COUPLING OF 3D NUMERICAL SOLUTION METHOD BASED ON NAVIER-STOKES EQUATIONS WITH SOLUTIONS BASED ON SIMPLER THEORIES

Transcription

1 COUPLING OF 3D NUMERICAL SOLUTION METHOD BASED ON NAVIER-STOKES EQUATIONS WITH SOLUTIONS BASED ON SIMPLER THEORIES Sven Enger Milovan Perić CD-adapco Nordostpark 3-5, Nuremberg, Germany Henrique Monteiro CD-adapco Av. Brigadeiro Faria Lima, São Paulo Abstract. In many applications there is a need to simulate transient flows around bodies over a longer period. While the flow usually takes place in a large domain, engineers are usually interested only in the solution in the immediate vicinity of the body. It is therefore very important to be able to reduce the size of the computational domain and thus reduce the computing effort while not compromising the accuracy and reliability of the solution. This paper describes one approach which can be applied, among others, to flows around floating or flying bodies. The idea is to force the solution of the 3D Navier-Stokes equations towards a solution based on some simplified theory (or 2D solution in a larger domain) over some distance around the body. This resolves the problem of specifying boundary conditions on the reduced solution domain boundaries. In this way, damping of waves reflected from bodies and propagating toward the inlet can also be achieved. The method has been implemented in the commercial flow solver STAR-CCM+ and tested on several applications examples. The results demonstrate the benefits of this approach compared to the alternative ways of simulating such flows. Keywords: Flow simulation, Free-surface flow, Forcing, Coupling

2 Coupling of different numerical solutions 1 INTRODUCTION In order to analyze safety of operation and structural integrity of off-shore structures under adverse weather conditions, it is often required to simulate unsteady free-surface flows around such structures and study the phenomena like wave impact, green water effects and slamming. Such long-lasting simulations are computationally expensive and therefore it is desirable to reduce the size of the solution domain to save the computing cost. On the other hand, specifying boundary conditions on the reduced solution domain boundaries is difficult due to the presence of free-surface waves, vortex shedding and other transient phenomena. For example, specifying inlet conditions using wave theories (such as 5 th -order Stokes wave or long-crested wave spectra like JONSWAP or Pierson-Moskowitz) can be problematic since waves reflecting off structures and propagating upstream also reflect at the inlet boundary, thus contaminating longer-lasting simulations in limited solution domains. While it is in principle possible to detect the upstream-propagating regular wave and modify the inlet boundary condition accordingly, this approach is not practical for 3D complex wave patterns as can be generated by offshore structures. Waves generated by floating bodies can be damped to avoid their reflection at boundaries (see Choi & Yoon, 2009), but this approach cannot be applied at the inlet since the incoming waves would be damped as well. A way to minimize the problem with boundary conditions on reduced-size domains is to couple the 3D solution of the Navier-Stokes equations in the zone of interest with a simpler solution from a larger (or infinite) domain which does not require a high computing cost. For example, Kim et al. (2012) in their Euler-Overlay Method used a 2D solution of Eulerequations in a very large solution domain without any obstacle as the background flow. They demonstrated that the impact of a rouge wave onto a cylinder can be efficiently simulated by coupling a commercial 3D flow solver applied in the zone around cylinder with an in-house 2D Euler-equations solver applied to the background flow. The 2D Euler equations were solved on a solution domain longer than 100 m and over a time period longer than 20 s, while the 3D Navier-Stokes equations were solved on a domain 2 m long and 1 m wide over just 1.5 s, thus covering in both space and time only the interval of interest capturing the wave impact. The approach of Kim et al. (2012) has been generalized to allow coupling of the 3D flow simulation using the commercial flow solver STAR-CCM+ with any of the following: (i) theoretical solution based on simplified theory (like wave theories or trivial flows that have analytical solution), (ii) numerical solution based on simplified theory (like potential flow or Euler-equations), (iii) 2D simulation using the same solver and either Euler- or Navier-Stokes equations, and (iv) tabulated solutions from external codes. This kind of coupling is also suitable for computing propagation of waves generated by a floating body over a large distance and their interaction with the shore or other bodies. Usually, the Navier-Stokes equations are required to compute the flow around the body due to turbulence effects, breaking waves and other complex phenomena, but this approach is computationally too expensive if the solution domain is large. However, propagation of waves away from body can be accurately computed using much cheaper methods based on potential theory. Thus, by coupling the two methods such problems could be computed accurately and efficiently. The following section provides a brief description of the mathematical model behind the flow solver implemented in the STAR-CCM+ code, the numerical solution procedure and the coupling method. This is followed by a presentation of results from three representative test

3 S. Enger, M. Perić & H. Monteiro cases which demonstrate the advantages of the forcing method compared to some alternatives. Finally, conclusions are drawn and directions for future research are outlined. 2 NUMERICAL METHOD This section describes the mathematical model and the discretization method employed in the software STAR-CCM+; in addition, the method of coupling with theories or other solutions is described. 2.1 Mathematical model The flow is assumed to be governed by the Reynolds-averaged Navier-Stokes equations, in which turbulence effects are included via an appropriate turbulence model, depending on application; the range includes linear and non-linear eddy-viscosity models (k-ε or k-ω) for all ranges of Reynolds numbers, Reynolds-stress model, large-eddy simulation (LES) and detached-eddy simulation (DES) models. Thus, the continuity equation (Eq. (1)), the momentum equations (Eq. (2)), and selected equations for turbulence properties (represented by the generic scalar conservation equation, Eq. (3)) are solved. These equations are: (1) (2) (3) In addition, the space-conservation law must be satisfied when control volumes (CVs) move and change their location and shape: (4) In these equations, ρ stands for fluid density, v is the fluid velocity vector and v b is the velocity of CV surface; n is the unit vector normal to CV surface whose area is S and volume V. T stands for the stress tensor (expressed in terms of velocity gradients and eddy viscosity), p is the pressure, I is the unit tensor, ϕ stands for the scalar variable (e.g. k, ε or ω, Reynolds stresses and temperature), Γ is the diffusivity coefficient, b is the vector of body forces per unit mass and b ϕ represents sources or sinks of ϕ. Since the CV can move arbitrarily, the velocity relative to CV surface appears in the convective flux terms, and the time derivative expresses the temporal change along the CV-path. When flows with free surfaces between immiscible fluids are computed, an additional equation is solved for the volume fraction of all but one component in order to account for arbitrary deformation of the free surface, including its possible fragmentation and surface tension effects. These equations have the same form as Eq. (3), except that the diffusion term is missing, ϕ is replaced by the volume fraction of the corresponding component and density ρ

4 Coupling of different numerical solutions is replaced by unity. The source term on the right-hand side is only present when the phases are compressible or when phase change takes place (e.g. when cavitation is modeled). When the motion of a flying or floating body is computed simultaneously, additional equations describing the motion of a rigid body are solved: (5) (6) Here m B is the body mass, I is the tensor of the body's moments of inertia, v C C is the velocity of the body's center of mass, ω is its angular velocity, F B B is the resultant force and M C the resultant moment acting on the body. The force is typically made up of flow-induced forces (tangential shear-stress and normal pressure forces) and body weight; the latter does not contribute to the moment about the center of mass: (7) (8) Here g stands for gravity acceleration and r for the position vector relative to a fixed reference frame; index B denotes body and C denotes center of body mass. Additional external forces and moments may act on the body (propulsion forces, spring-like forces due to moorings etc.). For all equations appropriate initial and boundary conditions have to be specified. Boundary conditions may change with time and are usually of either Dirichlet (specified values of the variables solved for) or Neumann (specified gradients of the variables) type. 2.2 Flow solver in STAR-CCM+ The numerical method used in STAR-CCM+ is of finite-volume (FV) type. It starts from conservation equations in integral form (Eqs. (1)-(3)) and by means of a number of discrete approximations leads to an algebraic equation system solvable on a computer. First, the spatial solution domain is subdivided into a finite number of contiguous control volumes which can be of an arbitrary polyhedral shape and are typically made smaller in regions of rapid variation of flow variables (see Fig. 1 for an example). The time interval of interest is also subdivided into time steps of appropriate size (not necessarily constant). The governing equations contain surface and volume integrals, as well as time and space derivatives. These are approximated for each CV and time level using suitable approximations. All integrals are approximated by the midpoint rule, i.e. the value of the function to be integrated is first evaluated at the center of the integration domain (CV face centers for surface integrals, CV center for volume integrals, time level for time integrals) and then multiplied by the integration range (face area, cell volume, or time step). These approximations are of second-order accuracy, irrespective of the shape of the integration

5 S. Enger, M. Perić & H. Monteiro region (arbitrary polygons for surface integrals, arbitrary polyhedra for volume integrals). Since variable values are computed at CV centers, interpolation has to be used to compute values at face centers and linear interpolation is predominantly used. However, first-order upwind interpolation is sometimes blended with linear interpolation for stability reasons when the mesh is too coarse or of poor quality. In order to compute diffusive fluxes, gradients are also needed at cell faces, while some source terms in equations for turbulence quantities require gradients at CV centers. These are also computed from linear shape functions (corresponding to central differences). More details related to the FV-method used in STAR- CCM+ can be found in Demirdžić & Muzaferija (1995), Weiss et al. (1999) and Ferziger & Perić (2004). Figure 1. An example of a polyhedral grid, used to compute the flow around a cylinder in a channel (left) and a single typical polyhedral CV (right). In the case of free-surface flows, the convective fluxes in the equations for volume fractions require special treatment. The aim is to achieve a sharp resolution of the interface between immiscible fluids (one cell wide), which requires specific interpolation of volume fractions. The method used here represents a blend of upwind, downwind, and central differencing, depending on the local Courant number, the profile of volume fraction, and the orientation of interface relative to cell face; for more details, see Muzaferija and Perić (1999). The scheme is adjusted to guarantee that the volume fraction is always bounded between zero and one, to avoid unphysical solutions. The scheme typically resolves the interface within one cell and effectively prevents mixing of liquid and gas, thus allowing long-time simulations with maintained accuracy. The solution of the Navier-Stokes equations is accomplished using either a segregated or a coupled iterative method; the former is preferred for transient flows since small time steps are required for accuracy reasons and only a few repetitions of the segregated solution sequence per time step are required (typically of the order of 5). In this approach, the linearized momentum component equations are solved first using prevailing pressure and mass fluxes through cell faces (inner iterations), followed by solving the pressure-correction equation derived from the continuity equation. Thereafter equations for volume fraction and turbulence quantities are solved; the sequence is repeated (outer iterations) until all non-linear and coupled equations are satisfied within a prescribed tolerance, after which the process advances to the next time level. When the motion of flying or floating bodies is also computed, the outer iteration loop within each time step is extended to allow for an update of body position. The equations of body motion are first solved to obtain the velocities using a predictor-corrector scheme of

6 Coupling of different numerical solutions second order (equivalent to the Crank-Nicolson scheme) and the estimated flow-induced forces. Then the translations and rotations are computed and the grid within the flow domain is adjusted to fit the new body position. A body deformation could also be computed at this stage. At the end of each time step, the computed body position and the fluid flow converge to a state that satisfies both the flow and body motion equations simultaneously. The solution method is thus fully implicit and fully coupled. The time step can be selected according to accuracy requirements as there are no limitations for stability reasons. The flow chart of the iterative solution method is shown in Fig. 2. For more details see Hadžić et al. (2005). Figure 2. Flow chart of the segregated iterative solution method employed to compute flows around floating or flying bodies. Grid adaptation to body motion requires special attention. When a single body in an infinite domain is considered, the whole grid can be moved with the body. This can be problematic in the case of large motions of a floating body due to the presence of a free surface, because the grid needs to be fine in a larger region in order to capture the free surface and waves properly. In the case of moderate motion, the grid near the body can be moved rigidly with the body and keep the grid further away from the body undeformed, while deforming the grid in the region between these two. This is achieved by solving equations for grid deformation (morphing) with appropriate boundary conditions (grid points fixed at the boundary, grid points allowed to slide along boundary etc.). The third possibility is to use overset grids, where one grid is adapted to the background (surrounding, free surface, waves etc.), while overlapping grids are attached to flying or floating bodies and move with them without deformation. In this case the grid quality remains the same all the time and grid motion is easier to handle; also, the motion of bodies is not constrained in any way, other than by solid walls in the surrounding region. All these options are available in STAR-CCM+.

7 S. Enger, M. Perić & H. Monteiro Linear equation systems are solved using an algebraic multigrid solver, which can be combined with conjugate-gradient type solvers to increase the efficiency and robustness. 2.3 Coupling method Coupling by forcing is achieved by adding a source term in the transport equations of the form (see Eq. (3)): bϕ = λ (ϕ ϕ*) (9) Here λ is the forcing coefficient, ϕ is the solution of the transport equation at the given CV centroid and ϕ* is the value towards which the solution is forced. This technique is used with a very large value of λ when the solution needs to be fixed to a certain value, since then the remaining parts of the discretized equation become negligible; for example, the value of turbulence dissipation rate ε in the k-ε turbulence model is fixed at the cells next to wall when wall functions are employed to (see Launder & Spalding, 1974): ε* = (Cµ 3/4 k 3/2 )/(κy) (10) Here Cµ and κ are turbulence model parameters (typically 0.09 and 0.41, respectively), y is the distance of cell-center from the wall and k is the value of turbulent kinetic energy at the cell centroid, as computed by solving the discretized equation for that cell. The discretized equation for ε is overridden by adding the source term according to Eq. (9) with λ = Instead of fixing variable values at cells next to a boundary, the source term from Eq. (9) can be applied with a variable forcing coefficient over a certain zone. Figure 3 shows schematically overlapping of two solution domains. The 3D Navier-Stokes equations are solved within the red and the green zone; inside the red zone, no forcing is applied, while within the green zone along solution domain boundaries (whose width can be different at different boundaries) the forcing source term is activated. The forcing coefficient varies smoothly from zero at the edge of the red zone to the maximum value at the outer edge of the green zone. Figure 3. Schematic presentation of coupling of two solution methods with volumetric overlapping of solution domains and a variable forcing coefficient. Kim et al. (2006) suggest the following variation of the forcing function: λ = λ0 cos 2 (πx*/2) (11)

8 Coupling of different numerical solutions Here λ0 is the maximum value of the forcing coefficient and x* is the relative coordinate within the damping zone (zero at the beginning and 1 at the end, viewed from the Navier- Stokes zone). This variation is adopted in the present study as well, although other variations are also possible. The maximum value of the forcing coefficient was here set to λ0 = 10. The optimal value is problem-dependent; Kim et al. (2006) used λ0 = 1, but in present tests, this was found to be too low; on the other hand, the value λ0 = 100 was found too high. The optimal width of the forcing zone is also problem dependent. Further comments on these issues will be given in the next section. The forcing does not have to be applied to all variables. For example, if a turbulent flow is computed using Reynolds-averaged Navier-Stokes equations and outside the forcing zone potential flow is assumed, there are no appropriate values for k* and ε* to be applied. In this case, the usual boundary conditions can be used for these variables as if no forcing was applied. Since the velocity field is forced towards the background field, the values of turbulence quantities (which affect the turbulent viscosity) are not of large relevance inside the forcing zone. In the present applications (as was also the case in Kim et al., 2006, and Kim et al., 2012), the coupling was only one-way, i.e. the background flow was assumed to be unaffected by the presence of obstacles around which the Navier-Stokes equations were solved. However, two-way coupling can also be realized. Ideally, the forcing zone for the background flow should not overlap with the forcing zone for the inner flow in order to ensure that ϕ* is computed from unaltered transport equations (i.e. without the forcing source term). The twoway coupling would be needed if the wave propagation in the wake of a body (ship or offshore structure) should be followed over a longer distance using e.g. a potential flow solver. When the background flow is described by a theory, it is easy to determine the value of ϕ* at the centers of CVs within the forcing zone. However, if the background solution stems from another numerical method, appropriate interpolation has to be performed to obtain the values of ϕ* at the required locations. Especially when moving bodies are considered and the grid moves to adapt to the body position in each iteration within the time step, an efficient interpolation procedure is essential to reduce the computational cost. In the present study only theoretical solutions are considered as background flow, so the interpolation issue has not been addressed. 3 APPLICATION EXAMPLES This section describes three application examples, designed to demonstrate the main features of the forcing method implemented in STAR-CCM Propagation of a 5 th -order Stokes wave In the first test case, a 2D simulation of propagation of a 5 th -order Stokes wave is performed, in which forcing towards a theoretical solution is applied both near the inlet and near the outlet boundaries. The Stokes wave with the following parameters was propagated over 7.5 wavelengths for 10 wave periods: wavelength 3.62 m, wave period 1.5 s, wave height 0.2 m. The grid was locally refined in the free-surface zone; in the finest zone extending over the range of free-surface motion, the cell size was mm, corresponding to ca. 116 cells per wavelength and 25 cells per wave height. The grid was

9 S. Enger, M. Perić & H. Monteiro sucessively coarsened with the growing distance from the free surface in both directions; see Fig. 4 for a detail image of the grid around the location x = 20 m, from where the grid was extruded with a growing streamwise size towards the outlet. The grid contains in total 61,345 cells. Since the propagation of undisturbed waves generates practically no turbulence, the flow was assumed to be laminar. Figure 4. Detail of computational grid in the vicinity of free surface (the grid was first generated in the range from 0 to 20 m and then extruded for another 7 m with a growing spacing in x-direction). The computation was performed using linear upwind scheme for convection fluxes, central-differencing scheme for diffusion fluxes, and quadratic backward scheme for time derivative (all being second-order approximations). In the equation for volume fraction of water, the convection flux was discretized using a special high-resolution interface-capturing (HRIC) scheme which is designed to keep the interface sharp. As can be seen from Fig. 5, the interface is indeed resolved by one cell, i.e., at any location, there is only one cell in vertical direction which is partly filled with water. The quadratic interpolation in time requires due to the sharp interface resolution that the interface moves less than half a cell per time step, in order to avoid overshoots or undershoots; the time step was therefore set to s, which means 300 time steps per wave period, i.e., the interface propagates roughly 39% of a cell size per time step. Five iterations were performed per time step, and the under-relaxation parameters were 0.5 for pressure and 0.9 for velocities and water volume fraction. The flow was initialized with the theoretical solution, but the effect of initialization disappears after 10 periods since the size of the solution domain is only 7.5 wavelengths. The forcing is applied over one wavelength next to the inlet and over two wavelengths next to the outlet, so that at both ends the theoretical flow solution is imposed (here the Stokes 5 th -order waves were generated following the theory by Fenton, 1985). This was done in order to assess the effect of discrepancy between the numerical solution of the Navier-Stokes equations and theory, which becomes significant after a few wavelengths due to discretization errors that accumulate along the propagation direction. In Fig. 6, the computed free surface shape after 10 periods is compared with the theoretical one. At the inlet, the computed solution corresponds to the theoretical one, as expected. Few wavelengths further downstream, there are some differences in both amplitude and phase: the amplitude of the computed wave is slightly lower and the period is slightly shorter than the theoretical values. However, since the grid and time step are fine enough, the

10 Coupling of different numerical solutions discrepancy is not too large and the forcing source terms can adapt the solution to the theoretical one without any visible disturbances. In the case of a significantly coarser grid and time step, or a longer solution domain so that a significant discrepancy is present where the forcing starts, smearing of the free surface can be expected (since over a few cells discretized equations would tend to deliver empty cells while theory predicts full cells, or vice-versa). When 3D flows are computed, the resolution of waves is likely to be worse, so imposing forcing at outlet or side boundaries may introduce undesirable effects. Figure 5. Distribution of volume fraction of water inside the solution domain after 15 s (10 wave periods). Figure 6. Comparison of computed and theoretical distribution of volume fraction of water inside the solution domain after 15 s (10 wave periods). 3.2 Wave impact onto a vertical cylinder In this test case, the wave impact on a vertical cylinder with a circular cross-section is examined. The cylinder diameter is 1 m and the parameters of the 5 th -order Stokes wave are: wavelength 3.2 m, wave height 0.2 m, wave period s. The solution domain was selected relatively small, so that the effects of wave reflection at boundaries are better visible: it is 9.2 m long and 6.4 m wide, with the cylinder axis being 3.8 m downstream of the inlet. The water depth was m and the cylinder was submerged 4 m, leaving a gap of m

11 S. Enger, M. Perić & H. Monteiro between the bottom of the cylinder and the bottom of the channel. Above the free surface, the cylinder was extended to a height well above the highest wave peak. The flow was assumed to be turbulent and the standard k-ε turbulence model with wall functions was used. Figure 7. Computational grid in a longitudinal cross-section through cylinder center, also showing distribution of volume fraction after 4 wave periods (flow from right to left). Figure 8. Computational grid in a horizontal cross-section through cylinder within free-surface zone, also showing distribution of forcing coefficient (blue: 10, red: 0; flow from right to left). The grid was locally refined around the cylinder and in the free-surface zone; one horizontal and one vertical section are shown in Figs. 7 and 8. There were 1.6 million cells altogether and the Stokes 5 th -order wave was resolved with 80 cells per wavelength and 20 cells per wave height. Further away from the cylinder the grid was kept coarse in lateral direction, since the flow is practically two-dimensional there; the longitudinal and vertical resolution was kept the same everywhere in order to avoid any disturbance of the propagating wave that could result from a grid change (see Fig. 8).

12 Coupling of different numerical solutions The solution of the 3D Reynolds-averaged Navier-Stokes equations was forced towards the undisturbed background flow according to Stokes 5 th -order theory (Fenton, 1985) along all vertical boundaries. The forcing zone was 1.2 m wide at the inlet, 2.4 m wide at the outlet, and 1.6 m wide at the lateral boundaries (see the distribution of the forcing coefficient in Fig. 8). The theory was also used to initialize the solution. The computation was also performed using the usual boundary conditions: specified Stokes wave conditions at inlet, symmetry condition at side boundaries and wave damping over a zone 2.4 m wide at the outlet boundary. It is expected that the waves generated by the cylinder will reflect off inlet boundary, which represents a major problem when the solution domain size is not large enough or simulation time is very long. The forcing is expected to damp the upstream-propagating waves before they reach the inlet boundary, thus allowing for long-lasting simulations to be performed on a reduced-size solution domain. This is especially important when the incoming waves are irregular and possible extreme events need to be captured reliably; disturbances by reflections from boundaries must then be eliminated. The predicted free surface shape in the longitudinal cross-section through the solution domain after 4 wave periods is shown in Fig. 9 together with the theoretical profile from the background flow, which would be obtained if the cylinder was not present. It can be seen that the computed free surface shape differs from theory around the cylinder, while it gradually merges with theory within the forcing zone next to both the inlet and the outlet boundary. Figure 9. Computed distribution of water volume fraction in a longitudinal cross-section through the cylinder, also showing the undisturbed theoretical free-surface shape. Figure 10 shows the computed free-surface shape when forcing is not applied, but the usual boundary conditions are specified instead. Several problems can be observed in this solution: firstly, the free-surface shape near the inlet does not correspond to the theory, neither in the symmetry plane nor at the side boundaries. This is due to the upstream-propagating circular waves generated by the cylinder, which reflect at both inlet and side (symmetry) boundaries. The disturbance is clearly seen in Fig. 11, which shows the whole free surface for both simulation approaches. The second problem is that the damping zone of 2.4 m is too short to damp the Stokes wave completely as it approaches the outlet boundary. Experience shows that the optimal damping zone length is around two wavelengths, which would require making the solution domain significantly longer since the damping zone cannot start too close to cylinder.

13 S. Enger, M. Perić & H. Monteiro Figure 10. Computed distribution of water volume fraction in a longitudinal cross-section through the cylinder (upper) and along the side boundary (lower) with standard boundary conditions, also showing the undisturbed theoretical free-surface shape. Figure 11 shows the comparison of the complete free surface after four periods, computed using the two approaches. While the solution is still very similar near the cylinder, differences are clearly visible near the inlet boundary. With longer lasting simulation, these disturbances would grow and eventually affect the solution around cylinder as well when using a traditional approach (boundary conditions with wave damping, but without forcing). Figure 11. Computed free surface shape after four wave periods: using forcing towards Stokes theory along all vertical boundaries (left) and using inlet, symmetry and outlet boundary conditions with wave damping (right). 3.3 Vortex shedding behind a cylinder in a channel Another situation where forcing towards a simpler solution can be useful is when vortex shedding behind a body occurs. The shed vortices usually retain their strength over a considerable distance, making it difficult to specify appropriate boundary conditions at the

14 Coupling of different numerical solutions outlet boundary. The usual practice is to prescribe constant pressure at outlet boundaries, or to extrapolate the velocity and enforce the flow rate. The former is obviously not appropriate since pressure is not constant when vortices are present; the latter is also not suitable since portions of the outlet boundary involve flow into the solution domain due to vortices crossing it. While it is possible to derive special convective boundary conditions which allow vortices to cross the boundary, they are not easily implemented for free-surface flows and reflection of pressure or free-surface waves is still possible. In this test case, the applicability of the forcing approach to one such problem is investigated. The geometry and the numerical grid are shown in Fig. 1. The cylinder diameter is 0.2 m, the channel width is 0.65 m and the cylinder distance to the bottom wall is 0.2 m. The channel is 4.5 m long, with the cylinder being positioned 1.5 m away from the inlet. The flow is two-dimensional and laminar, and the Reynolds number based on mean velocity in the channel upstream of the cylinder and the cylinder diameter is 200. A steady uniform flow is specified at inlet, side boundaries are no-slip walls, while at outlet either a constant pressure is specified or forcing towards a uniform flow (neglecting the presence of walls) is applied over a distance corresponding to 1.5 channel widths next to the outlet boundary. The polyhedral grid is locally refined around the cylinder in order to better capture flow separation and boundary layer effects. The prism layer at the cylinder wall has 180 cells along the perimeter and the first cell near wall has the thickness of 1/166 th of the cylinder diameter. The time step was set to 1/120 th of the period of lift oscillation (on average 1/60 th of drag oscillation period). Second-order schemes were used for all approximations. The underrelaxation parameters were 0.5 for pressure and 1.0 for velocities; 4 iterations per time step were performed. Since the solution domain is very long (15 diameters behind cylinder), the outlet boundary condition does not affect the force on cylinder, as shown in Fig. 12. Figure 12: Drag force on the cylinder, computed using forcing near outlet (red curve) and constant pressure boundary condition at outlet (black curve). The differences become obvious when looking at pressure and velocity distribution downstream of the cylinder, shown in Figs. 13 and 14. With outlet pressure boundary condition, the strength of vortices starts to oscillate as they get closer to the boundary. It can

15 S. Enger, M. Perić & H. Monteiro be seen in Fig. 13 that the third vortex upstream of the outlet boundary is stronger than the fourth (the pressure at its core is lower) while it can be expected that the vortices get weaker as they travel downstream due to viscous effects. When forcing towards a uniform flow is applied, the vortices gradually disappear within the forcing zone. The velocity field in Fig. 14 also shows the smooth transition towards uniform flow as the outlet boundary is approached. Figure 13: Computed pressure distribution in the channel after 20 s of simulation time: with constant outlet pressure as boundary condition (upper) and with forcing towards uniform flow (lower). Figure 14: Computed velocity distribution in the channel after 20 s of simulation time: with constant outlet pressure as boundary condition (upper) and with forcing towards uniform flow (lower).

16 Coupling of different numerical solutions 4 CONCLUSIONS Forcing the solution of the discretized Navier-Stokes equations towards another solution (theory, solution of simpler equations etc.) over certain distance is demonstrated to be a suitable approach to reduce the computing effort by being able to use reduced-size solution domain, or to avoid problems associated with reflections of pressure or free-surface waves at boundaries, owing to the damping feature of the gradual forcing. Future research is required regarding the choice of optimal forcing coefficient and its variation, as well as the optimization of interpolation when two numerical solutions need to be blended. Acknowledgements The authors acknowledge the help provided by Dr. J. W. Kim and co-workers from Technip through several discussions and exchanges of information and test cases in the course of this study. REFERENCES Choi J., & Yoon S. B., Numerical simulations using momentum source wave-maker applied to RANS equation model. J. Costal Engineering, vol. 56, pp Demirdžić, I., & Muzaferija S., Numerical method for coupled fluid flow, heat transfer and stress analysis using unstructured moving meshes with cells of arbitrary topology. Comput. Methods Appl. Mech. Engrg., vol. 125, pp Fenton, J. D., A fifth-order Stokes theory for steady waves. J. Waterway, Port, Coastal, Ocean Eng., vol. 111, pp Ferziger, J.H., & Perić, M., Computational Methods for Fluid Dynamics, 3 rd ed., Springer. Hadžić, I., Hennig, J., Perić, M., & Xing-Kaeding, Y., Computation of flow-induced motion of floating bodies. Appl. Math. Modelling, vol. 29, pp Kim, J.W., Kyoung, J. H., Ertekin, R. C., & Bai, K. J., Finite-element computation of wave-structure interaction between steep Stokes waves and vertical cylinders. J. Waterway, Port, Coastal, Ocean Eng., vol. 132, pp Kim, J. W., O Sullivan, J., & Read, A., Ringing Analysis on a Vertical Cylinder by Euler Overlay Method. OMAE Launder, B. E. and Spalding, D. B., The numerical computation of turbulent flows. Comp. Meth. Appl. Mech. Engng, vol. 3, pp Muzaferija, S., & Perić, M., Computation of free surface flows using interface-tracking and interface-capturing methods. In Mahrenholtz, O. & Markiewicz, M., eds., Nonlinear Water Wave Interaction, pp ,WIT Press. Weiss, J., Maruszewski, J.P., & Smith, W.A., 1999: Implicit solution of preconditioned Navier-Stokes equations using algebraic multigrid. AIAA J., vol. 37, pp