[qi.yang@polimi.it]

Hi,

I wrote a script to arrange the files based on the data post-processed by openfoam automatically, as below. However, I cannot use the original data in the 'p' files. Instead, I have to subtract p by a value. Anyone has ideas to make this change? Thanks.

patchname='patch_ground'
newpatchname='top'
variableFoldername=$patchname
variablename='p'
variaWriteName='p'
cp -r postProcessing/toppressuredata/surface .

for d in ./surface/* 
do

mkdir -p ./boundaryData/$newpatchname/$d/
#Write the default headline contents into the files
echo 'FoamFile
{
    version     2.0;
    format      ascii;
    class       scalarAverageField;
    object      values;
}
// **********************************************************************//
0.0' > ./boundaryData/$newpatchname/$d/$variaWriteName

#copy values from /surface folder to /boundaryData folder
cat 	./$d/$variableFoldername/scalarField/$variablename >> ./boundaryData/$newpatchname/$d/$variaWriteName
#mv ./boundaryData/newpatchname/$d ./boundaryData/newpatchname
done


#Transfer the format of the corresponding 'points' file
echo 'FoamFile
{
    version 2.0;
    format  ascii;
    class   vectorField;
    object  points;
}
// ******************************************************************************************//
'  > ./boundaryData/$newpatchname/points
cat  ./$d/$variableFoldername/faceCentres >> ./boundaryData/$newpatchname/points

#Transfer the format of the corresponding 'faces' file
echo 'FoamFile
{
    version 2.0;
    format  ascii;
    class   faceList;
    object  faces;
}
// ******************************************************************************************//
' > ./boundaryData/$newpatchname/faces
cat  ./$d/$variableFoldername/faces >> ./boundaryData/$newpatchname/faces

mv boundaryData/top/surface/* boundaryData/top

[Tobi]

If you are using an "incompressible" solver such as pimpleFoam or simpleFoam, the pressure is not the real pressure. This pressure field p is actually p' which is p' = p/rho. As the value of p' is not of interest for the numerical process (it does not matter if p' has negative values as we don't have any EOS) you commonly need to multiply your pressure value by the density and add a reference pressure such as the atmosphere one. You simply can see it by checking the pressure dimensions in the 0/p file.

[qi.yang@polimi.it]

Originally Posted by Tobi

If you are using an "incompressible" solver such as pimpleFoam or simpleFoam, the pressure is not the real pressure. This pressure field p is actually p' which is p' = p/rho. As the value of p' is not of interest for the numerical process (it does not matter if p' has negative values as we don't have any EOS) you commonly need to multiply your pressure value by the density and add a reference pressure such as the atmosphere one. You simply can see it by checking the pressure dimensions in the 0/p file.

Hi Tobi,

Thanks for your reply. I am using interfoam and the p is the real p that I need. Due to the fact that I require dynamic pressure, namely p-rho*g*h. Do you have any ideas to make this change based on my script?

[clapointe]

The solver actually computes (and writes) both! The field you're looking for is p_rgh (where p == p_rgh + rho*gh) -- you can check e.g. the pEqn to see this to be true.

Caelan

[qi.yang@polimi.it]

Originally Posted by clapointe

The solver actually computes (and writes) both! The field you're looking for is p_rgh (where p == p_rgh * rho*gh) -- you can check e.g. the pEqn to see this to be true.

Caelan

Yes, I understood this but what makes me confused is that the p_rgh and p is the same at the bottom of the wave. After I used p_rgh or p at the bottom minus rho*g*h is the correct dynamic wave pressure that I need. I don't know why. Additionally, my objective is to process the files. thanks anyway.

[qi.yang@polimi.it]

Hi,

I found p_rgh is definitely what I need after I modified the coordinates of gemetry. Now it is clear. Thank you both.

[Tobi]

Probably you can also change the "hRef" file (not given and is constructed by default).
It is similar to the gravity field and you specify the reference height here. This could solve your problem too.

Take a try and feel free to give feedback.

/*--------------------------------*- C++ -*----------------------------------*\ 
  =========                 |                                                   
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox             
   \\    /   O peration     | Website:  https://openfoam.org                    
    \\  /    A nd           | Version:  9                                       
     \\/     M anipulation  |                                                   
\*---------------------------------------------------------------------------*/ 
FoamFile                                                                        
{                                                                               
    format      ascii;                                                          
    class       uniformDimensionedScalarField;                                  
    location    "constant";                                                     
    object      hRef;                                                           
}                                                                               
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 
                                                                                
dimensions      [0 1 0 0 0 0 0];                                                
value           0.244;                                                          
                                                                                
// ************************************************************************* //

[qi.yang@polimi.it]

Originally Posted by Tobi

Probably you can also change the "hRef" file (not given and is constructed by default).
It is similar to the gravity field and you specify the reference height here. This could solve your problem too.

Take a try and feel free to give feedback.

/*--------------------------------*- C++ -*----------------------------------*\ 
  =========                 |                                                   
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox             
   \\    /   O peration     | Website:  https://openfoam.org                    
    \\  /    A nd           | Version:  9                                       
     \\/     M anipulation  |                                                   
\*---------------------------------------------------------------------------*/ 
FoamFile                                                                        
{                                                                               
    format      ascii;                                                          
    class       uniformDimensionedScalarField;                                  
    location    "constant";                                                     
    object      hRef;                                                           
}                                                                               
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 
                                                                                
dimensions      [0 1 0 0 0 0 0];                                                
value           0.244;                                                          
                                                                                
// ************************************************************************* //

Thank you Tobi. The hRef represents the height where I want to see the dynamic wave pressure or something else. I just put this file into the system folder with any file name?

[Tobi]

Hey,

it corresponds to the reference height which is related to:

p_rgh = p - rho*gh

The term gh is created in the createFields.H file:

#include "readGravitationalAcceleration.H"                                      
#include "readhRef.H"                                                           
#include "gh.H"

• read the graviational acceleration file constant/g
• read the hRef file constant/hRef (if exists - otherwise create one)
• build the gh file

    Info<< "\nReading hRef" << endl;                                            
    uniformDimensionedScalarField hRef                                          
    (                                                                           
        IOobject                                                                
        (                                                                       
            "hRef",                                                             
            runTime.constant(),                                                 
            mesh,                                                               
            IOobject::READ_IF_PRESENT,                                          
            IOobject::NO_WRITE                                                  
        ),                                                                      
        dimensionedScalar(dimLength, Zero)                                      
    );

As it is stated, the hRef file is read if present in the constant/ folder (named hRef and does have the value (0 0 0) as default. Finally, the gh field is calculated:

    Info<< "Calculating field g.h\n" << endl;                                   
    dimensionedScalar ghRef                                                     
    (                                                                           
        mag(g.value()) > SMALL                                                  
      ? g & (cmptMag(g.value())/mag(g.value()))*hRef                            
      : dimensionedScalar("ghRef", g.dimensions()*dimLength, 0)                 
    );                                                                          
    volScalarField gh("gh", (g & mesh.C()) - ghRef);                            
    surfaceScalarField ghf("ghf", (g & mesh.Cf()) - ghRef);

Hope this helps you.
Tobi

PS: Code snippet taken from v2106