J. Shanghai Jiaotong Univ. (Sci.), 2016, 21(5): 530-540 DOI: 10.1007/s12204-016-1759-3

Numerical Investigation of Characteristics of Water-Exit Ventilated Cavity Collapse QIN Nana∗ (

),

LU Chuanjinga,b (),

LI Jiea,b (

)

(a. School of Naval Architecture, Ocean and Civil Engineering; b. MOE Key Laboratory of Hydrodynamics, Shanghai Jiaotong University, Shanghai 200240, China)

© Shanghai Jiaotong University and Springer-Verlag Berlin Heidelberg 2016 Abstract: The collapse of the ventilated cavitation occurring on a cylindrical vehicle during the water-exit is numerically researched. The numerical model employs the finite volume method to solve the multiphase Reynoldsaveraged Navier-Stokes (RNNS) equations and uses the volume of fluid (VOF) method to capture the free surface. A practical water wave environment that the vehicle usually encounters is reproduced in a numerical wave flume, so that the water wave’s effect on the cavity collapse flow regime is investigated. The main feature of the waterexit collapse of a ventilated cavity is studied under the wave-free condition. The result indicates that a collapsing ventilated cavity experiences two stages, in which the pattern of cavity evolution is different. In the early stage, the cavity undergoes a rapid shrinkage as a closed body. In the late stage, the cavity releases gas from the front due to the increase of the cavity pressure. The water wave effect is investigated at three typical wave phases: the wave crest, the wave trough and the wave node. Results show that when the vehicle is launched under the wave node, the cavity collapse regime remains fairly axisymmetric and is similar to the wave-free case. However, when the vehicle is launched under the wave crest and trough, the cavity evolution presents highly three-dimensional (3D) features. The results of predicted cavity size, pressure distributions and hydrodynamic forces at different wave phases show that the wave effect is relatively weak at the wave node but becomes apparent at the wave crest and trough. Key words: water-exit, ventilated cavitation, cavity collapse, water wave effect CLC number: O 359.1 Document code: A

0 Introduction Artificial cavitation, or ventilation, is produced by injecting air into the low pressure region of the liquid flow. The primary purpose of generating such a flow regime is to reduce drag on the underwater moving bodies[1] . Ventilation decreases the near-wall density by replacing the liquid with a layer of gas, so that the friction can be greatly reduced and much higher body speed is attainable. When artificial cavitation is applied to an underwater vehicle which is designed to move through the water surface (such as an underwater-launched missile), a severe hydrodynamic problem arises. The cavity experiences an abrupt collapse during the water-exit. Very large impact load can be generated on the vehicle body[2] , and it makes impact on the body motion and increases the risk of structural damage. Understanding of the water-exit cavity behavior and the mechanism of Received date: 2015-11-17 Foundation item: the National Natural Science Foundation of China (Nos. 11102109 and 11472174) ∗E-mail: [email protected]

the impact load is important to the design and operation of underwater launched vehicles. However, the collapse of a water-exit cavity is a complicated multiphase flow. The highly unsteady and nonlinear nature of this problem brings challenges. The difficulty is further increased when the cavity collapse regime is coupled with the sea conditions in which the vehicle is operated. As the vehicle is approaching and moving through the water surface, the effect of water waves becomes significant. The interaction between the cavity and waves can dramatically affect the cavity evolution and the body surface pressure distributions. Reliable prediction of the water-exit cavity behavior and the impact load requires the practical water wave conditions taken into account. The water-exit problem has been studied for decades. Most of the research was under the non-cavitating condition. Moran[3] studied the problem of a slender symmetric body in uniform vertical motion through the free surface with a linear theory. The results are valid for large Froude numbers. Berdan and Leal[4] analytically solved the problem of a sphere translating normal to the interface. Lu[5] obtained the solution of a

J. Shanghai Jiaotong Univ. (Sci.), 2016, 21(5): 530-540

slender axisymmetric body vertically moving through an air-water interface under the assumption of inviscid flow. His solution is valid for arbitrary values of Froude number. The primary challenge of the multiphase flow calculation is to fulfill the nonlinear boundary conditions on the deformable free surface, which is unknown a priori. These theoretical approaches usually solve this problem by linearizing the free surface boundary conditions, and thus their solutions are only satisfactory for small free surface deformations. Different numerical methods can be used to directly treat the nonlinear free surface boundary condition. The commonly used methods are the boundary element method (BEM) based on potential theory and the computational fluid dynamics (CFD) based on the Navier-Stokes equations. Liju et al.[6] researched the surge effect during the water-exit of an axisymmetric body traveling normal to the water surface by both the experiments and the BEM simulations. They found that the free surface deformations could be accurately predicted for large Reynolds numbers. However, there are some computational difficulties when applying the BEM simulation to the problems involving large free surface deformations. For instance, the formation of thin jets and sprays always causes the calculations to break down. The CFD methods are generally more robust than the BEM to solve the violent water flow. Cai et al.[7] used the marker and cell method and the finite difference scheme to simulate the viscous flow around a flat-nosed cylinder vertically exiting water. Hu et al.[8] employed the volume of fluid (VOF) method to simulate the free surface evolution induced by a vertically launched semi-infinite cylinder. Wang et al.[9] simulated the underwater launch process of a vehicle subjected to natural cavitation. Based on the numerical results, they proposed a physical model of the pressure induced by cavity collapse. This work employs the finite volume method and the VOF method to model the multiphase flow of the waterexit cavity collapse, which serves two main purposes:  to research the main feature of the water-exit collapse of a ventilated cavity and study the mechanism of the impact pressure’s formation;  to investigate the variation of the water-exit flow regimes when the vehicle is launched in a water wave environment and examine the wave effect on the cavity evolution, the body surface pressure distributions and the hydrodynamic forces.

1 Problem Description The underwater-launch process of a vehicle is simulated. The axisymmetric vehicle consists of a conical nose (45◦ cone half angle) and a cylindrical after-body. The vehicle is vertically traveling at a constant speed U = 30 m/s. Non-condensable gas is injected from a nozzle located near the leading edge of the body with

531

constant flow rate. The air supply starts when the forebody is one body length beneath the undisturbed water surface. The problem is described in the earth-fixed frame of reference, as schematically shown in Fig. 1, where x and y are the lateral and axial coordinates, and g is the gravitational acceleration. The origin of time is set as the instant when the air injection starts.

Fig. 1

Schematic of the earth-fixed coordinate system

Let the body radius r, the vehicle speed U , the atmospheric pressure patm and the water density ρl be the characteristic scales. The non-dimensional variables, such as length, area, volume, time, velocity, pressure and force, are defined as follows: l A V l∗ = , A∗ = 2 , V ∗ = 3 , r r r t u ∗ ∗ , u = , t = r/U U p − p F atm p∗ = , F∗ = . 1 1 ρl U 2 ρl U 2 r 2 2 2 The non-dimensional air injection mass flow rate dem ˙ fined as m ˙∗ = is given a value of 0.002 in this ρl U r 2 paper. A regular wave field is reproduced based on the practical sea condition the vehicle usually encounters. The used wave parameters are: wave height H = 2.5 m, wavelength L = 75 m and wave period τ = 7 s.

2 Numerical Model 2.1 Governing Equations The VOF model is adopted to develop the differential equations of three species, i.e., liquid, vapor and noncondensable gas. Hereinafter, the subscripts g, v and l represent the non-condensable gas, vapor and liquid phases, respectively. Individual volume fraction equations are provided for the transport and generation of each phase. The ideal gas model is employed to describe the compressibility of the gas. Single equations for momentum and energy scalars are solved in which the fluid properties are dependent on the volume fraction. The governing equations based on the conservation law of

532

J. Shanghai Jiaotong Univ. (Sci.), 2016, 21(5): 530-540

mass, momentum and energy are

∂ ∂ (ρE) + [ui (ρE + p)] = ∂t ∂xi  ∂T  ∂ keff , ∂xi ∂xi

(2)

ε ε2 C1ε Gk − C2ε ρ , k k (3)

where ρ, E and T are density, energy and temperature of the fluid mixture, respectively; μeff and keff are the effective dynamic viscosity coefficient and heat conductivity, respectively; the subscripts i and j represent the indices of the Cartesian coordinates. In Eqs. (1)—(3), all physical quantities are shared by three phases, in a general form as follows: φ=

αq φq ,

(4)

q=1

where αq is the volume fraction of the qth phase. The sum of volume fractions of all three phases is one, i.e. 3 

αq = 1.

(5)

q=1

The phase volume fractions satisfy the following transport equations: ∂ ∂ (αg ρg ) + (αg ρg ui ) = 0, ∂t ∂xi ∂ ∂ (αv ρv ) + (αv ρv ui ) = Re − Rc , ∂t ∂xi

Gk − ρε, ∂ μt  ∂ε  ∂ ∂  μ+ + (ρε) + (ρεui ) = ∂t ∂xi ∂xj σε ∂xj

(6) (7)

where Re and Rc are mass transfer rates between liquid and vapor due to evaporation and condensation, respectively. The cavitation model suggested by Zwart et al.[10] is used to determine the source terms Re and Rc as follows: ⎫  3αnuc αl ρv 2 pv − p ⎪ ⎪ ⎪ Re = Fevap ⎪ rB 3 ρl ⎪ ⎪ ⎪ ⎪ ⎬ p  pv , (8)  ⎪ 3αv ρv 2 p − pv ⎪ ⎪ Rc = Fcond ⎪ ⎪ ⎪ rB 3 ρl ⎪ ⎪ ⎭ p > pv where αnuc is the nucleation site volume fraction; rB is the bubble radius; Fevap and Fcond are the coefficients of evaporation and condensation, respectively.

(9)

(10)

where k, ε and μ are turbulent kinetic energy, turbulence dissipation rate and viscosity, respectively; σk and σε are turbulent Prandtl numbers; Gk represents the turbulent kinetic production rate; C1ε and C2ε are empirical constants. The turbulence viscosity is determined by k2 μt = Cμ ρ , (11) ε where Cμ is a constant coefficient. 2.2 Numerical Wave Flume The configuration of the numerical wave flume is schematically illustrated in Fig. 2. A numerical wave maker is established at the inlet boundary of the computational domain by prescribing the wave surface height and the inflow velocities based on the theoretical solutions of the target wave. A numerical damping zone is arranged before the outlet boundary so as to remove the wave reflection. In the damping region, the wave-absorbing momentum source terms proposed by Zhou et al.[11] are employed as follows: Sx = ρ[C(x) − 1]× u  ∂u ∂ux  x x − ux + uy − Δt ∂x ∂y Sy = ρ[C(x) − 1]× u  ∂u ∂uy  y y − ux + uy − Δt ∂x ∂y

1 ∂p  , ρ ∂x

(12)

 1 ∂p −g , ρ ∂y

(13)

where C(x) is a weighted function that smoothly varies from one to zero along the damping zone; ux and uy are lateral and axial velocities, respectively. y Wave inlet

∂(ρui ) ∂(ρui uj ) ∂p + =− + ∂t ∂xj ∂xi  ∂u ∂uj  ∂  i + μeff + ρg, ∂xj ∂xj ∂xi

3 

μt  ∂k  ∂ ∂  ∂ μ+ + (ρk) + (ρkui ) = ∂t ∂xi ∂xj σk ∂xj

(1)

x Computational region

2 — 4 wavelengths Fig. 2

Damping zone

Larger than 2 wavelengths

Schematic of the numerical wave flume

Outlet

∂ρ ∂(ρui ) + = 0, ∂t ∂xi

The turbulence effect is modeled by the k-ε model. The model equations are as follows:

J. Shanghai Jiaotong Univ. (Sci.), 2016, 21(5): 530-540

1.0

0.6

Table 1 Mesh series

0 −0.2 0

Mesh parameters

Nnose

Ncylinder

Ntail

Coarse

80

270

80

Medium

120

360

120

Fine

160

560

160

Finest

240

750

240

The time histories of the axial force coefficient CF calculated with four meshes are presented in Fig. 3. Apparently, the magnitude of the force coefficient obtained with the “coarse” mesh is under-predicted. Figure 4 presents the comparison of the surface pressure coefficient distribution along the body surface, where s∗ is the non-dimensional axial distance. It seems that neither the “coarse” mesh nor the “medium” mesh is adequate to accurately capture the pressure peak at the cavity closure region. However, the curves are close to each other for the “fine” and “finest” cases. 0

Coarse Medium Fine Finest

CF

− 0.2 − 0.4 − 0.6 − 0.8 −1.0 0 Fig. 3

2

4

6

0.4 0.2

3 Mesh Convergence Analysis The accuracy of the numerical result is greatly influenced by the quality of the grid. In this section, the mesh convergence is analyzed based on the axisymmetric flow of the body exiting from calm water. Four sets of meshes with incremental fineness are investigated, as shown in Table 1, where Nnose , Ncylinder and Ntail represent the amount of mesh nodes on the vehicle’s nose, cylindrical section and tail, respectively.

8 10 12 14 16 18 20 t*

Comparison of axial force coefficients calculated with different meshes

Coarse Medium Fine Finest

0.8

p*

2.3 Numerical method The pressure-based segregated SIMPLE algorithm is employed to solve the equations. First order upwind scheme is used for the convective terms in both the momentum equation and the turbulence quantity equations. Geometric reconstruction scheme is adopted to estimate the convective term in the phase fraction equation. The gradients are computed by Green-Gauss cell based method. Finally, the first order implicit scheme is used for the temporal discretization.

533

Fig. 4

2

4

6 s*

8

10

12

Transient pressure coefficient distributions on body surface predicted with different meshes

It suggests that the accuracy of the “fine” mesh is satisfactory. Based on the grid parameters of this case, a three-dimensional (3D) computational mesh is composed of about 2 million structured grids which are generated for the calculation of the water-exit flow in a wave field, as shown in Fig. 5. Dynamic mesh techniques such as the sliding interfaces and dynamic layers are employed to accomplish the body motion. y O zx

Fig. 5

Sketch of the 3D computational mesh

4 Results and Discussions 4.1 Water-Exit Under Wave-Free Condition Figure 6 provides a series of predicted cavity shapes, selected streamlines and body surface pressure distributions at several typical instants of the water-exit process. The flow regime forms at large submersion depth, as shown in Fig. 6(a). We find that a high pressure region appears on the fore-body, which accelerates the liquid in the radial direction off the vehicle. A large recirculation zone is formed behind the body’s leading edge for the cavity development. The natural cavitation effect is dramatically limited by the ventilation. Vapor appears only in the small area near the leading edge of the body, as shown in Fig. 7, where r∗ represents the non-dimensional radial distance. Figures 6(b) and 6(c) show that the pressure on the fore-body drops with the reduction of the submersion depth. It leads to the crash of the separation zone and the contraction of

534

Fig. 6

J. Shanghai Jiaotong Univ. (Sci.), 2016, 21(5): 530-540

Predicted cavity shapes, streamlines and body surface pressure distributions at several instants of the water-exit process

J. Shanghai Jiaotong Univ. (Sci.), 2016, 21(5): 530-540

535

1.1

70

0.2

60

t*=8

0.1

r*

50 1.0

p*

V*

40 0 30

0.9

αv 0.05 0.15 0.25 0.35 0.45 0.55 0.65 0.75 0.85 0.95 Fig. 7 Contour of the vapor phase volume fraction

s*

20

− 0.1

10 − 0.2 2 4 6 8 10 12 14 16 18 20 22 24 26 t* Variations of the cavity volume and cavity pressure with time

0 Fig. 8

t* = 16.0 t* = 16.4 t* = 16.8 t* = 17.0 t* = 17.5 t* = 18.0 t* = 18.5

0.7 0.6 0.5 0.4 p*

0.3 0.2 0.1 0 −0.1 −0.2 0

0.5 0.4 0.3

2

4

6 8 10 12 s* (a) Early stage of cavity collapse t* = 20.0 t* = 20.4 t* = 20.7 t* = 21.0

t* = 21.5 t* = 22.0 t* = 23.0

0.2 p*

the cavity’s front section. Figure 6(d) captures the first appearance of the impact pressure, which is triggered when the water film covering the cavity is collapsing on the wall. During this process, the front end of the cavity is re-created. The impact pressure pulse moves along the wall with the shrinking cavity. The cavity pressure rises with the volume compression due to the noncondensable and elastic nature of the gas content. In Fig. 6(f), the cavity pressure exceeds the atmospheric value. This instant can be regarded as a critical point that divides the cavity collapse into the early stage and the late stage. After that, a new pattern of collapse arises, as shown in Figs. 6(g) and 6(h). The gas tends to escape the cavity from the front end where it encounters the weakest resistance. The front section of the cavity becomes a blurry area, which diminishes the impact pressure. The shed air pockets experience a rapid expansion, and the pressure inside the pockets drops dramatically. The strongly rotational flow induced by air pockets produces high pressure at the frontiers of the pockets where the streamlines hit the wall. Thus the shed air pockets become a main source of dynamic load in the late stage of cavity collapse. Figure 8 presents the time histories of the predicted cavity volume and cavity pressure. Two curves show perfect reverse trends to each other. The cavity experiences a re-growth process. It demonstrates the important role of the elastic nature of the gas content in the cavity evolution, especially in the late stage of cavity collapse. Figure 9 provides a series of predicted body surface pressure distributions. It shows that the feature of pressure distribution is quite different in the two stages of cavity collapse. In the early stage, the cavity evolves as a closed body and is bounded by two distinct ends. A sharp impact pressure appears at the cavity’s front end and sweeps over the wall with the shrinking cavity. In the late stage, the air release diminishes the impact pressure. Pressure oscillations appear at the frontiers of the shed air pockets. The shed air pockets tend to be attached on the vehicle, so a relatively stable pressure distribution is produced in the late stage of cavity

0.1 0

−0.1 −0.2 0

Fig. 9

2

4

6 8 10 s* (b) Late stage of cavity collapse

12

Variation of body surface pressure distributions during the cavity collapse

collapse. 4.2 Water-Exit Under Water Wave Conditions In this work, the second-order Stokes wave theory is used to describe the wave surface elevation η, the velocity field ux and uy , and the pressure distribution

536

J. Shanghai Jiaotong Univ. (Sci.), 2016, 21(5): 530-540

under the wave surface. H πH H cos Φ + × 2 8 L 2πd   cosh 4πd L + 2 cos 2Φ, cosh 2πd L sinh3 L 2π(y + d) πH cosh L ux = cos Φ+ 2πd T sinh L 4π(y + d) 3π2 H 2 cosh L cos 2Φ, 4LT 4 2πd sinh L 2π(y + d) πH sinh L uy = sin Φ+ 2πd T sinh L η=

4π(y + d) 3π2 H 2 sinh L sin 2Φ, 4LT 4 2πd sinh L p = patm − ρl gy+

(14)

Fig. 10

Schematic of the surface deformation, velocity and pressure distributions at the wave crest, node and trough

(15)

(16)

2π(y + d) cosh 1 L ρl gH cos Φ+ 2πd 2 cosh L 1 πH 3 ρl gH × 4πd 4 L sinh L ⎛ ⎞ 4π(y + d) cosh 1⎟ ⎜ L − ⎠ cos 2Φ− ⎝ 3 2 2πd sinh L   1 4π(y + d) πH 3 ρl gH − 1 , (17) cosh 4πd 4 L L sinh L where d is the water depth and Φ is the wave phase angle defined as x t − . (18) Φ = 2π L τ Note that the time and length scales of the wave motion are much larger than those of the local flow around the body. The wave phase angle variation throughout the water-exit is about 0.1π, a rather small value. Such a narrow wave phase window makes it possible to discuss “the wave effect at a certain wave phase”. The wave conditions generated at three typical wave phases (crest Φ = 0, node Φ = π/2 and trough Φ = π) are taken into account, as shown in Fig. 10.

4.2.1 Wave Effect on Cavity Evolution For the wave node case, the transient flow regime around the vehicle when it reaches the wave surface is presented in Fig. 11. It shows that the cavity shape is almost symmetric relative to the body on the direction of wave propagation. The distributions of the pressure and streamlines also show good axisymmetric feature. Such a good symmetry can be produced because the wave-induced velocity under the wave node is in the vertical direction which is parallel to the body axis. The subsequent cavity collapse presents slightly nonsymmetric feature, which is due to the interaction between the cavity and the oblique wave surface, as shown in Fig. 12. The oblique wave surface causes larger area

Fig. 11

Predicted cavity shape, streamlines and pressure distributions for the wave node case at t∗ = 14

Fig. 12

Cavity evolution during the water-exit at the wave node

J. Shanghai Jiaotong Univ. (Sci.), 2016, 21(5): 530-540

of the cavity exposed to the atmospheric pressure on the low water level side, and thus the cavity’s leading edge gradually inclines along with the slope of the wave surface. However, the non-symmetry induced by the oblique water surface is still secondary to the global axisymmetric feature. In contrast, the wave-induced velocity under the wave crest is in the same direction as the wave propagation, which causes the incoming flow relative to the body deviated from its axis. The angle of attack increases with the reduction of the submersion depth. The non-symmetric effect has apparently emerged when the body reaches the crest surface, as shown in Fig. 13. On the up-wave side, the streamlines are more parallel to the wall, and thus compress the low pressure region. While on the back-wave side, the more curved streamlines create larger low-pressure region for the cavity development. Both the thickness and length of cavity are increased on the back-wave side. The re-entrant jet reflects at the oblique closure line and increases its transverse velocity component. Liquid is swept back underneath the cavity pocket and gathers on the back-wave side, which generates a thick water layer lying between the air pocket and the wall, as shown in Fig. 14. Figure 15 presents the cavity evolution when the vehicle moves through the wave crest surface. The nonsymmetric feature of the cavity is further increased dur-

Fig. 13

Predicted cavity shape, streamlines and pressure distributions for the crest case at t∗ = 14

Fig. 14

Sketch of the 3D behavior of the re-entrant jet induced by an inclined cavity closure line

537

ing the collapse process. The whole cavity body moves to the back-wave side. The re-entrant jet penetrates the cavity’s leading edge and pushes the cavity away from the vehicle’s surface. The transverse velocity induced non-symmetry also presents in the wave trough case, in which the vehicle undergoes a velocity in the opposite direction of the wave propagation. Particularly, as the transverse velocities beneath the crest and trough are almost equal in magnitude, the non-symmetric features of the cavity in these two cases are expected to be similar. Figure 16 illustrates the cavity evolution during the waterexit stage at the wave trough. Comparing Fig. 16 with Fig. 15, we find that the cavity shapes generated at the crest and trough are approximate mirror images to each other on the direction of wave propagation.

Fig. 15

Cavity evolution during the water-exit at the wave crest

Fig. 16

Cavity evolution during the water-exit at the wave trough

It is clear that the flow non-symmetric effects induced by the oblique water surface and by the transverse velocity are quite different in strength. The former is generated indirectly via the asymmetric dynamic free surface boundary condition. It becomes apparent until the cavity is sufficiently close to the wave surface. In contrast, the latter effect is basically kinetic and it affects the cavity shape evolution more directly throughout the entire underwater-launch process. Therefore, the water-exit flow regime exhibits much stronger 3D feature at the wave crest and trough. The influence of the water wave on the cavity size is shown in Fig. 17. It is well known that the cavity development is dependent on the cavitation number which

538

J. Shanghai Jiaotong Univ. (Sci.), 2016, 21(5): 530-540

is defined as σ=

p − pc , 0.5ρl U 2

(19)

where pc is the cavity pressure. Combining Eq. (19) and Eq. (17) gives the approximated expression of cavitation number under wave condition: 2π(y + d) ρgη cosh patm − pc − ρgy L + σ= , 1 2 1 2 2πd ρV ρV cosh 2 2 L

water (covering the cavity) film. Lu and Li[2] proposed a simplified model of water impact which relates the strength of impact pressure with the magnitude of the radial velocity Ur of the collapsing water film as follows: pcollapse = Kρl Ur2 ,

(21)

where K is an empirical coefficient. Figure 20 illustrates the transient radial velocity distribution on a water film

(20) 0.5

where the second term represents the wave effect’s firstorder approximation about wave height, and it is proportional to the water surface displacement. Thus, the cavity growth is accelerated beneath the wave trough and slowed down beneath the wave crest, and the wave effect on cavity development is rather trivial in the wave node case, as shown in Fig. 17. On the other hand, the water surface displacement changes the distance of underwater travel; the time for cavity growth is extended in the case of wave crest and is reduced in the case of wave trough. As a result, the maximum cavity volume generated in different wave phase cases is approximately equivalent. 60

40

p*

0.3

0.1 −0.1 2 3 4 5

t*

6 7 8 9 10

Crest Trough Node No wave

0

1 2

3

4

11 5

V*

Up-wave side, Fig. 18

20

6 s*

7

8 9 10 11 12

Back-wave side

Body surface pressure distributions versus time in the wave node case

0.5 0

4

8

12

16

20

24

28

0.3

0.1

Cavity volume variations at different wave phases

4.2.2 Wave Effect on Pressure Distribution Figure 18 compares a series of body surface pressure distributions on up-wave side and back-wave side in the wave node case. It seems that the pressure magnitude and variation pattern are similar on two sides. Sharp impact pressure peaks are observed in the early stage of cavity collapse, and the pressure oscillations associated with the shed air pockets present in the late stage. It demonstrates that the flow regime of cavity collapse at the wave node remains fairly axisymmetric and is very similar to the wave-free case. For the case of wave crest, the amplitude of the impact pressure acting on the up-wave side is much sharper than that on the back-wave side, as shown in Fig. 19. It is known that the impact pressure is generated during the collision between the wall and the

−0.1 2 3 4 5 6 7 8 9 10 11 12 13 14

t*

Fig. 17

p*

t*

0

1 2

3 4

5

6 7 8 9 10 11 12 s* Up-wave side, Back-wave side

Fig. 19

Body surface pressure distributions versus time in the wave crest case

J. Shanghai Jiaotong Univ. (Sci.), 2016, 21(5): 530-540

539

section before it collapses on the wall. It shows that the radial velocity magnitude decreases dramatically from the up-wave side to the back-wave side due to the radial component of the wave-induced transverse velocity. Another interesting feature shown in Fig. 18 is that the impact pressure almost disappears on the back-wave side. It is caused by the re-entrant jet which acts as a “cushion” separating the collapsing cavity from the vehicle’s surface. For the case of wave trough, the flow regime is similar to the crest case but reversed in the x-axis. Thus the pressure distribution presents similar non-symmetric feature, and the strength of the impact pressure decreases on the up-wave side. The predicted results are given in Fig. 21.

4.2.3 Wave Effect on Hydrodynamic Forces The time histories of the axial and lateral nondimensional hydrodynamic forces acting on the vehicle at different wave phases are presented in Fig. 22. The results obtained in the wave free case are also provided as a comparison. The wave effect is relatively weak at the wave node but becomes significant at the wave crest and trough. Especially for the lateral force component, its magnitude increases with time and exhibits largeamplitude oscillations. Such strong transverse oscillations are corresponding to the highly non-symmetric flow regimes generated at the wave crest and trough. 0.2 0

y Fy*

− 0.2 ux cosθ

− 0.6

ux O

θ

− 0.4

− 0.8 0

ux sinθ

2

4

6

8 10 12 14 16 18 20 22 24 26 t*

2

4

6

8 10 12 14 16 18 20 22 24 26 t* Trough, Node, No wave

x 0.8

Up-wave side

Back-wave side

0.6

Fx*

0.4

Fig. 20

Radial velocity distribution on a collapsing water film section for the wave crest case at t∗ = 18

0.2 0 − 0.2 − 0.4 0

0.5

Crest,

p*

0.3 0.1

t*

−0.1 1 2 3 4 5 6 7 8 9 10 11 12 13

0

1 2 3 4

5

Up-wave side, Fig. 21

6 7 8 s*

9 10 11 12

Back-wave side

Body surface pressure distributions versus time in the wave trough case

Fig. 22

Time histories of the axial and lateral nondimensional hydrodynamic forces

5 Conclusion In this work, a numerical model based on the finite volume method and the VOF method is developed to simulate the water-exit flow of an axisymmetric vehicle subjected to artificial cavitation. The primary feature of the water-exit collapse of a ventilated cavity is investigated. A numerical wave flume is constructed to reproduce a practical wave environment, so that the wave effects on the cavity evolution, pressure distributions and hydrodynamic forces are investigated. (1) The collapse of a ventilated cavity may experience two stages. In the early stage, the cavity evolves as a closed body. A sharp impact pressure is generated at the front end of the cavity. In the late stage, the cavity releases gas from the front due to the increase of

540

the cavity pressure. The cavity experiences a re-growth phase at the end of the collapse process. The predicted cavity behavior is related to the non-condensible and compressible nature of the gas content. (2) When the vehicle is launched at the wave node, the cavity evolution and the pressure distributions are quite similar to the wave-free case. The non-symmetric effect induced by the interaction between the cavity and the inclined wave surface is rather weak. However, when the vehicle is launched from the crest and trough, the transverse velocity can produce highly nonsymmetric flow regimes. The 3D behavior of the reentrant jet enhances the non-symmetry of the body surface pressure distributions. Thus large-amplitude oscillations of the transverse hydrodynamic force occur during the water-exit at the wave crest and trough, which can make notable impact to the body motion.

References [1] MATVEEV K I. On the limiting parameters of artificial cavitation [J]. Ocean Engineering, 2003, 30(9): 1179-1190. [2] LU C J, LI J. Research on the collapse process and characteristics of water-exit cavity of underwater vehicle [C]//Proceeding of the 11th National Congress on Hydrodynamics & 24th National Conference on Hydrodynamics and Commemoration of the 110th Anniversary of Zhou Peiyuan’s Birth. Beijing: Ocean Press, 2012: 54-67 (in Chinese). [3] MORAN J P. The vertical water-exit and -entry of slender symmetric bodies [J]. Journal of the Aerospace Sciences, 1961, 28(10): 803-812.

J. Shanghai Jiaotong Univ. (Sci.), 2016, 21(5): 530-540 [4] BERDAN C, LEAL L G. Motion of a sphere in the presence of a deformable interface: I. Perturbation of the interface from flat: The effects on drag and torque [J]. Journal of Colloid and Interface Science, 1982, 87(1): 62-80. [5] LU C J. The vertical water exit and entry of a slender axisymmetric body [J]. Journal of Hydrodynamics, 1990, 5(4): 35-41 (in Chinese). [6] LIJU P Y, MACHANE R, CARTELLIER A. Surge effect during the water exit of an axisymmetric body traveling normal to a plane interface: Experiments and BEM simulation [J]. Experiments in Fluids, 2001, 31(3): 241-248. [7] CAI J H, HE Y S, YE Q Y. Numerical simulation of the viscous flow around a flat-nosed cylinder during its vertical water exit [J]. Journal of Hydrodynamics, 1990, 5(2): 115-121 (in Chinese). [8] HU Y Y, ZHU K Q, Xi B S. Numerical simulation of a semi-infinite cylinder exited from water [J]. Journal of Tsinghua University, 2002, 42(2): 235-238 (in Chinese). [9] WANG Y W, HUANG C G, DU T Z, et al. Mechanism analysis about cavitation collapse load of underwater vehicles in a vertical launching process [J]. Chinese Journal of Theoretical and Applied Mechanics, 2012, 44(1): 39-48 (in Chinese). [10] ZWART P J, GERBER A G, BELAMRI T. A twophase flow model for predicting cavitation dynamics [C]// Proceedings of Fifth International Conference on Multi-phase Flow. Yokohama, Japan: [s. n.], 2004: 152. [11] ZHOU Q J, WANG B L, LAN Y M, et al. Numerical simulation of wave overtopping over seawalls [J]. Chinese Quarterly of Mechanics, 2005, 26(4): 629-633 (in Chinese).