Tank Discharge System CFD Analysis - ANSYS Fluent Simulation

Project Overview

This computational fluid dynamics study investigates gravitational water discharge from a multi-tank system using ANSYS Fluent software. The simulation employs the Volume of Fluid (VOF) model to accurately capture the two-phase flow dynamics involving water and air phases throughout the interconnected tank network.

System Configuration

Multi-Tank Arrangement

The computational domain encompasses three interconnected storage tanks connected through a piping network. The primary tank features rectangular geometry with dimensions of 229.4 mm by 157.7 mm, designed to serve as the initial water reservoir. The secondary tank utilizes an octagonal configuration with uniform side lengths of 51.3 mm, providing intermediate storage capacity. The tertiary tank employs rectangular geometry measuring 229.4 mm by 100 mm, functioning as the final collection vessel.

Geometric Design and Computational Grid

Two-Dimensional Model Development

The geometric configuration was developed using Design Modeler software, incorporating realistic tank geometries and interconnecting pipe networks to simulate industrial discharge systems. The design includes air circulation pathways to maintain atmospheric pressure balance during discharge operations.

Mesh Generation Specifications

The computational grid was generated using ANSYS Meshing software with an unstructured mesh topology containing 15,310 elements. This mesh density provides adequate resolution for capturing the complex free surface dynamics and flow transitions between the interconnected tank systems.

CFD Simulation Configuration

Fundamental Modeling Assumptions

The simulation utilizes a pressure-based solver approach suitable for incompressible flow conditions. The analysis is conducted in transient mode to capture the temporal evolution of the discharge process and free surface movement. Gravitational acceleration of -9.81 m/s² is applied along the negative y-axis to drive the discharge phenomenon.

Multiphase Flow Modeling

The Volume of Fluid homogeneous model governs the two-phase flow field equations with air and water as the defined Eulerian phases. Sharp interface modeling with interfacial anti-diffusion capabilities ensures accurate free surface tracking throughout the discharge process. The implicit formulation with implicit body force treatment provides robust solution stability for gravitational flow applications.

Viscous Flow Treatment

Laminar viscous modeling is employed to solve the flow field equations, appropriate for the low Reynolds number conditions typical in gravitational discharge applications. This approach provides accurate representation of viscous effects without the computational overhead of turbulence modeling.

Material Properties

Air properties are defined with density of 1.225 kg/m³ and dynamic viscosity of 1.7894×10⁻⁵ Pa·s, representing standard atmospheric conditions. Water-liquid properties utilize density of 998.2 kg/m³ and dynamic viscosity of 0.001003 Pa·s, corresponding to water at standard temperature conditions.

Numerical Solution Methods

The pressure-velocity coupling employs the SIMPLE algorithm for iterative solution convergence. Pressure discretization utilizes the PRESTO! scheme, optimized for complex geometries with significant density variations. Momentum equations are solved using second-order upwind discretization for enhanced accuracy, while volume fraction transport employs the compressive scheme to maintain sharp interface definition.

Domain Initialization and Patching

Standard initialization is applied throughout the computational domain with subsequent patching operations to establish initial water distribution. The primary tank region is initialized with unity volume fraction for the water phase, corresponding to coordinates spanning from x = 0.08 m to x = 0.379 m and y = 0.2264246 m to y = 0.33 m.

Temporal Solution Configuration

The simulation employs adaptive time advancement with initial time step size of 1×10⁻⁵ seconds. The adaptive scheme maintains minimum time step of 1×10⁻⁵ seconds and maximum time step of 0.001 seconds, with total execution of 10,000 time steps to capture complete discharge dynamics.

Results and Flow Analysis

Discharge Process Characterization

The simulation results present comprehensive visualization of volume fraction distribution, pressure fields, velocity magnitude, and streamline patterns throughout the discharge evolution. The analysis demonstrates progressive water transfer from the primary tank to the secondary tank, with subsequent overflow to the tertiary tank as storage capacity limitations are exceeded.

Free Surface Dynamics

Volume fraction contours clearly illustrate the free surface evolution and interface tracking accuracy throughout the discharge process. The VOF model successfully captures the complex interface deformation as water flows through the connecting pipes and fills the downstream tanks.

Flow Field Analysis

Velocity and streamline visualizations reveal the flow patterns within each tank and connecting pipe network. The results demonstrate the influence of air circulation pathways in maintaining pressure equilibrium and preventing vacuum formation during discharge operations.

Engineering Insights

The simulation provides valuable insights into multi-tank discharge system design, including optimal pipe sizing, tank geometry effects, and air circulation requirements. The pressure distribution analysis enables assessment of system efficiency and identification of potential flow restrictions or optimization opportunities.