[oceanFoam]

Edit: I am aware that this question has been discussed here before with a user named Fauster, however I could not find the actual solution to his issue anywhere.



Hello Niels,


I have a question about the integration of moving mesh cases to waves2Foam. I followed your user manual for the ompiling of waveDyMFoam, but a few things there are a bit hard to follow for me.


First of all, this is the content of my interDyMFoam folder, as found in OpenFOAM v 1712

/home/simon/OpenFOAM/OpenFOAM-v1712/applications/solvers/multiphase/interFoam/interDyMFoam
correctPhi.H  createDyMControls.H  interDyMFoam.C  Make  pEqn.H  readControls.H

This on the other hand is the output of the "compareFiles.sh" script that can be found in the manual.

============ BEGIN: alphaCourantNo.H ============
diff: /home/simon/OpenFOAM/OpenFOAM-v1712/applications/solvers/multiphase/interFoam/alphaCourantNo.H: No such file or directory

============= END: alphaCourantNo.H =============

============ BEGIN: alphaEqn.H ============
diff: /home/simon/OpenFOAM/OpenFOAM-v1712/applications/solvers/multiphase/interFoam/alphaEqn.H: No such file or directory

============= END: alphaEqn.H =============

============ BEGIN: alphaEqnSubCycle.H ============
diff: /home/simon/OpenFOAM/OpenFOAM-v1712/applications/solvers/multiphase/interFoam/alphaEqnSubCycle.H: No such file or directory

============= END: alphaEqnSubCycle.H =============

============ BEGIN: alphaSuSp.H ============

============= END: alphaSuSp.H =============

============ BEGIN: correctPhi.H ============

============= END: correctPhi.H =============

============ BEGIN: createAlphaFluxes.H ============
diff: /home/simon/OpenFOAM/OpenFOAM-v1712/applications/solvers/multiphase/interFoam/createAlphaFluxes.H: No such file or directory

============= END: createAlphaFluxes.H =============

============ BEGIN: createFields.H ============
81,86c81,83
< //#include "readGravitationalAcceleration.H"
< //#include "readhRef.H"
< //#include "gh.H"
< volScalarField gh("gh", g & (mesh.C() - referencePoint));
< surfaceScalarField ghf("ghf", g & (mesh.Cf() - referencePoint));
< 
---
> #include "readGravitationalAcceleration.H"
> #include "readhRef.H"
> #include "gh.H"
143,144d139
< 
< relaxationZone relaxing(mesh, U, alpha1);

============= END: createFields.H =============

============ BEGIN: pEqn.H ============

============= END: pEqn.H =============

============ BEGIN: rhofs.H ============

============= END: rhofs.H =============

============ BEGIN: setDeltaT.H ============
diff: /home/simon/OpenFOAM/OpenFOAM-v1712/applications/solvers/multiphase/interFoam/setDeltaT.H: No such file or directory

============= END: setDeltaT.H =============

============ BEGIN: setRDeltaT.H ============
diff: /home/simon/OpenFOAM/OpenFOAM-v1712/applications/solvers/multiphase/interFoam/setRDeltaT.H: No such file or directory

============= END: setRDeltaT.H =============

============ BEGIN: UEqn.H ============

============= END: UEqn.H =============

============ BEGIN: waveFoam.C ============
56,58d55
< #include "relaxationZone.H"
< #include "externalWaveForcing.H"
< 
62a60
>     #include "postProcess.H"
67d64
< 
71,75d67
< 
<     #include "readGravitationalAcceleration.H"
<     #include "readWaveProperties.H"
<     #include "createExternalWaveForcing.H"
< 
80d71
<     #include "postProcess.H"
84,87c75,80
<     #include "readTimeControls.H"
<     #include "CourantNo.H"
<     #include "setInitialDeltaT.H"
<     
---
>     if (!LTS)
>     {
>         #include "readTimeControls.H"
>         #include "CourantNo.H"
>         #include "setInitialDeltaT.H"
>     }
97,99c90,99
<         #include "CourantNo.H"
<         #include "alphaCourantNo.H"
<         #include "setDeltaT.H"
---
>         if (LTS)
>         {
>             #include "setRDeltaT.H"
>         }
>         else
>         {
>             #include "CourantNo.H"
>             #include "alphaCourantNo.H"
>             #include "setDeltaT.H"
>         }
105,106d104
<         externalWave->step();
< 
113,114d110
<             relaxing.correct();
< 
142,144d137
< 
<     // Close down the external wave forcing in a nice manner
<     externalWave->close();

============= END: waveFoam.C =============

Most files in the wavesFoam directory do not exist in the interDyMFoam directory. Am I supposed to copy all of them into the



/home/simon/OpenFOAM/simon-v1712/applications/utilities/waves2Foam/applications/solvers/solvers1712_PLUS/waveDyMFoam


directory? These are for example setDeltaT.H and createFields.H


If that is the case, the only file I would actually have to adapt would be interDyMFoam.C, which would have to be renamed into waveDyMFoam.C and then adapted, according to the last section of the comparFiles.sh-output?


Thanks a lot for supplying and maintaining this toolbox, and all the support you are giving here!


Cheers,
Simon

[blaise]

Hi Simon,

I want to share the solution I came up together with a colleague of mine, in the hope that it will be helpful to others.
This is for the integration of dynamic mesh movement into waves2Foam in OpenFOAM-v1712.

1. Create a folder parallel to the waveFoam folder. I called it "waveInterFoam". This gives a directory: waves2Foam/applications/solvers/solvers1712_PLUS/waveInterFoam

2. Copy all the contents (not the directory itself!) from directory OpenFOAM-v1712/applications/solvers/multiphase/interFoam into this new folder. As I don't want to use overInterDyMFoam and interMixingFoam for now, I deleted those two directories from this folder, just for the sake of clarity (not necessary though).

3. The directory now looks like:

drwxr-xr-x 4 ofuser users 4096 26. Jun 14:16 .
drwxr-xr-x 6 ofuser users 4096 26. Jun 14:16 ..
-rw-r--r-- 1 ofuser users   44 26. Jun 14:16 alphaSuSp.H
-rw-r--r-- 1 ofuser users  169 26. Jun 14:16 correctPhi.H
-rw-r--r-- 1 ofuser users 2530 26. Jun 14:16 createFields.H
-rwxr-xr-x 1 ofuser users  322 26. Jun 14:16 diff_script.sh
drwxr-xr-x 3 ofuser users 4096 26. Jun 14:16 interDyMFoam
drwxr-xr-x 3 ofuser users 4096 27. Jun 10:03 Make
-rw-r--r-- 1 ofuser users 1567 26. Jun 14:16 pEqn.H
-rw-r--r-- 1 ofuser users   76 26. Jun 14:16 rhofs.H
-rw-r--r-- 1 ofuser users  654 26. Jun 14:16 UEqn.H
-rw-r--r-- 1 ofuser users 4197 26. Jun 14:16 waveFoam.C

4. In createFields.H you change the following lines:

//#include "readGravitationalAcceleration.H"           
//#include "readhRef.H"                                  
//#include "gh.H"                                          
volScalarField gh("gh", g & (mesh.C() - referencePoint));     
surfaceScalarField ghf("ghf", g & (mesh.Cf() - referencePoint

At the very end, you add this line:

relaxationZone relaxing(mesh, U, alpha1);

5. Rename the file interFoam.C to, lets say, waveFoam.C.
Edit like we did in the attached waveFoam.C file. This essentially is identical to the changes applied in the original waveFoam.C code, so you could actually just copy the original waveFoam.C file to our waveInterFoam folder. Edit Make/files so that it reads

waveFoam.C

EXE = $(FOAM_APPBIN)/waveFoam

Perhaps you might prefer to install the resulting waveFoam solver to the $FOAM_USER_APPBIN directory, if you are the only user who is going to use it. The version above will overwrite the original waveFoam solver, if it was installed in $FOAM_APPBIN.

I am not entirely sure if this step is really necessary, as it seems to simply create a duplicate of waveFoam. Perhaps Niels could clarify this?

6. Edit the file Make/options:

EXE_INC = \
    -I$(FOAM_SOLVERS)/multiphase/VoF \
    -I$(LIB_SRC)/transportModels/twoPhaseMixture/lnInclude \
    -I$(LIB_SRC)/transportModels \
    -I$(LIB_SRC)/transportModels/incompressible/lnInclude \
    -I$(LIB_SRC)/transportModels/interfaceProperties/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/incompressible/lnInclude \
    -I$(LIB_SRC)/transportModels/immiscibleIncompressibleTwoPhaseMixture/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude \
    -I$(LIB_SRC)/sampling/lnInclude \
    -DOFVERSION=1712 \
    -DEXTBRANCH=0 \
    -DOFPLUSBRANCH=1 \
    -DXVERSION=$(WAVES_XVERSION) \
    -I$(WAVES_SRC)/waves2Foam/lnInclude \
    -I$(WAVES_SRC)/waves2FoamSamplingNew/lnInclude \
    -I$(WAVES_GSL_INCLUDE)

EXE_LIBS = \
    -limmiscibleIncompressibleTwoPhaseMixture \
    -lturbulenceModels \
    -lincompressibleTurbulenceModels \
    -lfiniteVolume \
    -lfvOptions \
    -lmeshTools \
    -lsampling \
    -L$(WAVES_LIBBIN) \
    -lwaves2Foam \
    -lwaves2FoamSampling \
    -L$(WAVES_GSL_LIB) \
    -lgsl \
    -lgslcblas

To be sure all path settings are correctly sourced, open a new terminal window and change to our directory.
Then run wmake.
This is all to be done in this directory. Now change to folder interDyMFoam.

7. Rename interDyMFoam.C to waveDyMFoam.C. Apply the changes like we did in the attached waveDyMFoam.C file.

8. Edit the file Make/files:

waveDyMFoam.C

EXE = $(FOAM_APPBIN)/waveDyMFoam

Again, mind the $FOAM_APPBIN vs. $FOAM_USER_APPBIN issue.

9. Edit the file Make/options:

EXE_INC = \
    -I. \
    -I.. \
    -I$(FOAM_SOLVERS)/multiphase/VoF \
    -I$(LIB_SRC)/transportModels/twoPhaseMixture/lnInclude \
    -I$(LIB_SRC)/transportModels \
    -I$(LIB_SRC)/transportModels/incompressible/lnInclude \
    -I$(LIB_SRC)/transportModels/interfaceProperties/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/incompressible/lnInclude \
    -I$(LIB_SRC)/transportModels/immiscibleIncompressibleTwoPhaseMixture/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude \
    -I$(LIB_SRC)/sampling/lnInclude \
    -I$(LIB_SRC)/dynamicMesh/lnInclude \
    -I$(LIB_SRC)/dynamicFvMesh/lnInclude \
    -DOFVERSION=1712 \
    -DEXTBRANCH=0 \
    -DOFPLUSBRANCH=1 \
    -DXVERSION=$(WAVES_XVERSION) \
    -I$(WAVES_SRC)/waves2Foam/lnInclude \
    -I$(WAVES_SRC)/waves2FoamSamplingNew/lnInclude \
    -I$(WAVES_GSL_INCLUDE)

EXE_LIBS = \
    -limmiscibleIncompressibleTwoPhaseMixture \
    -lturbulenceModels \
    -lincompressibleTurbulenceModels \
    -lfiniteVolume \
    -ldynamicMesh \
    -ldynamicFvMesh \
    -ltopoChangerFvMesh \
    -lmeshTools \
    -lfvOptions \
    -lsampling \
    -L$(WAVES_LIBBIN) \
    -lOceanWave3D \
    -Lwaves2Foam \
    -Lwaves2FoamSampling \
    -lwaves2FoamProcessing \
    -L$(WAVES_GSL_LIB) \
    -lgsl \
    -lgslcblas

I am not sure if all the includes and linker directives are necessary, but this works.
Again: open a new terminal window and change to this directory again.
Then run wmake.

Additionally you should add the following to the controlDict of your cases, if you want to use the runtime surface sampling feature:

libs
(
    "libwaves2FoamSampling.so"
);

I hope I didn't forget anything...

Good luck and best regards,

Pascal.
--

[oceanFoam]

Originally Posted by blaise

2. Copy all the contents (not the directory itself!) from directory OpenFOAM-v1712/applications/solvers/multiphase/interFoam into this new folder.
--

Edit: When applying your changes I saw that you apparently deleted one line in the Make/options files when adding the new lines at the very end of the file. The line


- lwaveModels
is not in your code fragment. I suppose that got lost in the pasting process.





Hi Pascal,


thanks for this very thorough explanation. The way this looks to me however, you are basically creating a second directory (waveInterFoam) like waveFoam, without the additional files (alphaCourantNo.H etc). All the exisitng files however should be the same as the ones found in waveFoam.


In that case could it be possible, that just copying interDyMFoam into waveFoam, and making the necessary changes only in this subfolder solver1712_PLUS/waveFoam/interDyMFoam?


But before I try it, have you done that already and found that it doesn't work?


Kind regards,


Simon

[oceanFoam]

Originally Posted by oceanFoam

Edit: When applying your changes I saw that you apparently deleted one line in the Make/options files when adding the new lines at the very end of the file. The line


- lwaveModels
is not in your code fragment. I suppose that got lost in the pasting process.





Hi Pascal,


thanks for this very thorough explanation. The way this looks to me however, you are basically creating a second directory (waveInterFoam) like waveFoam, without the additional files (alphaCourantNo.H etc). All the exisitng files however should be the same as the ones found in waveFoam.


In that case could it be possible, that just copying interDyMFoam into waveFoam, and making the necessary changes only in this subfolder solver1712_PLUS/waveFoam/interDyMFoam?


But before I try it, have you done that already and found that it doesn't work?


Kind regards,


Simon

Hi Pascal,


I tried both options. First I just copied the whole interFoam folder into solvers1712_PLUS and applied the changes. In another try I just took the adapted interDyMFolder and placed it in the existing waveFoam directory.



Both times I got the same error message

In file included from /home/simon/OpenFOAM/OpenFOAM-v1712/src/OpenFOAM/lnInclude/postProcess.H:129:0,
                 from waveDyMFoam.C:56:
../createFields.H: In function ‘int main(int, char**)’:
../createFields.H:84:25: error: ‘g’ was not declared in this scope
 volScalarField gh("gh", g & (mesh.C() - referencePoint));
                         ^
../createFields.H:84:41: error: ‘referencePoint’ was not declared in this scope
 volScalarField gh("gh", g & (mesh.C() - referencePoint));
                                         ^
In file included from /home/simon/OpenFOAM/OpenFOAM-v1712/src/OpenFOAM/lnInclude/postProcess.H:129:0,
                 from waveDyMFoam.C:56:
../createFields.H:144:1: error: ‘relaxationZone’ was not declared in this scope
 relaxationZone relaxing(mesh, U, alpha1);
 ^
In file included from waveDyMFoam.C:65:0:
../createFields.H:84:25: error: ‘g’ was not declared in this scope
 volScalarField gh("gh", g & (mesh.C() - referencePoint));
                         ^
../createFields.H:84:41: error: ‘referencePoint’ was not declared in this scope
 volScalarField gh("gh", g & (mesh.C() - referencePoint));
                                         ^
In file included from waveDyMFoam.C:65:0:
../createFields.H:144:1: error: ‘relaxationZone’ was not declared in this scope
 relaxationZone relaxing(mesh, U, alpha1);
 ^
waveDyMFoam.C:138:43: error: ‘ghRef’ was not declared in this scope
                     gh = (g & mesh.C()) - ghRef;
                                           ^
/home/simon/OpenFOAM/OpenFOAM-v1712/wmake/rules/General/transform:28: recipe for target 'Make/linux64GccDPInt32Opt/waveDyMFoam.o' failed
make: *** [Make/linux64GccDPInt32Opt/waveDyMFoam.o] Error 1

The changes made to the createFields.H file seem to be causing errors, since the used variables are not declared. Do I have to add som #include lines at the top or are the files maybe required in the directory I am trying to compile?


Sorry but I am a bit lost here. Also it all seems to be quite far off from the description in the user manual. Niels, do you know what might be causing the trouble? Or could you maybe upload an overview of your solver1712_PLUS directory with the changes necessary for waveDyMFoam to github?


That would be really great!


Thanks a lot everyone for your help.


Cheers,
Simon

[blaise]

Hi Simon,

the linker directive -lwaveModels was not lost accidentally. As far as I understand it, this links the wave models of OpenFOAM-v1712 into the waves2Foam library, thereby superseding wave2Foam's own wave models. Therefore things like 'relaxationZone" are not known to the compiler, as the wave modeling in OpenFOAM-v1712 obviously works differently.

Hope that helps!

Cheers,

Pascal.
--

[blaise]

Originally Posted by oceanFoam

Edit: When applying your changes I saw that you apparently deleted one line in the Make/options files when adding the new lines at the very end of the file. The line


- lwaveModels
is not in your code fragment. I suppose that got lost in the pasting process.





Hi Pascal,


thanks for this very thorough explanation. The way this looks to me however, you are basically creating a second directory (waveInterFoam) like waveFoam, without the additional files (alphaCourantNo.H etc). All the exisitng files however should be the same as the ones found in waveFoam.


In that case could it be possible, that just copying interDyMFoam into waveFoam, and making the necessary changes only in this subfolder solver1712_PLUS/waveFoam/interDyMFoam?


But before I try it, have you done that already and found that it doesn't work?


Kind regards,


Simon

Hi Simon,

you may be right, but I can't remember if I tried it before or not. Looking again on the differences between the interFoam directory and the waveFoam directory there are four files (alphaCourantNo.H, alphaEqn.H, alphaEqnSubCycle.H, and createAlphaFluxes.H) that are not in the interFoam directory. I did not copy these files into my waveInterFoam directory. Instead of this I added the first line in the waveInterFoam/Make/options file, which includes these files in a similar way as the original interFoam/Make/options file does:

In interFoam:

EXE_INC = \
    -I../VoF \

In waveInterFoam:

EXE_INC = \
    -I$(FOAM_SOLVERS)/multiphase/VoF \

In hindsight I probably could have just copied the 4 files to my waveInterFoam directory. I will try that later. But very likely there was a very good reason for Niels to do it this way, maybe for more robustness against future updates of OpenFOAM.

So perhaps your approach turns out to be more elegant... let me know! :-) I am by far not an expert on these things, I admit I do a lot of trial and error, trying to draw my conclusions from the outcomes.

Cheers,

Pascal.
--

[oceanFoam]

Originally Posted by blaise

Hi Simon,

you may be right, but I can't remember if I tried it before or not. Looking again on the differences between the interFoam directory and the waveFoam directory there are four files (alphaCourantNo.H, alphaEqn.H, alphaEqnSubCycle.H, and createAlphaFluxes.H) that are not in the interFoam directory. I did not copy these files into my waveInterFoam directory. Instead of this I added the first line in the waveInterFoam/Make/options file, which includes these files in a similar way as the original interFoam/Make/options file does:

In interFoam:

EXE_INC = \
    -I../VoF \

In waveInterFoam:

EXE_INC = \
    -I$(FOAM_SOLVERS)/multiphase/VoF \

In hindsight I probably could have just copied the 4 files to my waveInterFoam directory. I will try that later. But very likely there was a very good reason for Niels to do it this way, maybe for more robustness against future updates of OpenFOAM.

So perhaps your approach turns out to be more elegant... let me know! :-) I am by far not an expert on these things, I admit I do a lot of trial and error, trying to draw my conclusions from the outcomes.

Cheers,

Pascal.
--

Hello Pascal,


thanks a lot for all your tips. I figured everything out and set it up the way you explained it. In the end I just had two mistakes. First I had some errors in my waveDyMFoam.C script. The second one took me much longer. I actually never sourced the waves2Foam/bin/bashrc file.


I always got the error message telling me that realaxationTime.H was missing. This was because I always ran the script with ./bashrc instead of . bashrc (or source bashrc)



Well I guess you learn something new every day.
Anyways I am quite keen to start working with the tool now!



Have a nice weekend everyone.



Cheers,
Simon

[oceanFoam]

EDIT: Problem is resolved. The svn server is available again.



Hello Niels,


could it be that there is a problem with the SVN server at the moment? I tried to install waves2Foam on our HPC cluster today and got an error message

svn: E170013: Unable to connect to a repository at URL 'http://svn.code.sf.net/p/openfoam-extend/svn/trunk/Breeder_1.6/other/waves2Foam'

The same appeares when I am trying the svn update command at my already installed version on my own PC.


Is the current version of the source code available on github maybe? Or is there a way that I can copy it from my own PC, where waves2Foam is already compiled?


Thanks a lot,


regards
Simon

[fsifsi]

Hello Simon
I compile wave2foam and interFoam in OF1812 and I got error as:
/home/leqt/OpenFOAM/leqt-v1812/applications/utilities/waves2Foam/src/waves2Foam/lnInclude/readWaveProperties.H:27:38: error: ‘g’ was not declared in this scope
referencePoint.value() = g.value()/Foam::mag(g.value());

Could you tell me how to sourcewaves2Foam/bin/bashrc file, please.
Thanks