A Perspective on Naval Hydrodynamic Flow Simulations

A.Arabshahi, M.Beddhu, W.Briley, J.Chen, A.Gaither, K.Gaither, J.Janus, M.Jiang, D.Marcum, J.McGinley, R.Pankajakshan, M.Remotigue, C.Sheng, K.Sreenivas, L.Taylor, D.Whitfield (Mississippi State University, USA)

ABSTRACT

A perspective of computational hydrodynamics is presented that is considered relevant to particular Naval hydrodynamic problems. This is not intended as a survey of the field in general; rather, it is a summary of the ongoing research and development of computational tools in the Computational Fluid Dynamics Lab at Mississippi State University. A discussion is given of the enabling technologies on which most of the computational tools are based. Example results are presented for submarines, surface ships, and propulsors, that attempt to illustrate the current status of certain Naval hydrodynamic computational capabilities. Some observations and comments are offered relating to various needs and possible directions of future computational hydrodynamic research and development.

1.0 INTRODUCTION

This invited paper deals primarily with the development and application of Reynolds Averaged Navier-Stokes (RANS) codes to Naval hydrodynamic problems. The paper discusses some of the computational tools being developed in the CFD Lab that can be brought to bare on these hydrodynamic problems, and it also attempts to address some interesting but difficult underlying questions related to an assessment of present and future computational fluid dynamics (CFD) capabilities and requirements.

Recent increases in computer speed have not reduced typical runtimes for complex or advanced simulations, primarily because decreases in computer memory cost have increased the memory available, which in turn has made it possible to obtain numerical solutions to larger and far more complicated problems. The emergence of parallel computing is providing large global memory and runtimes which are reduced by multiple processors, and this is also enabling the solution of larger and even more complicated problems. Three-dimensional computations are now being performed rather routinely. In many cases, these computations have been and are being performed for either isolated components of complicated configurations or for steady state flows, and usually for both. Parallelization is now making it possible to obtain some reasonable measure of turnaround time for complete configurations in which all components are accounted for in their true interaction mode, and in some cases this is being done for both steady and unsteady flow situations. The complexity of flow configurations that are feasible will continue to increase, and along with this will come the need to address widely-varying time and length scales in the same physical problem. This, in turn, will invite further advances in both solution methodology, computer hardware and computational software.

The present paper is not intended as a survey of CFD for Naval hydrodynamics. Rather, it is primarily a summary of ongoing research in the CFD Laboratory of the NSF Engineering Research Center at Mississippi State University and through its associations with other agencies within the Navy, NASA, and Air Force. Some of the enabling technologies that have contributed to the development of certain hydrodynamic tools are first briefly reviewed in Section 2. Example results are then presented in Section 3 for simulations related to submarines, surface ships, and propulsors. Section 4 then offers some observations and comments relative to an assessment and suggested direction of CFD for Naval hydrodynamics. This section should be considered for no more than what it is, namely the opinions of the authors. Some conclusions are drawn in Section 5.

2.0 ENABLING TECHNOLOGIES

This section reviews briefly the technologies that form the basis for the tools used for the computational hydrodynamics results presented in the following



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 920
Twenty-Second Symposium on Naval Hydrodynamics A Perspective on Naval Hydrodynamic Flow Simulations A.Arabshahi, M.Beddhu, W.Briley, J.Chen, A.Gaither, K.Gaither, J.Janus, M.Jiang, D.Marcum, J.McGinley, R.Pankajakshan, M.Remotigue, C.Sheng, K.Sreenivas, L.Taylor, D.Whitfield (Mississippi State University, USA) ABSTRACT A perspective of computational hydrodynamics is presented that is considered relevant to particular Naval hydrodynamic problems. This is not intended as a survey of the field in general; rather, it is a summary of the ongoing research and development of computational tools in the Computational Fluid Dynamics Lab at Mississippi State University. A discussion is given of the enabling technologies on which most of the computational tools are based. Example results are presented for submarines, surface ships, and propulsors, that attempt to illustrate the current status of certain Naval hydrodynamic computational capabilities. Some observations and comments are offered relating to various needs and possible directions of future computational hydrodynamic research and development. 1.0 INTRODUCTION This invited paper deals primarily with the development and application of Reynolds Averaged Navier-Stokes (RANS) codes to Naval hydrodynamic problems. The paper discusses some of the computational tools being developed in the CFD Lab that can be brought to bare on these hydrodynamic problems, and it also attempts to address some interesting but difficult underlying questions related to an assessment of present and future computational fluid dynamics (CFD) capabilities and requirements. Recent increases in computer speed have not reduced typical runtimes for complex or advanced simulations, primarily because decreases in computer memory cost have increased the memory available, which in turn has made it possible to obtain numerical solutions to larger and far more complicated problems. The emergence of parallel computing is providing large global memory and runtimes which are reduced by multiple processors, and this is also enabling the solution of larger and even more complicated problems. Three-dimensional computations are now being performed rather routinely. In many cases, these computations have been and are being performed for either isolated components of complicated configurations or for steady state flows, and usually for both. Parallelization is now making it possible to obtain some reasonable measure of turnaround time for complete configurations in which all components are accounted for in their true interaction mode, and in some cases this is being done for both steady and unsteady flow situations. The complexity of flow configurations that are feasible will continue to increase, and along with this will come the need to address widely-varying time and length scales in the same physical problem. This, in turn, will invite further advances in both solution methodology, computer hardware and computational software. The present paper is not intended as a survey of CFD for Naval hydrodynamics. Rather, it is primarily a summary of ongoing research in the CFD Laboratory of the NSF Engineering Research Center at Mississippi State University and through its associations with other agencies within the Navy, NASA, and Air Force. Some of the enabling technologies that have contributed to the development of certain hydrodynamic tools are first briefly reviewed in Section 2. Example results are then presented in Section 3 for simulations related to submarines, surface ships, and propulsors. Section 4 then offers some observations and comments relative to an assessment and suggested direction of CFD for Naval hydrodynamics. This section should be considered for no more than what it is, namely the opinions of the authors. Some conclusions are drawn in Section 5. 2.0 ENABLING TECHNOLOGIES This section reviews briefly the technologies that form the basis for the tools used for the computational hydrodynamics results presented in the following

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics section. The topics covered are the usual grid generation and flow solver summaries, followed by the approach used for the dynamic relative motion grid computations required by rotating propellers. Following these are brief discussions on parallelization, graphics, and lastly, some comments relative to a CFS (Computational Field Simulation) system that is being developed to aid in code utilization and technology transfer. 2.1 Grid Generation Structured multiblock grids have been used for some time for the computation of steady and unsteady Naval hydrodynamic problems. However, unstructured grid technology has been an active area of research, and the fruits of this effort are now beginning to be used for these same hydrodynamic problems. Consequently, both structured and unstructured grid generation capabilities are summarized. 2.11 Structured Multiblock The structured grid generation code is a General Unstructured Multi-Block (GUM-B) structured grid generation system that evolved from the research and development of the structured grid technology within the NGP system [1]–[5]. Unstructured Multi-Block pertains to the issue of partial face matching, and the emphasis is that the block faces can be composed of multiple interfaces or subregions that can be interconnected to other block faces. Through the use of the solid-modeling data structure, the block connectivity is explicitly defined, so user intervention is not required to indicate block interfaces and orientations [2] [3]. Grid information of shared elements is automatically distributed to the adjoining parts [2] [4], thus allowing the user the freedom to concentrate on the domain decomposition. The foundation of GUM-B has evolved to software reusability. The graphical user interface (GUI), Geometry/CAD, and graphics are now supported via independent libraries which are utilized by other research and educational efforts at the Engineering Research Center. The GUI was redesigned to be more intuitive and easy-to-read, and it was developed by an in-house package called GuiDe [6]. GuiDe provides easy-to-use GUI design and editing, prototyping of C code, and a convenient library of widget functions and links into the graphics server. The graphics server libraries have been developed on the Open Inventor object-oriented toolkit [7] [8]. The graphics server library was developed to take advantage of the available toolkit features, but is flexible enough to replace the underlying graphics, independent of GUM-B. The Geometry/CAD functions of NGP [1] [4] [5] were also packaged into a reusable library, allowing the underlying geometry engine to be replaceable within GUM-B, but usable for other systems. 2.12 Unstructured Grid Generation Marcum and Weatherill [9] developed a very efficient local-reconnection procedure using advancing-front point placement and a combined Delaunay/min-max (minimize the maximum angle) type local-reconnection for generation of triangular or tetrahedral element grids. This approach is known as AFLR (Advancing-Front/Local-Reconnection). It differs substantially from earlier methods in that the combined Delaunay/min-max reconnection criterion is the only criteria developed to date which allows effective optimization of a three-dimensional tetrahedral element connectivity, by making effective use of the existing grid as a search data structure. Point insertion is performed using direct subdivision of the elements that contain them. This methodology has also been extended for generation of high-aspect-ratio elements [10], right-angle elements [11], and solution-adapted grids [12]. An advancing-normal type point placement strategy is used for the generation of high-aspect-ratio elements. The local-reconnection procedure, in conjunction with the advancing-normal point placement procedure does produce sliver elements in three dimensions. These elements are generated only in regions of high-aspect-ratio elements with a very structured alignment. A modified process that does not produce sliver elements is used for three-dimensional cases. The element connectivity is generated along new points in high-aspect-ratio regions. Local-reconnection is not used to determine the connectivity in these regions. This procedure produces a very structured connectivity and allows the tetrahedral elements to be easily combined into structured type elements. Typically, the majority of the tetrahedral elements within the high-aspect-ratio region can be combined into six-node pentahedrons (prisms). The outer layer of this region may have some five-node pentahedrons (pyramids) to match the outer tetrahedral elements. In all cases, the pentahedral elements have strict node, edge and face matching to each other and to neighboring tetrahedral elements. High-quality grids have been generated about geometrically complex configuration using this procedure. Results verify that for isotropic grid generation, advancing-front point placement with a combined Delaunay/min-max connectivity criterion consistently produce the highest element quality in an efficient manner [13]. 2.2 Flow Solvers The discussion above of the structured and unstructured grid generation technology used is followed here by a brief discussion of both the structured and unstructured flow solvers.

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics 2.21 Structured Multiblock The numerical approach is to solve the three-dimensional time-dependent incompressible turbulent Navier-Stokes equations. These equations are first transformed to a time-dependent curvilinear coordinate system. The artificial compressibility idea of Chorin [14] is then introduced [15]–[17]. The use of artificial compressibility permits the experience gained in the numerical solution of compressible flow problems to be exploited in the numerical solution of incompressible flow problems [18]. The artificial compressibility form of the three-dimensional time-dependent Navier-Stokes equation in general curvilinear coordinates is (1) where In these equations, β is the artificial compressibility coefficient, with a typical value of 5~10; p is static pressure; u, v, and w are the velocity components in Cartesian coordinates x, y, and z. U, V, and W are the contravariant velocity components in curvilinear coordinate directions ξ, η, and ζ, respectively. Terms where k=ξ, η, and ζ, are the viscous flux components in curvilinear coordinates. J is the Jacobian of the inverse transformation, and kx, ky, kz, and kt with k=ξ, η, and ζ are the transformation metric quantities [17], where a subscript denotes differentiation. In this work, the thin-layer approximation is introduced to simplify the full Navier-Stokes equations. An algebraic turbulence model [19], a k-ε model, and a nonlinear k-ε model [20] have been implemented within the code and used for the turbulent flow computations. The details of treating the viscous terms are explained in the work of Gatlin [21]. In addition, improvements have been made by Chen [22] with regard to the computation of the wall shear stress by improving the computation of the tangential velocity derivatives normal to a solid surface. This improvement is simple to implement and works extremely well on grids that may be highly skewed [22]. Equation (1) is discretized into a cell-centered finite-volume form. The cell face numerical flux vector was obtained using the flux difference split scheme of Roe [23]. The nonlimited form of the dependent variable extrapolation method of Anderson, Thomas, and van Leer was used to obtain second and third-order flux vectors [24]–[27]. The numerical flux used for the results presented here is the third-order upwind-biased scheme [27]. The normal procedure for the solution of the discretized equations would be to linearize the spatial difference terms, move the terms not containing ΔQn to the right-hand side of the equations, and solve for ΔQn [28]. This is particularly true for problems expected to have steady state solutions because the sum of the spatial difference operator terms as well as ΔQn would both go to zero. However, for unsteady flow, the ideal situation would be to find Qn+1 such that, for one dimension (2) One way of attempting to solve this problem is to use Newton’s method. Newton’s method [29] for the function would be (3) where m=1, 2, 3,… and is the Jacobian matrix of the vector . In principle the generated sequence Qn+1, m+1 converges to Qn+1 and, hence, Eq. (2) is satisfied. A linear system of equations must be solved at each iteration of Newton’s method. For three-dimensional problems a direct solution seems to be impractical [30] and in this work symmetric Gauss-Seidel relaxation is used. Because the flux Jacobian of the flux vector based on Roe’s formulation is difficult to obtain analytically in three dimensions, and also in the interest of simplicity, the flux Jacobian is obtained numerically [30] [31]. The solution scheme is referred to as discretized Newton-relaxation [29], or the DNR scheme [30]. Multigrid is used to accelerate the numerical solutions [32]. This multigrid scheme has been extended to multiblock [33] and unsteady flow

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics [34]. The solution process is, therefore, a multigrid scheme for three-dimensional unsteady viscous flow on dynamic relative-motion multiblock grids. The basic flow solver, called UNCLE (UN-steady Computation of fieLd Equations), has been modified for free-surface capability. The important difference between free-surface flows and other kinds of flows is that one has to obtain the motion of the free surface as part of the solution. One uses the kinematic condition [35], [36] to track the motion and the dynamic boundary conditions [37] (together with the continuity equation) to obtain the velocity and pressure at the free surface. Since the problem involves the motion (deformation) of one of the fluid boundaries, the governing equations can be cast either with respect to an inertial frame or with respect to a non-inertial frame. In the UNCLE solver the non-inertial frame is used which means that the free surface is always represented by a constant curvilinear coordinate surface. This approach involves grid motion and regeneration of the grid below the free surface at every instant in time. The basic UNCLE solver has been extended to handle difficult free surface problems such as the wetted transom flow behind the DTMB 5415 model, incorporating all the above mentioned changes. 2.22 Unstructured Solver An efficient unstructured flow solver is being developed for simulations of three-dimensional unsteady compressible and incompressible high Reynolds number viscous flows about complete configurations. Clearly, achieving this goal is not easy, and requires that several limiting barriers be overcome. Firstly, the computational cost is one of the most pressing hurdles for performing large-scale simulations about a complete configuration. This computational cost is associated with the inherently large amount of memory required by unstructured solvers, and the relatively large CPU time required. Secondly, until very recently [38] there has been limited success at generating three-dimensional unstructured high-aspect ratio elements for realistic simulations of complex geometries in extremely large Reynolds-number flows. These fundamental issues must first be resolved in order for the unstructured approach to be useful in real-world applications of complete configurations. An efficient unstructured flow solver for three-dimensional compressible and incompressible turbulent flows is being developed and further advanced. The basic solution algorithm is that of Anderson, Rausch, and Bonhaus [39]. It solves the three-dimensional Reynolds averaged Navier-Stokes equations, with the artificial compressibility formulation for incompressible flow. The Spalart and Allmaras [40] one-equation turbulence model is used to model turbulence. The discretized scheme uses a node-based finite-volume upwind approximation. The numerical flux for the inviscid part is evaluated using a second-order Roe scheme, while the viscous flux is evaluated with a finite-volume formulation that is equivalent to a Galerkin type of approximation. The time-advancement algorithm is based on the linearized backward Euler time-difference scheme, which yields a linear system of equations for the solution at each time step. The Gauss-Seidel procedure is used to solve the linear system of equations at each time step. The current work introduces an effective multiblock strategy [41] and mixed-element method to significantly reduce the memory requirements and computational time. Multigrid acceleration, dynamic moving grid capabilities, and parallelization will be added to the solver to further improve the efficiency and to predict the trajectory of unsteady maneuvering vehicles by coupling the unstructured solver with the 6-DOF solver. 2.3 Dynamic Relative Motion Grid Computations The method used to include an actual rotating propulsor is one that has been continually developed and used for a number of years, primarily for compressible flows [42]–[47]. The approach is to use relative motion blocks with structured grids, whereby the blocks that include the rotating blades move relative to adjacent blocks with a region of the blocks near the relative motion interface being treated using the localized grid distortion technique introduced by Janus [43]. This method of handling relative-motion blocks insures the continuity of grid lines (although they do change partners periodically, or “click”) and restricts the maximum distortion of the grid to be of the order of the distance between grid points, which is of course small for viscous grids. This approach eliminates the need to interpolate the solution vector from one grid to another. The cell volumes do change in time, however, and the geometric conservation law must be satisfied [48]. 2.4 Transition to Scalable Parallel Computing for Complex Simulations The computer resources required for large-scale complex flow simulations are very substantial. Parallel computing can reduce the calendar time for running large cases by at least two or three orders of magnitude, and can provide access to the large global memory required for many larger problems. Consequently, portable scalable parallel implementations of the solution methodology are needed to enable the practical solution of large-scale problems and problems with long-term transient evolutions. Parallel solution algorithms have been developed and implemented in a parallel code that enables a validated transition from single-processor computations to scalable parallel solution on complex large-scale practical applications. The parallel code exploits

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics coarse/medium-grained parallelism using the Single Program Multiple Data (SPMD) model, and employs MPI for message passing in view of its extensive portability and functionality. Much of the validation was accomplished by re-running cases that had provided validation for single-processor versions of the code. The parallel code solves the three-dimensional incompressible unsteady RANS equations using an implicit finite-volume approximation in multiblock transformed coordinates, with characteristic-based upwind flux approximations. The implicit approximation is solved at each time-step using a Multigrid/Newton/Relaxation procedure analogous to that used in the sequential algorithm [31] [34]. Domain decomposition is used to partition and map the data space onto a set of processors. Static load balancing is done at the grid generation stage when possible, based on a heuristic performance estimator which takes into account the characteristics of the algorithm and the available system resources [49]. The time-linearized approximations at each time-step are solved using a block Jacobi symmetric Gauss-Seidel relaxation procedure that involves a point-to-point message exchange at each sub-iteration level. The code also uses point-to-point messages to handle the rotating interface required for handling propulsor calculations. The implementation of algebraic turbulence models includes user-defined collective operations over processor subsets. The parallel code has been used extensively for simulations of isolated propulsors and for various submarine geometries involving hull, sail, sail planes, stern appendages, propeller, and moving control surfaces. For example, solutions for a fully-configured submarine with rotating propeller using a 1.6 million-point grid have been obtained using 51 processors on an IBM-SP (thin nodes). The parallel runtime is 57 minutes (1.5 Gflops) for one propulsor revolution of 160 time-steps, whereas the sequential solver requires 32 hours per propulsor revolution on an IBM 590 workstation. Other examples have been run on a Cray T3E: A 4.5 million-point solution for a P5168 propeller with two-equation turbulence model requires 18.8 hours (42 processors) for the 1500 steps needed for a steady solution. An 11 million-point solution for the 11:6 count Sirenian propulsor requires 50 hours (87 processors) for five revolutions (5000 steps). A 4.5 million-point solution for a full-configuration SUBOFF geometry with k-ε turbulence model requires 7 hours (64 processors) per propeller revolution (300 steps). The parallel solutions typically have efficiencies (percent CPU utilization) of 80–95 percent. Sealability studies using heuristic performance estimates indicate that on current-generation hardware, parallel efficiencies of 80 percent and more can be achieved on up to 400 processors and 50 million points, using appropriately-sized grids. 2.5 Graphics Visualization of computed data presents several problems. First is the issue of the data itself. Current trends and technologies enable the solution of problems which produce enormous amounts of data. Often, a great deal of the post-processing time is spent just sifting through, culling out, and extracting data from files too large to read into the limited memory on a graphics workstation. Another issue is that of how to visualize the data. One often does not know a priori what features exist and which are important in the solution data. Consequently, much time is spent “stumbling” through the data in an effort to locate these features. This is especially true in data sets involving complex geometries and complex physics. Other problems exist due to the often cumbersome nature of many of the currently-available visualization software systems and to the constantlychanging state of the art. To address these problems, the people who perform the post processing and visualization tasks at the ERC work and communicate closely with those who perform the computational simulations. Several commercially-available software packages are currently used for post processing of CFD data, these including PLOT-3D, FAST, and PV3. Emerging technologies are continually sought and evaluated as to their capabilities and usefulness. Another software system called DIVA (Data Interactive Visualization and Analysis) [50] is under development at the ERC. DIVA is built upon graphics server and user interface libraries designed to be portable, reusable, and maintainable. The development of this software has been driven primarily by the visualization needs of the computational engineers. 2.6 CFS System Computing a computational field simulation (CFS) solution involves a number of steps, including components of geometry, grid generation, field simulation solvers, and visualization. Each of of these steps has traditionally been completed using a separate program. To facilitate a technology transfer vehicle that permits the creation of domain-specific problem solving environments for various field simulation applications, an integrated modular environment is being developed that provides a single and unified graphical user interface (GUI) to the software elements needed to compute a CFS solution. This environment is referred to as the CFS system. The software development goal is to build highly cohesive (all modules of a library are self-contained), loosely coupled (a module does not depend on modules outside its respective library) reusable software libraries with well defined application programmer interfaces (APIs) between the libraries. This approach reduces the amount of software maintenance, speeds up the development of new systems, and reduces errors.

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics The APIs isolate the application developer in one library from changes in another library. By using the reusable-library model, a number of grid generation and visualization subsystem components, including SolidMesh (unstructured grid generator), GUM-B (structured grid generator), and DIVA (solution visualization) have been incorporated into the CFS system. Graphics and the user interface are the issues of most concern when considering portability between computer platforms. The graphics server API abstracts the application programmer from a specific graphics language. OpenInventor has been used as the primary graphics language for the graphics server due to its portability across multiple platforms, including UNIX workstations and PCs. All user-interface activities are handled through the GuiDe API and are implemented in X Windows/Motif. 3.0 EXAMPLE NUMERICAL RESULTS A few example numerical results are presented and discussed in this section. These results are for submarines, surface ships, and propulsors. The submarine results include a rotating propeller, so in this context, the body and propulsor are coupled in their natural interaction mode, including crashback. However, there will also be a few results given on an isolated propulsor because there is a good set of experimental data with which to compare. 3.1 Submarines The submarine configuration considered here is the so-called SUBOFF geometry [51]. Numerous comparisons have been made with this configuration over the past few years. There are various appended configurations that include the bare hull, the bare hull with four stern appendages, and the bare hull with the sail. All of these configurations were considered in [52]. Numerous solutions at several angles of drift were computed and compared to experimental data in [52] [33] using the Baldwin-Lomax turbulence model. The results of this exercise resulted in extremely good agreement with experimental data, much better than one might expect, even to 18 degrees of drift. An example of this agreement is given in Figure 1 where the axial, normal, and pitching moment coefficients are compared with experimental data for the SUBOFF bare hull with four stern appendages. Figure 1. Numerical and Experimental Data Comparisons for the SUBOFF Body with Four Stern Appendages

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Figure 2. Unstructured Viscous Grid in Stern Region of SUBOFF Configuration Most of the numerical solutions in Figure 1 were carried out on a structured grid. However, one unstructured grid solution was obtained for 10 degrees angle of attack and the results are included in Figure 1. The unstructured grid used for this computation had 850,000 nodes for the complete configuration, whereas, the structured grid had 1.5×106 grid points for half the body. The stern region of the unstructured grid is shown in Figure 2. A more compelete configuration was constructed by adding a sail plane and rotating propeller to the basic SUBOFF geometry. The configuration then consisted of the hull, sail, sail plane, four stern appendages, and a rotating propeller. A visualization of the solution for this fully-configured geometry is shown in Figure 3. Maneuvering predictions were obtained for this configuration by combining the Navier-Stokes solver and a 6-DOF solver [53]. The first maneuvering prediction was carried out by Dreyer at ARL/Penn State [54] with a body-force propulsor in place of the rotating propeller. Subsequent to this calculation, a maneuvering prediction solution for a fully-configured geometry that included the actual rotating propeller in place of the body-force propulsor, was carried out by Davoudzadeh [55]. This maneuver included crashback. This computation was obtained by letting the body move roughly at cruise speed, which was determined from the coupled Navier-Stokes and 6-DOF solutions, and then the propeller rotation was decreased from the constant-rpm forward rotation speed, through zero, and up to a constant-rpm reverse rotation. The results of this maneuver are recorded in [55]. A propeller in crashback creates a vortex ring around the propeller as shown in Figure 4. The strength of this vortex ring depends on such things as the rotation rate of the prop and the velocity of the boat. The ring is not stable and unsteady side forces are created. Examples of the strength and orientation of this vortex ring are shown in [55]. Figure 3. Axial Velocity About the Full SUBOFF Configuration at 0° Angle of Attack Figure 4. Vortex Ring Produced by the Crashback Maneuver 3.2 Surface Ships A submarine in crashback is a difficult computation. However, a surface ship with a wetted transom stern flow is also a most difficult computation. The numerical solution of Model 5415 at a Froude number of 0.2756 is one such solution. The solution for the wave profile on the hull for this Froude number at a Reynolds number based on body length of 12.02 million is shown in Figure 5. The computed particle traces on the free surface in the transom stern region are also shown in Figure 5. The computed vortex, which can be seen in the enlarged view of the stern region, is in agreement with experimental measurements by Toby Ratcliff of DTMB [56]. The computed resistance at this Froude number and Reynolds number differs from Ratcliff’s experimental data by 1.2%. Details of this computation and additional comparisons with experimental data are given in [57]. There is considerable amount of experimental data available for the Wigley hull and the Series 60 hull. Both of these configurations have been computed and computational details and comparisons with experimental data for the Wigley hull form is given in [58], and the same for the Series 60 hull form are given in [59].

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Figure 5. Numerical and Experimental Results for Model 5415 at Fr=0.2756 3.3 Propulsors Where propulsors are included in their natural interactive mode, such as on a submarine configuration, the computations are carried out in the absolute frame. The SUBOFF results with the rotating propeller were obtained in this manner. Another example where this approach was used is the ΜIT notional geometry, known as Sirenian, designed by Kerwin [60]. This geometry had 11 inlet guide vanes, or stators, and 6 rotating blades, in other words, a non-even blade count stage propulsor. The grid had about 11 million points and an example of the grid for the propulsor region is shown in Figure 6. This propulsor is attached to a full body; therefore, the natural interaction of the propulsor with the hull boundary layer is taken into account. This solution was run using the parallel version of the UNCLE code and the grid consisted of 87 blocks. No experimental data exists for this configuration; however, the numerical results shown in Figure 7 for flow through this two blade-row propulsor seem plausible. Figure 6. Structured Grid About the 11:6 Blade Count Sirenian Configuration Figure 7. Numerical Solution of the Sirenian Configuration For isolated propellers, considerable CPU time and memory can be saved by using a relative-frame version of the propeller code. Numerous propeller solutions have been obtained using this approach and the results have been compared to experimental data where available. However, there is a particularly detail set of experimental measurements that were taken by Jessup [61] on propeller P5168 at the David Taylor Model Basin. The purpose of these experiments was to investigate the propeller blade-tip vortex. An example of the axial, radial, and tangential velocity components just downstream of the propeller is given in Figure 8 for an advance ratio of 1.1. Numerous grid sizes were investigated in these computations that included structured multiblock grid densities of 300,000 to 1,500,000 points. Also various turbulence models were investigated that included algebraic, two-equation linear models, and two-equation non-linear models. For these computations the non-linear models gave essentially the same result as the linear two-equation models. There was a difference, of course, among the different solutions as indicated by the line plots in Figure 8. However, the overall agreement between the numerical and exper-

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics imental results for essentially all the turbulence models and grid densities considered, was consider good. The numerical results in the shaded plots in Figure 8 used the fine grid Baldwin-Lomax algebraic turbulence model. 4.0 OBSERVATIONS AND COMMENTS The organizing committee asked that certain questions be addressed in this paper. Among these questions are: (1) what are the limitations of RANS codes and how well do they approximate the physics of real flows, (2) how well do the various turbulence models approximate the physics of flows, and for what type of flows of interest are the various turbulence models applicable, (3) how does grid selection influence the solution, (4) how does one check on uncertainty in the calculation, (5) have RANS codes been pushed as far as they can be and what future research needs to be done for development of RANS codes, and (6) what will be the new tools for the future? The authors do not feel qualified, capable, nor comfortable in attempting to answer these questions in a definitive way. However, something will be said about each topic, in no particular order, if for no other purpose than to stimulate thinking in those that may be capable of answering these questions. 4.1 An Application-Oriented Perspective on Flow Simulations and Turbulence Models The resolution needed for flow simulations (number of points and local distributions) is affected by both geometric and physical factors. The geometry introduces its own length scales and resolution requirements. For example, a submarine geometry typically has elements such as a hull, sail, sail/bow planes, stern appendages, propulsor, control surfaces and gaps, and corner regions near adjoining surfaces. Although the physical flow structure varies widely from problem to problem, external flow problems often have a uniform free stream (potential flow) with shear-layer development (laminar, transitional or turbulent) near solid surfaces. These surface layers require local resolution and also have important influences on the remaining flow structure. Vorticity generated on surfaces is transported by convection and diffusion, and the surface shear layers may themselves separate, detach or lift off of the surface, transporting vorticity and turbulence well away from the surface. This in turn generates new flow structures requiring local resolution, including vortices and wakes. If a surface layer is turbulent, then turbulent correlations or shear stresses arising from time averaging (RANS) or space averaging (LES) exert an important local influence on the flow. Once a surface layer detaches, the vorticity transported into the flow can manifest itself as regions of rotational inviscid flow in which turbulence itself (if present) may have negligible Figure 8. Numerical and Experimental Data Comparisons for Propeller P5168

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics influence on the flow behavior in an averaged sense, so that much of the flow is locally governed by the rotational inviscid Euler equations, even though the source of the vorticity is surface layers with turbulence. This can easily occur in three-dimensional flows, in which inviscid secondary flows are generated by turning a primary flow that has nonzero transverse vorticity. There is often strong physical interaction between the surface layers and the rotational inviscid regions, but the turbulence itself may be important only in very limited regions such as the surface layers and may not need to be modeled very accurately in much of the flow. If detached flow structures are present in which the turbulent shear stresses are not negligible, then they would require adequate modeling, provided they exert an important influence in the particular application of interest. In the authors experience, different implementations of specific turbulence models have given poor predictions by introducing too much modeled turbulence in what are essentially rotational inviscid regions resolvable by high-resolution flow solvers. The effects of turbulent transition are much more subtle and can be influenced or triggered by turbulence outside the wall layer which itself exerts negligible shear stress. The point of all this is that flow applications with turbulence are physically complicated, and the importance and difficulty of modeling turbulence and validating turbulence models may depend on the particular application domain. Thus, it is dangerous to generalize about the validity of turbulence models, and the lack of a generally valid universal turbulence model may not prevent substantial affordable progress in a given application domain. 4.2 Implications for Flow Solvers, Equation Sets and Turbulence Modeling To summarize some of these comments, although turbulence plays an important role in establishing the (averaged) flow structure to be resolved, much of the flow resolution requirements and computational cost for practical flow simulations can come from complex inviscid flow structures induced by geometry and wall layers. Since it is only recently becoming possible to obtain high resolution simulations for unsteady three-dimensional flows, the authors believe there is still much to be learned about the sources of error in specific applications of interest, whether from numerical, turbulence modeling, or experimental sources. Although systematic studies of error, uncertainty, verification and validation of flow simulation codes will continue to be needed, the effective use of flow simulation for complex applications is not becoming a routine exercise. Although the simulation code itself need not require a developer/specialist to use, it should be used by a specialist in simulations for the given application category. Since the interaction between localized turbulence and larger inviscid flow structures can be very complex and application dependent, and since the cost of proving grid independence for a complex unsteady three-dimensional simulation is very high, it will probably remain difficult for some time to distinguish numerical, experimental and turbulence-modeling errors in a general problem independent way. For cases in which the turbulence modeling is important in localized regions, it may be that refinements to existing RANS turbulence models, although not universally valid, can provide very effective tools in specific problem domains, when used appropriately. Recent increases in computing power, coupled with concerns about the lack of universality and predictive accuracy of RANS turbulence models have led to interest in Large Eddy Simulation (LES) methods for future simulations. The unsteady RANS equations are time-averaged over a time scale sufficient to average turbulent fluctuations into Reynolds stresses, while leaving the larger scale rotational inviscid motions to be resolved as unsteady phenomena. The LES equations employ a spatial averaging over a scale sufficient to filter scales not resolved by the particular grid being used, and the subgrid scale turbulence is then modeled. The unsteady RANS and LES approaches are very similar with regard to the solution algorithm, code development and validation needed, and both require some form of turbulence model that can be incorporated in modular form. The primary difference is in the degree of mesh resolution required, since LES resolves the larger eddies of the turbulence itself, whereas the unsteady RANS approach models the turbulence and resolves the unsteady structures larger than the turbulent eddies. Consequently, LES typically requires much higher grid resolution, at least locally, and is therefore more costly. On the other hand, LES only models the subgrid turbulence structures and is universally applicable to the extent that a universal grid-independent subgrid model can be established. Since the unsteady RANS and LES codes can presumably be implemented in modular form as alternative turbulence or subgrid models, they are on equal footing in regard to the need for efficient and accurate unsteady flow solvers, and validation studies. 4.3 Influence of Grid Selection In most practical simulations, solutions change in some degree when the grid is changed. The manner and degree of grid dependence is expected to depend on the problem, the flow solver, grid generation capabilities, and what is of particular interest in the solution. For example, the near-wall grid spacing required to resolve a turbulent boundary layer seems to depend on many things. Some approaches may require much finer resolution than others, and the spacing required to obtain an accurate numerical flux near a wall may be so small that the solver used cannot handle the numerical stiffness. On the other hand, the solver may be adequate for the

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics small mesh spacings, but the flux formulation used may require a very small spacing. Confronted with this, the developer may find the use of wall functions attractive, but, this approach still has it’s own requirements for grid resolution. Again, it is difficult at this time to generalize about quantitative grid requirements, and experience with individual flow solvers and specific problem objectives remains important. 4.4 Uncertainty and Validation There are now many articles on topics such as code verification, validation, certification, calibration, and quantification of uncertainty (e.g., [62]–[65]). The intent here is not to explore these topics in any detail, but rather to offer some (hopefully practical) comments as to what a user of a code, or a user of results from a code, can reasonably expect over the near term. Here, a user is considered to be one who uses the results of a code, whether or not this person is actually the one running the solutions. Although it is desirable for the user to know that the code producing the numerical results has been fully verified, validated, certified, calibrated, and/or uncertainty quantified, it appears unlikely that this will be achieved in the near future. This is not an easy process, and there is not general agreement on these issues, and in some cases the terminology. Consequently, it would seem that efforts devoted to these issues and how to achieve them should be continued. However, the user need not wait for this work to solidify because there are codes, whether fully or partially validated according to some definition, that can be of enormous help in the design and analysis process. Roach [62] has described verification as “solving the equations right,” and validation as “solving the right equations.” Although some of the cases considered here could be construed as associated with verification, the emphasis here is regarded as validation. From the very onset of developing the UNCLE codes there has been a concerted validation effort. A large number of test cases has been accumulated, and many of these are listed in Table 1. None of the validation cases in Table 1 was a trivial exercise, and each case proved to be a much more extensive exercise than initially anticipated. Consequently, much was learned by considering each example. The end result of these efforts was that some measure of good agreement was obtained for each of the cases listed in Table 1. Suffice it to say that each example was considered until the agreement with a theoretical solution was considered good or acceptable, or until the agreement with experimental data was within the uncertainty of the data. Although numerous examples have been considered, each of which is thought to be an appropriate step in validation associated with Naval hydrodynamic problems that were known to be of interest, it still may be inappropriate to say that the code is validated. For example, Roach [62] suggests that although individual calculations can be validated, it may never be appropriate to say a code is validated. This, fortunately or unfortunately, seems to be the case in much of the authors’ experience. Many problems of interest to the Navy are both physically and geometrically complex, and each problem seems to have it’s own peculiar difficulties. It is not clear at this point how a general set of validation procedures will be able to resolve this dilemma. For example, several grid levels were run for the tip vortex problem in Table 1. In this case, the grid quality is thought to be extremely important, but grid requirements for a given problem can depend on the particular solver used. For example, some solvers may not depend on grid density as much as they do on grid alignment (the present solver is one such example). In addition, solutions using what might be considered a coarse grid with one turbulence model may actually give better results than using another turbulence model with a finer grid. In view of the large number of influence variables, the number of solutions required for validation can quickly become a prohibitive number. Consequently, a skilled user who is experienced in a given problem category is likely to remain an important factor in obtaining quality numerical solutions for problems involving complex geometry and physics. 4.5 Further Developments Although it is important that existing tools be exploited to contribute to the design and analysis process, the authors believe there is a critical need to use this ongoing applications experience to drive the continued development of improved algorithms and simulation methodology for both structured and unstructured solvers. As mentioned earlier, runtimes have generally not decreased as computing power has increased, since as solutions of more complicated problems of practical interest are enabled, decreases in computer costs induce users to pay for the required computer resources. Further advances will enable the solution of larger and more complicated problems, of even more practical interest. Consequently, improvements in algorithm efficiency and memory requirements are still needed. There is also a need for improvements in structured and unstructured grid generation capabilities. Although much progress has been made in this area, it is only recently that the speed at which unstructured viscous grids can be built has improved to the point that one might consider a complete regridding for a moving body, rather than a partial regridding in order to save time. Grid generation still requires experienced users and needs further research and development of improved tools. Improvements in algorithms and grid generation, combined with increased computing power, will enable modeling approximations to be replaced with physics.

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics generation of grids suitable for full scale flow calculations. The improvements to the SAUNA system have enabled grids to be generated with suitable near wall spacing for both wall function based turbulence models and for down-to-the-wall based turbulence models. An example of a grid used for the SUBOFF AFF4 configuration is shown in figure 1. For clarity, only every alternate grid line has been reproduced. Figure 1 Example Grid The specific areas of grid generation which have been addressed are: Improved topology creation, with C-C grid around all appendages Detailed changes to surface grid generation to enable a wider range of configurations Improved accuracy and stability in the refinement algorithms for viscous grid generation to enable high quality grids with appropriate near wall grid spacings The SAUNA grid generation methodology allows direct comparisons to be made between down-to-the-wall and wall function approaches. For simple bodies, the grid refinement algorithm acts along a series of splines defined by a background O-O topology grid. To obtain suitable grid support for a particular turbulence model, the only changes which need to be made are the first cell spacing and the number of cells in the innermost blocks. This ensures that the grid resolution for the pressure field is maintained, irrespective of the required turbulence model and Reynolds’ number. Flow solution algorithm The flow solver used for this work was CFX4.2 produced by CFDS International. CFX4.2 is a commercially available multi-block structured, control volume based finite volume flow code. A third order accurate scheme for the convection terms was used and a PISO algorithm for pressure correction. The convection scheme ensures the turbulence parameters are positive throughout the calculations. The grids produced by SAUNA were converted into a smaller number of blocks to assist efficient vectorisation for the Cray C90. To ensure accuracy and robustness for such high Reynolds’ number problems, with small grid spacing, it was necessary to maintain high numerical precision at every stage in the flow solution process. Results for the Suboff AFF1 configuration Preliminary computations for the AFF1 configuration were made using CFX4.2. These computations were used to investigate the performance of the three turbulence models over a range of grid resolutions and Reynolds’ numbers. All computational residuals were reduced by at least four orders of magnitude. The results were found to be consistent for the higher grid resolutions. All the results shown in this section are for the highest grid resolution. The number of cells in the three background axisymmetric grids was 5,000, 10,000 and 25,000. The number of cells in the direction normal to the wall in the innermost layers was 41 for the Wilcox and Menter models and 25 for the RNG model with appropriate first cells spacing for each Reynolds number. Flow predictions were carried out for Reynolds’ number of 1.2×107, 3×107, 6×107, 1.2×108, 3×108, 6×108 and 1.2×109 for each of the turbulence models. Comparison of the boundary layer profiles of the axial velocity component and the turbulent kinetic energy respectively are given in figure 2 and 3 for the axial stations x/L=0.978 and 1.040. Profiles for the measured data are compared with the computed results for the model scale Reynolds’ number of 1.2×107.

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Figure 2 Axial velocity component at x=0.978 and x=1.040 Figure 3 Turbulent kinetic energy at x=0.978 and x=1.040 Figure 4 shows the pressure and skin friction coefficients along the length of the hull for each of the turbulence models for Reynolds numbers 1.2×107, 1.2×108 and 1.2×109. Figure 4 Pressure and skin friction coefficients along the hull for each Reynolds’ number Comparisons of the profiles for the axial velocity component and turbulent kinetic energy for the boundary layer at x=0.978 and for the wake along the axis are given in figures 5 to 7. Comparison between each of the turbulence models for three Reynolds’ numbers of 1.2×107, 1.2×108 and 1.2×109 are shown in figures 5, 6 and 7 for the boundary layer and wake profiles. The data for the RNG, Menter and Wilcox turbulence models are given as solid, dashed and dotted lines respectively.

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Figure 5 Boundary layer and wake profiles at Re=1.2×107 Figure 6 Boundary layer and wake profiles at Re=1.2×108

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Figure 7 Boundary layer and wake profiles at Re=1.2×109 The volumetric wake fraction w2 is given by This volumetric wake fraction at x=0.978 and x=1.040 for the complete range Reynolds’ numbers and turbulence models is given in table 4. Table 4 Volumetric wake fractions   x=0.978 x=1.040 Re RNG Menter Wilcox RNG Menter Wilcox 1.2×107 0.686 0.708 0.720 0.759 0.775 0.786 3.0×107 0.716 0.728 0.747 0.785 0.790 0.810 6.0×107 0.734 0.742 0.766 0.800 0.803 0.827 1.2×108 0.754 0.756 0.777 0.818 0.815 0.836 3.0×108 0.776 0.760 0.795 0.838 0.819 0.852 6.0×108 0.789 0.774 0.808 0.848 0.832 0.863 1.2×109 0.804 0.790 0.816 0.862 0.845 0.870 Results for the Suboff AFF4 configuration A series of calculations were performed for the AFF4 configuration using a number of grid resolutions for the underlying pressure field suitable for ‘wall functions’ and for ‘down-to-the-wall’ predictions. The topology of the local grids around the components was chosen to produce an O-O grid around the hull with C-C grids around the aft appendages. This provides the most efficient grid structure while maintaining sufficient grid support in the wake of the appendages. The number of cells necessary to obtain the required y+ spacings and maintain a reasonable expansion ratio in the innermost, viscous grid layers for the ‘down-to-the-wall’ grids meant that approximately 50% of the cells were dedicated to the resolution of the viscous boundary layer and wakes. Therefore, for underlying grid resolutions of 200,000 and 400,000 cells for the pressure field, approximately 250,000 and 500,000 cells were used for the ‘wall function’ grid with 500,000 and 1,000,000 cells used for the equivalent ‘down-to-the-wall’ grids. The same number of cells and first cell spacing in the innermost layers as described for the AFF1 configuration was used for each turbulence model and Reynolds’ number.

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Initial flow computations with the three turbulence models indicated that the convergence of the flow solution algorithm was incorrect in the wake for the two ‘down-to-the-wall’ models. There were only very weak wakes behind the appendages, especially for the Wilcox model. There was also evidence that the multi-block scheme was not producing a symmetric solution to the problem, especially for the turbulence fields. To obtain reasonable solutions for the ‘down-to-the-wall’ models, it was necessary to increase the first cell spacing in the wakes downstream of the appendages. It was also necessary to under-relax the solution procedure in CFX4.2 to obtain symmetric solutions. A larger number of iterations were required to develop the wake profiles downstream of the appendages. On examination of the results for the 500,000 cell cases, it was clear that the wake field for the Wilcox model was not sufficiently developed although the solution residuals had ‘converged’ by at least four orders of magnitude. Therefore, only results for the RNG and Menter turbulence models for Reynolds’ number of 1.2×107, 1.2×108 and 1.2×109 for the fine grids are given in this paper. Examination of the results from the RNG turbulence model showed consistent trends in the development of the flow around the AFF4 configuration. There was evidence of the development of small vortex structures embedded in the boundary layer of the hull which showed little variation with Reynolds’ number. The thickness of the wake structure behind the appendage reduced, and the relative intensity of the turbulent kinetic energy in the embedded vortices increased as the Reynolds’ number increased. However, the results for the Menter turbulence model showed different trends. The size and strength of the embedded vortices increased as the Reynolds’ number increased and the position of the stagnation point forward of the appendages moved upstream. Overall, the Menter turbulence model showed considerably more activity than the RNG model, especially in the boundary layer, which increased as the Reynolds’ number increased. This is illustrated by plots of the measured and computed flow parameters for radii at r/R=0.25, 0.3, 0.4 and 0.5 in the plane of the propulsor. Figure 8 shows the measured flow parameters ux, ur and k for each of the radii. The data are plotted at two degree intervals. Comparison between the Menter and RNG turbulence models for each Reynolds’ number is given in figures 9 to 14. These figures show the variation of the computed flow parameters ux, ur, k and ν for the same radii and axial position as the measured data. The data are plotted at intersections with the grid. Contours of the axial velocity magnitude in the plane of the propulsor at x=0.978 for each of the Reynolds’ numbers are given in figures 15 and 16 for the Menter and RNG models respectively. The contours range from 0.1 to 1.0 with an increment of 0.05. Figure 8 Measured experimental data at Re=1.2×107

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Figure 9 Wake profiles for Menter at x=0.978 and Re=1.2×107 Figure 10 Wake profiles for RNG at x=0.978 and Re=1.2×107

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Figure 11 Wake profiles for Menter at x=0.978 and Re=1.2×108 Figure 12 Wake profiles for RNG at x=0.978 and Re=1.2×108

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Figure 13 Wake profiles for Menter at x=0.978 and Re=1.2×109 Figure 14 Wake profiles for RNG at x=0.978 and Re=1.2×109

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Figure 15 Figure 16

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Discussion There are differences between the turbulence models which become more pronounced as the Reynolds’ number increases. The overall shape and features of the profiles and contours at the model scale Reynolds’ number are fairly similar but the results at full scale are quite different. It is not yet certain that these differences are purely due to the turbulence model and the associated boundary conditions. Further examination of the profiles for the AFF1 configuration show that the boundary layer profile is sensitive to the initial and boundary conditions. In particular, the estimates of boundary layer thickness, skin friction coefficient and the overshoot velocity all contribute to systematic differences in the predictions at model scale. In addition, although the value of the background turbulence is set at the start of the iterative scheme, the final value reduced by up to an order of magnitude. However, for this exercise, it was necessary to maintain a consistent specification of the initial condition which encompassed a range of Reynolds’ numbers. Examination of the wake profiles for AFF4 shows that the Menter turbulence model is predicting larger variations in the velocity and turbulence parameters than the RNG model at model scale. When the axial velocity component in figures 9 and 10, is compared with the measured data in figure 8, the overall characteristics of the wake are better captured by the Menter model. This would indicate that the Menter model predicts the magnitude of the wake harmonics better that the standard RNG model. However, when comparison is made between the radial velocity component, the Menter model predicts a deep minimum at θ=45°. This feature is absent in the experiment data and in the RNG predictions. The turbulent kinetic energy predicted by the Menter model is twice the experimental data on the innermost rake, rising to six times on the outermost rake. However, the values predicted on the plane of symmetry are close to the experimental values and on the inner rakes, the general behaviour of the experiment is followed closely. The peaks are more compact and there is a reduction from a relatively uniform value at θ=45°. The RNG predictions are featureless by comparison. The general levels of the experiment are predicted, but the features are either missing or very weak. This is particularly true in the wakes of the appendages. As Reynolds number increases, the flow features of the Menter predictions intensify. This is most apparent in the central region, away from the plane of symmetry and just outside of the appendage wakes. The radial velocity has its maximum on the bisecting plane and there are peaks of turbulent kinetic energy and of eddy viscosity on either side of this plane. The peaks start developing soon after the hull radius starts to decrease and appear to be associated with the outer part of the hull shear layer where blending between the ω and ε models occurs. The only no-slip surface in this region is the hull with smoothly varying normals. The operation of the blending function is therefore unlikely to be complicated by secondary flows in this region. This points to a potential mismatch between the conditions inside and outside of the hull shear layer rather than a natural phenonema. This is supported by the change observed in the ratio of μT/μ in the outer flow domain and the comparison with experimental data at model scale. In contrast, the RNG predictions change relatively little and there is no intensification of flow features. There is a gradual rise in axial velocity and a gradual reduction in both the turbulent kinetic energy and the eddy viscosity. The variation in radial velocity increases slightly. Overall, the predictions also become less symmetrical as the Reynolds number increases. There appears to be some dependency in the predicted flow field for both turbulence models on the order in which the flow solver addresses the blocks of the grid. This dependency becomes more pronounced as Reynolds’ number increases. The severity can be gauged from the extent of the deviation from symmetry in the radial profiles. The major concern that this raises is the level of convergence of the predictions. For the RNG predictions, this is unlikely to be an issue; the residuals have fallen by at least four orders of magnitude and the maximum change in the velocity variables, at least, is well below 0.1% of free stream. For the Menter predictions, although a larger number of iterations were used for each flow prediction, a greater degree of under-relaxation was required to maintain symmetric solutions. Therefore, the reduction in residuals was generally smaller than for the corresponding RNG prediction and the maximum change in velocity somewhat larger.

OCR for page 920
Twenty-Second Symposium on Naval Hydrodynamics Conclusions Predictions of the flow around an appended geometry have been obtained for a range of Reynolds’ numbers for different turbulence models. To obtain meaningful comparisons between the turbulence models for the range of Reynolds’ number it was necessary to increase the resolution and accuracy of all stages of the CFD process. The reliability of such comparison depends on how well the flow features are resolved. This imposes an increased level of rigour and control of factors such as grid resolution, computational accuracy and numerical precision. This also extends to the critical assessment of the predicted flow field, and its level of convergence. The RNG turbulence model in conjunction with wall functions and the Menter turbulence model can make predictions from model to full scale for appended and unappended bodies. For the AFF1 configuration, there is some consistency in the scaling of their predictions. This is not yet the case for the more complex AFF4 configuration. As a whole, the predictions point to an increased sensitivity of the Menter model to changes in Reynolds number. However, insufficient numerical implementations have been used to come to definitive conclusion on this matter. The performance of the particular solution algorithm appears to reduce somewhat when applied to appended geometries, especially when using the ‘down-to-the-wall’ turbulence models. There are some difficulties with the reliability of the solution algorithm, associated with the multi-block nature of the method. Further work is required to clarify the requirements for grid resolution and numerical stability for the more complex ‘down-to-the wall’ turbulence models, especially for fully appended geometries. 1. Bull P., “The Validation of CFD Prediction of Nominal Wake for the SUBOFF Fully Appended Geometry”, Proceedings of 21st Symposium of Naval Hydrodynamics, Trondheim, Norway 1996. 2. Eça L and Hoekstra M., “Numerical Calculations of Ship Stern Flows at Full Scale Reynolds’ Numbers”, Proceedings of 21st Symposium of Naval Hydrodynamics, Trondheim, Norway 1996. 3. Ju S., “Numerical Study of Ship Stern and Wake Flows at Model Scale and Full-Scale Reynolds; Numbers”, IIHR Report no 323, 1991 4. Watson S.J.P. and Bull P.W., “The Scaling of High Reynolds’ Number Viscous Flow Predictions using CFD Techniques”, Third Osaka Colloquium on Advanced CFD Applications to Ship Flow and Hull Form Design, Osaka, Japan, 1998. 5. Sotiropoulos F. and Patel V.C., “Second moment modelling for ship-stern and wake flows”, Proceedings of CFD Workshop for Improvement of Hull Form Designs, Toyko, 1994. 6. Deng G., Visonneau M., “Evaluation of Eddy Viscosity and Second-Moment Turbulence Closures for Steady Flows Around Ships”. Proceedings of 21st Symposium on Naval Hydrodynamics, Trondheim, Norway, June 1996. 7. Larsson L., Patel V.C. and Dyne G., (ed), Proceedings of 1990 SSPA-CTH-IIHR Workshop on Ship Viscous Flow, 1990. 8. Wilcox D.C, “Turbulence Modelling for CFD” 1994, DCW Industries. 9. Menter F.R., “Influence of freestream values on k-ω turbulence model prediction”, AIAA Journal 30.6, 1992. 10 “CFX4.2 User Guide”, 1997, CFX International, Harwell Laboratory, Oxfordshire, OX11 0RA, United Kingdom 11 “SAUNA Release 3.0 Volume 1 User Guide”, 1998, ARA Limited, Manton Lane, Bedford MK41 7PF, United Kingdom.