UFR 4-14 Test Case

Front Page

Description

Test Case Studies

Evaluation

Best Practice Advice

References

Flow in pipes with sudden contraction

Underlying Flow Regime 4-14               © copyright ERCOFTAC 2004

Test Case

Brief description of the study test case

Among the data available in the literature, those published by Durst and co-workers (Durst and Loy, 1985; Buckle and Durst, 1993), and by Bullen and co-workers (Bullen et al., 1990, 1996) are probably the most consistent and reliable, and have been used by the authors (ESDU) to define the two CFD Test Cases with the following geometries:

1.      Test Case 1 with s=0.286 and D=19.1 mm

2.      Test Case 2 with s=0.332 and D=110.17 mm

The experimental and numerical data for axial and radial velocity,and separation size by Durst and Loy (1985) and Buckle and Durst (1993) (s=0.286), and Bullen et al. (1990) and Bullen et al. (1996) (s=0.332) were used for comparisons. Comparisons for the pressure loss coefficient were carried out against the ESDU (2001) correlation, and the experimentally-based data of Bullen et al. (1996).

Test Case Experiments

4.1 Test Case 1 - 's' = 0.286

For this Test Case, LDA velocity measurements by Durst and Loy (1985), and Buckle and Durst (1993) are available. The test section consisted of a glass pipe with sudden change in cross section, mounted inside a channel filled with same fluid. The fluid was oil-Palatinol mixture with the same refractive index as the glass of the pipe wall, kept under controlled temperature conditions. A three-dimensional traversing system was used to allow precise positioning of the measuring point at any location inside the pipe. The Laser Doppler system consisted of a 15 mW-Helium-Neon-Laser and a compact optical system manufactured by OEI incorporating a double Bragg cell device for frequency shifting the laser beams. The effective measuring control volume was 200 mm in diameter and about 1600 mm in length. Measurements were carried at various sections upstream and downstream the contraction plane and for 23 £ ReD £ 1213.

Illumination by a laser light sheet allowed the observation of the recirculation regions. Measurements of the separation bubble developing downstream the separation plane are provided as length and height of the separation region. Details of the flow inside the separation could not be obtained, as a control volume of 20 mm is required. Based on the information provided and the scatter of the experimental data, it can be estimated that the measurements of this separation has an error up to ±30%. Within the experiments the upstream separation region could not be resolved and only visualization experiments were carried out to verify the variation of the recirculation size with Re.

Estimation of global uncertainty of measurements is with 95% confidence within 2%, derived as follows:

• Signal processing electronics of LDA-system 1%

• Traversing unit 1%

• Mass flow rate oscillations 0.5%

4.2 Test Case 2 - s =0.332

LDA velocity measurements by Bullen and co-workers at ReD=1.538×10⁵ and s =0.332are available for this Test Case. Bullen et al. (1990) used a Dantec three beam laser Doppler anemometer with a 7 mW Helium-Neon laser, in the forward scatter fringe mode with frequency shift to measure two velocity components simultaneously. The mean axial and radial velocities, turbulence kinetic energy and Reynolds stress distributions at twelve axial stations near the contraction plane were measured. The experimental rig was designed for water flow with ReD=3×10⁴ – 3×10⁵. A Perspex box for flow visualization and the application of LDA, filled with water to eliminate refraction problems, enclosed the test section. It consisted of 5.7 large diameters upstream and 9.1 downstream the contraction.

For the static pressure measurements necessary to derive the pressure loss coefficient, four circumferentially placed pressure tappings were used at each measurement point. Pressure was measured with inverted inclined manometers.

Uncertainty analysis for systematic and random error:

Wall static pressure ± 2.7 %

Flow rate ± 1.0 %

LDA axial velocity ± 0.35 % in the core region; ± 6.0 % near the wall

LDA radial velocity+ 1% systematic error

Turbulence quantities at inflow are not provided.

4.3 Pressure Loss Coefficient

The estimated error for the two contraction ratios analyzed can be summarized for the ESDU correlation (ESDU, 2001) as follows:

• 23 £ ReD £ 1200 around ± 20% as reported by Kaye and Rosen (1971)

• 4×10³£ ReD £ 10⁶ estimated –20% to +24%

The error for the pressure loss coefficient produced by Bullen et al. (1996) can be estimated as about ± 10%.

CFD Methods

Durst and Loy (1985) and Buckle and Durst (1993) solved the mass and momentum equations for a 2-D axisymmetric model of Test Case 1 using a finite volume method. The pressure correction method used was SIMPLE. The differencing scheme was Hybrid (combination of Central and Upwind solution schemes). The grid distribution allowed for mesh refinement at the wall and at the contraction plane. The largest mesh used in (Durst and Loy, 1985) was made of 4740 cells. This was increased to 38400 in (Buckle and Durst, 1993). The boundary conditions used were: velocity with parabolic profile at the inlet, and zero gradients for all variables at the outlet. The large tube length was L = 1.3 × D, the small tube length was l = D.

Bullen et al. (1990; 1996) produced CFD predictions produced using FLUENT (the version is not specified) with the standard k-ε turbulence model. The mesh was made of 8800 cells with a cell concentration around the contraction plane. Inlet and outlet boundary conditions were based on actual measurements. Bullen et al. (1990; 1996) do not specify what type of boundary conditions they used, but it is likely that inlet and outlet velocity boundary conditions with user specified profiles were used.

The CFD work carried out by the authors (ESDU) for the Test Cases 1 and 2 was generated using CFX 5 version 5.5.1 and 5.6 (website http://www-waterloo.ansys.com/cfx/products/cfx-5/). Results produced using both versions were almost identical. CFX 5 uses a coupled solver with a fully implicit discretization approach to solve the governing equations.

The lengths of the large and small pipes were taken as L=5×D and l=50×d, respectively, to ensure fully-developed flow at the inlet and outlet of the domain. The inlet flow rate was set using a user-specified velocity boundary condition. A parabolic inlet velocity profile was specified for laminar flow; a power law profile was specified for turbulent flow. For transition flow (ReD=1213 and 2000) both profiles were tested. The large pipe Reynolds Number ReD was varied between 23 and 10⁶. The outlet boundary condition was set at constant zero relative pressure. The fluid density was set to r=998 kg/m³, and the dynamic viscosity was set to m=0.001 Pa s (water at 20°C and atmospheric pressure).

2-D axisymmetric and 3-D steady state models were used. 3-D models using tetrahedral meshes were tested only for the Test Case 1 and laminar flow. A grid independence study was carried out with and without prismatic layers at the wall (inflation) for different mesh concentrations at the wall and at the contraction plane. The maximum number of cell size was made of about 2 million elements. It was found that, in order to capture the details of the flow separations upstream and downstream of the contraction, use of prismatic layers at the wall was essential. In particular the downstream separation was only predicted with wall prismatic layers. It was also important to have a fine distribution of the mesh in the wall layers. The number of layers was not crucial. Because of the mesh size required to achieve similar accuracy to the 2-D models, 3-D model analysis was not continued to generate results in turbulent flow and in this report only 2-D models results will be discussed.

The 2-D axisymmetric models were made of hexahedrons with mesh refinement at the wall and at the contraction plane. The mesh sensitivity of the solution was tested for the two Test Cases as follows. For laminar flow a mesh independent solution was obtained for highest Re-flow condition (ReD=1213). The maximum mesh size tested was made of about 150,000 cells. This mesh was then used to calculate solutions at lower laminar flow Re. For turbulent flow, mesh sensitivity was tested considering the turbulent model and near-wall treatment.

CFX5 provides both Wall Function and Low-Reynolds-Number methods for the near-wall treatment in turbulent flow. Low-Reynolds-Number methods as opposed to Wall Function methods solve for the flow in the viscosity-affected sub-layer close to the wall and are important to determine accurately the development of boundary layers and onset of separation. In the Wall Function approach, the viscosity affected sub-layer region is bridged using empirical formulas, i.e. logarithmic relation between the near-wall velocity and the wall-shear stress at the near-wall grid node, which is presumed to lie in the fully turbulent region of the boundary layer. In the Standard Wall Functions, the laminar sub-layer region of the boundary layer is not spanned adequately when the mesh at the wall is too refined and values of Yplus should be kept ³11. In the Scaleable Wall Function model (website http://www-waterloo.ansys.com/cfx/products/cfx-5/), it is assumed that the surface coincides with the edge of the viscous sub-layer, which is defined to be at Yplus=11. Therefore, all grids points are outside the viscous sub-layers and inconsistencies due to wall mesh refinement are avoided and arbitrarily fine meshes can be used.

The Automatic near-wall treatment model, developed by CFX for the k-ω based models, such as the k-ω and SST models, automatically switches from Wall Functions to Low-Re near wall formulation as the grid is refined. The k-ω model of Wilcox uses a known analytical expression for ω in the viscous sub-layer. The value for ω between the logarithmic and the near wall formulation is blended. The flux for the k-equation is artificially kept to be zero and the flux in the momentum equation is computed from the velocity profile. In the ω-equation, an algebraic expression is specified instead of an added flux, which is a blend between the analytical expression for ω in the logarithmic region and the corresponding expression in the sub-layers. Both the Scaleable Wall Function and the Automatic wall treatments can be run in arbitrarily fine grids. Further details of the equations used in these models can be found in CFX5 Version 5.6 (2003).

In this work, three turbulent models were tested: k-ε, SST (Menter, 1994), and k-ω (Wilcox, 1998). The near-wall treatment used for the k-ε turbulent model was Scaleable. The near-wall treatment used for the SST and k-ω models was Automatic. Some preliminary results obtained using the k-ω model with a Scaleable wall treatment produced similar results to the Scaleable k-ε turbulent model. The CFX5 default values for the inflow turbulence quantities were used for the three turbulence models. The default value of turbulence intensity is 3.7%. The turbulence length scale is auto-computed to approximate inlet values of k and ε. Meshes for each model were tested for different Yplus values, in the range of 0.1-100 for the maximum Yplus value. The maximum size of mesh tested for turbulent flow was made of about 250,000 cells. Both the Scaleable and Automatic near-wall treatments are designed to be Yplus independent unless very large values of Yplus are predicted. It was found that for all tested models, mesh refinement to reduce the maximum Yplus from about 100 to 0.1 produced a variation in the prediction of the pressure loss coefficient and upstream separation size of about 1%, but a variation in the downstream separation size of maximum 5 % for the SST and k-ω models and 30% for the k-ε model. Tests to study the sensitivity of the results to the inlet boundary conditions produced an error in the prediction of the pressure loss coefficient of about 0.5% per 0.5% variation of the inlet flow rate.

The advection algorithm used was the “2^nd order high resolution” scheme. The convergence criterion was based on very low RMS values of the residuals. While it was possible to achieve convergence for the pressure loss coefficient with RMS residuals below 10^-6, to achieve converged downstream separation sizes it was required to let the residuals settle until a nearly flat profile was achieved. This occurred for RMS residuals between 10^-6 and 10^-8, depending on the mesh and Re, and global velocity and mass balance less than 10^-10 %.

Axial and radial velocities, and pressure profiles were extracted at the different sections for comparisons with the experimental and numerical data. Cross-section averaged total pressure values were extracted at various inlet and outlet sections to derive the excess pressure drop and calculate the pressure loss coefficient (see Appendix A). Separation sizes were extracted form streamline plots. Comparisons of the ESDU CFD work with the CFD work by Durst and Loy (1985) and Buckle and Durst (1993) for Test Case 1, and Bullen et al. (1990; 1996) for Test Case 2 are discussed in the next section with the comparisons with their experimental data.

© copyright ERCOFTAC 2004

---

Contributors: Francesca Iudicello - ESDU

Front Page

Description

Test Case Studies

Evaluation

Best Practice Advice

References