Weighted essentially non-oscillatory library for the framework of OpenFOAM. Detailed information about the theoretical background and the implementation can be found in:
- J. W. Gärtner, A. Kronenburg, T. Martin, Efficient WENO library for OpenFOAM, SoftwareX, 2020
- T. Martin and I. Shevchuk, Implementation and Validation of Semi-Implicit WENO Schemes Using OpenFOAM, Computation, 2018
- Solving the Level Set Equation using High-order Non-oscillatory Reconstruction
A quick overview of the WENO scheme is provided in this presentation:
Please also check out the Discussion board of GitHub for more information about features or if you want to post a new idea.
Versions:
Major development stages of the library are marked by tags and recently also have a release with a DOI.
- OpenFOAM (ORG) v5.x - 8
- OpenFOAM (ESI) v1912
- Tobias Martin tobias.martin@ntnu.no
- Jan Wilhelm Gärtner jan.gaertner@outlook.de
When using this work please cite:
J. W. Gärtner, A. Kronenburg, and T. Martin, “SoftwareX Efficient WENO library for OpenFOAM”, SoftwareX, vol. 12, p. 100611, 2020, doi: 10.1016/j.softx.2020.100611.
T. Martin, and I. Shevchuk, “SoftwareX Efficient WENO library for OpenFOAM,” Computation, vol. 6(6), 2018, doi: 10.3390/computation6010006.
-
Clone the directory with
git clone https://github.com/WENO-OF/WENOEXT.git -
Execute
Allwmaketo build the library The compilation of the library uses cmake instead of wmake files!
GNU compiler version must be higher than 7. For g++ < v7 an error is reported for the specialisation template syntax. The syntax in the code is according to C++11 standard which is available for g++ v7 and higher.
To use the WENO scheme you have to add the library to your controlDict by editing system/controlDict
libs("libWENOEXT.so")
Within your system/fvSchemes file,
divSchemes
{
div(phi,U) Gauss WENOUpwindFit 2 1;
}
Here the first index '2' represents the order of the WENO scheme and the second index can be either '1' for bounded or '0' for unbounded.
Further options can be set in the WENODict located in the 'system/' folder:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object WENODict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// This dict contains expert parameters, which modify the standard WENO scheme.
//- Stencil extension ratio:
// - < 2.5 : decreased computational effort. May also decrease stability
// and accuracy
// - > 2.5 : higher stability. May influence the accuracy of the SVD
extendRatio 2.5;
//- WENO stencil weighting parameters:
p 4.0;
dm 1000.0;
//- Calculate best conditioned matrix
// This can save memory especially for high order WENO scheme
// Increases the calculation time! Default is off
bestConditioned true;
writeData true; // Write out the collected stencil list and matrix data
// default is 'true'
maxCondition 1E-05;// Inverse of the maximum condition that the pseudo
// inverse can have. Only change if you know what you
// are doing!
checkCondition false;// Check the condition of the pseudo inverse matrix
// If the central stencil has at least one zero entry
// the matrix is removed for all stencils of this cell.
// ************************************************************************* /The limited WENOUpwindFit scheme uses a cell limited approach known from other schemes such as linearUpwind. For scalar transport in the range 0 to 1 a specialized scheme called WENOUpwindFit01 is available. This schemes limits the value using the limiter of Zhang and Shu.
The code contains two tutorials from the standard cavity test.
To run the tutorials execute ./Allrun in the tutorial/ directory.
Testing is performed with the CATCH2 framework. You can compile and execute the tests
by executing ./runTest in the test directory. Further instructions are found in here
To check the code for different OpenFOAM implementations, e.g. OpenFOAM 8,
OpenFOAM v1912, etc. the code is copied into different docker containers
created with the Dockerfiles in CI/. In the docker container the code is compiled
and unit tests executed.
Executing the tests is controlled over the Makefile in the root directory. The different OpenFOAM versions can be tested with
# Just executing make runs all tests
make
# For OpenFOAM v5.x
make runTestsOF5
# For OpenFOAM 8
make runTestsOF8
This implementation allows to have the same testing on the local and remote branch.
This OpenFOAM library is under the GNU General Public License. This library contains the Blaze library licensed under the BSD license. Redistribution and use of the Blaze source code with or without modification, are permitted provided that the following conditions are met:
- Redistributions of source code must retain the above copyright notice, this list of conditions and the following disclaimer.
- Redistributions in binary form must reproduce the above copyright notice, this list of conditions and the following disclaimer in the documentation and/or other materials provided with the distribution.
- Neither the names of the Blaze development group nor the names of its contributors may be used to endorse or promote products derived from this software without specific prior written permission.