floodField

OpenFOAM utility for setting initial alpha.water field in interFoam simulations with free surface flow.

Description

floodField is a preprocessing tool designed to initialize the alpha.water field for interFoam simulations involving free surface flows, particularly useful when simulating scenarios with floating objects (e.g., a boat with an empty hull).

The standard setFields utility does not adequately handle cases where the water surface intersects with complex geometries. floodField solves this by using a flood-fill algorithm that:

1. Reads the mesh and initializes all alpha.water values to 0
2. Locates cells containing user-defined seed points (known to be underwater and outside solid regions)
3. Performs a breadth-first search from seed points, filling connected cells with water (alpha.water = 1) as long as they remain below the water surface

This approach naturally handles complex geometries like boat hulls, ensuring water is only placed in valid regions below the free surface.

Water Surface Definition

The water surface is defined by:

• Gravity vector: Read from constant/g (determines the direction of "down")
• Water level: A scalar value representing the projection along the -g direction

For standard gravity (0 0 -9.81), a water level of 5 corresponds to z = 5 m.

Directory Structure

floodField/
├── floodField.C          # Main application source
├── floodFieldDict        # Example configuration file
└── Make/
    ├── files             # Build configuration
    └── options           # Compiler/linker flags

tutorials/floodField/
├── Allrun                # Script to run the tutorial
├── Allclean              # Script to clean the tutorial
├── system/
│   ├── blockMeshDict     # Background mesh definition
│   ├── snappyHexMeshDict # Mesh refinement settings
│   ├── fvSchemes         # Discretization schemes
│   ├── fvSolution        # Solver settings
│   └── controlDict       # Time control
├── constant/
│   ├── g                 # Gravity vector
│   ├── transportProperties
│   └── triSurface/
│       └── boat.stl      # Boat hull geometry
└── floodedDomain.png     # Visualization of result

Compilation

To compile the utility, run:

git clone https://github.com/furstj/floodField.git
cd floodField
wmake

The compiled executable will be placed in $FOAM_USER_APPBIN/floodField.

Configuration

Copy floodFieldDict to system/floodFieldDict in your case directory:

// Water level as scalar projection along -g direction
// With gravity (0 0 -9.81), waterLevel 5 means z = 5 m
waterLevel 5;

// Seed points guaranteed to be underwater and outside solid regions
seedPoints
(
    (9 9 2)      // x y z coordinates
);

Usage

1. Prepare your mesh using e.g. blockMesh and optionally snappyHexMesh:

   blockMesh
   snappyHexMesh -overwrite

2. Run floodField:

   floodField

3. The utility will create/update the alpha.water field in the time directory.

Algorithm

The flood-fill algorithm works as follows:

1. Initialize all alpha.water values to 0
2. For each seed point, find the containing cell and add it to a queue
3. While the queue is not empty:
   • Pop a cell from the queue
   • Check all neighboring cells
   • If a neighbor has alpha.water = 0 and its center is below the water surface (projection along -g < waterLevel), set alpha.water = 1 and add to queue

Example

See tutorials/floodField/ for a complete example case featuring:

• A 10×10×10 m domain
• Water level at z = 5 m
• A boat hull without top face

License

This utility is provided as-is for use with OpenFOAM.