CFD Simulations AC6-02
Low-speed centrifugal compressor
Application Challenge 6-02 © copyright ERCOFTAC 2004
Overview of CFD Simulations
The CFD simulations were carried out in the Dept. of Fluid Mech. VUB (Vrije Universiteit Brussel). The CFD code used is Fine/Turbo with EURANUS/Turbo version 4.3.
Three test conditions (Low Flow (or Off-design), Design Flow, and High Flow) were modeled at which overall performance parameters are compared with experimental data. Comparisons with experimental data, including blade surface static pressure, and pitch-averaged static and total pressure, total temperature and absolute flow angle at station 2 are given only for low and design flow rates.
A grid with three blocks, obtained with the auto-grid generation software IGG/AutoGrid of NUMECA, is used in this study. The first block covers the flow passage, extended from 40% meridional shroud length upstream of the impeller, to 15% impeller tip radius downstream in the radial direction. The second block represents the region behind the blunt trailing edge. The third block occupies the space in the tip gap. A blunt blade tip is meshed, even though the real tested blade tips are rounded as reported by Chriss et al. (1996). The meshconsists of 61x73x129, 13x73x33 and 13x13x65 points, in the tangential, radial and streamwise directions, for blocks 1, 2 and 3 respectively. Hence there are 13 lines over the gap height and 13 lines across the blade profile. The total grid number is 616,739.
| NAME | GNDPs | PDPs (problem definition parameters) | SPs (measured parameters) | |||||||
|---|---|---|---|---|---|---|---|---|---|---|
| Re | Pr | M | Rotation speed (rpm) | Relative flow rate | Turb. Mod | Mesh Type | Gap size | Detailed data | DOAPs | |
| CFD 1 | .72 | .45 | 1862 | k-e | mesh-1 | design | -Blade pressure -Pitch averaged exit spanwise distributions | Pressure ratio, | ||
| CFD 2 | .72 | .45 | 1862 | k-e | mesh-1 | design | -Blade pressure -Pitch averaged exit spanwise distributions | Pressure ratio, | ||
| CFD 3 | .72 | .45 | 1862 | k-e | mesh-2 | design | -Blade pressure -Pitch averaged exit spanwise distributions | Pressure ratio, | ||
| CFD 4 | .72 | .45 | 1862 | k-e | mesh-2 | design | -Blade pressure -Pitch averaged exit spanwise distributions | Pressure ratio, | ||
| CFD 5 | .72 | .45 | 1862 | k-e | mesh-2 | design | Pressure ratio, | |||
| CFD 6 | .72 | .45 | 1862 | b-I | mesh-1 | design | -Blade pressure -Pitch averaged exit spanwise distributions | Pressure ratio, | ||
| CFD 7 | .72 | .45 | 1862 | k-e | mesh-1 | 50% design | -Blade pressure -Pitch averaged exit spanwise distributions | Pressure ratio, | ||
| CFD 8 | .72 | .45 | 1862 | k-e | mesh-3 | design | Pressure ratio, | |||
Table CFD-A Summary description of all test cases
<span id="table CFD-B"
Table CFD-B Summary description of all available datafiles, and simulated parameters.
Simulation cases CFD1 to CFD8
Solution strategy
The CFD simulations were carried out in the Dept. of Fluid Mech. VUB. The CFD code used is Fine/Turbo with EURANUS/Turbo version 4.3. Default values in EURANUS/Turbo were used. The Navier-Stokes code EURANUS/TURBO, already presented in Hirsch et al. (1992), solves the time-dependent Reynolds averaged Navier-Stokes equations, with either the algebraic turbulence model of Baldwin-Lomax or a two-equation k-ε model for closure. It is based on a structured multiblock, multigrid approach, including non-matching block boundaries and incorporates various numerical schemes, based on either a central or an upwind discretization. For all CFD simulations except CFD6, the linear k-ε model of Yang and Shih (1993), modified by Khodak and Hirsch (1996), is selected,in which the damped function used in the eddy viscosity is chosen to be a function of Ry = (k1/2y/n). For the CFD6 calculation, the algebraic turbulence model of Baldwin-Lomax is used. These calculations were performed with a second-order centered scheme, with second and fourth order artificial dissipation terms and a W-cycle multigrid technique. The numerical procedure applied a four-stage Runge-Kutta scheme, coupled to local time stepping and implicit residual smoothing for convergence acceleration. The computations are performed at a CFL number of 2.5.
Computational Domain
A grid with three blocks, obtained with the auto-grid generation software IGG/AutoGrid of NUMECA, is used in this study. The first block covers the flow passage, extended from 40% meridional shroud length upstream of the impeller, to 15% impeller tip radius downstream in the radial direction. The second block represents the region behind the blunt trailing edge. The third block occupies the space in the tip gap. A blunt blade tip is meshed, even though the real tested blade tips are rounded as reported by Chriss et al. (1996).
Mesh-1 consists of49x61x129, 13x61x33 and 13x13x65 points, in the tangential, radial and streamwise directions, for blocks 1, 2 and 3 respectively, resulting in 422,735 points in total. Hence there are 13 lines over the gap height and 13 lines across the blade profile. The second mesh, named Mesh-2 hereafter, has 61 points, instead of 49 in Mesh-1, over a pitch in Block 1and 73 points, instead of 61 in Mesh-1, from hub to shroud in Blocks 1 and 2.The total grid number is 616,739. The grid location near the blade surfaces produces Y-plus for the first cell center being about 1 for both Mesh 1 and 2. Mesh-3 is the one level coarse mesh of Mesh 2, with total grid number of about 77,000. The grid is shown in Figure 6 and figure 7.
Figure 6: Geometry and grid for the LSCC impeller
Figure 7: Geometry and grid for the LSCC impeller
Boundary Conditions
At the inlet plane, measured profiles of absolute flow angles, total pressure and uniform total temperature are imposed. At the radial outlet section, mass flow is imposed. As in the experiments, the hub wall of the impeller is moving with the rotor blade, while the diffuser hub is stationary. The whole shroud is stationary. All the solid wall boundaries are assumed to be adiabatic. Periodic conditions are enforced along the boundaries upstream and downstream of the passage, and also in the tip gap. In the computation with k-ε model, the inlet k and e were estimated in the following way.
Failed to parse (syntax error): {\displaystyle \[k_{inlet} = 1.5{(T_u V_z)}^2\]}
and
Failed to parse (syntax error): {\displaystyle \[E_{inlet} = 0.09k^2_{inlet}/\mu_{t} = 0.09k^2_{inlet}/10\mu_\imath\]}
with the inlet turbulent intensity Tu being 1%.
Application of Physical Models
In the CFD6 calculation, the algebraic turbulence model of Baldwin-Lomax is used whereas for all other calculations the two-equation low Reynolds k-ε model of Yang and Shih (1993), modified by Khodak and Hirsch (1996) is applied.In k-ε model, the damped function used in the eddy viscosity is chosen to be a function of Ry = (k1/2y/n). The grid location near the blade surfaces produces Y-plus for the first cell center being about 1 for both Mesh 1 and 2.
Numerical Accuracy
The computations are performed at a CFL number of 2.5 and are converged to near machine accuracy, that is 4 to 5 orders of residual reduction and constancy of mass flow. The error in mass flow between inlet and outlet of the computational domain is less than 0.1%.
CFD Results
File format for CFD1 results
(ASCII file; headers: Blade pressure distribution on pressure side at xx span from hub;
columns: z, r,
) cfd17.dat to cfd112.dat (ASCII file; headers: Blade pressure distribution on suction side at xx span from hub; columns: z, r,
) cfd115.dat (ASCII file, headers: Outlet spanwise distributions :station 2 columns: z,
, <T/tstd>),
), <absolute flow angle(deg) >,) DOAPs: cfd116.dat (ASCII file, headers: Pressure ratio and adiabatic efficiency Pressure ratio, had The file format for all other CFD calculations is the same as described above and the data file names are detailed in table CFD-B
References
Dean R.C., Senoo Y., 1960, “Rotating Wakes in Vaneless Diffusers”, Trans. ASME, Journal of Basic Engineering, Vol.82, pp. 563-574.
Dean R., 1971, “On the Unresolved Fluid Dynamics of the Centrifugal Compressor”, in Advanced Centrifugal Compressors, ASME Publications.
Moore, J., 1973, “A Wake and an Eddy in a Rotating Radial-Flow Passage,” J. of Eng. Power, Vol. 95, pp. 205-219.
Eckardt, D., 1976, “Detailed Flow Investigations Within a High-Speed Centrifugal Compressor Impeller”, J. of Fluids Engineering, Vol.98, pp. 390-402.
Johnson, M. W., and Moore, J., 1983a, “Secondary Flow Mixing Losses in a Centrifugal Impeller,” J. of Engineering Power, Vol. 105, No.1, pp.24-32.
Eckardt, D., 1979, “Flow Field Analysis of Radial and Bachswept Centrifugal Compressor Impellers, Part 1: Flow Measurements Using Laser Velocimeter”, Performance Prediction of Centrifugal Pumps and Compressors, Gopalakrishnan, ed. ASME publication, pp. 77-86.
Johnson, M. W., and Moore, J., 1983b, “Influence of Flow Rate on the Wake in a Centrifugal Impeller,” J. of Engineering Power, Vol. 105, No.1, pp.33-39.
Chriss, R. M., Hathaway, M. D., and Wood, J. R., 1996, “Experimental and Computational Results from the NASA Lewis Low-Speed Centrifugal Impeller at Design and Part-Flow Conditions”, J. of Turbomachinery, Vol. 118, pp.55-65.
Hirsch, Ch., Kang, S., and Pointet, G., 1996a, “A Numerically Supported Investigation on the 3D Flow in Centrifugal Impellers, Part I The Validation Base”, ASME paper 96-GT-151.
Hirsch, Ch., Kang, S., and Pointet, G., 1996b, “A Numerically Supported Investigation on the 3D Flow in Centrifugal Impellers, Part II Secondary Flow Structure”, ASME paper 96-GT-152.
Kang, S., and Hirsch, Ch., 1996, “Influence of Tip Leakage Flow in Centrifugal Compressors”, 3rd ISAIF, Sept., 1996, Beijing.
S. Kang, Ch. Hirsch, 1999, “Effect of flow rate on the development of three-dimensional flow in NASA LSCC impeller, based on numerical solutions”, ISABE Paper No. 99-7225.
S. Kang, Ch. Hirsch, 1999, “Numerical investigation of the three-dimensional flow in NASA low-speed centrifugal compressor impeller”. 4th International Symposium on Aerothermodynamics of internal flows. Sept. 1999, Dresden.
Kang, S., and Hirsch C., 2001, “Numerical Simulation and Theoretical Analysis of the 3D Viscous Flow in Centrifugal Impellers”, Invited lecture, to be presented in the 5th ISAIF, Sept. 2001, Gdansk, Poland, and Journal TASK Quarterly 5, No.4, pp.455-479.
Hathaway, M. D., Chriss R. M., Wood, J. R., and Strazisar, A. J., 1993, “Experimental and Computational Investigation of NASA Low-Speed Centrifugal Compressor Flow Field”, J. of Turbomachinery, Vol. 115, pp.527.
Hirsch, Ch., Lacor, C., Dener, C., and Vucinic, D., 1992, “An Integrated CFD System for 3D Turbomachinery Applications”, AGARD-CP-510.
Yang, Z., and Shih, T. H., 1993, “;New Time Scale Based on k-ε Model for Near-Wall Turbulence”, AIAA J., Vol. 31, No.7, pp.1191-1198.
Khodak, A., and Hirsch, Ch., 1996, “Seconda Order Non-Linear k-ε Models with Explicit Effect of Curvature and Rotation”, Computational Fluid Dynamics'96, Proceeding of the Third ECCOMAS Computational Fluid Dynamics Conference, 690-696.
© copyright ERCOFTAC 2004
Contributors: Nouredine Hakimi - NUMECA International
Site Design and Implementation: Atkins and UniS
Top Next