Desktop version

Home arrow Engineering

  • Increase font
  • Decrease font

<<   CONTENTS   >>

Numerical solution technique

The solver

The Finite Volume Method (FVM) is employed to solve the governing equations for the fluid mixture (air-water) phases. The computational domain is discretised into control volumes

Sketch of particle parcels within a typical computational control volume

Figure 1: Sketch of particle parcels within a typical computational control volume.

(cells) without overlapping (Figure 1). Unstructured meshes can be used to resolve complex geometry and achieve local grid refinement. In OpenFOAM®, all dependent variables are collocated at the centroid of the control volume. To overcome the checkerboard oscillation, Rhie-Chow interpolation (Rhie and Chow, 1983) is used. The velocity values at cell faces are evaluated via the discretised momentum equation with locally linearised convective terms, which are interpolated from adjacent grid nodes. With the exception of the sediment-fluid momentum transfer term as the additional source term in Equation 3 are incorporated into the L.H.S of the discretised momentum equation. In addition, a face limiting procedure in the OpenFOAM® library is also used to eliminate the localised over and under shoots during the reconstruction of gradients at cell centres.

For the solid phase, computational particles within a control volume are aggregated to calculate the solid fraction in each volume (see Figure 1). Particles are regarded to be inside a control volume as long as their centroids lie within the control volume boundary. As there are a large number of particles involved in scour processes, it is essential to introduce the concept of a parcel, which is assumed to be a group of particles with the same properties such as size, velocity and others. In this hybrid Eulerian-Lagrangian technique, parcels are used within the Lagrangian framework in order to reduce the computational expense to a level that is practicable.

Boundary and initial conditions

For a typical case, a rectangular domain is used as shown in Figure 2. An inlet boundary is specified at the upstream end with a prescribed water level, flow velocities and turbulence quantities. An outlet is used at the downstream boundary with all variables being linearly interpolated from internal node points to the boundary. The two cross-stream side (lateral) boundaries are specified as periodical boundaries. The structure is typically specified at the centre of the domain near the bottom with the surface being specified as a wall. The top boundary is treated as an inlet with an atmospheric pressure (zero pressure).

The initial conditions for the fluid mixture is typically specified at zero velocity. The volume fraction of water is prescribed as unity at levels below the free surface in the domain.

The requisite number of sediment particles are placed at the bottom of the domain within a pit with zero velocity initially (see Figure 2), to make up the prescribed total volume fraction. When a particle reaches the downstream boundary, it will no longer remain in the solution domain. If a periodic boundary condition is assigned, particles will enter from the corresponding boundary again into the computational domain.

Computational model set-up

Figure 2: Computational model set-up.

Solution procedure

The solution of the fluid mixture phase on the Eulerian grid follows the multiphase solver interFOAM in OpenFOAM®. The pressure-velocity coupling of the Navier-Stokes equat ions follows the PIMPLE algorithm of Issa (1986) for transient flows. In these algorithms, the equations are all solved in a segregated approach. The calculation starts with prescribed motion initially until the flow converges to steady or dynamic steady state. Once the fluid phase motion has been resolved, the results are then interpolated onto the particle position, and the position and velocity of each particle can be updated accordingly. In particular, the motion of each sediment parcel can be tracked through time using the following procedure:

  • 1. Interpolate relevant quantities (fluid density, fluid pressure gradient and ensemble- averaged fluid velocity) from the mesh to the particle location;
  • 2. Set a Lagrangian sub time step Atp of the Eulerian time step Д/ based on the Up value from the previous time-step;
  • 3. Update Up using the Euler difference form of Equation 8 with time step Дt.p; and
  • 4. Repeat until the Eulerian time step Д/ has been reached.

This procedure effectively integrates Equation 6 for each parcel to determine its new position at the end of the Eulerian (fluid) time step. A sub-time stepping procedure is used for the Lagrangian parcels to enable the code to run in parallel.

As one would expect, it is essential to know where the discrete Lagrangian particles are on the Eulerian grid, so that the correct particle-fluid interaction can be realised. The algorithm of Nordin (2000) and Macpherson and Weller (2009) is used in searching for the particles to reduce the total computational cost.

<<   CONTENTS   >>

Related topics