geometricVofExt

Overview

The geometricVofExt package is an unofficial module of the geometric Volume of Fluid (VOF) method for OpenFOAM. This extension has a suite of pre- and post-processing tools alongside various solvers dedicated to two-phase flow dynamics. The pre-processing utilities are methodically assembled to initialize fraction fields of arbitrary shapes with optional dynamic mesh refinement, and to set up scalar, vector or tensor fields that vary based on the fraction values. These utilities are designed to enhance the flexibility and accuracy of multiphase flow simulations.

Moreover, the geometricVofExt package features solvers that utilize the innovative SimPLIC method, which supports unstructured meshes composed of arbitrary polyhedral cells. The SimPLIC method integrates Piecewise Linear Interface Calculation (PLIC) with Simpson's rule, offering an accurate and efficient approach to solve the VOF equation. These solvers are also designed to simulate the phase change phenomena and floating body dynamics. Additionally, the solvers ensure high adaptability to complex simulation scenarios with optional dynamic mesh refinement.

Package Structure

The geometricVofExt package is a comprehensive collection that includes libraries, applications, and tutorials. This package is meticulously organized to facilitate easy navigation, allowing users to effortlessly utilize the solvers and utilities included in the package. The package structure is shown below.

It should be noted that the utilities, solvers and tutorials under test are used to replicate the results presented in this study (Dai, Dezhi, Haomin Yuan, Albert Y. Tong, and Adrian Tentner. "A Geometric VOF Method for Interface Flow Simulations." arXiv preprint arXiv:2402.05247 (2024)), which illustrates the concepts and efficiency of the SimPLIC method.

SimPLIC Library

The SimPLIC library embodies the implementation of the SimPLIC method.

Key features:

• Employs the PLIC-VOF method for precise interface capturing.
• Delivers efficient interface reconstructions for improved computational performance.
• Ensures accurate interface advections, maintaining the fidelity of the fluid interface over time.
• Implements Adaptive Mesh Refinement (AMR) that dynamically refines the mesh based on the fraction field.
• Accommodates overset meshes, enhancing the flexibility in handling complex geometries and moving boundaries.
• Supports run-time PLIC interface sampling.

The VOF equation solved in the SimPLIC library is written as: $$\frac{\partial \alpha}{\partial t} + \nabla \cdot \left(\alpha \mathbf{U}\right) = S_p \alpha + S_u,$$ where $\alpha$ represents the VOF function, $t$ denotes time, $\mathbf{U}$ is the velocity vector, and $S_p$ and $S_u$ correspond to the implicit and explicit contributions to the net source, respectively.

For incompressible two-phase flows without phase change, both $S_p$ and $S_u$ are zero ($S_p = S_u = 0$). In the case of compressible two-phase flows without phase change, $S_p$ remains zero ($S_p = 0$) and $S_u$ is given by $\left(\nabla \cdot \mathbf{U}\right) \alpha$. For incompressible two-phase flows involving cavitation, $S_p = \left(\nabla \cdot \mathbf{U}\right) + \dot{V}_v - \dot{V}_c$ and $S_u$ as $\dot{V}_c$, where $\dot{V}_v$ and $\dot{V}_c$ represent the volume change rates due to condensation and evaporation, respectively. Within OpenFOAM framework, the Kunz, Merkle or SchnerrSauer cavitation model in the phaseChangeTwoPhaseMixtures library is adopted to evaluate $\dot{V}_v$ and $\dot{V}_c$. A summary of the different scenarios along with the corresponding solver(s) is given in the table below.

Scenario	Solver(s)	$S_p$	$S_u$	Note
Incompressible Without phase change	interPlicFoam overInterPlicDyMFoam	$0$	$0$	$\nabla \cdot \mathbf{U} = 0$
Incompressible Cavitation	interPlicPhaseChangeFoam overInterPlicPhaseChangeDyMFoam	$\left(\nabla \cdot \mathbf{U}\right) + \dot{V}_v - \dot{V}_c$	$\dot{V}_c$	Cavitation models Kunz model Merkle model SchnerrSauer model

When employing AMR, the geometric interpolation of fraction field during refinement can be achieved by setting the control parameter mapAlphaField to true within fvSolution->solvers->"alpha.*". This innovative fraction interpolation scheme, initially introduced in VoFLibrary, has been reimplemented in the SimPLIC library. Its process is presented below, where the reconstructed interface within the parent cell is utilized to divide each of the child cells and compute their respective submerged volumes/fractions.

CGALVof Library

The CGALVof library acts as a bridge between OpenFOAM meshes and CGAL geometric algorithms.

Key features:

• Delivers accurate geometric predicates while providing approximate geometric constructions.
• Capable of transforming an OpenFOAM surface mesh (MeshedSurface<face>) or an OpenFOAM mesh cell into a CGAL polyhedral surface (CGAL::Surface_mesh<P>).
• Allows for the direct creation of CGAL polyhedral surface meshes for boxes or spheres based on given dictionaries.
• Supports the import of external surface mesh files, compatible formats include *.stl, *.vtk and *.ftl.
• Features a Boolean operation processor for the manipulation of two CGAL surface meshes.
• Enables the assessment of mesh cell locations in comparison to a designated surface mesh, typically denoting the interface between two distinct phases.

Applications

The current list of utilities distributed with geometricVofExt is given below:

Utility	Description
setVofField	Set the VOF field (alpha.*) with arbitrary shapes. Built-in shapes: box, sphere, cylinder and cone. External surface meshes: *.stl, *.stlb, *.vtk, etc. Fraction-based dynamic mesh refinement.
setShapedFields	Set field values using arbitrary shapes. Dictionary is similar to the one for setFields. Volume-fraction averaging for cells partially enclosed by the shapes.
writeVtkSeries	Generate and write a VTK series for a surfaces function object. Function name is <funcName>. Output file is <funcName>.vtp.series or <funcName>.vtk.series.

The following are solvers that utilize the SimPLIC method:

Solver	Description
interPlicFoam	Solver for two-phase flows. Incompressible, isothermal and immiscible fluids. Derived from interFoam and interIsoFoam. Using SimPLIC method. Dynamic mesh refinement.
overInterPlicDyMFoam	Derived from overInterDyMFoam and interPlicFoam. Incompressible, isothermal and immiscible fluids. Overset (Chimera) meshes.
interPlicPhaseChangeFoam	Derived from interPhaseChangeFoam and interPlicFoam. Incompressible, isothermal and immiscible fluids. Cavitating flows. Dynamic mesh refinement.
overInterPlicPhaseChangeDyMFoam	Derived from overInterPhaseChangeDyMFoam and overInterPlicDyMFoam. Incompressible, isothermal and immiscible fluids. Cavitating flows. Overset (Chimera) meshes.

Build geometricVofExt

Compatibility

The source code of geometricVofExt is developed and maintained for OpenFOAM v2312.

Before Starting

• Make sure that OpenFOAM v2312 has been compiled successfully on the target machine.

• Verify that CGAL has been successfully compiled/loaded. Otherwise, the CGALVof library, setVofField and setShapedFields will not be compiled.

Building

• Create a directory named modules within $WM_PROJECT_USER_DIR, then proceed to download the geometricVofExt source code into $WM_PROJECT_USER_DIR/modules, i.e.,

source <installation path>/OpenFOAM-v2312/etc/bashrc

[ -d $WM_PROJECT_USER_DIR ] || mkdir $WM_PROJECT_USER_DIR
cd $WM_PROJECT_USER_DIR

[ -d modules ] || mkdir modules
cd modules

git clone https://github.com/daidezhi/geometricVofExt.git

• Check CGAL library:

source <installation path>/OpenFOAM-v2312/etc/bashrc

cd $WM_PROJECT_USER_DIR/modules/geometricVofExt

./checkCGAL

• (Optional) Enable the utilities and solvers to produce iso-surfaces/plic-surfaces at the initial time (e.g., $t = 0$):

source <installation path>/OpenFOAM-v2312/etc/bashrc

cd $WM_PROJECT_USER_DIR/modules/geometricVofExt

./enableInitialTimeWriting

• Compile libraries, utilities and solvers of geometricVofExt:

source <installation path>/OpenFOAM-v2312/etc/bashrc

cd $WM_PROJECT_USER_DIR/modules/geometricVofExt

./Allwmake -j4

• (Optional) Build utilities/solvers in applications/test:

source <installation path>/OpenFOAM-v2312/etc/bashrc

cd $WM_PROJECT_USER_DIR/modules/geometricVofExt

./enableReconstructionTimeTrackingInIsoAdvector

./Allwmake.test

Gallery

damBreakWithObstacle.mp4	oilDeaeration.mp4
Dam break	Oil deaeration

dropletImpact.mp4	bubbleRising.mp4
Droplet impact	Bubble rising

axisymmetricHemispherical.mp4
Cavitation

Tutorials

• ./tutorials/utilities/setVofField/

Case	Result
variousShapes
variousShapesAMR1
variousShapesAMR2

• ./tutorials/utilities/setShapedFields/

Case	Result
variousShapesAMR1

• ./tutorials/solvers/interPlicFoam/

Case	Configuration
bubbleRising
damBreakWithObstacle
dropletImpact
oilDeaeration

• ./tutorials/solvers/overInterPlicDyMFoam/

Case	Result
floatingBody floatingBody_overInterDyMFoam	floatingBody.mp4
twoSimpleRotors twoSimpleRotors_overInterDyMFoam	twoSimpleRotors.mp4
twoSquaresOutDomain twoSquaresOutDomain_overInterDyMFoam	twoSquaresOutDomain.mp4

• ./tutorials/solvers/overInterPlicPhaseChangeDyMFoam/

Case	Result
twoSimpleRotors twoSimpleRotors_overInterPhaseChangeDyMFoam	twoSimpleRotorsCavitation.mp4

• ./tutorials/verificationAndValidation/

Case	Configuration/Result	Note
axisymmetricHemispherical	Case illustration Mesh independence Pressure coefficient distributions	Mesh independence study is performed by using interPlicPhaseChangeFoam. This case is configured to verify the SimPLIC method for solving cavitating flows and includes the following solver(s): interPlicPhaseChangeFoam interPhaseChangeFoam References: Rouse, Hunter, and John S. McNown. "Cavitation and pressure distribution: head forms at zero angle of yaw." (1948). ADINA Simulating Cavitation

• ./tutorials/test/

Case	Note
createIcosphere	Create three different icospheres.
calcSurfaceMeshNonUniformFlow	Calculate tool meshes at various time instants using different initial surface meshes: initialShapeMeshIcosphere.stlb (Figure 7(a) in arXiv:2402.05247) initialShapeMeshNonUniform.stlb (Figure 7(b) in arXiv:2402.05247) The tool surface meshes used in arXiv:2402.05247 are available at ./tutorials/test/toolSurfaceMesh.
plicVofOrientationFoam	Test four orientation schemes in SimPLIC: CAG NAG LS RDF using a hexahedral mesh of $\Delta s = 2^{-5} m$ (First row of Table 6 in arXiv:2402.05247).
plicVofAdvectionFoam	Test SimPLIC-LS method using a hexahedral mesh of $\Delta s = 2^{-6} m$ (Table 14 in arXiv:2402.05247).
isoAdvectorAdvectionFoam	Test isoAdvector-plicLS method using a hexahedral mesh of $\Delta s = 2^{-6} m$ (Table 14 in arXiv:2402.05247).

Change Log

• 05/13/2024. Initial release.

Contributors

• Dezhi Dai, Nuclear Science & Engineering (NSE) Division, Argonne National Laboratory (ANL), [email protected] (Main developer)
• Haomin Yuan, NSE, ANL (PI of HPC4EI project, SimPLIC development and review)
• Albert Y. Tong, Department of Mechanical and Aerospace Engineering (MAE), University of Texas at Arlington (UTA) (SimPLIC development and review)
• Adrian Tentner, NSE, ANL (SimPLIC development and review)
• Vimalan Adaikalanathan, MAE, UTA (AMR testing)

License

geometricVofExt is released as an extension of OpenFOAM: you can redistribute it and/or modify it under the terms of the GNU General Public License as published by the Free Software Foundation, either version 3 of the License, or (at your option) any later version. See the file COPYING in this directory or http://www.gnu.org/licenses/, for a description of the GNU General Public License terms under which you may redistribute files.

Acknowledgment

This work was initially funded by the U.S. Department of Energy High-Performance Computing for Energy Innovation (HPC4EI) program, support for this program was provided by the U.S. DOE Office of Science, Office of Fossil Energy, Office of Energy Efficiency & Renewable Energy.

This work was conducted at Argonne National Laboratory and was supported by the U.S. Department of Energy, Office of Nuclear Energy, under Contract DE-AC02-06CH11357.

---