Give the file the proper header for being used as TimeVaryingMappedFixedValue input

syavash · October 9, 2015, 19:01

Hi Foamers,

In the file foamFileSurfaceWriter.C in "src/sampling/sampledSurface/writers/foamFile" , I can see the following line

Code:

   // values
    OFstream(valuesDir/fieldName)()  << values;

which prints the sampled field, e.g. U as the output. I should sample velocity at the inlet BC at each time step, during a very long time. In this way, I would have a huge number of time folders, yet lacking the OpenFOAM header (just vector values and coordinates).

I want to feed these time series into another simulation as boundary condition using TimeVaryingMappedFixedValue BC. But this BC demands for input files with headers.

Unfortunately, it is not possible to add header to each file manually, because the number is huge!
I have tried something like the following code to add the proper header, but without success:

Code:

vectorAverageField values
    (
    IOobject
          (
        "values",
        runTime.constant()/valuesDir/fieldName,
        mesh,
        IOobject::NO_READ,
        IOobject::NO_WRITE
          )
       ,facesSet.size()
        );
        
        values.write()

the following error appears when compiling:

Code:

SOURCE=sampledSurface/writers/foamFile/foamFileSurfaceWriter.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/meshTools/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/surfMesh/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/fileFormats/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/triSurface/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/conversion/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/lagrangian/basic/lnInclude -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/foamFileSurfaceWriter.o
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C: In member function ‘void Foam::foamFileSurfaceWriter::writeTemplate(const Foam::fileName&, const Foam::fileName&, const pointField&, const faceList&, const Foam::word&, const Foam::Field<Type>&, bool, bool) const’:
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:82:6: error: ‘vectorAverageField’ was not declared in this scope
      vectorAverageField values
      ^
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:82:25: error: expected ‘;’ before ‘values’
      vectorAverageField values
                         ^
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:96:1: error: expected ‘;’ before ‘}’ token
 }
 ^
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C: In instantiation of ‘void Foam::foamFileSurfaceWriter::writeTemplate(const Foam::fileName&, const Foam::fileName&, const pointField&, const faceList&, const Foam::word&, const Foam::Field<Type>&, bool, bool) const [with Type = double; Foam::pointField = Foam::Field<Foam::Vector<double> >; Foam::faceList = Foam::List<Foam::face>]’:
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:157:1:   required from here
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:95:9: error: ‘const class Foam::Field<double>’ has no member named ‘write’
         values.write()
         ^
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C: In instantiation of ‘void Foam::foamFileSurfaceWriter::writeTemplate(const Foam::fileName&, const Foam::fileName&, const pointField&, const faceList&, const Foam::word&, const Foam::Field<Type>&, bool, bool) const [with Type = Foam::Vector<double>; Foam::pointField = Foam::Field<Foam::Vector<double> >; Foam::faceList = Foam::List<Foam::face>]’:
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:157:1:   required from here
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:95:9: error: ‘const class Foam::Field<Foam::Vector<double> >’ has no member named ‘write’
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C: In instantiation of ‘void Foam::foamFileSurfaceWriter::writeTemplate(const Foam::fileName&, const Foam::fileName&, const pointField&, const faceList&, const Foam::word&, const Foam::Field<Type>&, bool, bool) const [with Type = Foam::SphericalTensor<double>; Foam::pointField = Foam::Field<Foam::Vector<double> >; Foam::faceList = Foam::List<Foam::face>]’:
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:157:1:   required from here
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:95:9: error: ‘const class Foam::Field<Foam::SphericalTensor<double> >’ has no member named ‘write’
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C: In instantiation of ‘void Foam::foamFileSurfaceWriter::writeTemplate(const Foam::fileName&, const Foam::fileName&, const pointField&, const faceList&, const Foam::word&, const Foam::Field<Type>&, bool, bool) const [with Type = Foam::SymmTensor<double>; Foam::pointField = Foam::Field<Foam::Vector<double> >; Foam::faceList = Foam::List<Foam::face>]’:
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:157:1:   required from here
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:95:9: error: ‘const class Foam::Field<Foam::SymmTensor<double> >’ has no member named ‘write’
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C: In instantiation of ‘void Foam::foamFileSurfaceWriter::writeTemplate(const Foam::fileName&, const Foam::fileName&, const pointField&, const faceList&, const Foam::word&, const Foam::Field<Type>&, bool, bool) const [with Type = Foam::Tensor<double>; Foam::pointField = Foam::Field<Foam::Vector<double> >; Foam::faceList = Foam::List<Foam::face>]’:
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:157:1:   required from here
sampledSurface/writers/foamFile/foamFileSurfaceWriter.C:95:9: error: ‘const class Foam::Field<Foam::Tensor<double> >’ has no member named ‘write’
make: *** [Make/linux64GccDPOpt/foamFileSurfaceWriter.o] Error 1

Is there any way to solve this problem and adding the proper header to the files generated through the sampling??

Thanks,
Syavash

syavash · October 12, 2015, 07:43

Anyone who might be interested?? This is a real problem for me since I need inlet velocity at each time step to be saved and used as boundary condition for another LES simulation!
I also checked sample utility but it similarly only saves values and generates no header!

TimeVaryingMappedFixedValue demands a header for velocity like this:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       vectorAverageField;
    object      values;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

How can I generate a header like one in above for my sampled inlet boundary??

Thanks,
Syavash

syavash · October 12, 2015, 07:46

Anyone who might be interested?? This is a real problem for me since I need inlet velocity at each time step to be saved and used as boundary condition for another LES simulation!
I also checked sample utility but it similarly only saves values and generates no header!

TimeVaryingMappedFixedValue demands a header for velocity like this:

[CODE]

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       vectorAverageField;
    object      values;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

How can I generate a header like one in above for my sampled inlet boundary??

Thanks,
Syavash

syavash · October 13, 2015, 07:28

No one can help me??!

I am really stuck in this!

Likun · October 15, 2015, 04:23

Dear Syavash,

I also met similar problem before, and I have written a matlab script to add the head to the sampled file.

Suppose your sampleDict reads like this:

Code:

/*--------------------------------*- 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       dictionary;
    location    "system";
    object      sampleDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

//Example to output facecentres, faces and points for the selected patches

interpolationScheme cellPoint;

surfaceFormat foamFile;

surfaces
(
        mySampleSurface
        {
                type           plane;
                basePoint      (0.01 0.0 0.0);
                normalVector   (1.0 0.0 0.0);
//      type      patch;
//      patches  (OUTLET);
        }
);

//Not really required when run before a simulation as the velocity will be empty.
fields          ( U );

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

After sample you will have many timestep folders under the directory: 'xx/postProcessing/surfaces/' and within each timestep folder you have the sampled surface 'mySampleSurface/'.

Here is the matlab script that I used to add the header and to move the required files directly under the timestep folder.

Code:

num_time = 9; % Total number of timestep folders

stp_time = 1e-4;         % size of timestep

case_dir = 'xx/postProcessing/surfaces/';


for i = 1:num_time

    time_dir = (i-1)*stp_time;  
                  
    old_dir = strcat(case_dir, num2str(time_dir), '/mySampleSurface/vectorField/');
    
    new_dir = strcat(case_dir, num2str(time_dir), '/');
    
    fid = fopen([new_dir 'header'],'w');
    
    fprintf(fid,'/*--------------------------------*- C++ -*----------------------------------*\\');
    fprintf(fid,'\n| =========                 |                                                 |');
    fprintf(fid,'\n| \\      /  F ield          | OpenFOAM: The Open Source CFD Toolbox           |');
    fprintf(fid,'\n|  \\    /   O peration      | Version:  2.3.x                                 |');
    fprintf(fid,'\n|   \\  /    A nd            | Web:      http://www.OpenFOAM.com               |');
    fprintf(fid,'\n|    \\/     M anipulation   |                                                 |\n');
    fprintf(fid,'\\*---------------------------------------------------------------------------*/');
    fprintf(fid,'\nFoamFile \n{\n');
    fprintf(fid,'   version     2.0;\n');
    fprintf(fid,'   format      ascii;\n');
    fprintf(fid,'   class       vectorAverageField;\n');
    fprintf(fid,'   location    "constant/boundaryData/mySampleSurface/%s";\n', num2str(time_dir));
    fprintf(fid,'   object      U;\n}\n');
    fprintf(fid,'// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //');
    fprintf(fid,'\n\n');
    fprintf(fid,'//Average\n');
    fprintf(fid,'(0 0 0)\n');
    fclose(fid);       

    system(sprintf('%s %s%s %s%s', 'cp', old_dir, 'U', new_dir, 'U.org'));
    
    system(sprintf('%s %s%s %s%s %s %s%s', 'cat', new_dir, 'header', new_dir, 'U.org', '>', new_dir, 'U'));
    
    system(sprintf('%s %s%s', 'rm', new_dir, 'U.org'));
    
    system(sprintf('%s %s%s', 'rm', new_dir, 'header'));
    
end

system(sprintf('%s %s%s %s%s', 'cp', new_dir, 'mySampleSurface/faceCentres', case_dir, 'points.org')); 

fid = fopen([case_dir 'header'],'w');

fprintf(fid,'/*--------------------------------*- C++ -*----------------------------------*\\');
fprintf(fid,'\n| =========                 |                                                 |');
fprintf(fid,'\n| \\      /  F ield          | OpenFOAM: The Open Source CFD Toolbox           |');
fprintf(fid,'\n|  \\    /   O peration      | Version:  2.3.x                                 |');
fprintf(fid,'\n|   \\  /    A nd            | Web:      http://www.OpenFOAM.com               |');
fprintf(fid,'\n|    \\/     M anipulation   |                                                 |\n');
fprintf(fid,'\\*---------------------------------------------------------------------------*/');
fprintf(fid,'\nFoamFile \n{\n');
fprintf(fid,'   version     2.0;\n');
fprintf(fid,'   format      ascii;\n');
fprintf(fid,'   class       vectorField;\n');
fprintf(fid,'   object      points;\n}\n');
fprintf(fid,'// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //');
fprintf(fid,'\n');
fclose(fid);

system(sprintf('%s %s%s %s%s %s %s%s', 'cat', case_dir, 'header', case_dir, 'points.org', '>', case_dir, 'points'));

system(sprintf('%s %s%s', 'rm', case_dir, 'points.org'));
system(sprintf('%s %s%s', 'rm', case_dir, 'header'));


for i = 1:num_time
    
    time_dir = (i-1)*stp_time;  
                  
    old_dir = strcat(case_dir, num2str(time_dir), '/mySampleSurface/vectorField/');
    
    new_dir = strcat(case_dir, num2str(time_dir), '/'); 
    
    system(sprintf('%s %s %s%s', 'rm', '-r', new_dir, 'mySampleSurface')); 
    system(sprintf('%s %s %s%s', 'rm', '-r', new_dir, 'vectorField')); 
end

After this you can copy the folder ''mySampleSurface" to the ''constant/boundaryData" of your new case.

Hope this helps.

Best,
Likun

syavash · October 20, 2015, 14:09

Quote:

Originally Posted by Likun

Dear Syavash,

I also met similar problem before, and I have written a matlab script to add the head to the sampled file.

Suppose your sampleDict reads like this:

Code:

/*--------------------------------*- 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       dictionary;
    location    "system";
    object      sampleDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

//Example to output facecentres, faces and points for the selected patches

interpolationScheme cellPoint;

surfaceFormat foamFile;

surfaces
(
        mySampleSurface
        {
                type           plane;
                basePoint      (0.01 0.0 0.0);
                normalVector   (1.0 0.0 0.0);
//      type      patch;
//      patches  (OUTLET);
        }
);

//Not really required when run before a simulation as the velocity will be empty.
fields          ( U );

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

After sample you will have many timestep folders under the directory: 'xx/postProcessing/surfaces/' and within each timestep folder you have the sampled surface 'mySampleSurface/'.

Here is the matlab script that I used to add the header and to move the required files directly under the timestep folder.

Code:

num_time = 9; % Total number of timestep folders

stp_time = 1e-4;         % size of timestep

case_dir = 'xx/postProcessing/surfaces/';


for i = 1:num_time

    time_dir = (i-1)*stp_time;  
                  
    old_dir = strcat(case_dir, num2str(time_dir), '/mySampleSurface/vectorField/');
    
    new_dir = strcat(case_dir, num2str(time_dir), '/');
    
    fid = fopen([new_dir 'header'],'w');
    
    fprintf(fid,'/*--------------------------------*- C++ -*----------------------------------*\\');
    fprintf(fid,'\n| =========                 |                                                 |');
    fprintf(fid,'\n| \\      /  F ield          | OpenFOAM: The Open Source CFD Toolbox           |');
    fprintf(fid,'\n|  \\    /   O peration      | Version:  2.3.x                                 |');
    fprintf(fid,'\n|   \\  /    A nd            | Web:      http://www.OpenFOAM.com               |');
    fprintf(fid,'\n|    \\/     M anipulation   |                                                 |\n');
    fprintf(fid,'\\*---------------------------------------------------------------------------*/');
    fprintf(fid,'\nFoamFile \n{\n');
    fprintf(fid,'   version     2.0;\n');
    fprintf(fid,'   format      ascii;\n');
    fprintf(fid,'   class       vectorAverageField;\n');
    fprintf(fid,'   location    "constant/boundaryData/mySampleSurface/%s";\n', num2str(time_dir));
    fprintf(fid,'   object      U;\n}\n');
    fprintf(fid,'// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //');
    fprintf(fid,'\n\n');
    fprintf(fid,'//Average\n');
    fprintf(fid,'(0 0 0)\n');
    fclose(fid);       

    system(sprintf('%s %s%s %s%s', 'cp', old_dir, 'U', new_dir, 'U.org'));
    
    system(sprintf('%s %s%s %s%s %s %s%s', 'cat', new_dir, 'header', new_dir, 'U.org', '>', new_dir, 'U'));
    
    system(sprintf('%s %s%s', 'rm', new_dir, 'U.org'));
    
    system(sprintf('%s %s%s', 'rm', new_dir, 'header'));
    
end

system(sprintf('%s %s%s %s%s', 'cp', new_dir, 'mySampleSurface/faceCentres', case_dir, 'points.org')); 

fid = fopen([case_dir 'header'],'w');

fprintf(fid,'/*--------------------------------*- C++ -*----------------------------------*\\');
fprintf(fid,'\n| =========                 |                                                 |');
fprintf(fid,'\n| \\      /  F ield          | OpenFOAM: The Open Source CFD Toolbox           |');
fprintf(fid,'\n|  \\    /   O peration      | Version:  2.3.x                                 |');
fprintf(fid,'\n|   \\  /    A nd            | Web:      http://www.OpenFOAM.com               |');
fprintf(fid,'\n|    \\/     M anipulation   |                                                 |\n');
fprintf(fid,'\\*---------------------------------------------------------------------------*/');
fprintf(fid,'\nFoamFile \n{\n');
fprintf(fid,'   version     2.0;\n');
fprintf(fid,'   format      ascii;\n');
fprintf(fid,'   class       vectorField;\n');
fprintf(fid,'   object      points;\n}\n');
fprintf(fid,'// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //');
fprintf(fid,'\n');
fclose(fid);

system(sprintf('%s %s%s %s%s %s %s%s', 'cat', case_dir, 'header', case_dir, 'points.org', '>', case_dir, 'points'));

system(sprintf('%s %s%s', 'rm', case_dir, 'points.org'));
system(sprintf('%s %s%s', 'rm', case_dir, 'header'));


for i = 1:num_time
    
    time_dir = (i-1)*stp_time;  
                  
    old_dir = strcat(case_dir, num2str(time_dir), '/mySampleSurface/vectorField/');
    
    new_dir = strcat(case_dir, num2str(time_dir), '/'); 
    
    system(sprintf('%s %s %s%s', 'rm', '-r', new_dir, 'mySampleSurface')); 
    system(sprintf('%s %s %s%s', 'rm', '-r', new_dir, 'vectorField')); 
end

After this you can copy the folder ''mySampleSurface" to the ''constant/boundaryData" of your new case.

Hope this helps.

Best,
Likun

Dear Likun,

Thank you for sharing your solution.

Unfortunately, Matlab could not recognize 'cp' and 'rm' commands in your scrip! But I am aware that this is an issue with the version installed on my PC!
I could find a workaround. I could make the solver (pimpleFoam) to write the sampled plane (inlet bc) at each time steps. In this way, OpenFoam automatically generates a header with class vectorField just like the following:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       vectorField;
    location    "constant/boundaryData/inlet/0.2";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Then, I replaced keyword vectorField with vectorAverageField and '960'with '(0 0 0) 960', (960 is the number of faces in inlet bc) respectively using the following commands in linux terminal:

Code:

find ./ -type f -readable -writable -exec sed -i '0,/vectorField/s/vectorField/vectorAverageField/' {} \;

Code:

find ./ -type f -readable -writable -exec sed -i '0,/960/s/960/(0 0 0) 960/' {} \;

These command find and replace the desired keywords. The option '-i' allows the command 'sed' to be executed as 'in place', i.e. find a file in a folder, open and replace the desired word, save and then close to continue searching for another file.

Regards,
Syavash

ali.m.1 · January 11, 2016, 09:16

Quote:

Originally Posted by syavash

Dear Likun,

Thank you for sharing your solution.

Unfortunately, Matlab could not recognize 'cp' and 'rm' commands in your scrip! But I am aware that this is an issue with the version installed on my PC!
I could find a workaround. I could make the solver (pimpleFoam) to write the sampled plane (inlet bc) at each time steps. In this way, OpenFoam automatically generates a header with class vectorField just like the following:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       vectorField;
    location    "constant/boundaryData/inlet/0.2";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Then, I replaced keyword vectorField with vectorAverageField and '960'with '(0 0 0) 960', (960 is the number of faces in inlet bc) respectively using the following commands in linux terminal:

Code:

find ./ -type f -readable -writable -exec sed -i '0,/vectorField/s/vectorField/vectorAverageField/' {} \;

Code:

find ./ -type f -readable -writable -exec sed -i '0,/960/s/960/(0 0 0) 960/' {} \;

These command find and replace the desired keywords. The option '-i' allows the command 'sed' to be executed as 'in place', i.e. find a file in a folder, open and replace the desired word, save and then close to continue searching for another file.

Regards,
Syavash

Hi

If you got this to work, do you think it would be possible to run both simulations simultaneously?

So the 'inlet' BC reads the 'outlet' BC while the solver is running?

tomislav_maric · January 12, 2016, 11:57

The IOobject class has the member functions writeHeader and readHeader that write the appropriate headers to streams. Since files are abstracted as streams in C++, we can use the IOobject class to write a header to a file. Here is how the application looks like:

Code:

#include "fvCFD.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Main program:

int main(int argc, char *argv[])
{
    #include "setRootCase.H"
    #include "createTime.H"

    IOobject myObject 
    (
        "widget", 
        runTime.timeName(), 
        runTime, 
        IOobject::NO_READ, 
        IOobject::NO_WRITE
    ); 

    // Write the header to the output stream. 
    myObject.writeHeader(Info); 

    // Write the header to a file. 
    OFstream headerFile("myFile"); 
    myObject.writeHeader(headerFile); 

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

    Info<< "\nEnd\n" << endl;
    return 0;
}

When executed, it will write the header to the output stream, using the global messageStream Info object, and also to the output file stream (file), named "myFile".

If you want to change the parameters of the header, change the IOobject constructor arguments.

syavash · January 12, 2016, 12:56

Quote:

Hi

If you got this to work, do you think it would be possible to run both simulations simultaneously?

So the 'inlet' BC reads the 'outlet' BC while the solver is running?

Ali,

I am not really sure. The above-mentioned solution makes me able to perform a precursor simulation before doing the primary simulation.Adding that my computational resource does not allow me to have two simultaneous simulations!

Besides, I think it is the most appropriate solution for me to save data on a plane in advance, since I would be able to implement the data for as many simulations as I want to perform.

Regards

ali.m.1 · January 13, 2016, 08:15

Thanks Syavash

I'm planning on trying something like that, but it looks like it's going to be difficult!

regards

January 12, 2016, 11:57		#8
tomislav_maric Senior Member Tomislav Maric Join Date: Mar 2009 Location: Darmstadt, Germany Posts: 284 Blog Entries: 5 Rep Power: 21	The IOobject class has the member functions writeHeader and readHeader that write the appropriate headers to streams. Since files are abstracted as streams in C++, we can use the IOobject class to write a header to a file. Here is how the application looks like: Code: #include "fvCFD.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // // Main program: int main(int argc, char argv[]) { #include "setRootCase.H" #include "createTime.H" IOobject myObject ( "widget", runTime.timeName(), runTime, IOobject::NO_READ, IOobject::NO_WRITE ); // Write the header to the output stream. myObject.writeHeader(Info); // Write the header to a file. OFstream headerFile("myFile"); myObject.writeHeader(headerFile); // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Info<< "\nEnd\n" << endl; return 0; } When executed, it will write the header to the output stream, using the global messageStream Info object, and also to the output file stream (file), named "myFile". If you want to change the parameters of the header, change the IOobject constructor arguments. __________________ When asking a question, prepare a SSCCE.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[OpenFOAM.org] Patches to compile OpenFOAM 2.2 on Mac OS X	gschaider	OpenFOAM Installation	136	October 10, 2017 17:25
Trouble compiling utilities using source-built OpenFOAM	Artur	OpenFOAM Programming & Development	14	October 29, 2013 10:59
centOS 5.6 : paraFoam not working	yossi	OpenFOAM Installation	2	October 9, 2013 01:41
[OpenFOAM] Annoying issue of automatic "Rescale to Data Range " with paraFoam/paraview 3.12	keepfit	ParaView	60	September 18, 2013 03:23
Version 15 on Mac OS X	gschaider	OpenFOAM Installation	113	December 2, 2009 10:23

October 12, 2015, 07:43		#2
syavash Senior Member Syavash Asgari Join Date: Apr 2010 Posts: 473 Rep Power: 18	Anyone who might be interested?? This is a real problem for me since I need inlet velocity at each time step to be saved and used as boundary condition for another LES simulation! I also checked sample utility but it similarly only saves values and generates no header! TimeVaryingMappedFixedValue demands a header for velocity like this: Code: /--------------------------------- C++ -----------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: 2.3.1 \| \| \\ / A nd \| Web: www.OpenFOAM.org \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ FoamFile { version 2.0; format ascii; class vectorAverageField; object values; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // How can I generate a header like one in above for my sampled inlet boundary?? Thanks, Syavash

October 12, 2015, 07:46		#3
syavash Senior Member Syavash Asgari Join Date: Apr 2010 Posts: 473 Rep Power: 18	Anyone who might be interested?? This is a real problem for me since I need inlet velocity at each time step to be saved and used as boundary condition for another LES simulation! I also checked sample utility but it similarly only saves values and generates no header! TimeVaryingMappedFixedValue demands a header for velocity like this: [CODE] Code: /--------------------------------- C++ -----------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: 2.3.1 \| \| \\ / A nd \| Web: www.OpenFOAM.org \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ FoamFile { version 2.0; format ascii; class vectorAverageField; object values; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // How can I generate a header like one in above for my sampled inlet boundary?? Thanks, Syavash

October 13, 2015, 07:28		#4
syavash Senior Member Syavash Asgari Join Date: Apr 2010 Posts: 473 Rep Power: 18	No one can help me??! I am really stuck in this!

January 13, 2016, 08:15		#10
ali.m.1 Member Ali Join Date: Oct 2013 Location: Scotland Posts: 66 Rep Power: 12	Thanks Syavash I'm planning on trying something like that, but it looks like it's going to be difficult! regards