SESSION 7

VISCOUS FLOW: NUMERICAL METHODS



The National Academies | 500 Fifth St. N.W. | Washington, D.C. 20001
Copyright © National Academy of Sciences. All rights reserved.
Terms of Use and Privacy Statement



Below are the first 10 and last 10 pages of uncorrected machine-read text (when available) of this chapter, followed by the top 30 algorithmically extracted key phrases from the chapter as a whole.
Intended to provide our own search engines and external engines with highly rich, chapter-representative searchable text on the opening pages of each chapter. Because it is UNCORRECTED material, please consider the following text as a useful but insufficient proxy for the authoritative book pages.

Do not use for reproduction, copying, pasting, or reading; exclusively for search engines.

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics SESSION 7 VISCOUS FLOW: NUMERICAL METHODS

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics This page in the original is blank.

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics Navier-Stokes Computations of Ship Stern Flows: A Detailed Comparative Study of Turbulence Models and Discretization Schemes G.B.Deng, P.Queutey, and M.Visonneau (Ecole Centrale de Nantes, France) ABSTRACT A fully elliptic numerical method for the solution of the Reynolds Averaged Navier Stokes Equations is applied to the flow around the HSVA Tanker. The weaknesses of the simulation are analysed by comparing several discretisation schemes and grids as well as several turbulence models. Grid refinement in the near wake or application of new accurate discretisation schemes have a little effect on the quality of the solution in the wake. Systematic comparisons of various turbulence models and numerical experiments suggest that the solution is essentially affected by a too high level of turbulence viscosity in the core of the longitudinal vortex. NOMENCLATURE Variables (x,y,z) cartesian coordinates U average velocity vector p pressure t time Re Reynolds number uu Reynolds stress tensor k turbulent kinetic energy ε rate of turbulence dissipation I Identity tensor vT eddy viscosity Cμ,Cε1, Cε2,σk,σε k-ε coefficients Reff, Rk, Rε effective Reynolds numbers G production ξ,η,ζ curvilinear coordinates u,v,w contravariant components of the velocity U,V,W cartesian components of the velocity J jacobian j component of the contravariant vector bi gij contravariant metric tensor SU1 source term for the momentum equations Sk source term for the k transport equation Sε source term for the ε transport equation CNB influence coefficients at point C A,B normalized convective velocities ÛC pseudo-velocity at point C Operators Div divergence gradient 2 laplacian T transposed gradient 1. INTRODUCTION Advances in numerical solution methodology along with increased computer storage and speed have made it possible to seek numerical solutions of the three-dimensional Reynolds Averaged Navier Stokes Equations (RANSE) for moderately complex ship hulls. With the development of computers, wind tunnel or towing tank experiments are no more the only way to get information on ship performances and CFD tools appear to be able to generate an overwhelming amount of information on the flow with a level of details and flexibility which seems out of reach of a reasonable experimental approach. These computations are nevertheless mostly confined to double models, in which wave effects are absent, to

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics bare hulls without appendages or propulsors and conducted at laboratory Reynolds numbers. However, even for these simple configurations, it is crucial to locate as accurately as possible the limitations of numerical simulations in order to know (i) which level of details can be reasonably captured by a CFD tool, (ii) what are the leading weaknesses of the simulation and (iii) how to improve the accuracy of the numerical prediction. From that point of view, the so-called HSVA tanker is known as the best documented test case among all the available experimental ship flow data bases. It is why it was chosen as one of the two testcases of the 1990 SSPA- CTH-IIHR Workshop on Ship Viscous Flow which was held at Goteborg [1]. Some nineteen organizations coming from twelve countries participated in the Workshop and all of them calculated the first test case i.e. the flow around the HSVA tanker at the laboratory Reynolds number Re=5.0 106 on which this paper will be entirely focussed. Despite its seemingly geometric simplicity, the flow around this hull is rather complex. As the flow progresses along the hull, the geometry of the body gradually forces the boundary layer to pack in an area whose girthwise dimension decreases, implying a progressive convergence of the streamlines in some regions of the hull. Continuity requires a large normal velocity, a strong thickening of the boundary layer occurs often associated to the birth of a longitudinal vortex motion which is slowly relaxed in the wake at large distances downstream from the ship. A more detailed understanding of the flow is provided by the visualisation of the limiting streamlines (Figure 1 from [1]), actually the print of the flow on the hull; it clearly indicates the existence of a well defined line of convergence located just beyond the keel plane of symmetry. It is also quite clear that the behaviour of the limiting streamlines is complex since two convergence lines are visible. The first one (S1 line) is S-shaped and demarcates a vertical wall flow region and a small zone of flow reversal. The second convergence line (S2 line) is located just beyond the keel plane of symmetry and joins the S1 line at the end of the hull. Consequently, since this region seems to be characterized by a rapid normal variation of the velocity orientation from the wall to the so-called logarithmic region, it is plausible to think that such a complex three-dimensional behaviour can be hardly simulated by a wall function approach which cannot account for the high twist angle (>90º) between the wall flow and the external streamlines directions. Even more interesting are the measurements of the pressure and velocity components made at several cross-sections. Figs 2-a-b-c from [1] show the axial velocity contours at several locations, namely, x/L=0.908, 0.976 and 1.005. The longitudinal velocity contours indicate a very characteristic “hook” shape in the central part of the wake correlated with the core of the longitudinal vortex. This small region is characterised by a nearly uniform U component, a linear variation of the vertical component W preceding a maximum and again an “hook” shape of the pressure contours. These features confirm the existence of an intense longitudinal bilge vortex emanating from the hull and leads us to classify the HSVA tanker as an U-shaped hull rather than a V-shaped hull for which the longitudinal vortex is far more intense and does not create this very characteristic hook shape of the longitudinal velocity contours. The Goteborg workshop's results indicated that great progress has been made through the development of methods based on the Reynolds-Averaged Navier Stokes Equations. These methods generally simulate the gross features of the wake and predict the shape and location of the velocity contours with reasonable accuracy even on the rather coarse meshes recommended for the simulations. Nevertheless, neither the central part of the wake with this hook shaped velocity contour nor the entire wall flow behaviour can be captured by the methods presented at this time. The description of this phenomena could be of crucial importance for the design since the designer's task is to devise the best hull geometry leading to improvments to propulsive efficiency through better hull form/propeller matching. This is often a compromise between V-shaped stern sections which are associated to lower viscous resistance and less intense longitudinal bilge vortex and U-shaped stern sections for which the more intense longitudinal bilge vortex create an higher propulsive efficiency which partly compensates for the higher resistance. It is therefore fundamental to determine if the solution of the RANSE enables us to distinguish between the flows associated to U-shaped or V-shaped geometries without ambiguity. During the workshop, several hypotheses were put forward to explain the incapability of the RANSE-based methods to describe accurately the central part of the bilge vortex. Two types of explanations may be evocated, the first one favouring the discretization inaccuracies and the second one emphasizing the weaknesses of the turbulence modelisation. It is sensible to stress the numerical inaccuracy since the threedimensional grids are often too coarse to capture the details of the flow especially if we consider that most of the discretisation schemes are only first order accurate when the flow is dominated by the convection and not aligned with the coordinate lines. The numerical solution produced by such discretisation schemes is always too diffusive and local inhomogeneities such

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics as this hook shape are filtered by a too high artificial viscosity. On the other hand, it is reasonable to stress the weaknesses of the classical turbulence modelisation for this class of stern flows. As it was pointed out by V.C.Patel in [2], the turbulence in stern flows seems to behave in a very specific way. Let us compare with him the behaviour of the measured kinetic energy k plotted in outer variables, with U0 and δ as scales of velocity and length for two different flows, a thick boundary layer stern flow around the SSPA hull and a traditional flat plate flow (Fig. 3 from [2],[15]). The measurements for the strong thick boundary layer indicate a two layer structure, leading V.C.Patel to wonder if a single set of scaling parameters is adequate to modelize this flow. The outer zone is actually characterized by a lower level of the turbulence intensity, meaning that the conventional turbulence model might generate again a too diffusive flow. Then, the conjecture could be stated in these terms. What is the respective importance of the artificial viscosity compared with the likely inadequacy of the turbulence modelling? Actually, these aspects are strongly tied up if we think that the turbulence numerically produced by the discretised k-ε transport equations is somewhat modified by various numerical inaccuracies among which might be quoted the discretisation errors, an unsufficient level of coupling between the source terms of the turbulence transport equations or an unsatisfactory level of convergence for the nonlinearities. This is why some authors consider it safer to use a simpler 0 equation turbulence model like a Baldwin-Lomax model. The aim of this paper can be summarised as follows: (i) to determine what is the respective weight of the numerics compared to the turbulence modelisation for this class of stern flows, (ii) to show what has to be improved in the future to use the RANSE based methods as a reliable design tool in the naval architecture context. This paper is outlined as follows. In section 2, the alternative curvilinear formulations are described as well as the turbulence models used in the present study. Section 3 is devoted to a brief survey of the two numerical methods being the subject of comparisons. In section 4, the conditions of the computations are described and the relative influence of turbulence models and numerical approaches upon the simulation is investigated. Some concluding remarks are mentionned in Section 5. 2. EQUATIONS 2.1 The Basic Equations We consider the equations of motion in cartesian (x,y,z) coordinates for incompressible flows. The exact RANSE of continuity and momentum of the mean flow in dimensionless form are given by equations (2.1), (2.2) and (2.3): divU=0 (2.1) (2.2) (2.3) U,p and uu are respectively the velocity vector, the pressure and the Reynolds stress tensor. The resulting turbulent closure problem is solved by means of the classical k-ε turbulence model in which the Reynolds stress is linearly related to the mean rate of strain tensor through an isotropic eddy viscosity as follows: (2.4) If the k-ε turbulence model is used, the eddy viscosity vT is classically given by: (2.5) where the adimensional turbulent kinetic energy k and its dimensionless rate of dissipation ε are governed by the following transport equations: (2.6) (2.7) where G is the turbulence generation term: G=vTU:(U+TU) (2.8) The effective Reynolds numbers Rk, Rε, Reff have been defined by: (2.9)

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics Unless specified, the constants in the previous equations are taken to their standard values (2.10): In order to avoid the wall function approach, several near wall k-ε models are compared in this study. For the sake of brevity, the details concerning their implementation, which can be found in [ 4], [13] and [14], are omitted here. For a significant increase of numerical troubles and computing time (because the integration is carried out to y+≈1), the delicate problem of the three-dimensional specification of the log-law, dealt with only in [5], is avoided. The algebraic Baldwin-Lomax model [6] is also evaluated because it is less expensive in terms of CPU effort and rate of convergence. 2.2 The Equations In The Transformed Coordinate System For hydrodynamic applications, a numerical coordinate transformation is highly desirable in that it greatly facilitates the application of the boundary conditions and transform the physical domain in which the flow is studied into a parallelepipedic computational domain The partially transformed RANSE are given by the following relations in a fully conservative developped form. The contravariant components of the velocity are defined by and the physical cartesian components by (2.11) (2.12) with =U,V,W,k,ε where: (2.13) while =Reff if =U,V,W; =Rk if =k; =Rε if =ε Also, The alternative convective form needs to be introduced (2.14): (2.14) where: The additional source terms contain classically the pressure gradients and the turbulence contributions: (2.15) (2.16)

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics Endly, the metric coefficients involved in the transformation are given. They are the contravariant base, {bi}, normalized by the Jacobian, J, of the transformation and the metric tensor g: gij=J−2bibj; (2.17) (2.18) The convective form needs the functions fj which can be seen as purely geometrical convective coefficients or defined as stretching functions: (2.19) 3. THE NUMERICS In order to clarify the role played by the accuracy of the discretisation schemes, two approximation methods are evaluated. Before detailing the differences, let us first recall their common characteristics. For each of them, a cell-centered layout is used in which pressure, turbulence and velocity unknowns share the same location. This strategy simplifies coding and leads to significant savings in computational time and storage. Even if a steady solution is looked for, a local time step ensuring a fixed amount of diagonal dominance with respect to the momentum equations, is devised to accelerate the convergence towards the steady state. Endly, the momentum and continuity equations are coupled through the well known (one step) PISO procedure already detailed in [7]. 3.1 Method 1 The Convection Diffusion Schemes The momentum equations are written down under their convective form (2.14). When the Multi-exponential scheme is used, the normalized transport equation is splitted as follows : 2 A ξ−ξξ=D2−(R t+) (3.1) 2 B η−ηη=D1−(R t+) (3.2) where D1 and D2 are defined as: −D1=2Aξ−ξξ, (3.3) −D2=2Bη−ηη, (3.4) Using an exponential scheme for every equation and summing gives the so-called multi-exponential scheme: (CU+CD+CN+CS)C=CUU+CDD +CNN+CSS−(Rt+) (3.5) where (3.6) The multi-exponential scheme is very similar to the hybrid scheme. Its coefficients are always positive. It is second order accurate when the cell Reynolds numbers A, B are small, and it behaves as an upwind scheme when A, B dominate. Although the accuracy is similar to that of the hybrid scheme, this scheme is preferred since the coefficients resulting from this discretization vary smoothly, this factor is favorable for convergence. The Uni-exponential scheme is a skew upwind exponential scheme designed to decrease the numerical diffusion occuring in the previous scheme when the flow is not aligned with the grid lines. The idea is briefly outlined below for a 2D equation. After normalisation, the 2D transport equation can be written as: (3.7) where s is the local advection direction. The first term can be expressed by an exponential discretization, while other second derivatives are discretised by centered differences. A parabolic interpolation fonction is used to express the intermediate values U and D in terms of dependent variables, for instance: (3.8) which results in a 9 points formula. (3.9) Extension to the 3D case is straightforward and a 27 points formula is obtained. The 3D Uni-exponential scheme is not a positive scheme, but this fact does

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics not induce any troubles, neither in the convergence, nor in the monotony of the solution. Nevertheless, this scheme is only first order accurate when the flow is dominated by a balance between convection and pressure gradient. The Continuity Equation The fully conservative formulation is retained. The discretised form is a balance between unknown mass fluxes: (3.10) On the both sides of the control volume interface, the discretised momentum equations are available and can be written as: (3.11) where the contributions of neighbouring points and source term (except the pressure gradient) are accumulated into the pseudo-velocity (C). We must now reconstruct the contravariant velocity components ui needed at the control volume interfaces to enforce continuity and to avoid the chequerboard pressure oscillations. (3.12) Instead of interpolating U1 from available neighbouring values of the same species, U1 is linked to other dependent variables through a local ‘pseudo-physical' approximation of momentum equation at the control volume interface [8]. (3.13) A linear interpolation (in the computational domain) is used to build and but the pressure gradient is rediscretised at the respective interface. This is why this reconstruction is called “pseudo-physical”. Using the relation (3.12), the contravariant components are now given by: (3.14) Using relation (3.13), the mass fluxes are gathered in (3.10) to provide a pressure-pseudo-velocity equation which does not admit chequerboard oscillating solutions. 3.2 Method 2 The Convection Diffusion Scheme The major drawback of the previous discretisation schemes comes from the fact that the local variations of the convection or diffusion coefficients as well as the source term are not accounted for in the influence coefficients. The CPI (Consistent Physical Interpolation) scheme, based on a fully conservative formulation of the momentum equations, was proposed recently by the authors to remedy this weakness [9]. Its name stems from the fact that the fluxes are reconstructed from auxiliary (momentum) equations which are rediscretised at the interfaces of the control volume. This discretisation provides a “dynamical interpolation formula” linking the interfacial unknowns to the neighbouring cell-centered unknowns. For instance, the 2D reconstruction formula for the unknown u at the interface e is given by: (3.15a,b) with: (3.16a,b) The pseudo-velocities are no more interpolated from the available neighbouring like in the previous approach. They are linked to the surrounding velocities UNB through a discretisation of an auxiliary momentum equation. This is why the CPI approach is a generalisation of the previous recontruction: (i) this is a physical reconstruction, (ii) this technique is applied not only to the continuity equation but also to the momentum equations. For the sake of compacity, the details concerning the stencil and the

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics discretisation scheme which can be found in [9], are omitted here. After elimination of the interfacial unknowns and combination of the various fluxes, the CPI method yields a stable second-order accurate twenty-seven point stencil in the three-dimensional case. The Continuity Equation The available reconstructed mass fluxes are gathered into the continuity equation which provides a new pressure-pseudo velocities equation. 4. THE RESULTS The Grid Topology The flow domain covers 0.5<x/L<3, L being the length of the ship; rS<r/L<1. Starting from an a priori specified surface grid distribution, a volumic mesh is generated using a transfinite interpolation procedure. A new O-O topology is preferred to the previous H-O grid topology [7], This new topology enables us to optimize the number of points describing the hull and makes it possible a better description of the near wake flows. The fact that no a priori grid line is aligned with the dominant flow direction could appear as a disadvantage. Actually, since the fully elliptic RANSE are retained here, and since no particular anisotropic splitting is involved in the discretisation schemes, we think that the results are not too penalised by this choice. At the very most may we fear a slight increase of false diffusion in some parts of the flow domain. This likely drawback is largely compensated for by the fact that this fully body fitted grid allows a correct handling of the propeller boss, which was not possible with x=x(ξ) grids used in [7]. The Boundary Conditions Inlet velocity profiles (ξ=1) are generated in accordance with the method of Coles and Thompson [10] which needs the specification of δ, Uτ and Qe. These values are estimated from the specified data [11], [12] where: in order to match the solution to the measured data at X/L=0.646. However, it is felt that the influence of inlet conditions is forgotten at the stations on the afterbody and in the wake. Neumann conditions are used for the planes of symmetry (ξ=ξmax, ζ=1 and ζ=ζmax). No slip conditions is enforced on the hull (η=1) and free stream conditions (U=1, V=W=0) are applied at the outer surface (η=ηmax). Velocity profiles are slightly modified to enforce the global mass continuity constraint; hence, linear extrapolation is used for the extraneous pressure boundary conditions on all the surfaces limitating the flow domain instead of the usual Dirichlet condition p=0. The First Results Computations with Method 1 associated to a two-layer k-ε model [4] are performed on a 80×40×51 fully body fitted grid based on an O-O topology described before (Grid I). Figure 4 shows a perspective view of this grid. The clustering of the grid close to the hull is such that the boundary layer is always described by more than 25 points, the first point being located in the viscous sublayer (y+=1). The longitudinal pressure distributions are presented in figs. 5a-b. A very good agreement with the experimental results is observed on the waterline while the pressure distribution on the keel line presents the same trends as in [7], i-e an overestimation of about 40% near x/L=0.875. However, the spike that was present at X/L=0.90 in our previous computations [ 7] has disappeared here. Girthwise pressure distributions at several x-stations (figs 6a-b-c) exhibit the same trends as in [7]. The computational and experimental skin friction lines on the hull surface are presented in figs 7a-b. They both indicate that the flow close to the stern separates along an S convergence line (S1 line). The excellent agreement of the results with visualisation data is due to the eviction of the wall function approach associated to the use of a fully body fitted grid on which the propeller boss can be correctly accounted for. Nevertheless, the convergence line present in the visualisation data near the keel line (S2 line) is completely missed by the computations. The calculated skin friction lines go up from the keel line and cross this region without any distortion. The axial velocity contours at the propeller plane (x/L=0.976) are presented in figs 8a-b-c. Two convection-diffusion schemes have been employed to generate the computational results; the first one is the multi-exponential scheme based on a 7 points stencil and the second one is the uni-exponential one which leads to a 27 points stencil. They are both first order accurate when the flow is dominated by a balance between convection and pressure forces but the last one is preferred because the extraneous

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics corner points enable a more accurate representation of the convective direction and leads to a reduction of the directional numerical viscosity. Nevertheless, even if the results are improved when the Uni-exponential scheme is used—the axial velocity contours have a bulge on a level near the propeller centerline—the characteristic hook shape present in the measured velocity contours is not found by the computations. Endly, the velocity components U,V,W as well as pressure data are compared more extensively in figs 9–10–11. For each series of plots, the evolution is considered with respect to y for several depths z=cste. Here again, the calculations exhibit a correct agreement with the data except in the region close to the core of the longitudinal vortex. The experimental U profiles are characterised by a non-monotonicity which is forgotten by the computations. The maximum of W profiles is underestimated in the computations, indicating that the calculated longitudinal vortex is less intense than its experimental counterpart. The results of these simulations are in good agreement with the experimental measurements. The gross features of the wake such as the thin shear layer near the keel, the accumulation of low speed flow in the middle part of the hull and the related occurence of a longitudinal vortex are correctly captured by the computations. However, the simulated flow seems more regular than the experimental one and some very specific details, such as the low speed region in the vicinity of the propeller disk associated to the hook-shaped velocity contours, appear filtered by the simulation. Actually, the computed flow looks like the flow around a slender hull, which makes questionable the use of the results of simulations to improve the geometry via an interactive design process. Influence of Discretisation Errors Therefore, it is necessary to identify the parameters which have a dominant influence on the quality of the simulation for such hulls. As pointed before, the influence of the discretisation scheme does not seem negligible. In order to clarify the degree of importance of discretisation errors, two categories of tests are conducted. Test 1 For the first test, the usual methodology based on the Uni-exponentiel scheme and a Baldwin-Lomax model is retained (Method 1). The computations are performed on a refined mesh (121×61×60) (Grid II) based on the same O-O topology. The clustering of discretisation points is such that about twice more points per direction are present into the propeller disk region. Figure 12 shows the girthwise Cp distribution for three locations, namely, x/L=0.64, 0.87 and 0.94. For the first two stations, no spectacular improvment can be noticed. However, the strong gradient near the keel plane of symmetry is better captured on the finer grid. Figure 13 presents a visualisation of skin-friction lines on the hull which is not noticeably different from the one obtained on Grid I. Figure 14 shows the longitudinal velocity contours in the propeller disk. Again, no evident improvment can be noticed so that it seems that the results are more or less grid independant. Test 2 In order to assess the influence of the discretisation errors, a new convection diffusion scheme (CPI) leading to a totally new methodology, has been applied to this problem (Method 2). A Baldwin-Lomax turbulence model is again used here and the computations are performed on Grid I. Figures 15–16 show the girthwise Cp distributions and the wall flow which are not significantly different from the results obtained with Method 1 on Grid I. Figure 17 shows the axial velocity contours at x/L=0.976. The bulge is now slightly more developped but the innermost contours do not reveal any hook-configuration. Several numerical tests have been performed to evaluate the weight of numerical inaccuracies. Neither the computation on a refined grid, nor the use of a new discretisation method, have improved the computed simulation in the near wake. As a matter of fact, even if the global characteristics are slightly improved, the characteristic hook-shaped contours are not predicted in the propeller disk region. These numerical tests indicate that (i) the solution is more or less grid independent on Grid I, (ii) the simulated flow is too diffusive, (iii) the turbulence modelisation plays a major role in the mechanisms giving birth to these uneven vortex features. Influence Of The Turbulence Modelisation Errors To evaluate the influence of the classical newtonian turbulence models, the Baldwin-Lomax model has been compared to several k-ε models (Chen & Patel [4], Nagano & Tagawa [13], Deng & Piquet [14]) for which the wall function approach is always discarded. For the sake of brevity, the results are just mentionned and not analysed in detail. The k-ε models should be more accurate since the eddy viscosity depends on the two quantities k and ε which are obtained by solving transport equations. However, the supremacy of the k-ε models over the algebraic Baldwin-Lomax model is not demonstrated for this class of flows. As it was pointed out in [1], the aforementionned tested models produce

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics essentially the same too diffusive flow, especially in the near wake region. In order to get an idea of what has to be modified to improve the simulation, a last “heretic” computation has been performed by reducing the level of the eddy viscosity by a factor 2.5 in the core of the longitudinal vortex. Figure 18 shows the axial velocity contours at x/L=0.976. The hook-shaped configuration is now captured and figs 19a-b confirm the very good agreement between this computation and the experiments. The U component profiles are non-monotonic in the core of the longitudinal vortex and the W component profiles indicate that the predicted vortex is now far more intense. At last, fig. 20 shows a visualisation of the wall flow. It is very interesting to notice that the S2 convergence line is now present, which underlines the correlation between the extent and intensity of the longitudinal vortex and its trace on the hull. This numerical experiment indicates clearly that the turbulent eddy viscosity is the key parameter which controls the near wake of the flow. The classical turbulence models seem to produce a too high level of eddy viscosity in the central part of the wake which hides the characteristics of discretisation schemes. 5. CONCLUSION A detailed analysis of several numerical approaches and turbulence models has been performed in this work. The various discretisation schemes which have been evaluated, produce a similar flow in the near wake, characterized by a too moderate longitudinal vortex and no hook-shaped isowake contours. The computations on a refined grid revealing the same weaknesses, it is sensible to think that errors coming from the turbulence modelling are mainly responsible for the inaccuracies of the RANSE computations. This hypothesis is confirmed by the spectacular effect of a local reduction of the eddy viscosity. Therefore, the development of new turbulence models including more physics (Reynolds stress models, improvment of k-ε models, curvature effects,?..) seems to be the only way to improve the quality of RANSE based simulations for this class of flows. Acknowledgments Thanks are due to the Scientific Committee of CCVR and the DS/SPI for attributions of Cpu on the Cray 2 and on the VP200. REFERENCES 1. L.Larsson, V.C.Patel & G.Dyne (Eds) Proceedings of 1990 SSPA-CTH-IIHR Workshop on Ship Viscous Flow. Flowtech Int. Report Nº2, 1991. 2. V.C.Patel “Ship Stern and Wake Flows: Status of Experiment and Theory”, Proc. 17th Symp. on Naval Hydrodyn., The Hague, The Netherlands, 1988, pp. 217–240. 3. M.Wolfhstein “The Velocity and Temperature Distribution in One- Dimensional Flow with Turbulent Augmentation and Pressure Gradient”, Int J. Heat Mass Transfer, Vol.12, 1969, pp. 301–318. 4. H.C.Chen & V.C.Patel “Practical Near-Wall Turbulence Models for Complex Flows Including Separation”, AIAA-87–1300, 1987. 5. V.C.Patel, H.C.Chen & S.Ju “Ship Stern and Wake Flows: Solutions of the Fully Elliptic Reynolds Averaged Navier Stokes Equations and Comparisons with Experiments ”, IIHR Rept. 323, Iowa City, Iowa, 1988. 6. B.S.Baldwin and H.Lomax “Thin Layer Approximation and Algebraic Model for Separated Turbulent Flows”, AIAA Paper 78–257, 1978. 7. J.Piquet & M.Visonneau “Computation of the Flow past a Shiplike Hull”, Proc. 5th. Int. Conf. Num. Ship Hydrodynamics, Hiroshima, Mori, K.H. Ed., 1989. 8. C.M.Rhie & W.L.Chow “A Numerical Study of the Turbulent Flow past an Isolated Airfoil with Trailing Edge Separation”, AIAA-82–0998, 1982. 9. G.B.Deng, J.Piquet, P.Queutey & M. Visonneau “A Fully Implicit and Fully Coupled Approach for the Simulation of Three-Dimensional Unsteady Incompressible Flows” Paris GAMM Workshop, Notes on Num. Fluid Mech., Vol 36, M.Deville, T.H.Lê & Y.Morschoine Eds., 1991. 10. T.Cebeci, K.C.Chang and K.Kaups “A Three Dimensional General Method for Three-dimensional Laminar and Turbulent Boundary Layers on Ship Hulls”, Proc. 12th ONR Symp. Naval Hydro., Washington, 1978. 11. L.Larsson (Ed.) ( 1980) Proceedings of SSPA-ITTC on Ship Boundary Layers. SSPA Report Nº90. 12. K.Wieghardt and J.Kux “Nomineller Nachström auf Grund von Windkanal versuchen”, Jahrb. der Schiffbautechnischen Gesellschaft (STG), 1980, pp. 303–318. 13. Nagano, Y. & Tagawa, M. “An Improved k-ε Model for Boundary-Layer Flows”, J. Fluids Eng., 100, 1990, pp. 33–39. 14. Deng G.B. & Piquet J. “K-ε Turbulence Model for Low Reynolds Number Wall-Bounded Shear Flow ”, Proc. “8th Turbulent Shear Flow ”, 26–2, Münich, 1991. 15. Lofdahl, L. “Measurements of the Reynols Stress Tensor in the Thick Three-Dimensional Boundary Layer near the Stern of a Ship Model”, SSPA, Goteborg, Sweden, Report Nº61, 1982.

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics 92–0437, AIAA 30th Aerospace Sciences Meeting, Reno, Nevada, Jan. 6–9, 1992. 18. Degani, D., and Schiff, L.B.,” Computation of Turbulent Supersonic Flows around Pointed Bodies Having Crossflow Separation,” J. Comp. Phys., Vol. 66, pp173– 196, 1986. 19. Sung, C.H.,” A Multiblock Multigrid Local Refinement Method for Incompressible Reynolds-averaged Navier-Stokes Equations”, 6th Copper Mountain Conference on Multigrid Methods, Copper Mountain, Colorado, April 4–9, 1993. 20. Devenport, W.J., Dewitz, M.B., Agarwal, N.K., Simpson, R.L., and Poddar, K.,” Effects on the Flow Past a Wing Body Junction,” AIAA 2nd Tuebulent Shear Flow Control Conference, Tucson, Arizona, March, 1989. FIGURE 1. TYPICAL RATE OF CONVERGENCE WITH AND WITHOUT MULTIGRID FOR 96×32×48 GRID FIGURE 2. RMS DIFFERENCES BETWEEN MEASURED AND COMPUTED FLOW VARIABLES AT VARIOUS VALUES OF y1+

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics FIGURE 3. THE EFFECT OF TURBULENCE MODEL ON THE COMPUTED AXIAL VELOCITY PROFILES Grid 112×32×64, Measurement Uncertainty of

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics FIGURE 4. THE EFFECT OF TURBULENCE MODEL ON THE COMPUTED SHEAR STRESS PROFILES Grid 112×32×64, Measurement Uncertainty of

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics FIGURE 5. COMPARISON OF COMPUTED AND MEASURED AXIAL VELOCITY PROFILES Suboff Axisymmetric Body, RL=1.2×107, Grid 128×32×88 Turbulence Model: BL-GP, Measurement Uncertainty of u/U∞: ±0.025

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics FIGURE 6. COMPARISON OF COMPUTED AND MEASURED TURBULENT SHEAR STRESS PROFILES Suboff Axisymmetric Body, RL=1.2×107, Grid 128×32×88 Turbulence Model: BL-GP, Measurement Uncertainty of

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics FIGURE 7. COMPUTED AXIAL VELOCITY PROFILE AT X/L=0.978, DTNSRDC AXISYMMETRIC BODY 1 RL=6.6×106 and 2.5×107 Measurement Uncertainty of u/U∞=±0.025 FIGURE 8. MULTIBLOCK MULTIGRID LOCAL REFINEMENT RANS SOLUTION OF A APPENDAGE/FLAT PLATE JUNCTURE FLOW AT Rc=6.2×105, GRID: 96×48×48

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics FIGURE 9. COMPARISON OF EXPERIMENT AND MULTIGRID RANS SOLUTIONS WITH AND WITHOUT LOCAL REFINEMENT FOR APPENDAGE/ FLAT PLATE JUNCTURE FLOWS, Rc=6.2×105, U∞=32m/s, L=0.3045m.

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics TABLE 1. EFFECT OF TURBULENCE MODELS ON THE RMS DIFFERENCES BETWEEN MEASURED AND COMPUTED FLOW VARIABLES Grid 112×32×64 a) Suboff Axisymmetric Body, RL=1.2×107   u/U∞ Cp Cτ×104 Cf×103 y+ave Measurement Uncertainty ±0.025 ±0.01 ± 0.015 ±2.0     X/L 0.904 0.927 0.956 0.978 0.904 0.927 0.956 0.978         No. of Points 19 14 12 16 19 14 12 16 21 17     t 2.093 2.145 2.179 2.120 2.093 2.145 2.179 2.120 2.080 2.110     BL 0.050 0.013 0.007 0.049 0.089 0.111 0.131 0.116 0.023 3.0 2.778 7.658 BL-G 0.032 0.015 0.006 0.024 0.054 0.057 0.035 0.076 0.020 2.6 2.772 7.570 BL-PG 0.032 0.010 0.005 0.030 0.011 0.006 0.007 0.008 0.019 2.5 2.766 7.265 CF(ITTC): 2.907×10–3 b) DTNSRDC Axisymmetric Body 1, RL=6.6×106   u/U∞ Cp Cτ×104 Cf×103 y+ave Measurement Uncertainty ±0.025 ±0.01 ±0.015 ±2.0     X/L 0.755 0.934 0.964 0.978 0.755 0.934 0.964           No. of Points 15 14 16 35 12 9 11   11 9     t 2.131 2.145 2.120 2.000 2.179 2.262 2.201   2.201 2.262     BL 0.021 0.017 0.043 0.039 0.018 0.062 0.077   0.009 0.9 2.936 7.93 BL-G 0.021 0.011 0.028 0.014 0.019 0.021 0.019   0.010 1.2 2.919 7.78 BL-PG 0.021 0.006 0.020 0.010 0.023 0.009 0.010   0.012 1.0 2.879 7.78 CF(ITTC): 3.229×10−3 c) DTNSRDC Axisymmetric Body 2, RL=6.8×106   u/U∞ Cp Cτ×104 Cf×103 y+ave Measurement Uncertainty ±0.025 ±0.01 ±0.015 ±2.0     X/L 0.840 0.934 0.970 0.977 0.840 0.934 0.970 0.977         No. of Points 11 17 14 13 6 14 10 9 12 11     t 2.201 2.110 2.145 2.160 2.306 2.145 2.228 2.262 2.179 2.110     BL 0.025 0.028 0.064 0.033 0.022 0.064 0.113 0.115 0.017 2.1 3.217 5.50 BL-G 0.014 0.042 0.026 0.018 0.016 0.008 0.019 0.017 0.020 2.0 3.211 5.51 BL-GP 0.025 0.027 0.037 0.019 0.026 0.014 0.016 0.019 0.015 1.5 3.157 5.35 CF(ITTC): 3.212×10−3 d) DTNSRDC Axisymmetric Body 5, RL=9.3×106   u/U∞ Cp Cτ×104 Cf×103 y+ave Measurement Uncertainty ± 0.025 ±0.01 ± 0.015 ±2.0     X/L 0.704 0.831 0.951 0.987 0.704 0.831 0.951 0.987         No. of Points 21 18 26 27 21 9 13 17 15 14     t 2.080 2.101 2.056 2.052 2.080 2.262 2.160 2.110 2.131 2.145     BL 0.019 0.016 0.061 0.058 0.008 0.009 0.160 0.094 0.025 3.76 2.993 5.98 BL-G 0.018 0.016 0.025 0.013 0.008 0.010 0.024 0.026 0.023 2.75 2.978 5.89 BL-GP 0.019 0.015 0.023 0.015 0.008 0.007 0.027 0.018 0.019 2.23 2.926 5.87 CF(ITTC): 3.038×10−3

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics TABLE 2. MULTIBLOCK MULTIGRID LOCAL REFINEMENT COMPUTATION OF TURBULENT APPENDAGE/FLAT PLATE JUNCTURE FLOW ON CRAY C90 COMPUTER, RC=6.2×105 Sample Computation 1. 3-Level Local Refinement to Obtain Resolution of 96×48×48 Grid, y1+=8.4 MULTIGRID GRID CELLS MEMORY (MW) CPU(SEC)/ 100 CYCLES % SAVING MW RED. IN CPU TIME Without Local Refinement 221,184 11.5 430 – – With Local Refinement 49,536 3.4 99 70% 4.3 Sample Computation 2. 4-Level Local Refinement to Obtain Resolution of 192×96×96 Grid, y1+=3.7 MULTIGRID GRID CELLS MEMORY (MW) CPU(SEC)/ 100 CYCLES % SAVING MW RED. IN CPU TIME Without Local Refinement 1,769,472 80.0 3600 – – With Local Refinement 71,808 6.16 191 92% 19

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics DISCUSSION by Professor V.C.Patel, University of Iowa I have some questions that could be addressed also to authors of some previous papers in which the Baldwin-Lomax model is used with the first grid point at y+around 7 to 10. The questions are: “Are these the maximum or minimum, or just average values? How do you determine Cf, the friction coefficient? Do you simply use the slope at the wall? Do you make a correction for the pressure gradients, both longitudinal and transverse? If not, how accurate are Cf and related quantities?” Author's Reply In our paper the value of y1+at the first grid point around 7 to 10 is meant to say that the maximum value of y1+ is 10 and the arithmetic mean value is 7. When one value of y1+ is given that is the arithmetic mean value of y1+ for all the grid cells on the body. The local skin-friction coefficient Cf is calculated by where the value of is computed at the cell center of the first grid from the wall when the value of y1+ is less than 7. It is noted that the exact value at the wall must be used when the value of y1+is larger than 7, and can be obtained by extrapolating from the velocities parallel to the wall u(y1) and u(y2) of the first second grid centers at distances y1 and y2 normal to the wall, where u(y0) is set equal to 0 at the smooth wall y0 without drag reduction. No correction for the pressure gradients was made in computing Cf, but the effect due to the streamwise pressure gradient is added to the Baldwin-Lomax model. The total skin-friction was integrated from the local skin-friction. The accuracy of the computed local and total skin-friction coefficients is shown in Table 1.

OCR for page 365
Proceedings of the Sixth International Conference on Numerical Ship Hydrodynamics This page in the original is blank.