# CFD analysis of axial annular diffuser with both hub and casing diverging at unequal angles.

IntroductionThe function of a diffuser is the efficient conversion of kinetic energy into pressure. Many fluid-dynamical systems involve diffusion in annular passages. Need for annular diffusers may arise from a necessity to provide a central core to allow a coaxial shaft in a given situation. Annular diffusers are widely used in engineering, in particular, as outlet devices of pumps and turbines often located downstream of turbo machinery in a number of applications. In aircraft application, annular diffusers often operate downstream of compressors. Such diffusers handle flows having substantial amount of swirl and unsteadiness made up of turbulence and periodic flow components introduced by the turbo machinery. The swirling component of velocity may arise either from the presence of inlet guide vanes or any other components preceding the diffuser, e.g., a compressor, or from rotation of the central shaft through the diffuser. The introduction of presence of swirl alters the flow field considerably and this affects the overall performance of a system.

Swirling flows through annular diffusers have been investigated by Sovran and Klomp [3], Shrinath [4] Hoadley [7], Colodipietro et al. [8], Shaalan et al. [9], Kumar [10], Lohmann et al. and Sapre et al. [10] Agrawal et al. [14], Singh et al. [16, 20], Kochevsky [18], Mohan et al. [19], Japikse, D [20], Kochevsky, A. N [21] and Yeung et. al [22]. These investigators found improved diffuser performance with swirl till a point after that it deteriorated. The performance of an annular diffuser apart from swirl is dependent on a large number of geometrical and dynamical parameters. The effectiveness of annular axial diffusers worsens with flow separation. The separation of the flow can be suppressed or shifted from one location to another with the help of swirl. The efforts have been made to design an annular diffuser for no flow separation [2,5,6], however little success has been achieved.

Literature on annular diffusers reveals that earlier studies have been carried out either with parallel hub diverging casing and both hub and casing diverging. The experimental/ analytical data on the pressure recovery coefficient or coefficient of energy losses [1, 12] for a wide range of geometrical parameters and swirl intensities are scant. Experimental studies on annular diffuser [17] require sophisticated instrumentation and complicated time-consuming procedures which is not economically viable and thus has limited the research activity in the field of annular diffusers [12].

The present study is therefore carried out to examine with the help of Computational Fluid Dynamics (CFD), the detailed flow behavior of axial annular diffusers with both hub and casing diverging at unequal angles for same equivalent cone angle of 10[degrees] and area ratio of 2 and 0.. For the present case angle of hub has been fixed at 5[degrees] and the casing angle was varied according to area ratio and fixed equivalent cone angle of 10[degrees]. Experimental velocity profiles were obtained with the axial annular diffuser having hub parallel and casing diverging and area ratio of the experimental diffuser was 2.01, and equivalent cone angle of 10.09[degrees]. CFD analysis of the diffuser with same configuration and dynamic parameters was carried out with different turbulence models. The model which predicted the results more closely with the experimental results was chosen for further investigations. RNG k-[epsilon] model agreed reasonably well with the experimental/available data. CFD Study has been carried out to predict the effect of experimentally obtained inlet velocity profiles without swirl (0[degrees]) and with inlet swirl angles of 7.5[degrees], 12[degrees], 17[degrees]and 25[degrees] on the performance of annular diffusers.

The Experimental Setup

Figure 1 shows the actual experimental setup used for the present investigation. The test rig consists of a single stage centrifugal blower which delivers 1.5[m.sup.3]/s at 1m water gauge pressure. It draws air from the atmosphere through a very fine mesh filter and delivers it to a settling chamber through a well-designed conical divergence. A symmetrical damper placed at the blower intake controlled and kept the flow rate constant through the system. A piece of heavy fabric serving as flexible coupling was used to seal the gap between the blower and settling chamber in order to prevent the vibrations reaching to settling chamber from the blower. The settling chamber is provided with fine mesh screens and a honey comb section. The purpose of the screens is multifold in serving as flow steadying and straightening, reducing the level of turbulence and losses. It is further connected to a constant-area annular duct made up of two commercial pipes; through a smooth converging section. Smooth transition from the annulus to the conical casing of the diffuser was ensured by inserting suitable metal shims between flanges and the inside was finished off with plasticine. Diffuser hub was made from cast aluminum and machined smooth whereas the casing of the annular test-diffusers was made of transparent Plexiglas. This was done to permit flow visualization inside the annulus so formed. The air flowing through the diffuser was finally exhausted into the atmosphere.

The measurements of static pressure and yaw angle were made manually with the help of Cobra probe, Traversing Mechanism and Manometers. Figure 2 shows Annular diffuser Geometrical Parameters of the half section as the diffuser has been taken as axially symmetrical

[FIGURE 1 OMITTED]

[FIGURE 2 OMITTED]

CFD Modeling

Annular diffuser geometry was sketched with proper meshing scheme with the help of GAMBIT software. In the pre-study k-[epsilon] turbulence models such as standard, RNG and realizable were tried on the geometries for which experimental data were available. The results obtained were validated with the available experimental results. The boundary conditions fed at the inlet is the same velocity profile as experimentally obtained with turbulence specification of 0% turbulence and hydraulic diameter as calculated from the geometry of the diffuser inlet. The outlet boundary condition is pressure normal to the pressure outlet with turbulence specification of 0% turbulence and hydraulic diameter as calculated from the geometry of the diffuser outlet. The solution controls for momentum, swirl velocity, turbulence kinetic energy and turbulence dissipation rate are second order up winding. The convergence criteria for residuals are [10.sup.-6] for various parameters involved in the present study such as continuity, velocity components [v.sub.x], [v.sub.r],and [v.sub.Z], swirl, k and [epsilon]; the results were found to be stable.

The modeling was repeated for various mesh sizes varying from 50000 to 500000 mesh cells to attain the grid independence. It was found that the model which approached more closely to the experimental results was 2D axisymmetric RNG "renormalization group" k-[epsilon] turbulence model with moderate mesh size of 0.07cm. The RNG-based k-[epsilon] turbulence model [15] is derived from the instantaneous Navier-Stokes equations, using a mathematical technique called "renormalization group" (RNG) methods. The same model has been used for carrying out the analysis for other geometries considered for the present study.

Governing Equations

The governing equations for 2D axisymmetric geometries are written as follows: Continuity equation is

[partial derivative][rho]/[partial derivative]t + [partial derivative]/[partial derivative]x ([rho][v.sub.x] + [partial derivative]/[partial derivative]r ([rho][v.sub.r]) + [rho][v.sub.r]/r = [S.sub.m] (1)

Where x is the axial coordinate, r is the radial coordinate, [v.sub.x] is the axial velocity, and [v.sub.r] is the radial velocity.

Conservation of momentum [1] in an inertial (non-accelerating) reference frame is described by

[MATHEMATICAL EXPRESSION NOT REPRODUCIBLE IN ASCII] (2)

Where p is the static pressure, [??] is the stress tensor (described below), and [rho][??] and [??] are the gravitational body force and external body forces (e.g., that arise from interaction with the dispersed phase), respectively.

The stress tensor [??] is given by

[MATHEMATICAL EXPRESSION NOT REPRODUCIBLE IN ASCII] (3)

Where [mu] is the molecular viscosity, I is the unit tensor, and the second term on the right hand side is the effect of volume dilation.

For 2 D axisymmetric geometries, the axial and radial momentum conservation equations are given by

[MATHEMATICAL EXPRESSION NOT REPRODUCIBLE IN ASCII] (4)

and

[MATHEMATICAL EXPRESSION NOT REPRODUCIBLE IN ASCII] (5)

where

[nabla] x [??] [partial derivative][v.sub.x] / [partial derivative]x + [partial derivative][v.sub.r] / [partial derivative]r + [v.sub.r] / r (6)

The tangential momentum equation for 2D swirling flows may be written as

[MATHEMATICAL EXPRESSION NOT REPRODUCIBLE IN ASCII] (7)

and [v.sub.z] is the swirl velocity

Pressure recovery Coefficient

The static pressure rise non-dimensionalised with respect to the diffuser inlet dynamic head is defined as the static pressure recovery.

[C.sub.p] = [(p - [p.sub.i])]/1/2 [rho][v.sup.2.sub.i] (8)

For one-dimensional flow of perfect gas without any energy loss, the ideal pressure rise for given diffuser can be computed by considering energy conservation. The result is the ideal performance.

[C.sub.pi] = 1 - 1/[AR.sup.2] (9)

Grid Independence Test

The results of any computational model are based upon the meshing created in the specified geometry. Meshing consists of nodes, cells or grid. The size of the grid plays an important role in determining the output of the physical model. Coarser the mesh size or smaller number of meshes means the results obtained may not be accurate, on the other hand finer meshing or large number of meshes no doubt will give the better results. However with finer mesh the computation time increases enormously. So grid size needs optimization in order to obtain the results in lesser computational time without sacrificing pre determined accuracy.

In the present investigation grid independence was carried out on number of geometries with different models. One such grid independence test is explained here. Annular diffuser whose both hub and casing were diverging with equal angles on which experiment was also performed is chosen. The inlet velocity profile for computational model was taken the same profile which was obtained experimentally. The turbulence model studied for the present test was RNG k-[epsilon] model. Four different grids sizes were employed to examine the sensitivity of grid. The various diffusers having different geometrical parameters will have different number of grids depending upon grid size and geometrical dimensions. In the present investigation the size of the grid has been taken as a parameter to maintain the symmetry between various annular diffusers. The grid size has been taken in terms of the size of the side of a quadrilateral cell. The mesh sizes were varied from 0.06 to 0.09 cm were employed to study the impact of grid size on the accuracy achieved in comparison to experimental results and the computational time spent to achieve the results.

[FIGURE 3 OMITTED]

Figure 3 shows with k-[epsilon] RNG model the results of mesh size of 0.06, 0.07, 0.08 and 0.09 cm. The results of mesh size 0.06 and 0.07 remain almost same, thus mesh size of 0.07 cm has been considered for the present CFD analysis to reduce the computational time without foregoing the accuracy.

The same turbulence model was used to predict the performance of axial annular diffusers with various geometries.

Results and discussion

Velocity Profile

Figure 4 and 5 show the longitudinal velocity profiles. These profiles are represented as non-dimensional longitudinal velocity u/Um as a function of diffuser passage height y/Ym for the area ratios 2 and 0 respectively. The velocity profiles are shown for various inlet swirl angles 0[degrees], 7.5[degrees], 12[degrees], 17[degrees]and 25[degrees]. All the velocity profiles have been shown in terms of non-dimensional velocity as the ratio of local longitudinal velocity to the local maximum velocity of the transverse, where velocity is required. The non-dimensional velocity has been shown as a function of non-dimensional diffuser passage height of the particular traverse (y/Ym). The hub position of the traverse is represented by y/Ym =0, whereas y/Ym =1 represents the casing position. The graphs are shown at various traverses of the diffuser passage at x/L= 0.1, 0.0, 0.5, 0.7 and 0.9 for all the area ratios and inlet swirl angles.

Figure 4 and 5, both illustrate that the flow is hub generated for no swirl condition and there is shift in the flow from hub towards casing when the swirl is introduced. The peak of the velocity at x/L =0.9 occurs at y/Ym at 0. 45 for area ratio 2, whereas for area ratio 0, it is at y/Ym =0.41. With the introduction of swirl, the flow is pushed towards the casing.

The separation or reversal of flow is not observed on the hub as well as on the casing wall even with the introduction of 25[degrees] inlet swirl in both the diffusers of area ratio 2 and 0. However the peak velocity shifts for flow without swirl as one move down the diffuser passage towards the hub with the increase in the area ratio. It is quite significant as viewed in the fig. 4 and 5. The peak velocity in both cases shifts towards the casing side as the inlet swirl increases. The velocity on the hub side decreases with the increasing swirl for same area ratio and it is almost negligible for 25[degrees] inlet swirl.

It is also evident from the graphs of non swirling flow (0[degrees]), that the location of maximum non dimensional velocity shifts towards the hub for downstream of the diffuser passage. The shift increases to larger extent with the increase in the area ratio for same inlet velocity profile. This is due to the fact that the stall increases at the casing wall with increase in the area ratio for same equivalent cone angle diffusers. The stall tends to shift from casing to the hub wall with the introduction of swirl as observed by examining the Figures 4 and 5. The shift is stronger with the increase in the inlet swirl.

[FIGURE 4 OMITTED]

[FIGURE 5 OMITTED]

Pressure Recovery Coefficient

Figure 6 indicates pressure recovery coefficient at casing wall ([C.sub.p]) for diffuser for area ratios 2 and 0 as a function of non-dimensional diffuser passage x/L for various inlet swirl angles 0[degrees], 7.5[degrees], 12[degrees], 17[degrees] and 25[degrees]. [C.sub.p] increases with the diffuser passage in each case. The marginal increase in Cp is sharp in the beginning of the diffuser passage and later on it decreases with the diffuser passage.

For area ratio 2 diffuser, Cp is higher for increasing swirl. For 17[degrees] and 25[degrees] inlet swirl Cp is lower than the flow without swirl beyond x/L = 0.99 and 0.55 respectively. Cp is highest up to diffuser passage length of 0.06 for 25[degrees] inlet swirl. From x/L=0.06 to 0.69 it is maximum for 17[degrees] inlet swirl, then from 0.69 till end it is for 12[degrees] inlet swirl.

For area ratio 0 diffuser Cp is lower than the flow without swirl beyond x/L =0.64 and 0.00 for 7.5[degrees] and 25[degrees] inlet swirl respectively. Up to 0.2 of diffuser passage length, Cp is highest for 25[degrees] inlet swirls, from 0.2 to 0.4, it is for 17[degrees] inlet swirl and beyond that it is for 12[degrees] inlet swirl.

[FIGURE 6 OMITTED]

Conclusions

Validated CFG RNG k-[epsilon] model was used to predict the performance of the axial annular diffuser. Following inferences have been drawn from the predicted computational results for area ratios 2 and 3 for various inlet swirl angles.

1. As the flow proceeds downstream, the longitudinal velocity decreases continuously irrespective of whether the inlet flow is swirling or non-swirling.

2. Velocity profiles have different shapes at different locations of the flow passage due to the development of boundary layer.

0. The maxima of velocity at any diffuser transverse is not at the centre, rather it is towards the hub for non swirling flow, which shifts towards the casing with the introduction of swirl.

4. With the introduction of swirl, the flow is pushed towards casing wall thus making the flow stronger towards casing than hub wall.

5. Pressure recovery coefficient increases with the diffuser passage. However the marginal recovery decreases with the diffuser passage.

6. With the introduction of swirl the recovery is faster towards the casing wall. The effect of swirl appears to gradually decay as the flow proceeds downstream and the recovery is negligible or nil towards the diffuser exit.

7. CFD analysis in the pre study is reasonably in good agreement with the experimental data. The RNG k-[epsilon] turbulence model used in the present work can be used to predict the flow behaviour in advance and the pressure recovery coefficient can be computed.

Nomenclature

A Diffuser annular area

AR Area ratio

[C.sub.p] Pressure recovery coefficient

F Force

I Unit tensor

L Diffuser length

P Static pressure

R Radius

Re Reynolds number

V Velocity in Y direction

x/L Non-dimensional axial length

y/Ym Non-dimensional radial length

[theta] wall divergence angle

[eta] Diffuser effectiveness

[rho] Density

[mu] Molecular viscosity

[alpha] Inlet Swirl angle

[??] Stress tensor

[zeta] Diffuser loss coefficient

Suffix

c casing

h hub

i inlet

o outlet

r radial

x axial

z tangential or swirl

References

[1] G. K. Batchelor, "An Introduction to Fluid Dynamics", Cambridge University

Press, Cambridge, England, 1967 [2] Howard, J.H.G., Thorriton-Trurnp A.B. and Henseler, H.J, "Performance and Flow Regimes for Annular Diffusers", ASME Paper No. 67-WA/FE-21, 1967.

[3] Sovran, G and Klomp, E.D., "Experimentally Determined Optimum Geometries for Rectilinear Diffusers with Rectangular, Conical or Annular Cross-Section", Fluid Mechanics of Internal Flow, Ed. G. Sovran, Elsevier Amsterdam, pp.270-019, 1967.

[4] Srinath.T, "An investigation of the effects of swirl on flow regimes and performances of annular diffuser with inner and outer cone angles." M.A.Sc. thesis, University of waterloo, Canada 1968.

[5] Stevens, S.J and Markland, E., "The Effect of Inlet Conditions on the Performance of Two Annular Diffusers", ASME Paper No.68-WA/FE-08.

[6] Stevens, S.J., "The Performance of Annular Diffusers". Proc. Instn. Mech. Engrs., Vol. 182, Part 0D, pp.58-70,1968.

[7] Hoadley, D., "Three-Dimensional Turbulent Boundary Layers in an Annular Diffuser", Ph.D. Thesis, Department of Engineering, University of Cainbridge, London, 1970.

[8] Coladipietro, R., Schneider, J.H and Shridhar, K., "Effects ofIfflet Flow Conditions on the Performance of Equi-Angular Annular Diffusers", CSME Paper No. 70-84,1974.

[9] Shaalan, M.R.A and Shabaka, I.M.M., "An Experimental Investigation of the Swirling Flow Performance of an Annular Diffuser at Low Speed", ASME PaperNo. 75-WA/FE-17,1975

[10] D.S. Kumar, "Effect of swirl on flow through annular diffusers", Ph.D. Thesis, I.I.T. Delhi, 1977.

[11] Lohmann, R.P., Markowski, SJ and Prookman, E.T., "Swirling Flow Through Annular Diffusers with Conical Walls", Journal of Fluids Engineering, Trans. ASME, Vol.101, pp.224-229,1979.

[12] Chithambaran, V.K., Aswatha, Narayana P.A., Chandrashekra Swamy, N.V. "Mean velocity characteristics of plane diffuser flows with inlet velocity distortion." Journal of Indian Institute of Science, 65(A):79-90, 1984.

[10] Sapre, R.N., Singh, S.N., Agrawal, D.P and Malhotra, R.C., "Flow Through Equiangular Wide Angle Annular Diffusers", 15th NCFMFP, Srinagar, July, 1987.

[14] Agrawal, D.P., Singh, S.N., Sapre, R.N and Malhotra, R.C., "Effect of Hub Rotation on the Mean Flow of Wide Angle Annular Diffusers", HydroTurbo 1989, Czechoslovakia, 1989.

[15] D. Choudhury," Introduction to the Renormalization Group Method and Turbulence Modeling." Fluent Inc. Technical Memorandum TM-107, 1990.

[16] S.N. Singh, D.P. Agarwal, R.N. Sapre and R.C. Malhotra, "Effect of inlet swirl on the performance of wide angled diffusers", Indian journal of Engineering & Materials Sciences, Vol.1.pp 60-69.1994.

[17] Buice, C. U., and Eaton, J. K., "Experimental Investigation of Flow Through an Asymmetric Plane Diffuser", Report No.TSD-107, Thermosciences Division, Department of Mechanical Engineering, Stanford University, Stanford, CA, USA, 1997.

[18] Klomp, E.D., "Performance of Straight-Walled Annular diffuser with Swirling Flow", The Aeronautical Journal, Vol. 101, No. 1010, pp. 467-480, 1997.

[19] Mohan, R., Singh, S.N., and Agrawal, D.P., "Optimum Inlet Swirl for Annular Diffuser Performance Using CFD", Indian Journal of Engineering and Materials Sciences, Vol. 5, pp. 15-21, 1998.

[20] Japikse, D., "Correlation of Annular Diffuser performance with Geometry, Swirl, and Blockage", Proceedings of the 11th Thermal and Fluids Analysis Workshop (TFAWS), Cleveland, Ohio, August 21-25, 2000, pp. 107-118.

[21] Kochevsky, A. N. "Numerical Investigation of Swirling Flow in Annular Diffusers With a Rotating Hub Installed at the Exit of Hydraulic Machines", Journal of Fluids Engineering, Trans. ASME, Vol. 120, pp.484-489, 2001.

[22] Yeung, W. W. H. and Parkinson, G. V., "Analysis and Modeling of Pressure Recovery for Separated Reattaching Flows," ASME Journal of Fluids Engineering, Vol. 126, No. 0, pp. 055-061, 2004.

[23] Singh, S. N., Seshadri, V., Saha, K., Vempati, K. K., and Bharani, S., "Effect of Inlet Swirl on the Performance of Annular Diffusers Having the Same Equivalent Cone Angle", Proceedings of the Institution of Mechanical Engineers, Part G, Journal of Aerospace Engineering, Vol. 220, pp. 129-140, 2006.

B.B. Arora * and B.D. Pathak

Department of Mechanical Engineering, Delhi Technological University, (Formerly Delhi College of Engineering), Delhi, India

* Corresponding Author E-mail: prof_bbar@yahoo.com