[cryabroad]

Hi all,

For LES it is suggested that the DFSEM (Divergence-free synthetic eddy method) should be used as the boundary condition at the inlet. After google it, I found that it is available starting from OpenFOAM1606 (the one downloaded from www.openfoam.com). Check this link for example, https://www.openfoam.com/releases/op...conditions.php.

However, it seems like this BC is not supported in OpenFOAM downloaded from www.openfoam.org, even for the latest version OpenFOAM 6.0. I also tried to copy the source and header files from the .com one to the .org one and then compile the BC (after some minor cleaning of the code of course), but got error messages like this

In file included from lnInclude/eddy.H:253:0,
                 from turbulentDFSEMInletFvPatchVectorField.H:85,
                 from turbulentDFSEMInletFvPatchVectorField.C:26:
lnInclude/eddyI.H: In member function ‘Foam::scalar Foam::eddy::epsi(Foam::Random&) const’:
lnInclude/eddyI.H:35:19: error: ‘class Foam::Random’ has no member named ‘sample01’
     return rndGen.sample01<scalar>() > 0.5 ? 1 : -1;
                   ^
lnInclude/eddyI.H:35:34: error: expected primary-expression before ‘>’ token
     return rndGen.sample01<scalar>() > 0.5 ? 1 : -1;
                                  ^
lnInclude/eddyI.H:35:36: error: expected primary-expression before ‘)’ token
     return rndGen.sample01<scalar>() > 0.5 ? 1 : -1;
                                    ^
In file included from turbulentDFSEMInletFvPatchVectorField.H:368:0,
                 from turbulentDFSEMInletFvPatchVectorField.C:26:
turbulentDFSEMInletFvPatchVectorFieldTemplates.C: In member function ‘Foam::tmp<Foam::Field<Type> > Foam::turbulentDFSEMInletFvPatchVectorField::interpolateBoundaryData(const Foam::word&) const’:
turbulentDFSEMInletFvPatchVectorFieldTemplates.C:75:21: error: there are no arguments to ‘fileHandler’ that depend on a template parameter, so a declaration of ‘fileHandler’ must be available [-fpermissive]
         fileHandler().filePath
                     ^
turbulentDFSEMInletFvPatchVectorFieldTemplates.C:75:21: note: (if you use ‘-fpermissive’, G++ will accept your code, but allowing the use of an undeclared name is deprecated)
turbulentDFSEMInletFvPatchVectorFieldTemplates.C:91:21: error: there are no arguments to ‘fileHandler’ that depend on a template parameter, so a declaration of ‘fileHandler’ must be available [-fpermissive]
         fileHandler().NewIFstream
                     ^
turbulentDFSEMInletFvPatchVectorField.C: In member function ‘void Foam::turbulentDFSEMInletFvPatchVectorField::writeLumleyCoeffs() const’:
turbulentDFSEMInletFvPatchVectorField.C:111:25: error: ‘fileHandler’ was not declared in this scope
             fileHandler().filePath
                         ^
turbulentDFSEMInletFvPatchVectorField.C: In member function ‘const Foam::pointToPointPlanarInterpolation& Foam::turbulentDFSEMInletFvPatchVectorField::patchMapper() const’:
turbulentDFSEMInletFvPatchVectorField.C:233:12: error: no match for ‘operator*’ (operand type is ‘Foam::autoPtr<Foam::pointToPointPlanarInterpolation>’)
     return *mapperPtr_;

It seems to suggest that some of the classes are defined differently between the two OpenFOAM? Am I missing something here?

Thank you in advance.

[mAlletto]

It seems that the random number used in eddy.H ("cachedRandom.H") is not implemented in the openfoam.org version.

[cryabroad]

Hi mAlletto,

Thank you for your input, and you are absolutely right. The random number class used in the .org version and .com version have different member functions, and the .org one has a couple of more member functions. Initially I was going to modify the random number class in the .org version (I mainly work on this one) according to the .com one, but soon found out that the coding will need substantial efforts instead of minor changes. As for now my plan is to implement my own turbulentDFSEMInlet boundary condition (in a much simplified way, if I can) in the .org version.

I still have questions about why the .org version doesn't implement this type of boundary condition, is the code not running very well or not good enough? Or I simply missed it in the .org version?

Thank you again for reading my post.

Ruiyan

[mAlletto]

Actually I have no idea why this boundary condition is not implemented in the .org version.


But maybe if you are able to get a version which is running also in the .org version you can try to submit it and look if it is accepted

[cryabroad]

I will definitely try that and see how it goes.

[mAlletto]

Having a first look on the DFSE method in the .com version I saw that the two base classes from which the boundary condition is derived from are also present in the .org version.


So i would guess it is not to complicated to take the sources of the .com version and try to compile it with the .org version.


After that one has to check if the two base classes are implemented in the same way.



If this is the case one has to check if the header files included in the .com version are present in the .org version.



If not as a first step i would put them together in a subfolder and link against to them.


After that try to compile it.



If you proceed in this way and post the errors you get maybe i can help you out.

[cryabroad]

Sounds great! I'll work on it and get back to you.

[cryabroad]

Hi Alletto,

Just want to get back to you on the discussions we had before. After trying to compile the DFSEM B.C. in the .org version of OF for a while I found it being very hard for me. Instead, I searched through this forum and found a similar B.C.-the inflowGenerator developed at Rostock. Right now I've been testing this B.C. for a while and it works well.

I think these two B.C. both adopt the idea of synthetic eddies. The DFSEM is divergence free but the inflowGenerator may be not.

Thanks.

Ruiyan

[mAlletto]

I think the method of the guys of Rostock is divergence free. I die not check the equations implemented in the github code but they pubished a divergencefree Methode a while ago

https://www.researchgate.net/publica...vortex_dipoles

It is however only made for isotropic turbulence. A Mord general method is published but not availabel online (at least what I could Figuren out)

https://www.researchgate.net/publica...ary_Anisotropy

[cryabroad]

Thank you for the information Michael, I will definitely check these out!

[mAlletto]

A by the way, did you compile the github version of the inflow generator with a newer OF version of the 2.4?

[cryabroad]

Sorry Michael for the late response.

I am using OF-4.x, and I compiled the inflow generator in LEMOS-2.4.x, which you can find here: https://github.com/LEMOS-Rostock/LEMOS-2.4.x. It is in folder LEMOS-2.4.x/libLEMOS-2.4.x/boundaryConditions/inflowGenerator/

Cheers,

Ruiyan

[fedvasu]

Originally Posted by cryabroad

Sorry Michael for the late response.

I am using OF-4.x, and I compiled the inflow generator in LEMOS-2.4.x, which you can find here: https://github.com/LEMOS-Rostock/LEMOS-2.4.x. It is in folder LEMOS-2.4.x/libLEMOS-2.4.x/boundaryConditions/inflowGenerator/

Cheers,

Ruiyan

I was able to compile that inflowGenerator in OF-6 with one change, creating a random vector by hand, as vector01 function is removed in random class.

[fedvasu]

Originally Posted by cryabroad

Sorry Michael for the late response.

I am using OF-4.x, and I compiled the inflow generator in LEMOS-2.4.x, which you can find here: https://github.com/LEMOS-Rostock/LEMOS-2.4.x. It is in folder LEMOS-2.4.x/libLEMOS-2.4.x/boundaryConditions/inflowGenerator/

Cheers,

Ruiyan

Hi Ruiyan,

Could you please tell me, how to use this? in U, "decayingTurbulenceInfowGenerator", not found among BCs,Do I have to create my own dummy solver with links to the newly compiled libray?

I tried running pimpleFoam, it did not work

[zhangyan]

Originally Posted by fedvasu

Hi Ruiyan,

Could you please tell me, how to use this? in U, "decayingTurbulenceInfowGenerator", not found among BCs,Do I have to create my own dummy solver with links to the newly compiled libray?

I tried running pimpleFoam, it did not work

Hi
I've made it compilable in OpenFOAM-7.
Here is my code and reference case:
https://github.com/ZhangYanTJU/boundaryConditions

[fedvasu]

Originally Posted by zhangyan

Hi
I've made it compilable in OpenFOAM-7.
Here is my code and reference case:
https://github.com/ZhangYanTJU/boundaryConditions

Great, I have a question, is this for anisotropic turbulence as described in the new paper or the old (2007) isotropic version?

[sadsid]

Originally Posted by fedvasu

Great, I have a question, is this for anisotropic turbulence as described in the new paper or the old (2007) isotropic version?

Hi, I have issues with LEMOS implementation. If you managed to apply this then please let me know how to implement it. I am using OF-6.