Flow in pipes with sudden contraction

Underlying Flow Regime 4-14 © copyright ERCOFTAC 2004

Best Practice Advice

Best Practice Advice for the UFR

7.1 Key Physics

The flow through pipes with sudden contraction is characterized by separation regions, upstream and downstream of the contraction plane, which cause an increase in pressure loss. The upstream separation occurs at low Re (the lowest analysed was ReD=23), and its size increases for 100<ReD<10⁴, and reduces slightly for ReD>10⁴. The downstream separation appears at ReD>300-400, and its size increases for ReD<10⁴. For ReD>10⁴ the length of this separation reduces slightly, while the height is nearly constant. For ReD>100, the velocity profile immediately downstream of the contraction displays an overshoot close to the wall.

From the CFD studies conducted by ESDU on the flow in pipes with sudden contraction, the following recommendations for best practice advice are given in the next subsections.

7.2 Numerical Modelling Issues

• 2-D axisymmetric models can be used, although Bullen et al. (1996) observed a slight asymmetry at the reattachment point of the downstream separation.

• 3-D models with tetrahedral mesh need wall prismatic layers to capture correctly downstream and upstream separations. It is crucial for these layers to have an adequate first cell height (can be obtained from 2-D grid sensitivity analysis). The number of layers can be kept at around 20.

• In both 2-D and 3-D modelling use: (a) suitable mesh concentration at the pipe wall and at the contraction plane with a minimum element height of 1/50×d and a minimum expansion factor 1.04 in laminar flow, and a minimum element height to ensure Yplus <100 with the same expansion factor in turbulent flow; (b) low RMS convergence criterion making sure that residuals reach a flat curve profile, (c) 2^nd order high resolution scheme.

• For the inlet boundary condition: (a) use a pipe length upstream of the contraction of L=5×D, (b) use inlet velocity profiles from separate fully developed pipe-flow calculation, i.e. parabolic inlet velocity profile for laminar flow, and a power law velocity profile for turbulent flow.

• For the outlet boundary condition: (a) use a pipe length downstream of the contraction of l=50×d, (b) use a constant static pressure boundary

7.3 Physical Modelling

• Steady-state calculations can be used, but transient calculations should be used to analyse flow instabilities at the flow reattachment of the downstream separation.

• From the CFD results obtained using the three turbulence models and near-wall treatments tested in this report, i.e. the k-ε with Scaleable Wall Function, and k-ω and SST models with Automatic near-wall treatment, the following recommendations on the turbulence modelling can be given: (a) the Automatic near-wall treatment should be used to predict well flow separation sizes (the Scaleable Wall Function cannot predict well flow separation), (b) the SST turbulence model with Automatic near-wall treatment should be used to capture flow details quantitatively and qualitatively, (c) to predict reasonably well flow details and pressure loss the k-ω model with Automatic near-wall treatment should be used, (d) the poor performance of the k-ε model for predicting the sizes of the separation zones is attributable to the Wall Function (although Scaleable) used not to the model itself.

• In transitional flow, the k-ω model with Automatic near-wall treatment should be used to predict flow details and pressure loss.

7.4 Application Uncertainties

The Test Cases discussed in this UFR have compared CFD results against experiments and numerical results published by Durst and Loy (1985) and Buckle and Durst (1993), and Bullen et al. (1990, 1996). In these papers, geometry and boundary conditions of the experimental and numerical test-cases have been well defined, although information on the sharpness of the contraction edge and inflow conditions of turbulent quantities have not been provided.

7.5 Recommendations for Future Work

The recommendations given in this UFR are based on CFD results obtained using CFX5 and three turbulence models: k-ε with Scaleable Wall Function near-wall treatment, and k-ω and SST models with Automatic near-wall treatment. Further CFD calculations should be conducted using different CFD solvers with highly promising turbulence models such as the Spalart-Allmaras and v2f models. Also, future CFD work should be carried out to investigate the effect of different contraction ratios on the prediction of the flow key features and pressure loss.

Contributors: Francesca Iudicello - ESDU