I mean, they release a lot, but I assume they play on retrocompatibility not to need too much new documentation ?

oh I meant 'how the F. you find them' ahahah but for sure it is nice!

the thing is, this doc is only partial, and some part are just wrong / not up to date

Yeah, you can see in in the solver.C file, eg for ``simpleFoam``:

#include "fvCFD.H"
#include "dynamicFvMesh.H"
#include "singlePhaseTransportModel.H"
#include "turbulentTransportModel.H"
#include "simpleControl.H"
#include "fvOptions.H"

https://develop.openfoam.com/Development/openfoam/-/blob/master/applications/solvers/incompressible/simpleFoam/simpleFoam.C

And it also shows up in the equations, for instance in ``UEqn.H``:

tmp<fvVectorMatrix> tUEqn
    (
        fvm::div(phi, U)
      + MRF.DDt(U)
      + turbulence->divDevReff(U)
     ==
        fvOptions(U)
    );

Thanks a lot, that is exactly what I was searching for ! Now I will put this in interCondensatingEvaporatingFoam ✨

it already supports fvOptions, so you just need to use the model you want, or code your own if nothing suits your need

I want to be able to track the velocity of my "particles" (volume fraction) in a VoF solver with a function object. With time, preferably the velocity of the center of mass of my volume fraction field. Is there a function object that does this already, or what would be an appropriate starting point to make it myself?

You can try below one as the starting point and keep the outputs you need: https://github.com/tmaric/TwoPhaseFlow/blob/feature/density-ratio/run/rhoVoF/translatingDropletInQuiescentFluid3D/NewU-templateCase/system/FObubbleProcessing

so im trying to get cut planes to visualize flow but for some reason it is not saving the vtk files in the postprocessing file. is there something wrong with the way i have it set up

functions
{
    myCutPlane
    {
        type            surfaces;
        libs            ("libsampling.so");
        writeControl    writeTime;
        surfaceFormat   vtk;
        writeFormat     binary;
        fields          (p U); 
        interpolationScheme cellPoint;

        surfaces
        {
            myCutPlane
            {
                type            cutPlane;
                planeType       pointAndNormal;
                point           (0 0 0);
                normal          (0 0 1);
                interpolate     true;
            }
        }
    }
}

or does it pop up after i do

foamToVTK

i am using decomposePar as weel, wondering if that is causing the issue

the function is supposed to write the vtk files while the solver is running, no need for foamToVTK

and the files should be written every time the solver write to disk

what OpenFOAM version are you using?

OpenFOAM -13

The postProcessing/myCutPlane/0/ is always empty

Wait

I think I might be dumb, I'm running a 2d sim so the cut plane might not work for that

well, the function definition looks fine so my next question would be "are you sure about your point and normal values"

Point not so sure, but the plane is a xy plane so the normal will be the zplane

what was the script to link the path of a custom solver in the control dict again ? I cannot remember :/

Nvm, here is the solution 😉 solver compressibleLeeVoF; libs ( "libcompressibleLeeVoF.so" // your solver module (in $FOAM_USER_LIBBIN) // add any extra model libs you need too // "libLeeBoilingModels.so" );

Hey guys, I've been trying to figure this out for 3h and can't get it to work. I want to write .obj files of only the alphawater surface in openFoam v2406. I think the function doesn't even load. This is in my controldict:

functions
{
    alphaIso_asOBJ
    {
        type            surfaces;                 
        libs            ("libsampling.so");

        fields          ();
        
        isoSurfaces
        (
            (alpha.water 0.5)
        );      

        surfaceFormat   obj;
        writePrecision  6;
        parallelOutput  yes;                     
        writeControl    timeStep;                 
        writeInterval   10;                       
    }
}

Any help would be appreciated 🙂

According to the tutorials, syntax should look like this in v2406:

surfaces
{
    type            surfaces;
    libs            (sampling);
    writeControl    writeTime;

    surfaceFormat   vtk;
    fields          (Q);

    surfaces
    {
        isoQ
        {
            type            isoSurface;
            isoField        Q;
            isoValue        1000;
            interpolate     true;
        }
    }
}

Thank you very much, I'll try that. Where did you look this up? I'm new to openFoam and I didn't find good sources/documentation yet. (I'm a programmer, so a technical doc is fine)

Update: This is what worked for my case. Thank you @User!

functions
{
    waterSurface
    {
        type            surfaces;
        libs            (sampling);
        writeControl    timeStep;
        writeInterval   10;  
        
        surfaceFormat   obj;
        
        fields          (alpha.water);
        
        interpolationScheme cellPoint;
        
        surfaces
        {
            waterIso
            {
                type            isoSurface;
                isoField        alpha.water;
                isoValue        0.5; 
                interpolate     true;
                regularise      true; 

            }
        };
    }
}

Yann the goat

I just grepped the tutorials to see if there was an example somewhere:

grep -r "isoSurface" $FOAM_TUTORIALS

Online doc can help too (but it's not complete nor up-to-date): https://doc.openfoam.com/2306/tools/post-processing/function-objects/sampling/surfaces/isoSurface/

grepping ``$FOAM_SRC`` can help too, but I always find the sampling lib painful to explore