Adaptive Meshing in Multi-Phase Flow Simulation Using Ansys Fluent

In multiphase computational fluid dynamics (CFD) simulations, predicting the exact movement and location of fluid interfaces in advance is often impossible. Generating a static, uniformly fine mesh across an entire computational domain drastically increases cell counts and computation times.

The video "Adaptive Mesh in Multi Phase Flow Simulation Using Ansys Fluent" by Alpha Omega Product Development Systems demonstrates how to dynamically refine the mesh only near the air-water interface while maintaining a coarser mesh elsewhere. This approach reduces computational time while accurately capturing interface physics.

1. Geometry Setup & Watertight Meshing Workflow

The benchmark problem models a classic dam break scenario: a standing column of water inside a tank with a small bottom obstacle. When gravity is applied, the column collapses, flows across the tank, and impacts the obstacle.

  1. Watertight Geometry Import:Import CAD geometry from SpaceClaim into Ansys Fluent. The tank CAD geometry is loaded directly into Ansys Fluent using the Watertight Geometry workflow.
  2. Local Sizing Assignment:Target size of 2.5 mm on the bottom obstacle. Local mesh sizing is assigned to the obstacle to capture localized flow gradients.
  3. Poly-Hexcore Meshing: Poly-Hexcore volume mesh generation. A Poly-Hexcore volume mesh is generated with smooth boundary layer transitions, utilizing hex cells in core regions and polyhedra at boundaries to reduce overall cell count.

2. Solver Setup & Multi-Phase Physics

Once the volume mesh is generated with a minimum orthogonal quality of 0.31, the workflow transitions directly to the solution environment.

  • Physics & Gravity: Transient, pressure-based solver with gravity enabled.

  • Multiphase Model: Volume of Fluid (VOF) model with implicit body force and constant surface tension force enabled.

  • Turbulence Model: $k-\omega$ SST model.

  • Domain Initialization: The entire domain is initialized with air. A rectangular region register defines the initial water column boundaries using Adapt > Cell Registers before patching the water phase fraction.

3. Dynamic Mesh Adaption Configuration

To dynamically track the air-water boundary without manual mesh intervention, adaptive meshing parameters are configured:

  • Adaption Criteria: Set under Adapt > Refine/Coarsen using predefined VOF phase volume fraction gradients.

  • Dynamic Frequency: Execution frequency is set to run every 10 time steps.

  • Refinement Threshold: Cells with a volume fraction gradient greater than 0.06 are refined.

  • Coarsening Threshold: Cells with gradients below 0.05 are coarsened to conserve computational resources.

4. Key Takeaways & Results

As the water column collapses and surges toward the obstacle, Ansys Fluent continuously adapts the mesh around the moving fluid front.

  • Interface Resolution: Fine mesh resolution automatically follows the fluid front throughout the transient solve.

  • Efficiency: Eliminates the need for a fine grid across the entire domain, keeping cell counts low where flow gradients are uniform.

  • Practical Benefit: Significantly reduces compute time while maintaining sharp resolution at fluid interfaces.

For full setup details and execution steps, watch the video on YouTube: Adaptive Meshing in Multi-Phase Flow Simulation Using Ansys Fluent

Scroll to Top