
Date : Oct 22 2013
Time : 14:20:44
Host : "judah-Ubuntu"
PID : 18853
Case : /home/alex/V_V_Cases/AIJ-PWEAB/branches/2.1/CaseB/kEpsilon
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 mesh for time = 0

--> FOAM FATAL ERROR:
Cannot find file "points" in directory "polyMesh" in times 0 down to constant

From function Time::findInstance(const fileName&, const word&, const IOobject::readOption, const word&)
in file db/Time/findInstance.C at line 188.

FOAM exiting

------------------------------------

Any clue ?

alvinsim2013 · October 22, 2013, 03:21

Hi Masashi-san,

Is there supposed to be an include/slipPatches file in the orig0 folder, meant for U, epsilon and k for Case C?

Unable to find the include/slipPatches file in the URI of the repository.

Best regards

alvinsim2013 · October 22, 2013, 03:59

Hi,

I encountered the following error messages for Case D when ./Allrun was issued. Hope to seek advice to resolve them.
-----------------------------------------------------------------------------------------------------
The 'log.potentialFoam' file (within the 'xdeg' folder):

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.0-bd7367f93311
Exec : potentialFoam -writep
Date : Oct 22 2013
Time : 15:32:31
Host : "hpclogin2"
PID : 15351
Case : /gpfs/home/tssim1/OpenCAE/AIJ-new/OpenFOAM-VandV-SIG/AIJ-PWEAB/branches/2.1/CaseD/45deg
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 mesh for time = 0
Reading field p
Reading field U
　
Calculating potential flow
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
continuity error = 0
Interpolated U error = 0
ExecutionTime = 3.54 s ClockTime = 4 s
End

---------------------------------------------------------------------------------

In log.simpleFoam file:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.0-bd7367f93311
Exec : simpleFoam
Date : Oct 22 2013
Time : 15:32:35
Host : "hpclogin2"
PID : 15353
Case : /gpfs/home/tssim1/OpenCAE/AIJ-new/OpenFOAM-VandV-SIG/AIJ-PWEAB/branches/2.1/CaseD/45deg
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 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
bounding k, min: 0 max: 1 average: 1
bounding epsilon, min: 0 max: 1 average: 1
#0 Foam::error:

rintStack(Foam::Ostream&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#5 ?? at kEpsilon.C:0
#6 Foam::incompressible::RASModels::kEpsilon::kEpsilo n(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#7 Foam::incompressible::RASModel::adddictionaryConst ructorToTable<Foam::incompressible::RASModels::kEp silon>::New(Foam::GeometricField<Foam::Vector<doub le>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#8 Foam::incompressible::RASModel::New(Foam::Geometri cField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#9 main in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam"
#10 __libc_start_main in "/lib64/libc.so.6"
#11 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam"

-------------------------------------------------------------------------------------------------------------------------------
In the 'log.setDiscreteFields' file:

/usr/local/OpenFOAM/OpenFOAM-2.1.0/bin/tools/RunFunctions: line 47: setDiscreteFields: command not found

------------------------------------------------
Thanks a lot!

alvinsim2013 · October 22, 2013, 04:52

Hi,

For case E and case F, the following problems were found when ./Allrun script is issued.

1)
./makeInit: line 9: setDiscreteFields: command not found

2)
simpleFoam | tee log
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.0-bd7367f93311
Exec : simpleFoam
Date : Oct 22 2013
Time : 16:39:18
Host : "smpsvr"
PID : 1624
Case : /gpfs/home/tssim1/OpenCAE/AIJ-new2/OpenFOAM-VandV-SIG/AIJ-PWEAB/branches/2.1/CaseE/NNE
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 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
bounding k, min: 0 max: 0.5 average: 0.5
bounding epsilon, min: 0 max: 1 average: 1
#0 Foam::error:

rintStack(Foam::Ostream&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#5 ?? at kEpsilon.C:0
#6 Foam::incompressible::RASModels::kEpsilon::kEpsilo n(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#7 Foam::incompressible::RASModel::adddictionaryConst ructorToTable<Foam::incompressible::RASModels::kEp silon>::New(Foam::GeometricField<Foam::Vector<doub le>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#8 Foam::incompressible::RASModel::New(Foam::Geometri cField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#9 main in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam"
#10 __libc_start_main in "/lib64/libc.so.6"
#11 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam"
/usr/bin/R --vanilla < makextics.R
/bin/sh: /usr/bin/R: No such file or directory
make: *** [xtics.gp] Error 127
./makeInit 2>&1 | tee tmp.init

-------------------------------------------------------
Hope there is a solution to it.

Best regards

March 21, 2013, 15:49	Linux Question: Link Command	#4
JR22 Senior Member Jose Rey Join Date: Oct 2012 Posts: 134 Rep Power: 17	I am now trying to run the Case B which consists of a validation of several turbulent models for wind around a single building. When you call the Allrun script, it goes through an array of values that direct it to each directory. Each Allrun script for each model contains the following code: Code: link ../share/Allrun This command "link" is apparently there to save the author from repeating all the commands for each model in each script. However, it breaks and it gives me the following error message: Code: link: missing operand after `../share/Allrun' Try `link --help' for more information. The link command is expecting two operands and gets only one. I tried a couple of things, but cannot really get it to work. What do I have to change to get this "link" command to do what it is supposed to do? The complete Case B is at the SVN repository here: http://www.opencae.jp/svn/OpenFOAM-V...J-PWEAB/trunk/ This is the directory structure of Case B with the files highlighted: . ├── Allclean ├── Allrun ├── index.html ├── kEpsilon │ ├── 0 │ ├── Allclean │ ├── Allrun │ ├── constant │ ├── index.html │ └── system ├── LICENSE.GPL2 ├── NonlinearKEShih │ ├── 0 │ ├── Allclean │ ├── Allrun │ ├── constant │ ├── index.html │ └── system ├── README ├── realizableKE │ ├── 0 │ ├── Allclean │ ├── Allrun │ ├── constant │ ├── index.html │ └── system ├── RNGkEpsilon │ ├── 0 │ ├── Allclean │ ├── Allrun │ ├── constant │ ├── index.html │ └── system └── share ├── 0 ├── Allclean ├── Allrun <-- this one contains the juice ├── box.dat ├── caseBMesh.foam ├── constant ├── index.html ├── log.cellSet ├── log.makeMesh ├── log.setDiscreteFields ├── makeMesh ├── makeStructuredGridMesh.py ├── measured ├── org0 ├── postprocess.py ├── removeCellBoxes.py ├── system ├── x.dat ├── y.dat └── z.dat

October 22, 2013, 02:29	Case B -- Cannot find file "points" in directory "polyMesh" in times 0 down to consta	#17
Alex Lee New Member Alex Lee Join Date: Sep 2012 Posts: 15 Rep Power: 13	Dear all, While running the ./Allrun script in /CaseB/ folder, there is an error associated with simpleFoam. The error message is captured below for your reference: ---------------------------------------------------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: 2.1.1 \| \| \\ / A nd \| Web: www.OpenFOAM.org \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ Build : 2.1.1-221db2718bbb Exec : simpleFoam Date : Oct 22 2013 Time : 14:20:44 Host : "judah-Ubuntu" PID : 18853 Case : /home/alex/V_V_Cases/AIJ-PWEAB/branches/2.1/CaseB/kEpsilon 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 mesh for time = 0 --> FOAM FATAL ERROR: Cannot find file "points" in directory "polyMesh" in times 0 down to constant From function Time::findInstance(const fileName&, const word&, const IOobject::readOption, const word&) in file db/Time/findInstance.C at line 188. FOAM exiting ------------------------------------ Any clue ?

October 22, 2013, 03:59		#19
alvinsim2013 New Member Alvin TS Join Date: Oct 2013 Posts: 17 Rep Power: 12	Hi, I encountered the following error messages for Case D when ./Allrun was issued. Hope to seek advice to resolve them. ----------------------------------------------------------------------------------------------------- The 'log.potentialFoam' file (within the 'xdeg' folder): /---------------------------------------------------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: 2.1.0 \| \| \\ / A nd \| Web: www.OpenFOAM.org \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ Build : 2.1.0-bd7367f93311 Exec : potentialFoam -writep Date : Oct 22 2013 Time : 15:32:31 Host : "hpclogin2" PID : 15351 Case : /gpfs/home/tssim1/OpenCAE/AIJ-new/OpenFOAM-VandV-SIG/AIJ-PWEAB/branches/2.1/CaseD/45deg 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 mesh for time = 0 Reading field p Reading field U 　 Calculating potential flow GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0 continuity error = 0 Interpolated U error = 0 ExecutionTime = 3.54 s ClockTime = 4 s End --------------------------------------------------------------------------------- In log.simpleFoam file: /---------------------------------------------------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: 2.1.0 \| \| \\ / A nd \| Web: www.OpenFOAM.org \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ Build : 2.1.0-bd7367f93311 Exec : simpleFoam Date : Oct 22 2013 Time : 15:32:35 Host : "hpclogin2" PID : 15353 Case : /gpfs/home/tssim1/OpenCAE/AIJ-new/OpenFOAM-VandV-SIG/AIJ-PWEAB/branches/2.1/CaseD/45deg 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 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 bounding k, min: 0 max: 1 average: 1 bounding epsilon, min: 0 max: 1 average: 1 #0 Foam::error:rintStack(Foam::Ostream&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 __restore_rt at sigaction.c:0 #3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #5 ?? at kEpsilon.C:0 #6 Foam::incompressible::RASModels::kEpsilon::kEpsilo n(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #7 Foam::incompressible::RASModel::adddictionaryConst ructorToTable<Foam::incompressible::RASModels::kEp silon>::New(Foam::GeometricField<Foam::Vector<doub le>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #8 Foam::incompressible::RASModel::New(Foam::Geometri cField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #9 main in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam" #10 __libc_start_main in "/lib64/libc.so.6" #11 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam" ------------------------------------------------------------------------------------------------------------------------------- In the 'log.setDiscreteFields' file: /usr/local/OpenFOAM/OpenFOAM-2.1.0/bin/tools/RunFunctions: line 47: setDiscreteFields: command not found ------------------------------------------------ Thanks a lot!

October 22, 2013, 04:52		#20
alvinsim2013 New Member Alvin TS Join Date: Oct 2013 Posts: 17 Rep Power: 12	Hi, For case E and case F, the following problems were found when ./Allrun script is issued. 1) ./makeInit: line 9: setDiscreteFields: command not found 2) simpleFoam \| tee log /---------------------------------------------------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: 2.1.0 \| \| \\ / A nd \| Web: www.OpenFOAM.org \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ Build : 2.1.0-bd7367f93311 Exec : simpleFoam Date : Oct 22 2013 Time : 16:39:18 Host : "smpsvr" PID : 1624 Case : /gpfs/home/tssim1/OpenCAE/AIJ-new2/OpenFOAM-VandV-SIG/AIJ-PWEAB/branches/2.1/CaseE/NNE 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 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 bounding k, min: 0 max: 0.5 average: 0.5 bounding epsilon, min: 0 max: 1 average: 1 #0 Foam::error:rintStack(Foam::Ostream&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 __restore_rt at sigaction.c:0 #3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #5 ?? at kEpsilon.C:0 #6 Foam::incompressible::RASModels::kEpsilon::kEpsilo n(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #7 Foam::incompressible::RASModel::adddictionaryConst ructorToTable<Foam::incompressible::RASModels::kEp silon>::New(Foam::GeometricField<Foam::Vector<doub le>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #8 Foam::incompressible::RASModel::New(Foam::Geometri cField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #9 main in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam" #10 __libc_start_main in "/lib64/libc.so.6" #11 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam" /usr/bin/R --vanilla < makextics.R /bin/sh: /usr/bin/R: No such file or directory make: *** [xtics.gp] Error 127 ./makeInit 2>&1 \| tee tmp.init ------------------------------------------------------- Hope there is a solution to it. Best regards

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
CFX problem in ubuntu (linux)	Vigneshramaero	CFX	0	July 13, 2012 10:22
CFX-Pre problem, pls help!!!	cth_yao	CFX	0	February 17, 2012 00:52
Porous jump in urban environment	samygero	FLUENT	0	February 14, 2011 18:26

October 9, 2013, 16:45		#5
kingjewel1 Senior Member Join Date: Jul 2009 Posts: 260 Rep Power: 17	Did you ever work out what the problem was with B?

October 18, 2013, 08:13	Case A	#7
Alex Lee New Member Alex Lee Join Date: Sep 2012 Posts: 15 Rep Power: 13	Dear Imano San, I try to run the Case A from the files I download from your depository: \OpenFOAM-VandV-SIG_AIJ-PWEAB – オープンCAE学会_files Using the ./runAll script. However, seems like there is a problem related to ¥constant/boundaryData/x_. ( File missing….. ) Could you please kindly advise what is the problem I encountered and how to resolve it ? Thank you. Sincerely Yours,

October 21, 2013, 03:51		#9
alvinsim2013 New Member Alvin TS Join Date: Oct 2013 Posts: 17 Rep Power: 12	Hi Imano San, I had the same problem with case A, described by Alex. I had already added in the files you gave for the boundaryData to my constant folder. However, my 'log.sample' and 'log' files showed up error messages, as follow. May you advise me how can I best solve it? 'log' file error: //==================================== 　 --> FOAM FATAL IO ERROR: cannot find file file: /gpfs/home/tssim1/tssim1-2.0.1/AIJ/CaseA/constant/boundaryData/x_/points at line 0. From function regIOobject::readStream() in file db/regIOobject/regIOobjectRead.C at line 73. FOAM exiting ------------------------------------------------------------------------------ 'log.sample' file error: //====================================== Create time Create mesh for time = 0 Reading set description: verx_-075 verx_-050 verx_-025 verx_000 verx_050 verx_075 verx_125 verx_200 verx_325 Time = 0 　 --> FOAM FATAL IO ERROR: cannot find file file: /gpfs/home/tssim1/tssim1-2.0.1/AIJ/CaseA/constant/boundaryData/x_/points at line 0. From function regIOobject::readStream() in file db/regIOobject/regIOobjectRead.C at line 73. FOAM exiting Thanks a lot. Best Regards, Alvin

October 21, 2013, 05:50		#10
imano Member Masashi IMANO Join Date: Mar 2009 Location: Tokyo, Japan Posts: 34 Rep Power: 17	Dear Alvin san, Probably this is because "constant/boundaryData/x_/points" is still missing. Please attach the result of following commands on the CaseA directory. Code: ls -R If the "points" file does not exist, please confirm that "svn update" has finished correctly. Best regards, Masashi

October 21, 2013, 05:58		#11
alvinsim2013 New Member Alvin TS Join Date: Oct 2013 Posts: 17 Rep Power: 12	Attached is the result of the command "ls -R" CaseA]$ ls -R .: Allclean Makefile profilek.gp setSet.batch z.dat Allrun makeStructuredGridMesh.py profileU.gp system constant orig0 README x.dat exp paraview.foam res.gp y.dat ./constant: boundaryData polyMesh RASProperties transportProperties triSurface ./constant/boundaryData: x_ ./constant/boundaryData/x_: 0 points ./constant/boundaryData/x_/0: epsilon k U ./constant/polyMesh: boundary ./constant/triSurface: building.stl ./exp: resutlsHolSec0125.txt resutlsHolSec1250.txt resutlsVerSec.txt ./orig0: epsilon include k nut p U ./orig0/include: slipPatches ./system: changeDictionaryDict decomposeParDict fvSolution controlDict fvSchemes sampleDict

October 21, 2013, 06:05		#12
imano Member Masashi IMANO Join Date: Mar 2009 Location: Tokyo, Japan Posts: 34 Rep Power: 17	Dear Alvin san, Hmm, "points" files exists... Then how about an output of "ls -lR constant" ? Best regards, Masashi

October 21, 2013, 06:29		#13
alvinsim2013 New Member Alvin TS Join Date: Oct 2013 Posts: 17 Rep Power: 12	I have a question about the case A file in trunk folder versus that in branches folder. What are the differences between these 2 case A files?

October 21, 2013, 10:07		#15
alvinsim2013 New Member Alvin TS Join Date: Oct 2013 Posts: 17 Rep Power: 12	My OF is 2.0.

October 22, 2013, 00:33		#16
alvinsim2013 New Member Alvin TS Join Date: Oct 2013 Posts: 17 Rep Power: 12	Dear Masashi-san, I have changed to OF2.1 and included the boundaryData's points, k, U and epsilon in the constant folder. All the log files did not show up any error messages, except 'log' file. /---------------------------------------------------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: 2.1.0 \| \| \\ / A nd \| Web: www.OpenFOAM.org \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ Build : 2.1.0-bd7367f93311 Exec : simpleFoam Date : Oct 22 2013 Time : 12:22:58 Host : "hpclogin2" PID : 16674 Case : /OpenFOAM-VandV-SIG/AIJ-PWEAB/branches/2.1/CaseA 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 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 FATAL IO ERROR: Unknown patchField type nutkAtmRoughWallFunction for patch type wall Valid patchField types are : 65 ( advective atmBoundaryLayerInletEpsilon buoyantPressure calculated codedFixedValue codedMixed cyclic cyclicAMI cyclicSlip directionMixed empty epsilonWallFunction fan fanPressure fixedFluxPressure fixedGradient fixedInternalValue fixedPressureCompressibleDensity fixedValue freestream freestreamPressure inletOutlet inletOutletTotalTemperature kappatJayatillekeWallFunction kqRWallFunction mapped mappedField mappedFixedInternalValue mappedFixedPushedInternalValue mixed nonuniformTransformCyclic nutLowReWallFunction nutTabulatedWallFunction nutURoughWallFunction nutUSpaldingWallFunction nutUWallFunction nutkRoughWallFunction nutkWallFunction omegaWallFunction oscillatingFixedValue outletInlet outletMappedUniformInlet partialSlip processor processorCyclic rotatingTotalPressure sliced slip symmetryPlane syringePressure timeVaryingMappedFixedValue totalPressure totalTemperature turbulentHeatFluxTemperature turbulentInlet turbulentIntensityKineticEnergyInlet turbulentMixingLengthDissipationRateInlet turbulentMixingLengthFrequencyInlet uniformDensityHydrostaticPressure uniformFixedValue uniformTotalPressure waveSurfacePressure waveTransmissive wedge zeroGradient ) 　 file: /OpenFOAM-VandV-SIG/AIJ-PWEAB/branches/2.1/CaseA/0/nut::boundaryField::z_ from line 27 to line 30. From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&) in file /usr/local/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 135. FOAM exiting Thanks a lot.

October 22, 2013, 03:21		#18
alvinsim2013 New Member Alvin TS Join Date: Oct 2013 Posts: 17 Rep Power: 12	Hi Masashi-san, Is there supposed to be an include/slipPatches file in the orig0 folder, meant for U, epsilon and k for Case C? Unable to find the include/slipPatches file in the URI of the repository. Best regards