CFD Simulation AC6-05

From QNET
Jump to navigation Jump to search

Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice

Annular compressor cascade with tip clearance

Application Challenge 6-05 © copyright ERCOFTAC 2004


Overview of CFD Simulations

The flow in the NTUA annular compressor cascade has been simulated by means of the Reynolds-Averaged-Navier-Stokes equations. Differential and algebraic turbulence models were employed for closure. In the open literature, there exist two papers reporting on the computational predictions for the first set of experimental data. In the first one (Bonhommet and Gerolymos, 1998), results were obtained using the turbo_3D code, which was developed at UPMC/LEMFI, on fine grids of about 1.5 million points using the Launder-Sharma new-wall low-Reynolds-number k-ε turbulence model. In the second paper (Politis et al., 1998), the ELISA code, which has been developed at NTUA/LTT for the studying of tip-clearance effects in turbomachinery bladings, was employed for the solution of the flow field on a grid of 0.22 million points. The standard high-Reynolds-number k-ε turbulent model in conjunction with the wall functions technique was incorporated for closure. Both methods gave similar results. Satisfactory agreement is observed in the blade passage, whilst all computations failed to capture the mixing of the tip-clearance vortex with the main flow, downstream of the blades. As reported in open literature, this inability of the k-ε type turbulence models is a common feature of these models and is attributed to the fact that all such models are unable to account for departure from equilibrium conditions, which is closely related to non-isotropic behaviour

The same set of experimental data was used for a systematic investigation of the grid dependence and a validation of turbulence models in the frame of APPACET project. In this context, both methods mentioned above have been used for computations, incorporating even finer grids (up to 2.5 million points for the turbo_3d code and up to 0.34 millions for the ELISA code) and alternative turbulent models (as the standard low-Reynolds-number k-ε or the Craft-Launder-Sharma non-linear k-ε turbulent model for the turbo_3d code). In addition, the CANARI code was used for computations in grids comprising 1 up to 2 million points. This method has been developed at SNECMA and employed a mixing length turbulent model. Finally, EURANUS/Turbo code, which has been developed at VUB, with such turbulence models as the Baldwin-Lomax and the Yang-Shih linear k-ε, in grids consisting of up to 0.5 million points was used for computations. Two interesting features are common in all calculations performed using these four computational methods. All of them resulted in near grid independent solutions. On the other hand, all turbulence model variants tested, failed to reproduce the correct physical processes downstream of the blade, while they succeeded in matching the experimental patterns in the blade passage.

For the second test of data, computations have been carried out using the ELISA code. The findings from the comparisons between the experimental and the computational results from the corresponding test cases are coherent with the findings of the first set of data. In conformity to the experimental test cases the summary of the CFD simulation results is provided in Table CFD-A. The test case that corresponds to a tip-clearance size 2% and a rotating hub has been computed twice in order to perform a grid dependency study. In Table CFD-B, the available data files that correspond to the circumferential mass average span-wise distributions of the flow quantities are listed. As in the experimental distributions, mass averaging has been accomplished by a simple averaging technique, with the mass flow rate being the weighting factor.


CASE GNDP PDPs SPs
Re m (kg/s) t/C (%) N (rpm) Detailed data DOAPs
CFD1 1.1 13.2 2 6540 Circumferential mass average PLC.
CFD2 1.1 13.2 2 6540 Circumferential mass average PLC.
CFD3 1.1 13.2 2 0 Circumferential mass average PLC.
CFD4 1.1 13.2 4 6540 Circumferential mass average PLC.
CFD5 1.1 13.2 4 0 Circumferential mass average PLC.


Table CFD-A : Summary of all computed cases. All simulations included herein have been performed using one code, the ELISA. This code is briefly presented in the following section.

CASE SP1 SP2 SP3
Span (%), Ps (Pa), Pt (Pa), PLC at Station 2 Span (%), Ps (Pa), Pt (Pa), PLC at Station 8 Span (%), Ps (Pa), Pt (Pa), PLC at Station 9
CFD1 Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd11.dat Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd12.dat Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd13.dat
CFD2 Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd21.dat Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd22.dat Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd23.dat
CFD3 Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd31.dat Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd32.dat Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd33.dat
CFD4 Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd41.dat Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd42.dat Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd43.dat
CFD5 Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd51.dat Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd52.dat Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif Tick.gif cfd53.dat

Table CFD-B: Summary of all simulated parameters and available data files.


Solution strategy

Code ELISA is a pressure correction algorithm solving the RANS equations, capable of dealing with steady-state flow problems for a wide range of Mach numbers, from incompressible up to transonic flows. It implements structured grids, along with a cell-centred, finite-volume discretization scheme. Modelling of the exact tip-clearance shape is accomplished by means of the decomposition of the flow domain into two patched sub-domains that are filled with H-type grids (see Figure 8). These sub-domains are treated sequentially and their coupling is achieved by exchanging flow quantities over the blade-to-blade surface at the blade tip. This mesh surface is differently meshed in each sub-domain allowing for both a structured grid to be generated in the tip-clearance gap and an efficient communication strategy to be set up between the two sub-domains (see Figure9). In the past, the code ELISA has been successfully applied to flow-prediction in turbomachinery blades (Politis et al. 1997b and 1998a) and stages, in which the rotor-stator interaction phenomena do not dominate the flow (Politis et al. 1997a and 1998b). Turbulence is approximated by the numerical solution of the high-Reynolds-number k-ε model equations (Jones and Launder, 1972). The wall function technique is used to bridge the gap between solid boundaries and the first grid nodes off the walls, in a manner applicable to both stationary and rotating walls.


Image508.gif

Figure 8: Multi-domain decomposition of the flow field in the NTUA annular compressor cascade.

Image509.gif Image510.gif

Figure 9: Left: Two-dimensional layout of the computational grids. Right: Detail near the leading edge region (red line: tip-grid, green line: main grid).

Within each block grid, all governing equations are solved in a segregated manner, by means of the approximate factorisation of a coefficient matrix into lower and triangular matrices. Central differences for the diffusion and a quadratic upwind interpolation scheme (QUICK, Leonard, 1979) for the convective terms of the momentum equations are used. For stability reasons the latter terms in the k-ε equations are simulated by a first-order upwind scheme. In order to diminish the computational requirements, a common coefficient matrix is assembled for all convection-diffusion type equations.

The continuity constraint is enforced by means of a pressure correction equation. The pressure correction field is appropriately linked to components of either the Cartesian velocity or the momentum fluxes in incompressible and compressible flow problems, respectively. Imposing residual minimization constraints, the numerical solution of the pressure correction equation is enhanced. The algorithm incorporates a density retardation scheme, decomposing the momentum fluxes into their constituent quantities during the correction step. A retarded density is employed to reinstall the hyperbolic nature of the governing equations in transonic regions, whereas in subsonic regions it coincides with density. A detailed presentation of the solution method is available in Politis (1998) and in Politis and Giannakoglou (1997).


Computational Domain and Boundary Conditions

By means of the multi-domain modelling of the tip-clearance that is described in the previous section, an accurate simulation of the actual flow domain is accomplished. The extent of the rotating part of the hub was also accurately modelled during the generation of the computational grids. Their dimensions in the pitch-wise, the span-wise and the stream-wise directions are listed in Table CFD-C. In all these cases, the number of nodes used was about 320.000, the exact figure depending on the tip-clearance size. Only one span-wise distribution of nodes was generated and used in both tip-clearance configurations. As a result, the total number of nodes in the span-wise direction is the same (75) for both tip-clearance test cases, the only difference being that a small number of nodes (8) that belongs to the main grid in CFD-1 and CFD-3 is transferred to the tip-grid in CFD-4 and CFD-5. Both the span-wise distribution of nodes, as well as the pitch-wise distribution were appropriately stretched, so as the first layers of grid nodes off the walls to fall in the range of applicability of the wall functions. A blade-to-blade layout of the generated grids is illustrated in Figure 9. For a grid dependency study to be performed, a second grid (CFD-2) was generated and simulated test case EXP-1.


CASE PDPs Grid Dimensions
t/C (%) N (rpm) Main Passage Tip Grid Nodes
CFD-1 2 6540 45*65*95 51*11*95 331.170
CFD-2 2 6540 45*45*85 51*11*85 219.810
CFD-3 2 0 45*65*95 51*11*95 331.170
CFD-4 4 6540 45*57*95 51*19*95 335.730
CFD-5 4 0 45*57*95 51*19*95 335.730


Table CFD-C: Number of grid nodes in the pitch-wise, the span-wise and the stream-wise direction. It is very important to stress that the inlet to the computational domain was placed at 90%Cax upstream of the blade’s leading edge, in order to impose circumferentially uniform boundary distributions of the flow quantities at the inlet. These are the, available from measurements at Station 2, span-wise distributions of the circumferential mass average total pressure and flow angles in the peripheral and the span-wise direction. The impact of imposing measured quantities at a different from the measuring station will be addressed at the section entitled “Evaluation–Comparison of Test data and CFD”. Uniform total temperature over the whole flow field was also imposed. At the exit, located at 138%Cax downstream of the blade’s trailing edge, the measured distributions of the static pressure at Station 9 have been imposed, appropriately modified in each case so that the computations would match the nominal mass flow-rate (m=13.2kg/sec). As far as turbulence quantities at the inlet are concerned and since there exist no measurements of turbulence quantities, values of 1.5% and 20 for the turbulent intensity and the ratio of turbulent to molecular viscosity, respectively, have been imposed. No parametric study of the impact of the values of the inlet turbulent quantities to the results has been carried out for the sake of computational time. Previous computations using different computational methods with alternative turbulence models and boundary conditions for the turbulent quantities have resulted in very similar results. So, it was presumed that using realist estimates of the inlet turbulence quantities their impact on the DOAPs would be low. The remaining boundaries are either periodic or walls. Walls, rotating or stationary, are assumed smooth and adiabatic and modelled using the wall functions technique.


Application of physical models

Modelling of turbulence is accomplished by coupling the RANS equations with the standard high-Reynolds-number k-ε model (Jones and Launder, 1972). Near wall closure is carried out by means of the wall function technique, which is used to model the shear stresses on a smooth wall assuming local equilibrium conditions, as



where t and n denote the parallel and the normal to the wall directions, respectively. The velocity, u, is the relative to the wall system of reference. Parameter Λ is defined as




In the above equation, the subscript p denotes values calculated at the first node p off the wall, lying at distance y from it. The non-dimensional distance from the wall is calculated as


In this manner, wall modelling can be readily applied to both stationary and rotating walls with being the relative to the wall velocity in both cases. It is written in a vector form to denote that the shear force acting on the finite-volume surfaces, which are in contact with a solid wall, is aligned with the local tangential velocity.

For the turbulent quantities, the value of turbulent kinetic energy dissipation, ε, is imposed at the first control volume, as



while the generation term in the k-equation is modified as



and k is zeroed at wall.

The range of the computed y+ values at the first grid nodes off the walls for the different wall surfaces is summarized in Table CFD-D. From the values listed in the table it is concluded that the generated meshes were appropriate enough to allow for an accurate application of the wall functions technique.


CASE PDPs Range (min value' max value)
t/C (%) N (rpm) Blade surfaces Hub Shroud
CFD-1 2 6540 2.0'76.0 9.0'49.0 10.0'60.0
CFD-2 2 6540 24.0'116.0 12.0'50.0 9.0'60.0
CFD-3 2 0 19.0'77.0 14.0'49.0 9.0'57.0
CFD-4 4 6540 22.0'79.0 14.0'50.0 9.0'78.0
CFD-5 4 0 20.0'77.0 14.0'50.0 12.0'51.0

Table CFD-D: Range of y+ at the first grid points off the walls.

Numerical Accuracy

For the mean flow equations, the discretization schemes used are of third-order accuracy for the convective terms and second-order accuracy for the diffusive terms, allowing for an overall second-order formal accuracy for the complete algorithm. For the sake of stability the turbulence equations are numerically solved with an overall first-order accurate scheme.

Convergence was measured by means of the maximum over the control volumes residual for every equation solved. Convergence was attained when the residuals of all equations solved were minimised by at least two orders of magnitude from their initial value. Additionally, the maximum allowed difference of the mass flow rate crossing each computational plane that is perpendicular in the stream-wise direction from its inlet plane value was of the order of ±0.2%. Coherency between experiments and calculations is accomplished by means of equal mass flow, which is achieved by modifying the imposed distributions of the static pressure at the cascade exit (Station 9) during the computational procedure.

In order to account for the grid sensitivity to the solution, two grids have been generated and used for calculations in test case EXP-1. They correspond to the simulation cases CFD-1 and CFD-2. The fine grid (CFD-1) of about 320.000 nodes had approximately 50% more nodes than the coarse one (CFD-2). The span-wise distributions of the circumferential mass average flow quantities at Stations 2, 8 and 9 (see Figure 10, Figure 11 and Figure 12, respectively) are very similar for both grids. This similarity suggests that near grid independent results are attainable when wall functions are employed for closure in the end-walls, provided that the grid size exceeds a ‘reasonable’ lower limit.


Image511.gif Image512.gif Image513.gif


Image514.gif Image515.gif Image516.gif

Figure 10: Span-wise distributions of the circumferential mass average flow quantities at Station 2 for EXP-1. Red lines: CFD-1, green lines: CFD-2.

Image517.gif Image518.gif Image519.gif


Image520.gif Image521.gif Image522.gif


Image523.gif

Figure 11: Span-wise distributions of the circumferential mass average flow quantities at Station 8 for EXP-1. Red lines: CFD-1, green lines: CFD-2.

Image524.gif Image525.gif Image526.gif


Image527.gif Image528.gif Image529.gif


Image530.gif

Figure 12: Span-wise distributions of the circumferential mass average flow quantities at Station 9 for EXP-1. Red lines: CFD-1, green lines: CFD-2.

References

+ Bonhommet–Chabanel, C., and Gerolymos, G. A., (1998), “Analysis of Tip Leakage Effects in a High Subsonic Annular Compressor Cascade,” ASME Paper 98-GT-195, Presented at the International Gas Turbine & Aeroengine Congress & Exhibition, Stockholm, Sweden, June 2-5, 1998.

+ Gregory–Smith, D. G. and Crossland, S. C., (2000), “Synthesis Report on the NTUA Annular Compressor (TC1),” Final Technical Report on APPACET project, July 2000.

+ Jones, W. P. and Launder, B. E., (1972), “The Prediction of Laminarization with a Two-Equation Model of Turbulence,” International Journal of Heat and Mass Transfer, Vol. 15, pp. 301-314

+ Leonard, B. P., (1979), “A Stable and Accurate Convective Modelling Procedure Based on Quadratic Upstream Interpolation,” Computer Methods in Applied Mechanics and Engineering, Vol 19, pp. 59-98.

+ Politis, E. S., (1998), “Development of a Navier-Stokes Solution Method for Flow Analysis in Turbomachinery Bladings With or Without Tip-Clearance,” Ph.D. Thesis, National Technical University of Athens (in Greek).

+ Politis, E. S. and Giannakoglou, K. C., (1997), “A Pressure-Based Algorithm for High-Speed Turbomachinery Flows,” International Journal for Numerical Methods in Fluids, Vol. 25, pp. 63-80.

+ Politis, E. S., Giannakoglou, K. C. and Papailiou, K. D., (1997a), “Axial Compressor Stage Analysis through a Multi-Block Navier-Stokes Solution Method,” ASME Paper 97-GT-093, Presented at the International Gas Turbine & Aeroengine Congress & Exhibition, Orlando, USA, June 2-5, 1997.

+ Politis, E. S., Giannakoglou, K. C. and Papailiou, K. D., (1997b), “Implicit Method for Incompressible Flow Calculations in Three-Dimensional Ducts and Cascades,” AIAA Journal, Vol. 35, No. 10, pp. 1581-1588.

+ Politis, E. S., Giannakoglou, K. C., and Papailiou, K. D., (1998a), “High-Speed Flow in an Annular Cascade with Tip Clearance: Numerical Investigation,” ASME Paper 98-GT-247, Presented at the International Gas Turbine & Aeroengine Congress & Exhibition, Stockholm, Sweden, June 2-5, 1998.

+ Politis, E. S., Giannakoglou, K. C. and Papailiou, K. D., (1998b), “Leakage Effects in the Rotor Tip-Clearance Region of a Multistage Axial Compressor, Part 2: Numerical Modelling,” ASME Paper 98-GT-592, Presented at the International Gas Turbine & Aeroengine Congress & Exhibition, Stockholm, Sweden, June 2-5, 1998.


Simulation Case CFD-1

CFD Results

RANS simulation of the flow in the annular cascade for a tip-clearance size t/C=2%, a hub rotational speed N=6540rpm and a mass flow rate m=13.2kg/s. High-Reynolds-number k-ε turbulence model with wall functions. Cartesian coordinate system. Cell-centred storage of variables. Post processing (interpolation to find the flow quantities at a given location and averaging using the mass flow rate as weighting factor) of the numerical values results in the circumferential mass average distributions of flow quantities (axial component of velocity, Vaxial, peripheral component of velocity, Vper, radial component of velocity, Vrad, flow angle, a, Mach number, M, total pressure, Pt, and static pressure, Ps) at three stations. PLC distributions are derived using Equation (1). Velocity components are non-dimensional with respect to the peripheral velocity at hub.

cfd11.dat (ASCII file; headers: Station 2, t/C=2%, N=6540rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

cfd12.dat (ASCII file; headers: Station 8, t/C=2%, N=6540rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

cfd13.dat (ASCII file; headers: Station 9, t/C=2%, N=6540rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

Simulation Case CFD-2

CFD Results

RANS simulation of the flow in the annular cascade for a tip-clearance size t/C=2%, a hub rotational speed N=6540rpm and a mass flow rate m=13.2kg/s. High-Reynolds-number k-ε turbulence model with wall functions. Cartesian coordinate system. Cell-centred storage of variables. Post processing (interpolation to find the flow quantities at a given location and averaging using the mass flow rate as weighting factor) of the numerical values results in the circumferential mass average distributions of flow quantities (axial component of velocity, Vaxial, peripheral component of velocity, Vper, radial component of velocity, Vrad, flow angle, a, Mach number, M, total pressure, Pt, and static pressure, Ps) at three stations. PLC distributions are derived using Equation (1). Velocity components are non-dimensional with respect to the peripheral velocity at hub.

cfd21.dat (ASCII file; headers: Station 2, t/C=2%, N=6540rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

cfd22.dat (ASCII file; headers: Station 8, t/C=2%, N=6540rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

cfd23.dat (ASCII file; headers: Station 9, t/C=2%, N=6540rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

Simulation Case CFD-3

CFD Results

RANS simulation of the flow in the annular cascade for a tip-clearance size t/C=2%, a still hub (N=0rpm) and a mass flow rate m=13.2kg/s. High-Reynolds-number k-ε turbulence model with wall functions. Cartesian coordinate system. Cell-centred storage of variables. Post processing (interpolation to find the flow quantities at a given location and averaging using the mass flow rate as weighting factor) of the numerical values results in the circumferential mass average distributions of flow quantities (axial component of velocity, Vaxial, peripheral component of velocity, Vper, radial component of velocity, Vrad, flow angle, a, Mach number, M, total pressure, Pt, and static pressure, Ps) at three stations. PLC distributions are derived using Equation (1). Velocity components are non-dimensional with respect to the peripheral velocity at hub.

cfd31.dat (ASCII file; headers: Station 2, t/C=2%, N=0rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

cfd32.dat (ASCII file; headers: Station 8, t/C=2%, N=0rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

cfd33.dat (ASCII file; headers: Station 9, t/C=2%, N=0rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

Simulation Case CFD-4

CFD Results

RANS simulation of the flow in the annular cascade for a tip-clearance size t/C=4%, a hub rotational speed N=6540rpm and a mass flow rate m=13.2kg/s. High-Reynolds-number k-ε turbulence model with wall functions. Cartesian coordinate system. Cell-centred storage of variables. Post processing (interpolation to find the flow quantities at a given location and averaging using the mass flow rate as weighting factor) of the numerical values results in the circumferential mass average distributions of flow quantities (axial component of velocity, Vaxial, peripheral component of velocity, Vper, radial component of velocity, Vrad, flow angle, a, Mach number, M, total pressure, Pt, and static pressure, Ps) at three stations. PLC distributions are derived using Equation (1). Velocity components are non-dimensional with respect to the peripheral velocity at hub.

cfd41.dat (ASCII file; headers: Station 2, t/C=4%, N=6540rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

cfd42.dat (ASCII file; headers: Station 8, t/C=4%, N=6540rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

cfd43.dat (ASCII file; headers: Station 9, t/C=4%, N=6540rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

Simulation Case CFD-5

CFD Results

RANS simulation of the flow in the annular cascade for a tip-clearance size t/C=4%, a still hub (N=0rpm) and a mass flow rate m=13.2kg/s. High-Reynolds-number k-ε turbulence model with wall functions. Cartesian coordinate system. Cell-centred storage of variables. Post processing (interpolation to find the flow quantities at a given location and averaging using the mass flow rate as weighting factor) of the numerical values results in the circumferential mass average distributions of flow quantities (axial component of velocity, Vaxial, peripheral component of velocity, Vper, radial component of velocity, Vrad, flow angle, a, Mach number, M, total pressure, Pt, and static pressure, Ps) at three stations. PLC distributions are derived using Equation (1). Velocity components are non-dimensional with respect to the peripheral velocity at hub.

cfd51.dat (ASCII file; headers: Station 2, t/C=4%, N=0rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

cfd52.dat (ASCII file; headers: Station 8, t/C=4%, N=0rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)

cfd53.dat (ASCII file; headers: Station 9, t/C=4%, N=0rpm, m=13.2Kg/s, columns: span, Ps, Pt, Vaxial/Vref, Vper/Vref, Vrad/Vref, a, M, PLC)



© copyright ERCOFTAC 2004


Contributors: Dr. E.S. Politis; Prof. K.D. Papailiou - NTUA

Site Design and Implementation: Atkins and UniS


Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice