[mohanphy]

Dear All,

I am trying to Compile boundary condition as a new dynamic library. I following this tutorials: http://openfoamwiki.net/index.php/Tu....28OF-1.4.1.29

I have done the following steps :

openfoam@Mohan:~/OpenFOAM/openfoam-1.6/src/finiteVolume/fields/fvPatchFields/derived$ svn checkout http://openfoam-extend.svn.sourcefor...bolicVelocity/
A parabolicVelocity/parabolicVelocityFvPatchVectorField.C
A parabolicVelocity/parabolicVelocityFvPatchVectorField.H
U parabolicVelocity
Checked out revision 1738.

I have downloaded it :

openfoam@Mohan:~/OpenFOAM/openfoam-1.6/src/finiteVolume/fields/fvPatchFields/derived$ cd parabolicVelocity/


openfoam@Mohan:~/OpenFOAM/openfoam-1.6/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity$ ls
parabolicVelocityFvPatchVectorField.C parabolicVelocityFvPatchVectorField.H

openfoam@Mohan:~/OpenFOAM/openfoam-1.6/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity$ mkdir Make

openfoam@Mohan:~/OpenFOAM/openfoam-1.6/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity$ ls
Make parabolicVelocityFvPatchVectorField.H
parabolicVelocityFvPatchVectorField.C

openfoam@Mohan:~/OpenFOAM/openfoam-1.6/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity$ cd Make/

openfoam@Mohan:~/OpenFOAM/openfoam-1.6/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity/Make$ vim files

openfoam@Mohan:~/OpenFOAM/openfoam-1.6/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity/Make$ vim options

wmake will show the following message :

openfoam@Mohan:~/OpenFOAM/openfoam-1.6/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity/Make$ wmake libso

wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file parabolicVelocityFvPatchVectorField.C
SOURCE=parabolicVelocityFvPatchVectorField.C ; g++ -m32 -Dlinux -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-40 -I/home/openfoam/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -IlnInclude -I. -I/home/openfoam/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/home/openfoam/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linuxGccDPOpt/parabolicVelocityFvPatchVectorField.o
'/home/openfoam/OpenFOAM/openfoam-1.6/lib/linuxGccDPOpt/libmyBCs.so' is up to date.
openfoam@Mohan:~/OpenFOAM/openfoam-1.6/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity$ ls
lnInclude parabolicVelocityFvPatchVectorField.C parabolicVelocityFvPatchVectorField.H
Make parabolicVelocityFvPatchVectorField.dep

It has successfully creates "libmyBCs.so" in /home/openfoam/OpenFOAM/openfoam-1.6/lib/linuxGccDPOpt/libmyBCs.so

The tutorials saying that I need to add the following line in system/controlDict file: libs ("libmyBCs.so");

The problem is I don't know where is the system/controlDict file (absolute path). some one please explain me to find system/controlDict file.

Thanks & Rg
Mohan L

[sihaqqi]

Mohan

I am after this parabolic velocity patch .C and .H. I use openFoam 2.1. the link you have given does not have these files. Can you please post these. The need is very urgent because first I have to understand them as a beginner in OpenFoam and then I shall have to convert in 1/7th power law.

I shall be grateful

regards

[wyldckat]

Greetings sihaqqi,

They are available here: https://github.com/ogoe/OpenFOAM-1.6...bolicVelocity/

Direct links:

• https://raw.github.com/ogoe/OpenFOAM...hVectorField.C
• https://raw.github.com/ogoe/OpenFOAM...hVectorField.H

Best regards,
Bruno

[sihaqqi]

Dear Bruno

Many thanks for this.
Thanks & Regards

Sihaqqi

[sihaqqi]

Bruno

Can you please advise where I can get Make files and options from for this thing

Regards

[wyldckat]

Originally Posted by sihaqqi

Can you please advise where I can get Make files and options from for this thing

It's explained in the first link on this thread: http://openfoamwiki.net/index.php/Tu....28OF-1.4.1.29

[nadine]

Hello,

I don't know if I am really unlucky, but none of the links refering to parapolicVelocity are working!!!

Can someone help me and post a valid link so I can add this condition and compile it?

Thanks a lot,
Nadine

[nadine]

Re-Hello,

Finally i found source files using this link:

https://github.com/Unofficial-Extend...eld.H.svn-base

I saved both the .C and .H in a file outside openfoam and followed the instructions givin in wiki to add my library and linked it dynamically by adding libs ("libmyBCs.so"); in my controlDict.

Than I ran the simulation but I got an error message, indicating that there is no such a boundary condition and giving me choices between the classical boundaries found in openfoam!!!

what did I do wrong and how can I fix it!
Help!

Waiting for your answers, even if it s summer time

Nadine,

[alexeym]

Originally Posted by nadine

Re-Hello,

Finally i found source files using this link:

https://github.com/Unofficial-Extend...eld.H.svn-base

I saved both the .C and .H in a file outside openfoam and followed the instructions givin in wiki to add my library and linked it dynamically by adding libs ("libmyBCs.so"); in my controlDict.

Than I ran the simulation but I got an error message, indicating that there is no such a boundary condition and giving me choices between the classical boundaries found in openfoam!!!

what did I do wrong and how can I fix it!
Help!

Waiting for your answers, even if it s summer time

Nadine,

Can you, please, post your case files?

[wyldckat]

Greetings to all!

@Nadine: I don't know if you've fixed the problem you reported about, but here is summary and updated building instructions, based on 1.6-ext and http://openfoamwiki.net/index.php/Tu....28OF-1.4.1.29 - edit: and yes it should work for almost any version of OpenFOAM!

Run these commands:

mkdir -p $FOAM_RUN
cd $FOAM_RUN/..
mkdir parabolicVelocity
cd parabolicVelocity

wget "http://sourceforge.net/p/openfoam-extend/OpenFOAM-1.6-ext/ci/master/tree/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity/parabolicVelocityFvPatchVectorField.C?format=raw" -O parabolicVelocityFvPatchVectorField.C
wget "http://sourceforge.net/p/openfoam-extend/OpenFOAM-1.6-ext/ci/master/tree/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity/parabolicVelocityFvPatchVectorField.H?format=raw" -O parabolicVelocityFvPatchVectorField.H

mkdir Make
echo 'parabolicVelocityFvPatchVectorField.C'  > Make/files
echo 'LIB = $(FOAM_USER_LIBBIN)/libmyBCs'  >> Make/files

echo 'EXE_INC =  -I$(LIB_SRC)/finiteVolume/lnInclude'  > Make/options
echo 'EXE_LIBS = '  >> Make/options

wmake libso

The I used the tutorial "incompressible/simpleFoam/pitzDaily" as basis and edited the files:

• "system/controlDict" - Added the line:
  

  libs ("libmyBCs.so");

• "0/U" - changed the BC "inlet" to this:
  

      inlet
      {
          type            parabolicVelocity;
          n               (1 0 0);
          y               (0 1 0);
          maxValue        1;
          value           (0 0 0); // Dummy for paraFoam, which will NOT show a correct profile at time 0.
      }

Then to run the case, I simply run:

blockMesh
simpleFoam

Best regards,
Bruno

[wzx1989221]

Dear Bruno,

I find your post very useful. Just want to know if it is possible to do the parabolic inlet in that way using OF 2.1? Or is it only applicable in OF 1.6-ext version?

Looking forward to your reply. Thank you very much.

Best regards,
Tony

[wyldckat]

Greetings Tony,

Originally Posted by wzx1989221

I find your post very useful. Just want to know if it is possible to do the parabolic inlet in that way using OF 2.1? Or is it only applicable in OF 1.6-ext version?

Good question! I've updated post #10 to add a note about that.

I forgot to mention back then, but it's sort-of implied that these instructions are for any OpenFOAM version, but rely on the source code of OpenFOAM-1.6-ext. Actually, now it's foam-extend 3.0, but this boundary condition is pretty much the same .

Best regards,
Bruno

[wzx1989221]

Dear Bruno,

Thank you very much for the reply. Actually I have checked out that it works well with OF 2.1.

One thing is that I tried to use it for 3D pipe flow, but the profile turned out to be varying in only one direction like in channel. Any suggestions on making it work for pipe?

Best regards,
Tony

[wyldckat]

Hi Tony,

Mmm... what you are looking for is a paraboloid: http://en.wikipedia.org/wiki/Paraboloid
But this boundary condition from 1.6-ext is only "parabolic"

The idea is that you need to modify the source code of the method "updateCoeffs()". Essentially, you need to modify these two lines of code:

 // Calculate local 1-D coordinate for the parabolic profile
scalarField coord = 2*((c - ctr) & y_)/((bb.max() - bb.min()) & y_);

vectorField::operator=(n_*maxValue_*(1.0 - sqr(coord)));

Right now I don't have much time to look into this. But let me know if you don't manage to solve this by yourself. And if you are able to, do share the solution!

Best regards,
Bruno

[wzx1989221]

Hi Bruno,

Many thanks for the tips. I will look into that to see if I can resolve it. I will share the solution if I make it.

Regards,
Tony

[vipin1431]

Originally Posted by wzx1989221

Hi Bruno,

Many thanks for the tips. I will look into that to see if I can resolve it. I will share the solution if I make it.

Regards,
Tony

hi tony,
I followed the above instruction to get parabolic inlet velocity and also i got same profile like i.e. variation along one direction only did you get it corrected....if yes, please help me to correct it.


regard
vipin

[rudolf.hellmuth]

Paraboloid velocity profile on a circular patch:

    inlet
    {
        type            codedFixedValue;
        value           uniform (0 0 0);
        redirectType    Poiseuille;   
        code
        #{
            const fvPatch& boundaryPatch = patch(); 
            const vectorField& Cf = boundaryPatch.Cf(); 
            vectorField& U = *this;
        
            //gfunc calculates the function on decomposed patches for parallel runs.
            scalar patchArea = gSum(boundaryPatch.magSf());
            //Info << "Patch area: " << patchArea << endl;
            
            vector ctr = gSum(boundaryPatch.magSf()*Cf)/patchArea;
            //Info << "Patch center: " << ctr << endl;
            
            scalar R = sqrt(patchArea/constant::mathematical::pi);
            //Info << "Patch radius: " << R << endl;
            
            vector n = gSum(boundaryPatch.magSf()*boundaryPatch.nf())/patchArea;
            //Info << "Patch mean normal: " << normal << endl;
            
            scalar Umean = 1.0;
            
            forAll(Cf, i)
            {
                U[i] = -n*2.0*Umean*(1.0 - sqr(mag(Cf[i] - ctr)/R));
            }
            // operator==(vector(1.0, 0.0, 0.0));
        #};
    }

This codedFixedValue BC is working for me. You can use this code to compile a PoiseuilleBC.so if you want.

I hope it can help you,
Rudolf

[vidyadhar]

Originally Posted by rudolf.hellmuth

Paraboloid velocity profile on a circular patch:

    inlet
    {
        type            codedFixedValue;
        value           uniform (0 0 0);
        redirectType    Poiseuille;   
        code
        #{
            const fvPatch& boundaryPatch = patch(); 
            const vectorField& Cf = boundaryPatch.Cf(); 
            vectorField& U = *this;
        
            //gfunc calculates the function on decomposed patches for parallel runs.
            scalar patchArea = gSum(boundaryPatch.magSf());
            //Info << "Patch area: " << patchArea << endl;
            
            vector ctr = gSum(boundaryPatch.magSf()*Cf)/patchArea;
            //Info << "Patch center: " << ctr << endl;
            
            scalar R = sqrt(patchArea/constant::mathematical::pi);
            //Info << "Patch radius: " << R << endl;
            
            vector n = gSum(boundaryPatch.magSf()*boundaryPatch.nf())/patchArea;
            //Info << "Patch mean normal: " << normal << endl;
            
            scalar Umean = 1.0;
            
            forAll(Cf, i)
            {
                U[i] = -n*2.0*Umean*(1.0 - sqr(mag(Cf[i] - ctr)/R));
            }
            // operator==(vector(1.0, 0.0, 0.0));
        #};
    }

This codedFixedValue BC is working for me. You can use this code to compile a PoiseuilleBC.so if you want.

I hope it can help you,
Rudolf

Hello Rudolf,

I have seen your post on paraboloid profile for a circular patch.

I would like to implement paraboloid profile for a square patch, since, in my case, I have to give fully developed profile at the inlet to a square channel.

Can you help me in implementing the same.

Thanks & Regards,
vidyadhar

[rudolf.hellmuth]

Originally Posted by vidyadhar

Hello Rudolf,
I would like to implement paraboloid profile for a square patch, since, in my case, I have to give fully developed profile at the inlet to a square channel.

I can easily help you to make this "paraboloid" if your rectangular patch is on a plane orthogonal to the Cartesian coordinates. If it is diagonal to the Cartesian coordinates, then you'd have to either give the patch orientation as input, or you'd have to figure out a way of obtaining the patch orientation with the patch data.

Try this:

// patch area
    scalar A = gSum(patch().magSf());
    
    // patch normal vector is the weighted mean of patch face normal
    // vectors
    vector np = gSum(patch().magSf()*patch().nf())/A;
    
    // patch centre is the weighted mean of patch face centres
    vector O = gSum(patch().magSf()*patch().Cf())/A;
   
    // local position of cell centres (referenced on the patch centre)
    scalarField pos = mag(patch().Cf() - O);
    
    // patch lengths on x and y directions
    scalar X = 1.0;
    scalar Y = 1.4;
        
    fixedValueFvPatchVectorField::operator==
    (
      -np*vmean*2.0 *(1.0 - sqr(pos.x()/X))*(1.0 - sqr(pos.y()/Y))
    );

I haven't tested that, it's just an idea. There are two parabolas, one on the x direction and the other on the y direction. I hope this code can help you.

Good luck!
Rudolf

[vidyadhar]

Hello Rudolf,

Thank you for the immediate help.

I will test the code and get back to you with the outcomes.

Thanks & Regards,
vidyadhar