https://linen.dev logo
Join Discord
Powered by
# function-objects
  • a
    i am using decomposePar as weel, wondering if that is causing the issue
  • y
    the function is supposed to write the vtk files while the solver is running, no need for foamToVTK
  • y
    and the files should be written every time the solver write to disk
  • y
    what OpenFOAM version are you using?
  • a
    OpenFOAM -13
  • a
    The postProcessing/myCutPlane/0/ is always empty
  • a
    Wait
  • a
    I think I might be dumb, I'm running a 2d sim so the cut plane might not work for that
  • y
    well, the function definition looks fine so my next question would be "are you sure about your point and normal values"
  • a
    Point not so sure, but the plane is a xy plane so the normal will be the zplane
  • m
    what was the script to link the path of a custom solver in the control dict again ? I cannot remember :/
  • m
    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" );
  • t
    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:
    Copy code
    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 🙂
  • y
    According to the tutorials, syntax should look like this in v2406:
    Copy code
    surfaces
{
    type            surfaces;
    libs            (sampling);
    writeControl    writeTime;

    surfaceFormat   vtk;
    fields          (Q);

    surfaces
    {
        isoQ
        {
            type            isoSurface;
            isoField        Q;
            isoValue        1000;
            interpolate     true;
        }
    }
}
  • t
    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)
  • t
    Update: This is what worked for my case. Thank you @User!
    Copy code
    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; 

            }
        };
    }
}
  • f
    Yann the goat
  • y
    I just grepped the tutorials to see if there was an example somewhere:
    Copy code
    grep -r "isoSurface" $FOAM_TUTORIALS
  • y
  • y
    grepping ``$FOAM_SRC`` can help too, but I always find the sampling lib painful to explore
  • o
    hello, anyone has a function object to generate a field for the share stress? in the complete mesh? not only on the surface?
  • s
    You'll need a codedObject :/
  • s
    But it is not that difficult.
  • s
    The turbulenceModel class offers the "devReff()" method. That's your viscous + Reynolds shear stress tensor
  • s
    Copy code
    const incompressible::turbulenceModel& trbPtr =
    mesh().lookupObject<incompressible::turbulenceModel>
    (
      "turbulenceModel"
    );
// Stress tensor
tmp<volSymmTensorField> Reff_(trbPtr.devReff());
  • s
    You may, otherwise, modify your solver to call "devReff()" there
  • o
    I m in a laminar simulation 🥲
  • z
    Then don't you just need the velocity gradient?
  • z
    and multiply by viscosity?
  • z
    Well, it's a little more complicated than that, but the velocity gradient gives all the info you need from memory