How to create isoSurface in the solver itself
 

Dear forum,
I am interested in coputation of Nu number on some internal surface (let say surface with the same radius, and I already have computed volScalarField R ). I want to interpolate my velocity and temperatue field in the solver (without usoin sample libriary).
Any suggestions how to do it?
I tried this constructor
Foam:: isosurface mysurf(mesh, U, R) but it does not pass compilation.
many thanks,
Yuri

Have a look to sampledIsoSurface
 

Dear Yuri,

The class you are looking for is sampledIsoSurface or sampledIsoSurfaceCell (they are define in the following directory $FOAM_SRC/sampling/sampledSurface/isoSurface/)

You have to construct it from a dictionary (I advice you to create your own dictionary) like this
Where your dictionary should look like the sub-entry required in sample dict:
Then to generate the surface, call the method "update". And to sample other fields on the surface use the function "sample".
If you want to interpolate the value to the surface, it is a bit more complex. But I think the following code should do the trick.
Best regards,

Frederic

Dear Frederic,
Thank you so much for a such comprehensive explanation. I have already started to implement it and faced with several problems.

1. I created my own dictionary. I called it sDict and put into the "system" directory of the case:

FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object sampleDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Iso surface for interpolated values only
interpolationScheme cellPointFace;
surfaces
(
midSphere
{
type isoSurface; // always triangulated
isoField R;
isoValue 0.4285;
interpolate true;
//zone ABC; // Optional: zone only
//exposedPatchName fixedWalls; // Optional: zone only
// regularise false; // Optional: do not simplify
}
);
now in my new solver I added two lines to create the dictionary ;


const fileName sDict("/raid0/yurifeld/OpenFoam/run/tutorials/heatTransfer/buoyantBoussinesqPimpleFoam/SpherGap/Gap0714/Ra510e4/system/sDict");
const dictionary SampleDict(sDict);

and then I create the sampling surface by

sampledIsoSurface midSphere("midSphere", mesh, SampleDict);
midSphere.update();
tmp<vectorField> interpolatedU = midSphere.sample(U);
tmp<scalarField> interpolatedT = midSphere.sample(T);


for some reason the program does not recognize the file so I am gettin a runtime error :
-> FOAM FATAL IO ERROR:
keyword isoField is undefined in dictionary "/raid0/yurifeld/OpenFoam/run/tutorials/heatTransfer/buoyantBoussinesqPimpleFoam/SpherGap/Gap0714/Ra510e4/system/sDict"
file: /raid0/yurifeld/OpenFoam/run/tutorials/heatTransfer/buoyantBoussinesqPimpleFoam/SpherGap/Gap0714/Ra510e4/system/sDict
From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 395.

2. As far as I understand if I sample volScalarField or volVectorField on the isosurface I already get an interpolated values. In this case this is not clear for me why separate interpolation functions are necessray. And how can I sample now surface field of temperature gradient:

surfaceScalarField heatFlux =fvc::snGrad(T);

if I just write
tmp<scalarField> dTdn= midSphere.interpolate(Foam::interpolation<scalar>( T));
I get a compilation error.

3. How can I write out the interpolated/sampled fields for visualizing/debugging. I saw that there is a function print(IOstream) bu it is not clear how to work with it.
Many many thanks,
Yuri

Answers to your questions
 

1. The dictionary should contain only the sub-entries of midSphere because by calling directly the class sampleIsoSurface you do a part of the job of sample: meaning you already specify that it is a surface and you give a name, so the only information missing are the parameters for the isoSurface.
To put it in a nutshell, your dictionary should look like
2. No, if you look at the code in "sampledIsoSurfaceTemplates.C", you can clearly read that it is just returning the value of the field in the cells cut by the iso-surface.
It is just a guess. But I think, it will do the job (N.B. doing an interpolation is more complicated as I said before, it looks like (see sampleSurfacesTemplates.C) that the following code should do the trick):
3. That also very tricky, another guess by looking again in sampleSurfacesTemplates.C and presuming you want to write it in VTK format
interpolateBoolean is a flag true if the value are interpolated, false otherwise.

N.B. Your code won't work if used in parallel... if this is mandatory I advice you to understand exactly the function sampleAndWrite of sampledSurfacesTemplates.C

I hope it will work.

Kindly,

Frederic

Hi,
I am trying similar thing, but I have some more basic problem.
Namely, my solver does not want to compile after I add line:
#include "sampledIsoSurface.H"

I guess I need it to define:
sampledIsoSurface midSphere("midSphere", mesh, SampleDict);

I have strange error, which seems to point on some OpenFOAM files:

SOURCE=cuette_spr.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam210/src/finiteVolume/lnInclude -I/opt/openfoam210/src/meshTools/lnInclude -I/opt/openfoam210/src/surfMesh/lnInclude -I/opt/openfoam210/src/triSurface/lnInclude -I/opt/openfoam210/src/conversion/lnInclude -I/opt/openfoam210/src/sampling/lnInclude -I/opt/openfoam210/src/lagrangian/basic/lnInclude -IlnInclude -I. -I/opt/openfoam210/src/OpenFOAM/lnInclude -I/opt/openfoam210/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/cuette_spr.o
In file included from /opt/openfoam210/src/OpenFOAM/lnInclude/triangle.H:42:0,
from /opt/openfoam210/src/OpenFOAM/lnInclude/triPointRef.H:35,
from /opt/openfoam210/src/OpenFOAM/lnInclude/triFace.H:48,
from /opt/openfoam210/src/triSurface/lnInclude/labelledTri.H:38,
from /opt/openfoam210/src/triSurface/lnInclude/triSurface.H:40,
from /opt/openfoam210/src/sampling/lnInclude/isoSurface.H:66,
from cuette_spr.C:49:
/opt/openfoam210/src/OpenFOAM/lnInclude/Random.H: In function ‘int main(int, char**)’:
/opt/openfoam210/src/OpenFOAM/lnInclude/Random.H:43:1: error: ‘namespace’ definition is not allowed here
In file included from /opt/openfoam210/src/OpenFOAM/lnInclude/triPointRef.H:35:0,
from /opt/openfoam210/src/OpenFOAM/lnInclude/triFace.H:48,
from /opt/openfoam210/src/triSurface/lnInclude/labelledTri.H:38,
from /opt/openfoam210/src/triSurface/lnInclude/triSurface.H:40,
from /opt/openfoam210/src/sampling/lnInclude/isoSurface.H:66,
from cuette_spr.C:49:
/opt/openfoam210/src/OpenFOAM/lnInclude/triangle.H:48:1: error: ‘namespace’ definition is not allowed here
/opt/openfoam210/src/OpenFOAM/lnInclude/triangleI.H:32:1: error: a template declaration cannot appear at block scope
In file included from /opt/openfoam210/src/OpenFOAM/lnInclude/triangle.H:248:0,
from /opt/openfoam210/src/OpenFOAM/lnInclude/triPointRef.H:35,
from /opt/openfoam210/src/OpenFOAM/lnInclude/triFace.H:48,
from /opt/openfoam210/src/triSurface/lnInclude/labelledTri.H:38,
from /opt/openfoam210/src/triSurface/lnInclude/triSurface.H:40,
from /opt/openfoam210/src/sampling/lnInclude/isoSurface.H:66,
from cuette_spr.C:49:
/opt/openfoam210/src/OpenFOAM/lnInclude/triangleI.H:46:1: error: expected ‘;’ before ‘template’
/opt/openfoam210/src/OpenFOAM/lnInclude/triangleI.H:60:1: error: a template declaration cannot appear at block scope
/opt/openfoam210/src/OpenFOAM/lnInclude/triangleI.H:69:1: error: expected ‘;’ before ‘template’
/opt/openfoam210/src/OpenFOAM/lnInclude/triangleI.H:75:1: error: a template declaration cannot appear at block scope
/opt/openfoam210/src/OpenFOAM/lnInclude/triangleI.H:81:1: error: expected ‘;’ before ‘template’
/opt/openfoam210/src/OpenFOAM/lnInclude/triangleI.H:88:1: error: a template declaration cannot appear at block scope
/opt/openfoam210/src/OpenFOAM/lnInclude/triangleI.H:95:1: error: expected ‘;’ before ‘template’
/opt/openfoam210/src/OpenFOAM/lnInclude/triangleI.H:102:1: error: a template declaration cannot appear at block scope
/opt/openfoam210/src/OpenFOAM/lnInclude/triangleI.H:109:1: error: expected ‘;’ before ‘template’
createFields.H:192:11: warning: unused variable ‘pRefCell’ [-Wunused-variable]
createFields.H:193:12: warning: unused variable ‘pRefValue’ [-Wunused-variable]
cuette_spr.C:180:1: error: expected ‘}’ at end of input
make: *** [Make/linux64GccDPOpt/cuette_spr.o] Błąd 1

I hope you can help me with this...
Best
MM

Dear Frederic,
Dear Yuri,
Please ignore my previous post. I fixed this problem.

I did everything like suggested in yours thread, but I still have this runtime error:
Do you know maybe how to fix this problem ?

Best and thanks
ZMM

Hi fcollonv,

When we calculate the other quantities on this iso-surface, can we also calculate the normal and tangential gradients at the points on that iso-surface? This correspond to the local coordinates maybe not the original coordinates. Thank you.

Dear Mieszkor,

I know the topic is old but I have the same error.

Remember how you solved this problem ?

Thanks.

Hi All,

i am trying to extract normal vectors from the constructed iso-surface. To do this i have to loop over the faces of the iso-surface and then loop over the points that belong to a particular face. If the points are arranged in the right way (i.e, clockwise or anticlockwise) the face area vectors should always point in the same direction (i.e inward or outward). This does not seem to be the case here. I printed the area vectors to check the orientation and they are not pointing in the same direction, some vectors point inward and some vectors point outward. Does this mean that the point labels in the face list are arranged randomly?..sounds weird

Best,
Andrea

Hello everyone,

I am relatively new to OpenFoam.

I am trying to use the sampledIsoSurface function in my solver like this:

const fileName sdict(runTime.path()/"system/SurfDict");
const dictionary surf(sdict);
Foam::sampledIsoSurface iso("iso",mesh,surf);

But when compiling the solver I get the following error:

IsointerFoam.C:75: error: ‘sampledIsoSurface’ is not a member of ‘Foam’
IsointerFoam.C:75: error: expected ‘;’ before ‘iso’

I looked through all the files but was unable to find the solution to this problem myself. Can someone please point out what am I doing wrong in this addition to the code?

This is not valid C++.

Hi all,

@akidess

Why? runTime.path() is fileName instance with overloaded / operator.

@raunakbardia

Do you include sampledIsoSurface.H header?

Because you can't just concatenate a string without an operator. I'm not aware of an overloaded "/"-operator to concatenate strings.

Edit: Operator is indeed overloaded here: https://github.com/OpenFOAM/OpenFOAM...ame/fileName.C

Thanks for your replies!

@Anton: I came across the use of this forward slash operator on some online forum and it seems to be working fine here. When I tried to output the file name stored in the variable sdict, it gave me the correct output.
As you rightly mentioned in the link, there is a friend operator on line # 431 which might be defining this functionality. Also, the compilation does not show any error on this statement when I run it separately as well.

@Alexey: I had tried adding that header file earlier but I got this error.

"could not open file sampledIsoSurface.H for source file IsointerFoam.C"

I assumed that the source files are added in the dependency list on their own so I should not be including it separately. Please correct me if I am wrong.

If indeed, I have to add this header file separately, then I am not sure why I am getting the aforementioned error.

Thanks again for your help!

Try to remove Foam:: and just use

add

in IsointerFoam.C, and add

in Make/option.
In my case it works just fine in this way

Soon after I wrote my last question, I realized I should be looking at the library dependencies.

Thanks for your reply Andrea. That definitely solved the problem. My two cents to that addition is that the compilation also requires two other libraries if they are not already added in your solver

EXE_INC = \
...
-I$(LIB_SRC)/sampling/lnInclude \
-I$(LIB_SRC)/triSurface/lnInclude \
-I$(LIB_SRC)/meshTools/lnInclude

EXE_LIBS = \
...
-lsampling \
-lmeshTools \
-ltriSurface


However, the compiled solver still doesn't work. I am facing the same error as mentioned in the posts above:

but no one mentioned how they solved the problem. This is how my dictionary looks like:

I am clearly mentioning the isoField in the dictionary but the solver fails to recognize it?

sounds weird, there is probably something wrong in the way you read the dictionary. It is difficult to say more than this without seeing your source code.

best,

andrea

Thanks Andrea.

I was able to solve the issue.

Instead of reading the dictionary directly I created an IOdictionary object in the createFields.H and obtained the inputs from that dictionary to create the isosurface. This idea was from one of your other posts: https://www.cfd-online.com/Forums/op...ce-normal.html

I am not sure why this method worked while the other didn't but I will stick with this for now.

Hello All, Does this idea works on parallel run? I am facing problems in parallel run but not in serial run.