Welcome to the IsoAdvector project

What is IsoAdvector?

IsoAdvector is a geometric Volume-of-Fluid method for advection of a sharp interface between two incompressible fluids. It works on both structured and unstructured meshes with no requirements on cell shapes. IsoAdvector is meant as a replacement for the interface compression with the MULES limiter implemented in the interFoam family of OpenFOAM solvers.

The isoAdvector concept and code was originally developed at DHI and was funded by a Sapere Aude postdoc grant to Johan Roenby from The Danish Council for Independent Research | Technology and Production Sciences (Grant-ID: DFF - 1337-00118B - FTP). Co-funding was also provided by the GTS grant to DHI from the Danish Agency for Science, Technology and Innovation.

The ideas behind and performance of the isoAdvector scheme is documented in:

Roenby J, Bredmose H, Jasak H. 2016 A computational method for sharp interface advection. R. Soc. open sci. 3: 160405. http://dx.doi.org/10.1098/rsos.160405

Videos showing isoAdvector's performance with a number of standard test cases can be found in this youtube channel:

https://www.youtube.com/channel/UCt6Idpv4C8TTgz1iUX0prAA

Important notice

Due to rapid and extensive api changes in the OpenFOAM Foundation (openfoam.org) version, the current repo is no longer kept up to date with the latest releases of that OpenFOAM version. The isoAdvector maintenance and development is now taking place in the OpenCFD version (openfoam.com) of OpenFOAM. In that code, the solver using isoAdvector is called interIsoFoam. The source code can be found here:

IsoAdvector library:
https://develop.openfoam.com/Development/openfoam/-/tree/master/src/transportModels/geometricVoF
InterIsoFoam application:
https://develop.openfoam.com/Development/openfoam/-/tree/master/applications/solvers/multiphase/interIsoFoam
setAlphaField application:
https://develop.openfoam.com/Development/openfoam/-/tree/master/applications/utilities/preProcessing/setAlphaField \

Compatibility

The isoAdvector code is developed and maintained for the newest OpenFOAM releases but the script isoAdvector/bin/generateCodeForOldVersion copies the code in isoAdvector/OpenFOAM to isoAdvector/OpenFOAM-[oldLoadedOFversion] and attempts to modify this code to become compatible with an older sourced OpenFOAM version. The code should work with the following OpenFOAM versions:

7, 6, 5.x, 4.x, 3.0.1, 2.2.2, 2.2.0

There are known to be issues with the following versions:

2.3.0, 2.3.1, 2.4.0

so using isoAdvector with these versions is not recommended.

OpenFOAM-v1706 and later vXXYY version contain an integration of the isoAdvector code with the interFlow solver named interIsoFoam. For more info on the v1706 integration see:

https://www.openfoam.com/news/main-news/openfoam-v1706/numerics#numerics-isoadvector

Note that compiling the github.com/isoAdvector code with v1706 and later vXXYY versions may lead to problems because the OpenFOAM finiteVolume library already contains classes named isoAvection, isoCutCell and isoCutFace.

Compatibility with OpenFOAM-dev is regularly checked, but the developers tend to frequently introduce minor API changes breaking the compatibility of isoAdvector with the OpenFOAM-dev. If you experience compilation errors with dev, please notify me at the e-mail address below, and I'll fix it as soon as possible.

A foam-extend version of the code is also available in isoAdvector/foam-extend. This was developed for foam-extend-32 and will most likely need modifications to work with newer versions. It does not contain the latest code developments.

Installation

0. Source your OpenFOAM environment, e.g.:

   source /home/$USER/OpenFOAM/OpenFOAM-6/etc/bashrc
   

1. In a linux terminal download the package with git by typing:

   git clone https://github.com/isoAdvector/isoAdvector.git
   

2. Execute the Allwmake script by typing (will finish in ~1 minute):

   cd isoAdvector
   ./Allwmake
   

   Applications will be compiled to your FOAM_USER_APPBIN and libraries will be compiled to your FOAM_USER_LIBBIN (You can check where e.g. the environmental variable FOAM_USER_APPBIN point to by typing

   echo $FOAM_USER_APPBIN
   

   in the terminal).

3. Test installation with a simple test case by typing (finishes in secs):

   cp -r OpenFOAM-6/run/prescribedU/discInConstantFlow/baseCase ~
   cd ~/baseCase
   ./Allrun
   

   Open Paraview and color the mesh by the alpha.water/alpha1 field.

4. (Optional) If you want to test the code on unstructured meshes, a number of such meshes can be donwloaded by using the downloadMeshes script in the bin directory. These meshes will take up ~2GB and will be placed in a folder called meshes. The meshes will be loaded by the scripts in discInConstantFlows, discInReversedVortexFlow, sphereInConstantFlow and sphereInReversedVortexFlow cases in run/prescribedU.

   Alternatively, the meshes can be downloaded directly from here:

   http://dx.doi.org/10.5061/dryad.66840
   

   The downloaded meshes.tar.gz file should be extracted to the isoAdvector root directory.

   Unstructured meshes can also be generated with the scripts generateTetUnitCube and generateTriUnitSquare in the bin folder. This requires gmsh (see headers).

Code structure

src/

• Contains the three classes implement the IsoAdvector advection scheme:
  • isoCutFace
  • isoCutCell
  • isoAdvection These are compiled into a library named libIsoAdvection.
• For comparison we also include the CICSAM, HRIC and mHRIC algebraic VOF schemes in finiteVolume directory. These were previously compiled into a library called libVOFInterpolationSchemes but are currently not compiled and are only included as legacy code.

applications/

• solvers/interFlow

  • A copy of the interFoam solver with the option to use isoAdvector instead of MULES in the interface advection step. To use add set application in controlDict to interFlow and add the following to the dicitonary fvSolution.solvers."alpha.water.*":

    "alpha.water.*"
    {
        //interfaceMethod can be set to "MULES", or "isoAdvector" (default).
    
        interfaceMethod "isoAdvector";
        
        //isoFaceTol is the precision with wich the isosurface cutting a cell 
        //into subcells should reproduce the cell's volume fraction. Typically 
        //between 1e-6 and 1e-8 (default).
    
        isoFaceTol  1e-8;
        
        //surfCellTol defines which cells are treated as surface cells. If 
        //
        //  surfCellTol < alpha1 < 1 - surfCellTol
        //
        //a cell will be treated with isoAdvector. Typically between between 
        //1e-6 and 1e-8 (default).
        //Important note: From experience p_rghFinal should be 10-100 times
        //smaller than surfCellTol or unphyiscal bubbles may be created by
        //isoAdvector in the water column because it interprets the continuity
        //errors in cells as presense of a fluid interface.
    
        surfCellTol 1e-8;
        
        //nAlphaBounds is the number of times the volume preserving bounding 
        //procedure should be applied after the advection step to repair 
        //fluxes of unbounded cells. Default is 3.
        
        nAlphaBounds 3;
    
        //If snapTol > 0 then after advection and volume preserving 
        //bounding all remaining alpha's closer to 0 than snapTol will be 
        //set to 0 and all alpha's closer to 1 than snapTol will be set 
        //to 1. Default value is 1e-12.
        
        snapTol 1e-12; //Previously called clipAlphaTol (and snapAlphaTol)
    
        //If clip is set to true/yes/1 then after advection and volume 
        //preserving bounding any alpha < 0 will be set to 0 and any alpha > 1 
        //will be set to 1.
    
        clip   true; //Previously called clipAlpha
    
        //To write out case/isoFaces/isoFaces#tIndex.obj change this to true:
    
        writeIsoFaces false;
    
        //For tri and tet meshes the standard isoAdvector method may result in 
        //large variations in the interface normal orientation in neighbouring
        //cells. A much smoother interface normal orientation is obtained by 
        //enforcing use of a smoothed gradient for the isoface orientations.
        //This method is activated by changing this to true:
    
        gradAlphaNormal false;
    }
    

    To use the functionality of a prescribed flow you can set momentumCorrector to no and nCorrectors to -1 in the fvSolution.PIMPLE directory and add the following to the dicitonary fvSolution.solvers.U:

    U
    {
        //If prescribedU and PIMPLE.nCorrectors is set to -1, then the velocty
        //and pressure equations will not be solved. Useful for pure advection 
        //test cases.
    
        prescribedU true;
    
        //In cases with prescribed U there is an option to make the prescribed 
        //velocity field periodic by multiplying it by a factor 
        //cos(2*pi*runTime.time()/period) if period > 0:
    
        period      0;
    
        //In cases with prescribed U there is an option to reverse the 
        //velocity field when a when the time reverseTime is reached:
    
        reverseTime 0;
    }
    

    Please see cases in OpenFOAM/run for examples of usage. Note that the first versions of the isoAdvector code had the following other solvers: isoAdvector, mulesFoam, passiveAdvectionFoam. With the introduction of the prescribedU switch described above, the functionallity of these solvers is now included in the interFlow solver and they have therefore been removed.

• utilities/preProcessing/setAlphaField
  • Sets the initial volume fraction field for a sphere, a cylinder, a plane or a sinus wave. See setAlphaFieldDict for usage. Previsouly called isoSurf.
• utilities/postProcessing/calcAdvectErrors
  • For cases with spheres and discs in steady uniform flow calculates errors relative to exact VOF solution. Previously called uniFlowErrors.
• test/isoCutTester
  • Application for testing isoCutFace and isoCutCell classes.

run/

• prescribedU/
  • Contains pure advection test cases (prescribedU = true) from literature.
• interFlow/
  • Contains test cases using interFlow coupling IsoAdvector with the PIMPLE algorithm for the pressure-velocity coupling.
• isoCutTester/
  • Case for testing the isoCutFace and isoCutCell classes.

Classes

IsoAdvection

• Calculates the total volume of water, dVf, crossing each face in the mesh during the time interval from time t to time t + dt.

IsoCutCell

• Performs cutting of a cell given an isovalue and the alpha values interpolated to the cell vertices.
• Calculates the submerged volume of a cell for a given isovalue.
• Calculates the isovalue given a specified target volume fraction of a cell.

IsoCutFace

• Performs cutting of a face given an isovalue and alpha values interpolated to the face vertices.
• Calculates the submerged face area given an isovalue and alpha values interpolated to the face vertices.

Contributors

• Johan Roenby, STROMNING, johan@stromning.com (Inventor and main developer)
• Hrvoje Jasak, University of Zagreb (General coding guidance, consistent treatment of boundary faces including processor boundaries, parallelisation, code clean up, provided algebraic schemes, CICSAM, HRIC etc.)
• Henrik Bredmose, DTU Wind Energy (Participated in conceptual development)
• Vuko Vukcevic, University of Zagreb (Code review, profiling, porting to foam-extend, bug fixing, testing)
• Andrew Heather, OpenCFD (Code clean up, porting to OpenFOAM+)
• Henning Scheufler, DLR (Extensive validation and bug fixing, gmsh based mesh generation)