This paper presents a computational analysis of the flow and pressure drop within nine ductwork fittings, from which representative fitting pressure-loss coefficients were calculated. The fittings analyzed are presented in Fig. 1. The objective of the work reported in this paper was to determine the applicability of using commercially-available CFD analytical tools for such a purpose. Where applicable, the ASHRAE Duct Fitting Database (DFDB) served as the source of published fitting pressure-loss coefficient data and identification (ID) code.

Prior work reported in the literature compares Computational Fluid Dynamics (CFD) results with experimental values for two general situations. One situation covers individual fittings acting alone, including rectangular transitions and elbows with round, square, rectangular and flat oval cross-sections. The other situation involves the behavior of close coupled duct fittings, including the interactions of two elbows, an elbow and a transition, and an air-handling unit and associated transitions and elbows. The literature cited above for individual fittings reported good correlation between CFD results based upon the k– turbulence model and experimental or other published data. For close coupled fittings, agreement was also generally good between the CFD work and published or experimental data. This paper explores many additional duct fittings. It also identifies the potential importance of including surface roughness in the CFD models used to analyze low-loss fittings, a topic not addressed in the literature cited above.

A commercial software package, was used to carry out the CFD numerical analysis. A DEC 300 Model 400 workstation served as the computer platform.

The following equations are coded into the commercial software. The Navier–Stokes equations describe the conservation of linear momentum. The continuity equation ensures “that the CFD code does not play God by creating extra fluid where it should not be”. The energy equation ensures that energy is neither created nor destroyed. The stress tensors relate stress to the rate of shear in the flow.

The commercial CFD software uses turbulence models because mankind is incapable of solving the Navier–Stokes Equations directly, for these practical flows in anything approaching a reasonable time. The turbulence length scales vary from the microscopic to a meter or more. The cell size required to capture the process completely and accurately would be so small and dense that the computer time required, even on a very large machine, would be prohivitive. The software makes available three choices of turbulence models, as described below.

First is the Standard k– model. k is the turbulent kinetic energy, and is the dissipation rate of k. This model is an eddy-viscosity model based upon the Boussinesq Hypothesis where the Reynolds stresses are assumed to be proportional to the mean velocity-gradients. The constant of proportionality is the turbulent eddy viscosity. The isotropic nature of the turbulent eddy viscosity in this model can be a major limitation in complex flows.

The second available turbulence model is the Reynolds Stress Model (RSM). The transport equations are solved for the individual stresses based upon a third-order velocity and pressure correlation. For very complex highly-swirling flows, this turbulence model may provide better results than the Standard k– model.

The final turbulence model available is the Renormalization Group Theory (RNG) k– model. This model may provide improved accuracy when modeling separated flows, flows with high streamline curvature, low Reynolds number flows, and transition or relaminarization.

The flow domain must be divided into discrete control volumes using a grid. The gridding activity will be presented later. The governing equations for each individual control volume must then be integrated to construct the algebraic equations for the discrete unknowns (pressure, velocities and stress components). The discretized equations are then solved using one of three available finite-difference schemes.

The first of the finite-difference schemes available in the commercial CFD software is the Power Law. This scheme interpolates the face value of a variable using the exact solution to a one-dimensional convection diffusion equation. This is the simplest and quickest of the schemes.

The Quadratic Upstream Interpolation for Convective Kinematics (QUICK) finite-difference scheme is also available. This scheme computes the face value of an unknown variable based on the values stored at two adjacent cell centers and on a third cell center at an additional upstream point.

The third available finite-difference scheme is the blended Second Order Upwind-Central (2nd UW) difference scheme. This scheme is similar to QUICK but with a different method of bounding the solution to eliminate oscillations and overshoots.

Gridding or grid generation is a very time-consuming activity, and is practised with considerable art. The node density normally should increase toward areas of high fluid dynamic gradients and areas of special interest. The commercial software package provides a preprocessor that may be used to create a structured grid based upon curvilinear body-fitted coordinates. The grid may include non-orthogonal grid lines and multiple connected regions. The grid points may be non-uniform with a distribution defined by hyperbolic tangent functions. A simple Cartesian mesh may also be generated.

Based upon extensive modeling studies by Mumma et al., it was concluded that the Standard k– turbulence Model and the Power Law Differencing Scheme produced the most favorable results. The inflow boundary conditions consisted of constant axial velocity with cross-flow components set to zero. The turbulence length scale was set to the duct inlet hydraulic radius. A 10 hydraulic diameter section of straight ductwork before and beyond the fitting was used to permit flow development and redevelopment for most cases. The convergence criteria required that the normalized residuals be less than 0.001.

While the size of the computational domain may be limited by the machine, taking advantage of symmetry within the geometry can significantly reduce convergence time. Each of the fittings contained a plane of symmetry. In some cases this saving was used for better resolution, while in others it was used to decrease convergence time.

A properly designed computational domain anticipates large pressure or velocity gradients. In regions where high gradients were expected, grid spacing was reduced. In regions where the flow was relatively uniform, grid spacing was increased. When generating non-uniform grids, care was given to minimize the rate of change of grid spacing. The axial grid spacing was increased at the ends of the computational domain where gradients were small, and decreased within the fitting where maximum change was expected. Non-uniform grid spacing was also used in the lateral directions, with much closer spacing near the walls.