Changhong Hu,Mohamed M.Kamra

Research Institute for Applied Mechanics, Kyushu University, Fukuoka, Japan

Abstract:An unstructured mesh Reynolds-averaged Navier-Stokes(RANS)solver has been developed for numerical simulation of violent sloshing flows inside a tank with complicated inner structures.The numerical solver employs the unstructured multi-dimensional tangent hyperbolic interface capturing method (UMTHINC)for free-surface capturing combined with various turbulence models.The sloshing motion is numerically modeled using the body-force method which introduces a source term into the momentum equation corresponding to the tank motion profile. Numerical simulationsof the tank sloshing problems are performed for different test cases with various oscillation frequencies.The performance of the interface capturing method has been discussed and the effect of turbulence model choice on loading predictions is highlighted by studying several RANSmodels and analyzing its effect on fluid motion and impact pressure. Numerical simulationsof thesloshing inside the tank with a vertical baffle hasalso been conducted and a discussion isprovided on different numerical treatment of thebaffle.

Key words:Unstructured mesh RNASsolver,UMTHINCscheme, violent sloshing flow

Introduction

Violent sloshing phenomena inside a tank has been an important hydrodynamic problem for several decades in ship and ocean engineering research field.Such sloshing flows are generally strongly non-linear,in-homogeneous,and three-dimensional.The sloshing loads are significantly affected by violent flow phenomena such as impact,wave breaking,and splashes.Experimental studies have been widely used to get a better understanding of such flows.However,it is often difficult to correctly scale all the physics involved and extend the obtained results to full scale.Moreover,experimental studiesrequire a hugeamount of time,and are limited to relatively simple cases with simplified geometries[1-2].Computational fluid dynamics(CFD)method is considered as an efficient tool for study of such violent sloshing problems,in which the Navier-Stokes equations are solved using finite difference,finite volume or more recently finite element discretization methods.A suitable method for treating the moving interface(free surface)is employed to handle the multi-fluid system.

Turbulence models are of particular importance for violent sloshing simulation.A discussion on this has been made by Liu et al.[3]in which the laminar approach,the turbulent approach including Reynolds averaged Navier-Stokes equations (RANS)model,large eddy simulations(LES),and very large eddy simulations (VLES),are compared.The choice of the turbulence model plays a critical role in obtaining accurate numerical solutions.Sufyan et al.[4]has applied a dynamic mesh-adaptation algorithm based on an unstructured mesh to solve sloshing problems by a finite element method.The study shows that dynamic adaption can reduce the computational cost by at least half.However,the relative mass error cannot be negligible when the base grid resolution is insufficient.

Free surface treatment is another key research issue on the sloshing simulations.Multi-phase model has to be used for violent sloshing CFD.An accurate and non-diffusive interface capturing scheme is essentially important for long-term simulation.Level set (LS)method and volume of fluid (VOF)method are two popularly used interface capturing methods.LS method uses the signed distance function to track the interface identified by the zero level-set contour.The method provides high accuracy in curvature computation for surface tension dominated flows as well as the easy application of the boundary conditionsat the interface as in the case of single-phase free surface flows.However,original level set methods don’t guarantee mass/volume conservation thus cause the disappearanceof tiny droplets.Many improvements have been proposed to treat this issue by applying re-distancing/re-initialization of the level set field[5],introducing conservation formulation or simply coupling the method with a VOF method[6].Recently extension of the method to unstructured meshesare also carried out[7-8].VOF method is currently the most widely used interface capturing scheme,for which a volume fraction field ranging between zero and one is introduced.The volume fraction signifies the ratio of the volume of fluid in a computational cell so it serves as a means of identifying each fluid in the field.VOF methods are generally classified into two main categories,the geometric VOF methods[9]and the algebraic VOF methods[10].

The purpose of this study is to conduct numerical simulation of violent sloshing flows inside a tank with complicated inner structures.Due to the irregular body boundaries,unstructured mesh method is preferable.Although most of the commercial CFD codes are unstructured mesh based,we decided to develop our own unstructured mesh code because we want to apply up-to-date interface capturing schemes in order to achieve better performance on violent free surface computation.The scheme implemented in our code is the unstructured multi-dimensional THINC (UMTHINC)scheme[11].The THINC(tangent hyperbolic interface capturing)was proposed by Xiao et al.[12],which is a different approach of the algebraic VOF methods,utilizing a tangent hyperbolic function to reconstruct the volume fraction field.The methods provide a conservative advection scheme in which interface jump thickness can be controlled and maintained throughout the time evolution by a single parameter.The method was originally proposed for uniform Cartesian grids,later it was successfully extended to unstructured triangular and tetrahedral meshes[13]and quadrilateral and hexahedral meshes[14].In the UMTHINC method,a formulation for prismatic and pyramid cells was recently introduced making the method fully applicable to all cell shapes in unstructured meshes.Now the quality of the results produced by the method is quite competitive with other VOF methods with hardly any complexity during implementation on unstructured meshes.

In this paper,at first the governing equations and numerical method are described.Then,the model problem and computational grid used in this work is provided followed by the validation and case results discussion.Finally,some concluding remarks on improvementsand further research are made.

1.Governing equations and numerical method

The numerical computations are carried out using the in-house developed CFD code based on the finite-volume discreti-zation of the incompressible Navier-Stokes equations.Details about the method can be found in Ref.[15].The Reynolds averaging approach is applied to the Navier-Stokes equations for turbulence modeling,resulting in the following governing equations.

To calculate the turbulent eddy viscosity,three turbulence models are employed for turbulence closurein the RANSapproach,Standard -k εmodel,Realizable -k ε model,and Wilcox-k ωmodel.Their performances are investigated in this paper by using a tank sloshing case.

In our numerical model,the volume of fluid method is used for the time evolution of the free surface.In the VOF method,different fluids are assigned each an indicator (color)function ( , )C t x which has a value of one inside the fluid and zero otherwise.In the finite volume discretization,the volume fraction αis defined as the volume average of the indicator function over thecomputational cell.

whereΩdenotes the cell volume.The one-fluid model is adopted in this work.Therefore,the material properties in the fluid are updated based on the volumefraction as

The UMTHINC scheme is employed for the treatment of the free surface.The method ensures sharp interface at the free surface while maintaining simple and efficient implementation even for hybrid unstructured grids.In this method,the interface jump is defined as a smoothed piecewise hyperbolic tangent profile,so the indicator function is now approximated as

In the present method,the three-dimensional incompressible turbulent flow is solved using the non-iterative time advancement pressure-implicit with splitting of operator (PISO)algorithm with 4 neighbor correction and one non-orthogonality correction steps during each time step to ensure that both the continuity and momentum equations are satisfied.For more details on the method,the reader is referred to Ref.[17].For the time discretization of the momentum equation a second order three level time implicit scheme is applied.For the convection term the second order total variation diminishing (TVD)limited linear upwind scheme is used with the Sweby limiter[18].The cell-based Green-Gauss gradient method is used to compute the velocity and pressure gradients.

The treatment of the temporal,convection,and diffusion term for all the transportation equations,including the momentum equations and the turbulence field equations,is conducted in a similar manner.However,in turbulence field equations,the source terms can either be treated implicitly or explicitly.A convention method[19]is that the source term is treated implicitly when it has a negative sign so it would contribute to the improvement of the stability and convergence of the underlying linear system of equations by increasing the matrix’s diagonal dominance.For the same reason,the source term is treated explicitly if it hasa positivesign.

The finite volume formulation of the VOF function is written as

2.Model problem and computational grid

In this paper,two simple sloshing problems of a rectangular tank are studied,the first is for the purpose of validation and examination of the numerical method while the second is for demonstration and further discussions.In both problems,water and air at 20°C are selected as the liquid and gas inside the rectangular tank, respectively.

Fig.1 (Color online)Geometry and pressure sensor locationsfor the rectangular tank sway case[24]

The second numerical example is for demonstration purpose,in which the above-mentioned tank model is modified by introducing a vertical baffle with a thickness of 6mm at =0x and a height flushing with the free surface.The effect of the vertical baffle on the reduction of impact pressure is examined.The numerical treatment of the baffle is also investigated by considering the finite thickness(actual case)approach and the zero thickness (shell)approach on the numerical accuracy and computational efficiency of the solution.Despite the possibility of using structured mesh for this test case,a 2-D hybrid unstructured mesh is generated to assess the accuracy and efficiency of the developed in-house code.The generated mesh contains 20 quadrilateral layers attached to the walls of the tank,with the thickness of 0.5 mm for the first layer to ensure sufficient resolution of the boundary layer.Triangular cells are used for the remaining region of the domain,as shown in Fig.2.During mesh generation,attention is directed to the region around the free surface to ensureenough resolution of theinterface.

Fig.2 A 2-D unstructured grid for the validation test case

3.Validation and discussion

We first examine the performance of the proposed unstructured mesh code by comparing to the experiment.The case with the shorter motion period,case A with T =1.74 s ,is chosen for this purpose since it represents a more violent phenomena.In the following numerical results,the UMTHINC sharpness parameter βis set to 6.This choice is based on many numerical experiments which emphasize on temporal numerical stability while maintaining high accuracy and sharp interface capturing[15].

The effect of turbulence model choice on the accuracy of the numerical results is investigated.Examination of the governing equation for the three RANSmodels considered in this work shows that the realizable-k εis slightly more computationally expensive than the other two models.This can be attributed to the additional computations necessary to evaluate Cμ,which has been discussed in Ref.[15].

Comparison of the pressure time-history is depicted in Fig.4 which confirms our previous findings and shows that the realizable -k εmodel gives a shorter impact duration when compared to the other models.The Wilcox -k ωmodel and the standard -k εmodel give very close predictions with the-k ωmodel being more accurate when compared to experimental data.Based on those results,the-k ω model isused for simulation of case B.

Fig.3 (Color online) A comparison of the turbulent fluctuation field

For case B,Fig.5 shows the instantaneous free surface profile from the numerical simulation when compared with the experimental video snapshots at approximately the same time instant within the motion cycle(period).Theagreement isvery good in termsof the general freesurface shape.

Figure 6 shows a comparison of the pressure time-history with the experimental data.The overall qualitative and quantitative agreement is very good especially for the two pressure spikes where the first spike represents the sloshing liquid impacting the side wall and the second spike represent thesloshing liquid collapsing after it had climbed the wall.

4.Tank sloshing with vertical baffles

Fig. 4 (Color online) A comparison of the turbulent fluctuation field

Since the final goal of the present research is to develop an unstructured mesh code to simulate the violent sloshing flows inside a tank with complicated inner structures,it is necessary to study the numerical treatment of the inner structures(baffles).As a preliminary investigation,we study a tank sloshing problem by introducing a 6 mm vertical baffle at the center line of the rectangular tank.The excitation motion used in this test case has an amplitude of 0.06 m and a period of 1.94 s.The results are then compared to a zero-thickness approximate baffle model to check the effect of baffle thickness on the sloshing flow.The shell baffle model allows for simpler grid generation even with complex internal structures.It further allows for easier implementation of flexible baffle cases where baffle displacement/ deflection can be done by simply perturbing the vertices coinciding on the baffle and its surrounding layers thus avoiding grid regeneration and providing some performance savings.

Two unstructured gridsare generated in a manner similar to the previous validation case.The baffle is also fitted with 20 quadrilateral layers to provide accurate resolution of the boundary layers as shown in Fig.7.The grid for the finite thickness baffle case is comprised of 108.8K cells whilethe approximate shell baffle case is nearly 101.65K cells for nearly identical grid resolution over thedomain.

In Fig.8,a comparison of the pressure field for the two baffle cases as well as the free surface depicted by a thick black contour line is presented.The figure shows very similar behavior in the region surrounding the baffle where significant air pockets and bubbles are observed.Although the free surface profile seems qualitatively similar, a clear difference in thestatic pressure field is observed between the two cases.The shell baffle case seems to significantly over-predict the pressure field especially in the region of the wall that is being impacted by the wave.

Fig.5 (Color online) Comparison of the 2-D free surface profile at selected time instants for case B

Further examining the pressure time-history is given by Fig.9,which clearly showsthat,as expected,the vertical baffle has significantly suppressed the impact pressure at the side wall.Thefigure also shows the shell baffle approximation gives 50%higher impact pressure than the finite thickness case.Phase difference is also observed in the pressure time evolution between the two considered approaches.In order to explain this numerical behavior,however,it is necessary to compute more test cases for larger and smaller thickness baffles with the shell baffle case being a limiting/asymptotic case.

Fig.6 (Color online)Comparison of the pressure time-history for case B

Fig.7 (Color online) A 2-D unstructured grid,associated with local enlarged graph of the plate tip

5.Conclusions

Fig.8 (Color online)Comparison of the pressure field at selected time instants

Fig.9 (Color online) Comparison of the pressure time-history on thesidewall at P2 for the finitethicknessbaffle case

The final goal of the present research is to develop an unstructured mesh code to simulate the violent sloshing flows inside a tank with complicated inner structures. In this paper, our newly developed twophase turbulent flow solver based on UMTHINC method has been described.Some preliminary numerical results on 2-D numerical simulation of an experimental case with a rectangular tank are presented and discussions on the performance of the proposed numerical model are made by comparing to the experiment.It has been shown that the UMTHINC method ensures sharp interface at the free surface while maintaining simple and efficient implementation even for hybrid unstructured grids.Examining several RANS turbulence models confirms nonnegligible turbulent fluctuations in both water and air.Although all turbulence models give fairly good agreement for the pressure time-history with experiment data,the-k ωmodel is found to give the best matching.The numerical results are validated against experimental data thus demonstrating very good agreement both qualitatively and quantitatively.As expected,introducing a vertical baffle to rectangular tank managed to significantly suppress the pressure impacts,especially the peaks,on the tank walls.Although the approximated shell baffle approach is able to qualitatively give a similar free surface profile as the finite thickness baffle approach,significant difference is observed for the pressure prediction which warrants additional investigations.Important issues for future research include further investigation of the baffle thickness on the predicted pressure,modeling air compressibility and the buffer effect of bubblesand air pocketson load predictions.

Acknowledgement

This research was supported by Nippon Kaiji Kyokai(ClassNK).