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 mesh consists 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	$1.610^{7}$	.72	.45	1862	100% $m_{d}$	k-e	mesh-1	design	-Blade pressure -Pitch averaged exit spanwise distributions	Pressure ratio, $\eta _{ad}$
CFD 2	$1.610^{7}$	.72	.45	1862	78.7% $m_{d}$	k-e	mesh-1	design	-Blade pressure -Pitch averaged exit spanwise distributions	Pressure ratio, $\eta _{ad}$
CFD 3	$1.610^{7}$	.72	.45	1862	100% $m_{d}$	k-e	mesh-2	design	-Blade pressure -Pitch averaged exit spanwise distributions	Pressure ratio, $\eta _{ad}$
CFD 4	$1.610^{7}$	.72	.45	1862	78.7% $m_{d}$	k-e	mesh-2	design	-Blade pressure -Pitch averaged exit spanwise distributions	Pressure ratio, $\eta _{ad}$
CFD 5	$1.610^{7}$	.72	.45	1862	133% $m_{d}$	k-e	mesh-2	design		Pressure ratio, $\eta _{ad}$
CFD 6	$1.610^{7}$	.72	.45	1862	100% $m_{d}$	b-I	mesh-1	design	-Blade pressure -Pitch averaged exit spanwise distributions	Pressure ratio, $\eta _{ad}$
CFD 7	$1.610^{7}$	.72	.45	1862	100% $m_{d}$	k-e	mesh-1	50% design	-Blade pressure -Pitch averaged exit spanwise distributions	Pressure ratio, $\eta _{ad}$
CFD 8	$1.610^{7}$	.72	.45	1862	100% $m_{d}$	k-e	mesh-3	design		Pressure ratio, $\eta _{ad}$

Table CFD-A Summary description of all test cases

	Blade pressure at six different spans (5%, 20%, 49%, 79%, 94%, 98%) (PS)	Blade pressure at six different spans (5%, 20%, 49%, 79%, 94%, 98%) (SS)	Exit spanwise distribution	DOAPs
CFD 1	cfd11.dat cfd12.dat cfd13.dat cfd14.dat cfd15.dat cfd16.dat	cfd17.dat cfd18.dat cfd19.dat cfd110.dat cfd111.dat cfd112.dat	cfd115.dat	cfd116.dat
CFD 2	cfd21.dat cfd22.dat cfd23.dat cfd24.dat cfd25.dat cfd26.dat	cfd27.dat cfd28.dat cfd29.dat cfd210.dat cfd211.dat cfd212.dat	cfd215.dat	cfd216.dat
CFD 3	cfd31.dat cfd33.dat cfd34.dat cfd35.dat cfd36.dat	cfd37.dat cfd38.dat cfd39.dat cfd310.dat cfd311.dat cfd312.dat	cfd315.dat	cfd316.dat
CFD 4	cfd41.dat cfd42.dat cfd43.dat cfd44.dat cfd45.dat cfd46.dat	cfd47.dat cfd48.dat cfd49.dat cfd410.dat cfd411.dat cfd412.dat	cfd415.dat	cfd416.dat
CFD 4	cfd41.dat cfd42.dat cfd43.dat cfd44.dat cfd45.dat cfd46.dat	cfd47.dat cfd48.dat cfd49.dat cfd410.dat cfd411.dat cfd412.dat	cfd415.dat	cfd416.dat
CFD 5				cfd51.dat
CFD 6	cfd61.dat cfd62.dat cfd63.dat cfd64.dat cfd65.dat cfd66.dat	cfd67.dat cfd68.dat cfd69.dat cfd610.dat cfd611.dat cfd612.dat	cfd615.dat	cfd616.dat
CFD 7	cfd72.dat cfd73.dat cfd74.dat cfd75.dat cfd76.dat	cfd77.dat cfd78.dat cfd79.dat cfd710.dat cfd711.dat cfd712.dat	cfd715.dat	cfd716.dat
CFD 8				cfd81.dat

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 ${\mbox{R}}_{y}=(k^{1/2}y/\nu )$ . 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.

$k_{\text{inlet}}=1.5{(T_{u}V_{z})}^{2}\qquad \qquad {\text{and}}$

$E_{\text{inlet}}=0.09k_{\text{inlet}}^{2}/\mu _{t}=0.09k_{\text{inlet}}^{2}/10\mu _{l}$

with the inlet turbulent intensity T_u 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 R_y = (k^1/2y/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

cfd11.dat to cfd16.dat

(ASCII file; headers: Blade pressure distribution on pressure side at xx span from hub;

columns: z, r, <p/p_std>)

cfd17.dat to cfd112.dat

(ASCII file; headers: Blade pressure distribution on suction side at xx span from hub;

columns: z, r, <p/p_std>)

cfd115.dat (ASCII file, headers: Outlet spanwise distributions :station 2

columns: z, <P/p_std>, <T/t_std>), <p/p_std>), <absolute flow angle(deg)>),

DOAPs:

cfd116.dat (ASCII file, headers: Pressure ratio and adiabatic efficiency

Pressure ratio, h_ad

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.

Contributors: Nouredine Hakimi - NUMECA International

Site Design and Implementation: Atkins and UniS