Numerical propusion test for a tug boat using a RANS solver

Transcription

1 Numerical propusion test for a tug boat using a RANS solver R. Broglia, A. Di Mascio, D. Calcagni & F. Salvatore INSEAN, Italian Ship Model Basin, Rome, Italy ABSTRACT: This paper deals with the analysis of the flow field around a tug boat advancing in calm water. The main goal of the ongoing project, of which this work is part, is the characterization of the hull wake and in particular of the inflow to the propeller; to this aim, two operting conditions, at low and high Froude number, at both model and full scale Reynolds number are simulated for the propelled and unpropelled tug boat. The analysis is carried out by using numerical simulations based on the RANS equations; free surface is handled by means of a one phase level set approach, propeller effects are taken into account by a non iterative body force model. Some preliminary results in terms of velocity flow field and wave pattern are presented. 1 INTRODUCTION The periodic update of aged fleet vessels represents a practical demand for shipowners continuously facing economic competition and new regulations imposed by international maritime organizations. Typically, existing vessel performance is improved by means of local hull stern modifications and/or installation of new propulsors. Classical requirements are that modifications should be achieved at reduced costs, with short dry-docking times and, expecially, with clear indication of the expected performance benefits. Modern Computational Fluid Dynamics (CFD) represents an appealing tool to help designers matching the above requirements. Scope of the present paper is to describe the application of a state-of-the-art RANS model to the design of improved performance propellers for an aged fleet of tug boats. Specifically, the hull flow of the aged vessel is studied to determine the exact working conditions of the propeller and hence to provide necessary information for the new propeller design. The characterization of the hull wake and in particular of the inflow to the propeller represents the main goal of the computational analysis here described. The hydrodynamic interaction between propeller and hull is studied by means of a body-force approach. This methodology is based on the assumption that reliable predictions of the wakefield behind a propelled ship can be achieved combining a viscous flow solver to study the unpropelled flow with a propeller-flow model based on inviscid-flow assumptions. By this approach, the numerical solution of the RANS equations around a complete hull propeller configuration is made unnecessary and hence many computational issues are prevented. The capability of a coupled RANS/actuator-disc model to predict basic hull-propeller interaction parameters is demonstrated by a vast scientific literature where applications of this combined methodology to simulate propulsion tests is reported, as given by e.g., Zhang et al. (1992), Larsson (1993),

2 Chen and Lee (2003), and in particular Zhou (1994), where ducted propeller and ducted stator/rotor configurations are addressed. Propeller performance predictions for the evaluations of body-force terms are achieved here using a non iterative model based on the assumption that the thrust coefficient, the torque coefficient, the advancement ratio and the radial distribution of the circulation are known (Hough and Ordway (1965)). 2. SHIP FLOW MODELLING BY RANS The mathematical model employed in the simulations is described by the Reynolds Averaged Navier Stokes (RANS) equations, the turbulent viscosity being calculated by means of the one-equation model developed by Spalart and Allmaras (1994). The problem is closed by enforcing appropriate conditions at the physical and the computational boundaries. On solid walls, velocity is set to zero (whereas no condition on the pressure is required); at the inflow boundary, velocity is set to the undisturbed flow value, and the pressure is extrapolated from inside; on the contrary, the pressure is set to zero at the outflow, whereas velocity is extrapolated from inner points. At the free surface, the dynamic boundary condition requires continuity of stresses across the surface, whereas its location is determined by the kinematic condition. For the numerical simulation of the steady state solution of the RANS equations a pseudo-compressible formulation is used. Discretization of the physical domain is achieved by means of a multi-block structured overlapping grid. These equations are approximated by a finite volume technique with pressure and velocity co located at the cell centre, where viscous terms are computed by means of a standard second order centered finite volume approximation, while for the non viscous part, a second order Essentially Non Oscillatory (ENO) scheme has been adopted. Time integration of the discrete model is achieved by means of an implicit Euler scheme and the resulting discrete system of algebraic equations is solved in delta form. Convergence toward steady state is accelerated by local time stepping and a multi-grid algorithm. The free surface is handled by a single-phase level set algorithm with an ENO technique (similar to the one used for the bulk flow) used for solving the level set equations. More details about the implementation and the application of the single-phase approach to naval hydrodynamic problems can be found in Di Mascio et al. (2001, 2003, 2006). The presence of the propeller is taken into account by a model based on the actuator disk concept, according to which body forces are distributed in the flow field within a disk of finite thickness. Both axial and tangential forces are used in the computation in order to simulate both the acceleration and the increase in swirl that the flow undergoes when passing through the propeller. The prescribed body forces distributions are computed by assuming that the thrust coefficient K T, the torque coefficient K Q, the advance ratio J and the radial distribution of the circulation are known. In the non-iterative model of Hough and Ordway (1965), which is used here, the radial distribution of the circulation is assumed to be proportional to r r 1, where r is the non dimensional radial distance from the root of the propeller blade. 3. NUMERICAL RESULTS 3.1 Operating conditions The theoretical and computational methodology described above is applied here to study the flowfield around a representative tug boat with propeller, reported in figure 1. Tug-boats generally operate in both free-running condition at relatively high speed (10 14 knots, vessel unloaded), and towing condition at low speed (4-6 knots) while pushing/pulling a vessel or a barge.

3 Figure 1: Unit Val by Ocean S.r.l. (Trieste, Italy): the representative tug-boat considered in the present study. The propeller removed from nozzle is shown on the right. Of course, design procedures for tug-boats propulsors have to take into account that performance should be maximized both for free-running and towing operations. In view of this, the two operating conditions are considered in both computational analysis and experimental activities. Considering the computational studies on the tug-boat addressed here, the following conditions at full-scale are identified: free-running at 11.5 knots; towing at 4.0 knots. As described above, numerical simulations of the flow field around the ship hull are performed both at model scale and at full scale. Model scale ratio, λ = 10.75, is identical to that considered for testing activity to be performed at INSEAN facilities. Recalling the considered vessel length is m, and the operating conditions at full scale indicated above, the parameters defining the flow conditions in the two configurations (model/full scale) are summarized in Table 1, where F n and Rn denote, respectively, Froude and Reynolds numbers. Both propelled and unpropelled operating conditions are simulated. condition free-running towing speed [kn] Full scale Fn Rn Model scale Fn Rn Table 1: Test conditions for tug-boat flow simulations. Scale ratio is λ = Computational mesh The physical domain around the hull has been discretized by a volume grid; the overlapping grid technique described above has been extensively used to improve the resolution in those regions that can be critical for geometry complexities (such as the stern region and the region of the keel). The computational domain considered for the present analysis is delimited by an inflow plane placed Lpp (length between perpendiculars, with Lpp = 24.5 m at full scale and Lpp = 2.28 m at model scale) upstream, an outflow plane placed around 1.0 Lpp downstream, and a side plane placed at 1.5 Lpp. The overlapping mesh is formed by seven groups of blocks (see figure 2). The first one is the cartesian background grid which is composed by 160, 000 volumes. Three groups of blocks (with O O

4 Figure 2: Chimera grid around the tug-boat hull. Global view of the grid close to the hull. topology) are used for the discretization of flow field near the hull; these blocks are composed by a total of around 1,000,000 volumes. In order to resolve the boundary layer, points are clustered toward the surface hull, the first point being placed at 1 2 wall units from the wall. Two groups of blocks have been used to resolve the flow field in the region of the keel; the group in the stern region is also used to improve the resolution on the wake of the hull. This allows an accurate prediction of the wake flow which impinges on the propeller blades. These blocks are composed by around 560,000 volumes. Three blocks have been used to improve the resolution in the free surface region, with points clustered around the free surface position given by the measured trim and sinkage (around 560,000 volumes). A two blocks O O topology mesh is used to resolve the flow around the nozzle surrounding the propeller (around 75,000 volumes); body force terms of the propeller model are distribuited in a toroidal block with a total of around 33,000 volumes. Despite the complex geometry of this hull, the use of overlapping blocks allows the construction of a high quality, almost orthogonal mesh. The global mesh is composed by almost 2,500,000 volume for the demi hull. The origin of the axis is placed on the symmetry plane, at the intersection between the aft perpendicular and the water line at the operating condition (trim and sinkage are fixed, the values are taken from model experiments). The x axis lies on the water plane and on the symmetry plane (the x = 0.0 coordinate coincides with the propeller plane); the y axis is normal to the symmetry plane positive starboard, the z axis is positive upward. In the next sections preliminary results computed by using the medium mesh (obtained by removing every other point from the original mesh) are presented. Limitations of results are to be discuss and the ongoing activity in order to improve the prediction is addressed. 3.3 Model and full scale simulations: free surface In figure 3 perspective views of the wave patterns around the tug boat obtained by the numerical simulations are presented, colors blue to red denoting local wave elevation values. On the top the result for the lower speed condition (unpropelled, full scale) is shown, whereas, at the bottom, the wave pattern for the higher speed operating condition (unpropelled, full scale) is reported. As expected, the free surface elevation for the lower speed condition is small (and not resolved because the grid is too coarse), whereas at higher Froude number a clear wave pattern (with both longitudinal and transversal

5 Figure 3: Three dimensional view of the free surface around the tug boat. Top: unpropelled full scale at 4.0 knots; bottom: unpropelled full scale at 11.5 knots. wave systems) develops. In this operating condition, a breaking wave appears at the bow region, followed by a deep throat; the shoulder wave also develops. Two dimensional view of the wave patterns obtained by the numerical simulations for the unpropelled operating conditions (at model scale) are presented in figure 4, from which the observations already made on the main features of the wave system around the hull can be more clearly analyzed. Moreover, by comparison of the wave patterns obtained at the same Froude number at model and full scale (not shown), it is clear that the influence of the Reynolds number on the free surface elevation is negligible, as it should be expected for high Reynolds number. From the results presented it is clear that, in order to have a more accurate prediction of the free surface, a more refined grid at the bow region, i.e. where the maximum wave height (with a possible breaking wave), is required. Moreover, the wave pattern for the lower speed case is completely lost because the grid spacing is too large for the expected wave lenght. 3.4 Model and full scale simulations: hull flow and wake In figures 5 and 6 axial velocity contours (on the symmetry plane and on different cross sections) for the higher Froude number, propelled and unpropelled, at both model and full scale operating

6 Figure 4: Wave pattern around the tug boat. Operating conditions: unpropelled, model scale, 4.0 knots on the left and 11.5 knots on the right. conditions are presented. Sections are placed from x = 0.8 L pp (i.e. close to the bow region) to x = 0.0 L pp (i.e. at the propeller plane). From these figures some considerations can be made. The boundary layer on the hull surface develops, its thickness is increasing toward the stern; the large increase of the boundary layer thickness in the stern region is due to the restriction of the cross section of the hull shape; the propeller is operating in this wake flow, with a large velocity defect. By comparison between the results obtained at the same Froude number but at different Reynolds numbers it is evident that the Reynolds number effects are well reproduced by the numerical simulation, with a decrease of the boundary layer thickness as the Reynolds number increases for both propelled and unpropelled cases. The differences at the same scale but at different Froude number (not shown) are less relevant. The influence of the operating propeller on the flow field around the ship hull is evident in figure 6; the acceleration that the flow undergoes when passing through the propeller is clear, as well as the suction effect in the stern region of the hull. From these pictures, it is also evident that some improvement in the description of the keel region is required in order to better estimate the wake flow toward the propeller, as well as in the nozzle and in the wake regions. 4 CONCLUSIONS The computational analysis of the flow field around a tug-boat vessel using a RANS model has been presented. Aim of the activity is to provide a complete characterization of the hull flow and in particular of the hull-induced wake incoming to the propeller. The analysis is performed both at model scale and full scale, and is repeated for two operating conditions: free-running at 11.5 knots and towing at 4.0 knots. In the paper, the theoretical and computational methodology based on RANS is briefly described, and results of the flow field simulations are presented. The analysis of flow field predictions reveals that the boundary layer generated by the ship hull is correctly described. In particular, the effect of different Reynolds number at full scale and model scale is reasonably predicted. Although a direct validation of tug boat flow field predictions is not available, it may be concluded that a reliable evaluation of the hull wake and hence of the velocity field at the propeller plane has been accomplished. Another important conclusion from numerical results is that free surface effects have a relevant effect on the velocity field at the propeller plane. This is particularly true at high speed, where a strongly perturbed wave pattern is observed and the clearance between free surface and propeller nozzle is limited.

7 Figure 5: Axial velocity contours around the tug boat. Operating conditions: 11.5 knots, unpropelled, model scale (top) and full scale (bottom). Further work to improve the flow field simulations has been identified. In particular, a computational grid with a higher number of cells could be helpful to provide a better description of local flow features as the free surface and the velocity field in the propeller region. The present work has been partly supported in the frame of the FP6 Project SUPERPROP, Superior Life Time Operation Economy of Ships Propellers, under EU grant The authors wish to thank Mr. Sigfrid Wojnar from Ocean S.r.l. (Italy) for providing data about the vessel considered in the calculations. REFERENCES Chen, H.C., Lee, S.K Time-Domain Simulation of Propeller-Ship Interactions Under Turning Conditions. Proceedings of the 16th ASCE Engineering Mechanics Conference, Seattle, USA. Di Mascio, A., Broglia, R., and Favini, B A Second Order Godunov-Type Scheme for Naval Hydrodynamics. Godunov Methods: Theory and Applications, Kluwer Academic/Plenum Publishers, pp Di Mascio, A., Muscari, R., and Broglia, R Computation of Free Surface Flows Around Ship Hulls by a Leve-Set Approach. Proc. of the 8th Int. Conf. on Numerical Ship Hydrodynamics, Busan, Korea.

8 Figure 6: Axial velocity contours around the tug boat. Operating conditions: 11.5 knots, propelled, model scale (top) and full scale (bottom). Di Mascio, A., Broglia, R., and Muscari, R. 2006, On the Application of the One-Phase Level Set Method for Naval Hydrodynamic Flows. To appear on Computers and Fluids. Hough, G.R. and Ordway, D.E The generalized actuator disk, Developments in Theoretical and Applied Mechanics, 2, Larsson, L A new Navier Stokes solver for hydrodynamics applications. Proceedings of the Int. CFD Conference, Ulsteinvik (Norway), paper no. 5. Spalart, P. R. and Allmaras, S. R A One Equation Turbulence Model for Aerodynamic Flows. La Recherche Aérospatiale, 1, Zhang, D.H., Broberg, L., Larsson, L, Dyne, G A method for computing stern flows with an operating propeller. RINA Transactions, 134. Zhou, L. and Zhao, F An integrated method for computing the internal and external viscous flow field around the ducted propulsor behind an axisymmetric body. Proceedings of the 20 th ONR Symposium, pp