Study of a Body Subjected to a Vertical Drop into Water – Experiment and Simulations

(1)

Study of a Body Subjected to a Vertical

Drop into Water – Experiment and

Simulations

Josefin Andersson & Monika Englund

Mechanical Engineering, master's level

2018

Luleå University of Technology

(2)

Abstract

In computational fluid dynamics (CFD), the computational domain can be discretized using mesh-based methods or particle mesh-based methods. During this project; a CFD method that uses smoothed particle hydrodynamics (SPH), in which the computational domain is discretized by particles, is modelled and compared to mesh-based CFD methods, in which the domains are broken into a set of discrete volumes. The aim with this master thesis project is to determine whether the SPH method can replace mesh-based methods in cases that involve free surface flows and fluid-structure interac-tions (FSI’s) in order to avoid mesh-deformainterac-tions. The comparison is done by studying a free fall of a torpedo shaped object, 500 mm in length, both experimentally and with numerical simulations. The CFD methods that are compared are mesh-based one-way FSI, mesh-based two-way FSI and the SPH method. The methods are created in the two simulation software ANSYS (one-way and two-way FSI) and LS-DYNA (two-way FSI and SPH).

The comparisons are made by looking at experimental and numerical accelerations. The experiment gave uncertain results and there were difficulties in comparing experimental results to numerical results. When looking at all results, it is concluded that the mesh-based methods give reasonable maximum values while the SPH method gives too high values.

For the mesh-based methods in ANSYS, air is present which is not the case for the methods mod-elled in LS-DYNA. When comparing the computation time for all methods, it is concluded that the presence of air increases the computation time considerably and based on the results in this project, air is not necessary to take into consideration.

The aim of this project is reached by concluding that the mesh-based method in LS-DYNA is the most suitable method for the studied case, based on the following: acceleration behaviour, maximum acceleration values, computation time and the possibility to neglect air. The conclusion might be revised when future work on the SPH method has been done.

(3)

(4)

Acknowledgements

Writing this thesis has been both interesting and rewarding. We have learnt a lot but without the help from a number of people this thesis work would have been impossible. These people have con-tributed to our master thesis in many different ways and it is a pleasure to thank those who made it possible.

We want to thank: Bo Axelsson regarding the design of the experimental body; Mikael ˚Akerlind and Nils Hjertner who manufactured the experimental body; Thomas Johansson and Marcus Tim-gren at the LS-DYNA support (DYNAmore Nordic support team) for help with LS-DYNA; Emma Ekbladh for information regarding ANSYS; Maria Pettersson, James Melander and Kristian Erlands-son for the indispensable help with the measuring equipment; Anders EdeErlands-son for equipment necessary for the experiment and Anders Rydell for information about torpedoes.

We especially want to thank our supervisors Erik Storg¨ards and Karl Storck at Saab Dynamics, for all the aid and support given to us. Last but not least, we want to thank our examiner Gunnar Hellstr¨om for all the help during the past five months.

JOSEFIN ANDERSSON MONIKA ENGLUND June 2018

(5)

List of Abbreviations

2D Two dimensional 3D Three dimensional

ALE Arbitrary Lagrangian-Eulerian CAD Computer-aided design CFD Computational fluid dynamics CV Control volume

EOS Equation of state FDM Finite difference method FEM Finite element method FSI Fluid structure interaction FVM Finite volume method

ICFD Incompressible computational fluid dynamics PDE Partial differential equation

PID Part ID

(9)

(10)

1 Introduction

The project described in this report is a master thesis project made by two mechanical engineering students in collaboration with the defence company SAAB Dynamics AB. Different numerical simulation methods have been used to simulate an object, in the shape of a torpedo, falling freely in air and hitting a water surface that causes a large stir of the fluid. The simulation of this fluid structure interaction (FSI) between the object (structure) and the water (fluid) is performed by a computer using computational fluid dynamics (CFD). The behaviour of the structure is studied through CFD in order to estimate the load that the structure is subject to when impacting the water surface. This information is of great importance since the structure has to be designed to withstand the applied load from the water impact, without breaking and/or significantly deforming.

CFD is a tool to virtually generate a solution for a physical phenomenon where fluid flow is involved. The fluid flow is described by partial differential equations (PDE’s) that can not be solved analytically except in very special cases. The PDE’s constitute a mathematical model of the physical problem. An approximate numerical solution of the PDE’s are obtained by applying a discretization method which approximates the PDE’s by a system of algebraic equations. These equations can then be solved on a computer. The approximations are applied to small domains in space and/or time, the numerical solution therefore provides results at discrete locations in space and time [1, 2].

The most important discretization methods are: the finite difference method (FDM), the finite volume method (FVM) and the finite element method (FEM). The FD method is the oldest and easiest method to use. In this method, the solution domain is covered by a grid. At each grid point, the PDE’s are replaced by approximations in terms of the nodal values of the functions. This gives one algebraic equation per grid node, in which the variable value at that and a certain number of neighbour nodes appear as unknowns. In the FV method, the solution domain is subdivided into a finite number of contiguous control volumes (CVs) and the equations are applied to each CV. The FE method is very similar to the FVM; the solution domain is broken into a set of discrete volumes or finite elements. What is distinctive about the FE method is that the equations are multiplied by a weight function before they are integrated over the entire domain [1, 2]. The structure of the CFD project and its stages is visualized in Figure (1). Figure (2) shows a numerical solution, obtained from using CFD, of the velocity of fluid flow around a circle.

(11)

Figure 2: A two dimensional (2D) CFD solution of the velocity of fluid flow around a circle.

1.1 Background to this project

In CFD, FSI problems are generally modelled using methods in which the mesh of the fluid domain deforms to adapt to the solid domain deformation. This is costly and of complex implementation. Further, large fluid domain deformations can not be handled without re-meshing. Re-meshing increases the computational cost of simulations significantly [3]. Figure (3) shows a water splash caused by a stone falling into the water which causes a large stir of the fluid. Simulating this water splash will cause large fluid domain deformations. Other FSIs that will cause fluid domain deformations when modelled are for example hull slamming (which refers to the impact of the hull of a boat as it re-enters the water) and the water landing of an aircraft.

Figure 3: A water splash caused by a stone falling into water.

A different approach from the mesh-based methods is smoothed particle hydrodynamics (SPH) which is a fully mesh-free method that also is used to model fluid evolution in the context of FSI’s [3]. The problems of mesh distortion and the need to re-mesh is avoided with SPH. Different methods exist to model the structure responses in FSI problems when using SPH. One way is to adopt an SPH-FEM coupling where the structure makes up the FEM part and the fluid makes up the SPH part. Other ways are to model the structure as an SPH part as well, for example by modelling the structure with an elastic SPH model. In most numerical simulations for free surface flows, the air phase above the fluid surface is not considered when using the SPH method [4]. Figure (4) below shows an SPH model for an FSI problem where the air phase is neglected and where SPH-FEM coupling is used. The structure (the half sphere) consists of a gradient square-shaped mesh and the fluid consists of SPH particles [5].

(12)

Figure 4: SPH model of an FSI problem where SPH-FEM coupling is used. Figure from [5].

1.2 Aim

The aim of this master thesis is to investigate if the mesh-free CFD method SPH is better to use than classical mesh-based CFD for modelling problems that involve free surface flows and fluid-structure inter-actions, where the fluid domain undergoes large deformations; such as an object falling into water.

1.3 Project description

The project involves an experiment where a torpedo shaped body, a half meter in length, is released approximately 1 meter above the water surface. The size of the body is scaled for laboratory purposes, the size of a commercial torpedo is larger. The body is dropped several times at an angle of 30◦and then several times at an angle of 45◦. These angles are the angles of impact that the body has relative to the water surface. The angle of impact Θ is measured as in Figure (5).

Figure 5: Angle Θ of impact.

Looking at Figure (1), the physical problem that is to be simulated with different CFD methods in this project is the experiment. For all CFD methods, the mathematical model of the physical problem is the incompressible Navier-Stokes equations. The numerical solutions from the different CFD methods

(13)

are compared to data retrieved from the experiment in order to determine which of the methods that is the most preferable one, which is the aim with this project. The most preferable method is the method that gives satisfying results without having to use an unreasonable amount of computational power and calculation time. The CFD methods that are to be compared are mesh-based one-way FSI, mesh-based two-way FSI and the SPH method. In two-way FSI, the fluid impacts the structure and vice versa. In one-way FSI, the fluid is not impacted by the structure. The air phase is almost always neglected when applying an SPH method, so is the case for the SPH method modelled in this project as well. Though, it is of interest to see whether the neglect of the air phase alone has any significant impact on the result. Therefore, a mesh-based CFD method in which the air phase is neglected is also modelled.

A significant limitation during this project is the computational power. The limited amount of compu-tational power sets a lower boundary for the size of the discretized domains in the CFD models.

(14)

2 History of torpedoes

At the end of the 16th _{century, the first machine that resembles a torpedo was used. This machine was}

for a long time called a torpedo but have later changed name to a floating mine. Even so, the torpedo would never exist if the floating mine never was invented. It is said that the torpedo got its name from a fish with the same name. The torpedo fish gives enemies an electric shock which incapacitate them. This resembles the course of action of actual torpedoes [6].

The torpedoes of today are successors to a torpedo invented by Robert Whitehead in 1866. The biggest difference between Whiteheads torpedo and earlier inventions is that Whiteheads torpedo had propellers which made it possible for the torpedo to attack instead of waiting for the target [6, 7].

In the early years, the torpedo was dropped from a boat by hand in the exact direction of the location of the enemy, or at least of the location where the enemy was thought to be. Later on, the torpedoes have developed into controllable devices. This makes it possible to launch the torpedoes from different kinds of vehicles such as helicopters, aircraft, submarines and ships. At SAAB Dynamics the torpedoes are controlled by a wire, which makes it possible to navigate and change direction of the torpedo. This feature is important when the torpedo is used in shallow waters like the Baltic sea [8, 9].

Different manufacturers produce different torpedoes with different diameters, lengths and launch weights. Figure (6) shows a torpedo developed and manufactured by SAAB Dynamics.

Figure 6: A Torpedo 62 (TP62) [10].

A torpedo that launches from an aircraft can sometimes be equipped with a parachute. The parachute is used to slow down the torpedo before entering the water, which will reduce the force on internal components. If the parachute is neglected, the torpedo will experience high forces when entering the water and for some cases the force will damage internal components. This results in a torpedo that works incorrectly [9].

(15)

3 Theory

In this section, necessary theory for the CFD-simulations is presented. The simulation software that have been chosen to model the different CFD methods are ANSYS, which will be used to model mesh-based one-way and two-way FSI methods, and LS-DYNA, which will be used to model a two-way FSI method and an SPH method.

3.1 Governing equations for fluid dynamics

The governing equations for fluid dynamics are based on the following three physical laws of conserva-tion:

• Conservation of Mass: Continuity Equation,

• Conservation of Momentum: Momentum Equation of Newton’s Second Law, • Conservation of Energy: Energy Equation.

The governing equations state that mass, momentum and energy are stable constants within a closed system; what comes in, must go out somewhere else. The movement of a fluid can be investigated using either the Lagrangian description or the Eulerian description. The first description mentioned is based on the theory to follow an individual fluid particle from the beginning of the movement to the end. The coordinates at time t0 and the coordinates at time t1for the individual fluid particle has to be examined.

In the Eulerian method no specific particle is followed, instead, the velocity field is examined as a function of time and position. Figure (7) demonstrates the difference between the two approaches well. In the Lagrangian approach, the location of every point is taken up at the beginning of the domain and the path of each point is traced until the end. In the Eulerian method, a CV within the fluid is considered and the particle flow within the CV is analysed [2].

Figure 7: The difference between a Lagrangian and an Eulerian approach. The figure is inspired from a figure in [2].

The SPH method is a fully Lagrangian method [3] while the mesh-based methods (used in this thesis project) use an arbitrary Lagrangian-Eulerian (ALE) formulation. Section (3.2) below explains the ALE formulation for the mesh-based methods further.

3.2 FSI in the mesh-based methods

All information in this chapter is from the ANSYS documentation, referenced in [11], and from the LS-DYNA ICFD theory manual, referenced in [12].

In both ANSYS and LS-DYNA a partitioned (or staggered) method is available for FSI problems. In the partitioned method, fluid and solid equations are uncoupled which allows for using specifically designed

(16)

codes on the different domains. With this method smaller and better conditioned subsystems are solved instead of a single problem.

In ANSYS, fluid equations can be solved with the software ANSYS CFX and the structural equations can be solved with the software ANSYS Mechanical. ANSYS CFX is a CFD software tool that uses an element-based FV method to solve the partial differential equations. ANSYS Mechanical is a mechanical engineering program for structural analysis. Both ANSYS CFX and ANSYS Mechanical use an implicit time integration solver. For an explanation about implicit (and explicit) time integration, see for example [13]

In LS-DYNA, fluid equations can be solved by the built in ICFD (Incompressible CFD)-solver and the solid equations are solved by the mechanical solver. The ICFD-solver uses the FE method for solving the system of differential equations. LS-DYNA offers two schemes in the partitioned approach, these are the weakly coupled scheme and the strongly coupled scheme. In the weakly coupled scheme, the mechanical solver uses explicit time integration and in the strongly coupled scheme, the mechanical solver uses implicit time integration. The ICFD-solver always uses implicit time integration. The weakly and strongly coupled schemes are explained below.

In weakly coupled schemes only one solution of either field per time step, in a sequentially staggered manner, is required. This makes the explicit scheme appealing regarding efficiency, but when the ”added-mass effect” is significant the scheme becomes unstable. Added ”added-mass or virtual ”added-mass is the inertia added to a system because an accelerating or decelerating body must move some volume of surrounding fluid as it moves through it. The same physical space can not be occupied simultaneously by the object and the fluid. In literature the name added-mass effect indicates the numerical instabilities that typically occur in the internal flow of an incompressible fluid whose density is close to the structure density.

For strongly coupled schemes, the fluid and solid variables at the interface need to converge. After an iterative process, a strongly coupled scheme gives the same results as non-partitioned schemes. Implicit schemes are however, just like explicit ones, subjected to the added mass effect. Since the strongly coupled scheme is still a partitioned approach, convergence may still be a challenge for some problems.

For both ANSYS and LS-DYNA, the data transfer between the fluid and the solid must be on wall boundaries. Data transfer cannot take place in the free stream. The CFD analysis in both programs is fully Eulerian while the boundaries between solid and fluid are Lagrangian and deform with the structure. Hence, an ALE formulation is achieved for the mesh-based methods in ANSYS and LS-DYNA

The interaction between ANSYS CFX and ANSYS Mechanical is shown in Figures (8) and (9). Figure (8) shows the interaction in one-way coupling while Figure (9) shows the interaction in two-way coupling. In the one-way coupling, the CFD-analysis transfers the pressure to the FE-analysis while the FE-analysis doesn’t transfer anything to the CFD-analysis. In the two-way coupling, a force is transferred from the CFD-analysis to the FE-analysis. This force is based on the pressure from a wall boundary in CFX. The pressure is relative to the specified reference pressure. The displacement transferred the other way around in the two-way FSI represents the incremental displacement for the current time step.

(17)

Figure 8: The interaction between ANSYS CFX and ANSYS Mechanical in one-way FSI.

Figure 9: The interaction between ANSYS CFX and ANSYS Mechanical in two-way FSI. Figure (10) below gives a simplified overview of the two-way coupling and interaction between the ICFD-solver and the mechanical ICFD-solver in LS-DYNA. In cases of strong FSI coupling the ICFD-solver will, after the first time step, solve the fluid equations. The forces computed will then be transferred to the solid mechanics solver that will return the node displacements as boundary conditions for the fluid solver. The procedure is repeated until convergence has been reached.

Figure 10: The interaction between the ICFD-solver and the mechanical solver in LS-DYNA. The figure is inspired by a figure in [12, p.27].

3.3 Mesh-based CFD in ANSYS

(18)

3.3.1 Multiphase flow and Free Surface flows

In a multiphase flow each fluid may possess its own flow field or they share a common flow field. ANSYS CFX has a variety of different multiphase models where multiple fluid streams, bubbles, droplets, solid particles and free surface flows are some of them. A multiphase flow in ANSYS CFX is either an Eulerian-Eulerian multiphase model or a Lagrangian Particle Tracking multiphase model. The Eulerian-Eulerian-Eulerian-Eulerian multiphase model is divided into the sub-models homogeneous and inhomogeneous. For the homogeneous model the fluids share the same velocity field and for the inhomogeneous model each fluid has separate velocity (and other fluid quantities) fields. The most common application of the homogeneous multiphase flow is the free surface flow model.

3.3.2 Meshing and re-meshing of the fluid domain

The mesh program in the ANSYS suite is called ANSYS Meshing. ANSYS Meshing is integrated within every solver in ANSYS and chooses mesh options based on the type of analysis and geometry. ANSYS Meshing can mesh both three dimensional (3D) bodies and 2D bodies.

For two-way FSI in ANSYS, the fluid domain can not be re-meshed because re-meshing is not sup-ported.

3.4 Mesh-based CFD in LS-DYNA

The theory presented in this section is from the LS-DYNA ICFD theory manual. 3.4.1 Free surface flows

The ICFD-solver in LS-DYNA uses a level set method to track and represent moving interfaces. An implicit function φ is defined throughout the whole computational domain where the zero isocontour, φ = 0, of this function represents the interface. The isocontour defining the interface is one dimension lower than the implicit function. As a convention, the fluid domain where the Navier-Stokes equations will be solved is defined by φ > 0 and the vacuum is defined by φ < 0. The implicit function φ is in other words a distance function to the interface.

The implicit function is used both to represent the interface and to evolve the interface. The evolution of the implicit function is defined with the simple convection equation

∂φ ∂t

− →

V ·−→∆φ = 0 (1) in which−→V is the fluid velocity.

3.4.2 Meshing and re-meshing of the fluid domain

An automatic volume mesher for fluid domains is used in the ICFD-solver which simplifies the pre-processing stage. A good quality body fitted surface needs to be provided for the automatic volume meshing to function well. The surface must consist of 2D triangles.

The mesh building steps are described below.

• Step 1: the surface nodes and elements given by the user are read by the solver. The determined surfaces are not allowed to overlap. No gaps or open spaces between the surface boundaries and duplicate nodes are allowed to exist. Each surface element must also be orientable which means that a normal vector defining the interior/exterior faces can be associated to each of the surface elements.

• Step 2: if the conditions in step 1 are not met the solver returns an error. If the conditions are met the solver continues by joining the initial surface nodes in order to build an initial volume mesh. • Step 3: after the initial volume mesh is built the solver progressively adds nodes to the volume

mesh. Every time a new node is added, its ”host” tetrahedra/triangle will be divided into smaller tetrahedra/triangles. This procedure is repeated until the desired size of the volume elements is

(19)

reached. The size is based on a linear interpolation of the surface sizes that define the volume enclosure.

The default setting for the ICFD-solver in LS-DYNA is that it only rebuilds the CFD mesh if elements get inverted but it is possible to trigger a re-meshing of elements that have been distorted by the mesh movement algorithm and that no longer meet the initial mesh size.

3.5 SPH in LS-DYNA

The SPH model requires a different calculation method than mesh-based methods. In absence of a grid, the particles are the computational framework on which the governing equations are resolved. The general SPH formulation is briefly explained in Appendix. The theory presented in this chapter is from the SPH section in the LS-DYNA theory manual, referenced in [14].

3.5.1 Calculation cycle

The calculation cycle for an SPH simulation in LS-DYNA is shown in Figure (11):

Figure 11: SPH calculation cycle. The figure is inspired from a figure in [14, p.38.6].

A simple and classical first-order scheme for integration in the calculation cycle is used. The time step is determined by the expression

δt = CCF LM ini hi ci+ vi (2) where the factor CCF L is a numerical constant.

(20)

using a bucket sort. The sort is performed within the boxes which means that the closest neighbours of a specific particle will be in the same box as the specific particle or in the boxes closest to the box that the specific particle resides in. With this method the number of distance calculations are reduced and therefore also the CPU time.

3.5.2 Geometrical and physical properties

Initially, the set of particles created will have two kinds of properties: physical and geometrical. The physical properties are mass, density and constitutive laws. The geometrical properties decides the initial placement of the particles. For this, two different parameters need to be fixed: ∆xilengths and the CSLH

coefficient. The CSLH coefficient is a constant applied to the smoothing length of the particles.

The SPH mesh must be as regular as possible. As an example, Mesh 1 is better than Mesh 2 in Figure (12) since Mesh 2 contains too many inter-particle distance discrepancies. Mesh 1 is more uniform and therefore better.

Figure 12: Mesh number 1 is more uniform than mesh number 2. Figure is from [14, p.38.7]. 3.5.3 Finite element coupling

As for the finite element coupling, finite elements and SPH elements are coupled by using contact algo-rithms. Any ”nodes to surface” contact type can be used as long as the SPH elements constitute the slave part and the finite elements constitute the master part. As an example, the half sphere in Figure (4) must be the master part.

(21)

4 Experiment

The experiment involves the water impact of an object in the form of a down-scaled and simplified torpedo. The experimental setup is shown in Figure (13) and the object is shown in Figure (14). The experiment results in accelerations from two accelerometers that are compared with the accelerations numerically calculated in ANSYS and LS-DYNA. The accelerometers are installed at different locations inside of the object and they give the acceleration for the experimental body at the position of the accelerometer. A camera is mounted on the side of the water tank and takes snapshots over the water impact.

Figure 13: Experimental Setup. The object is seen hanging above the water surface.

Figure 14: The experimental body.

The dimensions of the measurements A-C shown in Figure (14) are specified in Table (1) where the shell thickness and weight of the body also are defined. The weight of the body is measured with a dynamometer. The experimental body will be dropped into an indoor pool which is 3600x4800 mm and 3400 mm deep.

(22)

Table 1: Geometrical dimensions of the experimental body A [mm] B [mm] C [mm] Thickness [mm] Weight [kg] 500 70 R10 5 1.8

Figure (15) below shows the different parts that make up the experimental body.

Figure 15: The different parts that the experimental body consists of: a back lid (1), a pipe (2), four rulers (3) and a front lid (4).

Five accelerometers from the manufacturer PCB with product number 352C33 are used. They have a sensor constant of 100 mV/g-force. Four of the accelerometers are mounted to two rulers that are attached inside the walls of the body and the last one is mounted to the inside of the front lid. The placement of the accelerometers are shown in Figure (16) together with the accelerometer measuring directions drawn as arrows. The placement of the accelerometers are also shown in Figure (17) viewed from the ”front” with the front lid removed. Experimental data is saved for all five accelerometers. The accelerometers give the absolute acceleration in one direction.

Figure 16: A cross section drawing of the experimental body showing the accelerometer positions and measuring directions. The measurements are in mm.

(23)

Figure 17: The placement of the accelerometers viewed from the front. The front lid has been removed.

4.1 Equipment

Except for the experimental body and the five one-dimensional accelerometers, the equipment used for the experiment is:

• a GoPro camera and a MicroSD card,

• a portable data acquisition system called Siemens LMS SCADAS XS and a MicroSD card, • the data acquisition application LMS Smart scope used for the LMS SCADAS XS, installed on a

Huawei tablet,

• necessary cables and adapters for the accelerometers and the LMS SCADAS XS, • ropes.

The GoPro camera is used to capture the water impact of the body. The snapshots are saved in a microSD card inside the camera. The LMS SCADAS XS is a portable data acquisition system. This system gives the accelerometers the right amount of voltage that they need in order to function and it also handles the data before the data is saved to a MicroSD-card installed inside the system. With the application LMS Smart scope on the tablet, the output together with sensor constants for each of the accelerometers are set. The output for the accelerometers is acceleration in g-force. The sample rate is set to 51200 Hz. The cables and adapters are used to transfer the signals from the accelerometers to the data acquisition system. Ropes are used for hanging the body above the water surface and for adjusting the position and impact angle of the body. Two ropes are used for securing the body to the bridge.

4.2 Setup and Execution

(24)

Figure 18: An explanatory figure over the experimental setup.

The cables from the accelerometers exits the body through the back lid and are connected to the data acquisition system. When all of the accelerometers are attached to the right position, the back and front lid are firmly attached to the body with thread tape. The thread tape is used as a means to water proof the body. The body is hung to an overhead crane by a rope that is slung over the crane. Two different impact angles are set with two ropes. The impact angles are 30◦ and 45◦. The distance between the water surface and the body is one meter. Figure (18) shows where the experimental body is initially located with respect to the water surface.

When the rope slung over the crane is released, the experimental body will launch towards the water. The velocity of the body right before it enters the water is calculated to be 4.43 m/s with the equation v =√2gh. This velocity is true when the air resistance is neglected. The true velocity will be lower but it is assumed that difference between calculated and true velocity will have a negligible impact on the experimental results. The data collection starts ten seconds before the rope is released. The body is released five times for each impact angle and the data collecting procedure is the same for every release. The ropes that are used for securing the experimental body to the bridge are seen in Figure (18) as ”safety rope”. These ropes stop the body from falling to the bottom of the pool and from fully submerging into the water. Two ropes are used for this in case one of the ropes would break.

(25)

5 CFD methods

The CFD methods that have been used to simulate the experiment, described in Chapter (4), are pre-sented in this chapter. In the mesh-based method in LS-DYNA, the air will be modelled as vacuum which means that the air phase is neglected. In ANSYS, vacuum can not be modelled. Two different mesh sizes will be used in the simulations for each of the CFD methods in order to study grid convergence.

5.1 Computer data

Two identical computers have been used for running the simulations during this thesis project. The computers have an Intel®Xeon® processor with the process number E5-1607 V4, 4 cores and a clock rate of 3.10 GHz. All analyses are made on a SSD hard drive on each of the computers and the computers have 32 GB in installed memory (RAM).

5.2 Models

The 3D models that are used for each of the different CFD methods are described below. All models are created in the ANSYS built-in computer-aided design (CAD) software SpaceClaim.

The 3D model of the torpedo shaped experimental object is seen in Figure (19) below, with the global coordinate system seen in the lower left corner of the figure. This 3D model is used for all CFD methods. The body is created as a solid type body. Solid type means that the body has both a surface area and volume. The body is then changed into a surface type in DesignModeler, another built-in CAD software in ANSYS that has a tool for creating surface bodies from solid bodies. Surface type means that the body has a surface area, but not a volume. The body is created in the same dimensions as the body used in the experiment, see Table (1).

Figure 19: 3D model of experimental body used for all CFD methods.

The 3D models that are used for ANSYS CFX and for the ICFD-solver in LS-DYNA are created from a basis model consisting of one solid type rectangular cuboid on top of another. The bottom cuboid and the top cuboid will be used as water volume and air volume respectively. The top face of the bottom cuboid (the face on which the top cuboid is placed) and the bottom face to the top cuboid coincide and are regarded as one face/surface. This face represents the water surface. The basis model is modified into two different models; one model to be used in LS-DYNA and one model to be used in ANSYS.

For the LS-DYNA model, the cuboids are changed into surface type bodies (in DesignModeler). This change is necessary since the ICFD-solver in LS-DYNA uses surface meshes to create the fluid volume mesh. A total of four surface body parts are created from the two original cuboids. The reason for this is that the different surface bodies will have different boundary conditions applied to them and for that, they need to be individual parts. For the ANSYS model the cuboids are kept as solid type bodies. The

(26)

LS-DYNA model is seen in Figure (20) below, with the global coordinate system seen in the lower left corner of the figure. The different surface parts have their own individual colour. Three part colours are seen in the figure, the colour that is not seen is the colour of the surface part between the red and the blue part. This is the ”water surface” part.

Figure 20: 3D model of water and air, used in LS-DYNA.

The dimensions of A-D in Figure (20) are specified in Table (2) below. The dimensions have been chosen by what is best suited for the numerical simulations in terms of the size of the falling body and the computation time of the simulation.

Table 2: Dimensions of A-D, seen in Figure (20). A [mm] B [mm] C [mm] D [mm] 1700 1700 800 1000

In ANSYS, the water surface is not defined with a geometry. Therefore, the face between the two cuboids is deleted. For the ANSYS model, a cube with an edge length of 500 mm is also added. The cube encloses the fluid volume where the body is located and moves in the same way as the body during the ANSYS simulation. This keeps the fluid mesh around the body consistent in size and shape; large fluid domain deformation around the body is thus avoided. The ANSYS model is seen in Figure (21) below, with the global coordinate system seen in the lower left corner of the figure. The volume occupied by the body is seen inside the 500 mm cube. This volume is a void in the ANSYS 3D fluid model.

(27)

Figure 21: 3D model of water and air, used in ANSYS CFX.

In the SPH method only water is modelled. The fluid/SPH part is made from a cuboid of solid body type. This cuboid is seen in Figure (22) below, with the global coordinate system seen in the lower left corner of the figure. The top face of the cuboid represents the water surface.

(28)

Figure 22: 3D model of water, used in the SPH method.

The dimensions of A-C in Figure (22) are specified in Table (3) below. The fluid volume in the SPH method is considerably smaller than the water fluid volume for the mesh-based methods. Trial-and-error work during this project has shown that a large volume for the SPH part is not necessary. This is an advantage since a smaller computational domain requires less computing power, leading to reduced computation time and a lower computational cost.

Table 3: Dimensions of A-C, seen in Figure (22). A [mm] B [mm] C [mm]

300 500 500

5.3 Simulation description and progression

In the initial state, which is at the simulation time ts= 0, the lowest part of the falling body is located

10 mm above the water surface. The velocity of the body in the initial state is -4.41 m/s in the y-direction of the global coordinate system. An acceleration (gravity) of -9.81 m/s2 _{is also present in this direction}

which will accelerate the body as the simulation progresses. When the body reaches the water surface, at approximately ts= 2.3 ms (analytically calculated), it will have reached an impact velocity the same

size as in the conducted experiment. The body has no rotational or translational movement, except for the translational movement in negative y-direction, in the initial state. External factors, such as wind and water waves, are not considered. The total simulation time is 30 ms.

The body is modelled as a shell with the same thickness and mass as the body used in the experiment, see Table (1). The fluid and material constants used in the simulation are presented in Table (4) and in Table (5) below.

Table 4: Fluid properties for water and air. The values are from predefined fluid property values in the ANSYS software.

Fluid Density [kg/m3_] _{Dynamic viscosity [kg/m s]}

Air 1.185 1.831e-5 Water 997.0 8.899e-4

(29)

Table 5: Constants for Aluminium. Values are from [15].

Material Density [kg/m3_] _{Youngs modulus [GPa]} _{Poissons ratio [−]}

Aluminium 2700 70 0.33

5.4 Mesh-based one-way FSI in ANSYS

A one-way FSI simulation in ANSYS is divided into a steady-state CFD-, a transient CFD- and a transient FE-analysis. The steady-state CFD analysis stabilises the water surface. During the steady-state analysis the location of the object is above the water surface. The transient CFD analysis is used to calculate the pressure field acting on the body due to the water impact. The pressure field is mapped to the FE-analysis in order to calculate deformation, strain and stress for every time step. The output files from the mesh-based one-way FSI simulation are attached in Appendix.

5.4.1 Meshing

The meshing of the fluid and solid geometries are made in ANSYS Meshing. For the fluid geometry, tetrahedral elements (Tet4) are used. For the solid geometry, triangle (Tri3) and quadrilateral (Quad4) elements are used. The mesh quality is checked to ensure that the values for critical parameters (skewness, small angels etc.) are within recommended values. Figure (23) shows one of the meshes used for the fluid geometry. The fluid mesh is refined around the location of the body and at the water surface since the results from these locations are the ones of interest. When the body translates during the simulation the elements outside of the 500 mm cube will deform. Since the deformed elements will not be near the location of the body it is assumed that the deformation will not affect the results significantly. Figure (24) shows the mesh used for the solid geometry.

(30)

Figure 24: The mesh used for the solid geometry. Mesh sizes

The meshes used for the fluid geometry are a coarse mesh, where the refined elements have a size of 12 mm, and a finer mesh, where the refined elements have a size of 10 mm. The structural element size is 5 mm for both the coarse mesh and the finer mesh.

5.4.2 Stationary CFD analysis in ANSYS CFX

The boundary conditions for all faces of the fluid geometry, except for the top face, are set to no slip walls. The top face is set to be an opening with a pressure of zero, so that the pressure in the simulation is shown as gauge pressure. The boundary between the 500 mm cube and the surrounding is set to a fluid-fluid interface. Gravity is present through the buoyancy term. The fluid geometry contains both water and air. A Homogeneous model is selected together with a standard free surface model, which is used when there is a distinct interface between the present fluids. The Shear Stress Transport (SST) turbulence model is used for the simulation. This model uses the k- turbulence model in the free shear flow and the k-ω turbulence model in the inner region of the boundary layer.

For the standard free surface model, a surface tension coefficient and a primary fluid have to be specified. The surface tension coefficient is set to 0.072 N/m and water is set as the primary fluid. The inter-phase transfer between the water and air is set to free surface.

Initial conditions are set for the velocity, static pressure, turbulence and volume fraction. The Cartesian velocity components [U, V, W ] are set to [0, 0, 0] m/s and the pressure is set to:

P ressure = W aterV ol · (DensityW ater · Gravity · (Y water − y)), (3) where W aterV ol equals

W aterV ol = if (y <= Y water, 1, 0). (4) In Equation (3) and (4), Y water is equal to 0 m. Equation (4) decides where the water surface is located and will result in a value of 1 or 0. When the y-coordinate is less than or equal to Ywater the expression equals 1 which means that water is present. The turbulence is set to Intensity and Eddy Viscosity Ratio and the volume fractions for water and air are set to W aterV ol and AirV ol respectively, where AirVol equals 1 − W aterV ol.

5.4.3 Transient CFD analysis in ANSYS CFX

The difference between the stationary and the transient simulation is that a time step, a total simulation time, a rigid body and a moving mesh are specified. A time step of 0.1 ms is wanted to fully capture the

(31)

evolution of the water impact. However, a simulation with a time step this small takes too long time for ANSYS to solve given the available computational power. A time step of 0.5 ms is used for the ANSYS simulation instead.

The location of the rigid body is where the solid geometry should be. This is the empty volume in the fluid mesh. The rigid body is specified with a mass and a moment of inertia. The moment of inertia for the rigid body is shown in Table (6). The values have been calculated by a built in calculator in LS-DYNA. The rigid body is given one translational degree of freedom in the global y-direction. The rigid body has no other translational or rotational degrees of freedom. Gravity is implemented and an initial velocity is set for the rigid body.

Table 6: Inertia for the rigid body about the global coordinate system. Angle [◦] 30 45 Mass [kg] 1.8 1.8 Ixx [kg m2] 0.0326748 0.0224935 Iyy [kg m2] 0.0123121 0.0224935 Izz [kg m2] 0.0428561 0.0428561 Ixy [kg m2] 0.0176346 0.0203626 Ixz [kg m2] -4.58134e-10 -4.81123e-10 Iyz [kg m2] 6.22854e-10 -3.5809e-10

For the fluid walls that intersect with the rigid body walls, the mesh motion is set to rigid body with ignored rotations. The 500 mm cube is set to use the same mesh motion as the rigid body. The initial conditions for the transient analysis are the results from the steady-state analysis.

5.4.4 Pressure export from ANSYS CFX

For all time steps in the transient CFD-simulation, the pressure over the fluid walls that intersect with the rigid body is exported. The pressure for each time step is exported as a .csv-file and is imported to ANSYS Workbench through the External data command. Only the x-, y- and z- coordinates from the first .csv-file are used.

5.4.5 Transient structural analysis in ANSYS Mechanical

The external data containing the pressure from ANSYS CFX is imported into ANSYS Mechanical by connecting it to the transient structural setup. The external data is mapped to the structural mesh for every time step.

The structural mesh in ANSYS Mechanical has an initial velocity equal to the velocity of the rigid body in the transient CFD analysis. A distributed mass, shell thickness and a material is applied to the geometry. Gravity is also enabled, which is done by adding the boundary condition Standard earth gravity. To get the wanted output each solution-file has to be selected, for example Total deformation, directional velocity or Equivalent (Von-Mises) stress.

5.5 Mesh-based two-way FSI in ANSYS

The differences between the transient one-way FSI simulation and the two-way FSI simulation is that the rigid body in ANSYS CFX is removed. The data exchange happens between the fluid walls in ANSYS CFX that enclose the empty volume in the fluid domain and the structural body surface in ANSYS Mechanical. This is done by setting the mesh motion of the fluid walls to system coupling.

The boundary between the 500 mm cube and the surrounding is set to conservative interface flux and the mesh motion of the 500 mm cube is set to unspecified.

5.5.1 Settings for the FE-analysis

To enable the data transfer in ANSYS Mechanical, a Fluid Solid Interface has to be specified. The fluid solid interface is set to all surfaces that will interact with a fluid. The step end time has to be specified to

(32)

a value larger or equal to the total time specified in the system coupling. Apart from the data transfer, the settings for the FE-analysis are the same as in the the one-way FE-analysis. The data transfer begins at the start of an iteration. The output files from the mesh-based two-way FSI simulation are attached in the appendix.

5.6 Mesh-based two-way FSI in LS-DYNA

In LS-DYNA, all settings and inputs to the solvers are made with LS-DYNA keyword cards. The keyword cards contain parameters specific for each card and different settings are made by giving these parameters specific values. The keyword cards can be created and edited with a text editor or with PrePost. LS-PrePost is a pre- and post-processor that has been created specifically for LS-DYNA. In this project, LS-PrePost version 4.5 is used to create the keyword cards for both the mesh-based FSI and the SPH method in LS-DYNA. The input keyword cards used for the CFD methods in LS-DYNA are attached in Appendix. In this chapter, a description over the meshing process and over important settings for the mesh-based two-way FSI method in LS-DYNA are presented. Information in this chapter is retrieved from the LS-DYNA Keyword User’s manuals and from the LS-DYNA ICFD theory manual. A few other sources are also used, these are cited in the text.

5.6.1 Meshing

The surface part of the body is meshed with mixed 2D elements in the finite element pre-processor HyperMesh [16]. The mesh of this part is the structural mesh or solid mesh in the FSI analysis (as opposed to the fluid mesh). The structural mesh, and settings for the solid part, are processed by the mechanical solver. The fluid mesh, and settings for the fluid, are processed by the ICFD-solver. The mesh of the solid part is displayed in Figure (25). The size of the elements in the figure is 5 mm. Each meshed part has its own unique part ID (PID), this is needed in order to assign a part a certain boundary condition and other specific settings. In Figure (25), the PID is displayed in white colour (PID 10).

Figure 25: 2D mesh of Part 10 .

The surface parts of water and air are also meshed in HyperMesh but with 2D triangular elements. As mentioned in the theory, triangular elements are required by the ICFD-solver. A finer mesh size is wanted in the centre of the computational domain where the body translates and impacts the water surface. Since the size of the fluid mesh depends on the mesh size of the surface that define the fluid enclosure, the surface part that represents the water surface is meshed with a finer mesh in the centre. The mesh on this surface part increases gradually towards the edges, where the mesh doesn’t have to be as fine. This is shown in Figure (26). The mesh size transition on the surface part is slow in order to avoid numerical instabilities.

(33)

Figure 26: Meshed part termed Surface with a finer mesh in the centre that increases gradually towards the edges.

In order for the ICFD-solver to be able to read the meshed surface parts, the meshes are converted into ICFD surface meshes using LS-PrePost. The ICFD meshed surface parts, or ICFD parts for short, are now considered fluid parts by the ICFD-solver. Figure (27) shows the meshed fluid geometry in LS-PrePost with two sides blanked. The numbers are the PIDs for each of the fluid parts. Figure (27) shows that an ICFD part of the body surface is also made. This part will be used as the fluid surface that is in contact with the solid surface for the FSI analysis.

(34)

Figure 27: ICFD surface (fluid) mesh with two sides blanked. Mesh sizes

The mesh sizes used for the FSI model are a coarse ICFD mesh, where the smallest surface elements are 9 mm and the largest are 36 mm, and a finer ICFD mesh, where the smallest surface elements are 5 mm and the largest are 18 mm. The ICFD mesh shown in Figure (27) is the coarse mesh. The element size of the structural mesh is 5 mm for both the coarse ICFD mesh and the finer ICFD mesh.

5.6.2 Fluid settings

The fluid settings are read by the ICFD-solver. Parts 2, 3 and 5 in Figure (27) are given non-slip boundaries. For part 4, a fluid pressure is imposed on the boundary, so that the pressure in the simulation is shown as gauge pressure. The pressure is defined with the curve y = 0 that is created in LS-PrePost. Section properties and physical properties are specified for all the ICFD parts. ICFD parts 1 and 2 are given the physical properties of water. The other parts are given the physical properties of vacuum. Air is modelled as vacuum by setting the density of it to zero. Fluid properties are associated with a fluid volume by defining the surface parts that enclose the fluid volume and by assigning section and fluid properties to the volume. The parts enclosing the void volume are parts 1, 3, 4 and 5 in Figure (27). Part 5 has to be defined as an enclosing surface part to the void/air volume because the volume inside this part is not to be assigned any fluid properties.

The volume space that is to be meshed is determined by defining the surface parts that enclose it. The ICFD parts in Figure (27) that defines the volume that is to be meshed are parts 2, 3, 4 and 5. The volume inside ICFD part 5 is not to be meshed. A mesh refinement of the volume mesh near the body is implemented by defining a boundary layer mesh for part 5. The number of elements normal to the surface (in the boundary layer) is set to 1. The fluid volume is set to be re-meshed every fourth time step in the simulation. The ICFD part that represents the water surface, part 1 in Figure (27), is specified to be a fluid interface. The time step of the CFD simulation is set to 0.1 ms. The time step is chosen to be this small in order to fully capture the evolution of the short duration water impact.

(35)

5.6.3 Settings for the structural part

For the structural part; material, shell thickness and mass are specified. The initial velocity of the body is set by giving an initial velocity to a set of nodes consisting of all nodes on the structural mesh. A strongly coupled scheme for the FSI simulation is implemented by activating implicit analysis. The time step size for the implicit analysis must be the same as the time step size for the ICFD-solver. Implicit dynamic analysis is activated and is set to use Newmark time integration. Newmark time integration is chosen for the analysis because this method is used in an LS-DYNA example simulation case (similar to the simulation case in this project) created by the company behind LS-DYNA. See [17] for further information. GAMMA and BETA are Newmark time integration constants that need to be assigned values. GAMMA is set to 0.6 and BETA is set to 0.4. These values are used in the LS-DYNA example simulation case referenced in [17]. The governing equations for the fluid are non-linear and the implicit solution is therefore set to be non-linear.

Since the results from the simulations of the experimental case are to be compared with experimental data from accelerometers attached to the falling body, a local coordinate system corresponding to the coordinate system of the accelerometers is created. The origin and direction of the coordinate axes of the local coordinate system is defined by three nodes on the structural mesh. Figure (28) contains two subfigures that show the placement of the local coordinate system on the structure from different angles. The global coordinate system is shown to the lower left in the subfigures. In order to get the nodal outputs, from certain nodes, in the local coordinate system; these nodes have to be selected. In Figure (28), the selected nodes are marked with white triangles.

(a) The selected nodal points and the local coordinate system.

(b) A more visible view of the x-axis of the local coordinate system.

Figure 28: The nodal points whose responses are to be output in the local coordinate system shown in different angles.

The placements of the nodal points on the structural mesh correspond to the placements of the accelerom-eters on the experimental body. The translational output for each selected nodal point is set to be the projection of the node’s relative translational motion onto the local system. This setting enables the local system to change orientation according to the movement of the three defining nodes. The outputs of the nodal accelerations are set to be averaged between output intervals. Gravity is defined with the curve y = 9.81, the curve is created in LS-PrePost. The gravity is read by both the ICFD- and the mechanical solver.

The output from the simulation is controlled with ”Database keywords”. See these keywords in Appendix. The time interval between simulation outputs is specified with a curve that has been created in

(36)

LS-PrePost, just like the gravity curve and pressure curve. The time interval between outputs is 0.1 ms from the start of the simulation until the simulation time ts= 10 ms. The water impact happens within the

first 10 ms. From 10 ms, the time interval changes to 0.5 ms until the end of the simulation. 5.6.4 FSI-coupling

The ICFD-solver is coupled to the structural solver with the keywords *ICFD CONTROL FSI and *ICFD BOUNDARY FSI. With the former keyword, the coupling direction is selected. For two-way coupling, loads and displacements are transferred across the FSI interface which solves the full non-linear problem. The *ICFD BOUNDARY FSI keyword is used to define which fluid surfaces that are in contact with the solid surfaces. Fluid surface part 5 in Figure (27) is in contact with the solid surface in Figure (25). The LS-DYNA version that is used for running the mesh-based FSI simulation is LS-DYNA (smp double precision) release R9.2.0.

5.7 SPH method in LS-DYNA

Since the same structure is used in the SPH method as in the mesh-based FSI method, the keyword cards used in the SPH simulation include all the ones used for the structural part in the mesh-based FSI simulation. The only keywords not used for the structural part in the SPH method are the keywords used to activate implicit analysis, since the SPH method is explicit. In this chapter, a description over the SPH generation and over the settings for the SPH particles are presented. Information in this chapter is retrieved from the LS-DYNA Keyword User’s manuals and from the LS-DYNA theory manual. A few other sources are also used which are cited in the text.

5.7.1 SPH generation

In the process of making the SPH particles, a solid mesh is first created out of the geometry in

Figure (22). The geometry is meshed with cubic elements in HyperMesh. Figure (29) shows this 3D mesh in LS-PrePost. The element size is 5 mm.

Figure 29: 3D mesh used to create SPH particles.

The SPH particles are created in LS-PrePost from the 3D mesh. The particles have a distance between each other that corresponds to the size of the elements in the 3D mesh. The filling property is set to 100 %, this means that the whole volume of the 3D mesh is used when generating the particles. The density of the SPH particles is set to the density used for water. The generated SPH particles from the solid mesh shown in Figure (29) are seen in Figure (30) below. The SPH particles are also regarded as

(37)

nodes in LS-DYNA and the words ”SPH particles” and ”SPH nodes” will be used interchangeably in the text.

Figure 30: Generated SPH particles created from a 3D mesh. Particle distances

The computational power available in this project sets a limit for the distance between particles to not be smaller than 5 mm. According to an SPH mesh refinement study, in [5], the most accurate results were achieved when the distance between SPH particles was 60 % of the element size of the structural mesh. In the study, the smallest distance between particles was 50 % of the element size of the structural mesh and the largest distance was 150 % of the element size. A distance between SPH particles that is approximately 60 % of the element size, corresponds to an element size of 9 mm for the structural mesh in this project, which is almost too coarse. Since the particle distance can not be smaller than 5 mm (due to the computational power) a 9 mm element size for the structural mesh must be used if the particle distance is to be 60 % of the structural element size. The SPH mesh refinement study in this project is done by using two different mesh sizes for the structural mesh. The sizes used are 9 mm and 5 mm. A structural mesh size of 5 mm gives a distance between SPH particles that is 100 % of the structural element size. Figure (31) below shows the 9 mm structural mesh used.

(38)

Figure 31: 9 mm structural mesh used for the SPH mesh refinement study. 5.7.2 Settings for the SPH particles

The fluid volume is contained by applying constraints to all the SPH nodes on the surface of the SPH part except for the nodes on the top face (only the SPH nodes on the rim of the top face are applied constraints). The nodes are constrained in translational local x-,y- and z-direction and rotationally about the local x-,y- and z-axis.

For the SPH particles; section properties, material properties and an equation of state (EOS) are defined. One of the section properties is the smoothing length of the particles. The smoothing length has to be assigned a constant. The default constant value of 1.2 applies for most problems and is recommended. In the material properties, a value is set for a parameter PC which is the pressure cutoff. The value for this parameter is taken from [18, p.62].

The EOS is used to correlate the volume of the fluid to the pressure [19]. There are different types of EOS’s; in LS-DYNA, the EOS called Gruneisen is commonly used to represent water and other liquids [18]. Gruneisen is therefore the used EOS in this project. An EOS is defined with state variables and the assigned values to the parameters in the Gruneisen equation are taken from [18, p.62].

The space dimension for the SPH particles is set to 3D. The particle approximation theory used is decided with the parameter FORM on the *CONTROL SPH card. Two versions of the SPH method are made in this project, one where the parameter FORM is set to 0 (default formulation) and one where it is set to 5 (fluid particle approximation, this approximation should give the best results of all available SPH formulations when fluid materials are present).

The finite element coupling is accomplished by using the keyword *CONTACT AUTOMATIC NODES TO SURFACE ID. A set of all the SPH particles is created and this set is specified to be the slave segment. The structural part is specified to be the master segment, in accordance with theory. The time step size of the SPH simulation is set to be determined by the mechanical solver itself, this is done by setting the step size to zero. The completed SPH model is seen in two different views in Figure (32) below. In the figure, it is the 9 mm structural mesh that is shown. The LS-DYNA version that is used for running the SPH simulation is LS-DYNA (smp single precision) release R9.2.0.

(39)

(a) SPH model shown from one side. (b) SPH model shown in an isometric view.

(40)

6 Results

CFD results from nodal points, given in a local coordinate system, can not be retrieved from ANSYS. Therefore, the experimental results can only be compared to numerical results from LS-DYNA. Since the accelerometers give the acceleration as a scalar quantity and the simulations give the acceleration as a vector quantity, the results from the accelerometers can not be compared directly to the numerical results from the nodal points. It was decided to only use the result data from two accelerometers perpendicular to each other and to compare the resultant experimental acceleration from these two accelerometers to a resultant numerical acceleration. The two accelerometers used are referenced as nodes 1 and 2 in Figure (33) below. Node 2 is located on the side of the experimental body that will submerge into the water last when dropped.

Figure 33: The position of the two accelerometers used for the comparison between experimental and numerical results.

The resultant experimental acceleration is compared to the resultant numerical acceleration in y- and z-direction (of the local coordinate system) from the nodal point that corresponds to the accelerometer termed node 1 in Figure (33). Figure (34) shows the nodal point that corresponds to the accelerometer termed node 1.

Figure 34: The nodal point in the simulations that is used for the comparison between experimental and numerical results. The nodal point is marked by a white triangle in the figure.

(41)

In order to evaluate the results from ANSYS, the CFD methods are compared to each other by comparing the acceleration of the whole body in global y-direction from each of the methods. The global acceleration can be compared between all methods because they have identical global coordinates.

6.1 Experimental results

Below, the resultant acceleration from the accelerometers termed node 1 and node 2 are presented. The separate accelerations from each of the nodes are attached in Appendix. The water impact from one of the drops is shown in Figure (35). Five drops were made for each of the impact angles. These drops are referred to as ”runs” in this text. The expected behaviour of the acceleration curve is an acceleration of zero in the beginning followed by a peak in acceleration caused by the water impact. Some milliseconds after the peak that is caused by the water impact, a larger peak caused by the safety ropes bringing the falling body to a halt should be seen.

Figure 35: The water impact from one of the drops.

The resultant accelerations for each of the runs with impact angle 30◦ are shown in Figure (36). The curves for the resultant accelerations in runs 1, 2 and 5 show some similarities but it is only run 2 that shows the expected behaviour; a smaller peak followed by a larger peak. Run 3 and run 4 show completely inaccurate results. Run 3 shows inaccurate results because the acceleration is registered as zero during the whole run. This means that the run 3 measuring has failed. The acceleration in run 4 does not behave as expected at all.

(42)

Figure 36: The resultant acceleration. The angle of impact is 30◦.

Figure (37) shows the resultant accelerations for each of the runs with impact angle 45◦. All runs except runs 1 and 4 have failed. None of the runs show the expected behaviour. The curve for run 4 shows a larger peak but no smaller peak before the larger peak.

Figure 37: The resultant acceleration. The angle of impact is 45◦.

6.2 Comparison between experimental results and numerical results

Note that the numerically calculated accelerations presented in this section are calculated in the local coordinate system. The curve for run 2 in Figure (36) and the curve for run 4 in Figure (37) are used in the comparisons with the numerically calculated accelerations. The experimental curves have been filtered for the comparisons. Only the 30 ms that have been simulated are shown in the comparison figures. The moment where the nose of the body first touches the surface is marked with a red vertical line in all figures in this section. Note that it is not known exactly when the body hits the water in the experimental curves; for run 2 for example, it is a qualified guess that the impact at approximately 0.525

(43)

seconds in Figure (36) is the peak caused by the body hitting the surface. The figures containing curves for the experimental results have a second red vertical line that marks the beginning of the peak that is caused by the safety ropes.

Figures (38) and (39) show the experimental acceleration and the numerically calculated acceleration from the mesh-based two-way FSI in LS-DYNA for impact angles 30◦ and 45◦ respectively. The numerical results are from the simulation that uses the coarse fluid mesh. Figure (38) shows that as the body enters the water, the numerical acceleration behaves in the same way as the experimental acceleration; though, the experimental acceleration phase is approximately 3-4 ms while the numerically calculated acceleration phase is less than half of that. Both accelerations are approximately 2 g-forces as the body hits the water. After the water entry, the experimental acceleration goes back to zero while the numerically calculated acceleration does not. The fluctuations shown for the numerically calculated acceleration could be from numerical instabilities and this could be the reason why the numerically calculated acceleration does not go back to zero. The larger peaks from the experimental accelerations in Figures (38) and (39) are from when the safety ropes brings the body to a halt. This peak is obviously not shown in the numerically calculated accelerations since the safety ropes are not simulated. For the experiment where the impact angle is 45◦ (Figure (39)), no change in acceleration is seen before the peak caused by the safety rope. This means that the water impact has not been registered by the accelerometer.

Figure 38: Comparison between the experimental acceleration and the numerically calculated acceleration from the mesh-based two-way FSI in LS-DYNA. The angle of impact is 30◦.

(44)

Figure 39: Comparison between the experimental acceleration and the numerically calculated acceleration from the mesh-based two-way FSI in LS-DYNA. The angle of impact is 45◦.

Figures (40)-(43) contain the numerical results from the SPH method when the impact angle is 30◦. These graphs were supposed to be shown together with the curves in Figure (38), but since the accelerations in Figures (40)-(43) are roughly 400-500 times higher than the accelerations in Figure (38), the results from the SPH method have to be shown in separate figures. Figure (40) shows the acceleration when a 5 mm structural mesh is used and when the parameter FORM equals to either 0 (default approximation of SPH particles) or 5 (fluid particle approximation of SPH particles). The graph for FORM= 5 shows a higher maximum acceleration than the graph for FORM= 0. Figure (41) shows the acceleration when a 9 mm structural mesh is used and when the parameter FORM equals to either 0 or 5. This Figure also shows that FORM= 5 gives a higher maximum acceleration than FORM= 0. Figure (42) shows the acceleration when FORM= 0 is used and when the structural mesh is either 5 mm or 9 mm. The graph for the 5 mm mesh gives a significantly higher acceleration than the graph for the 9 mm mesh. Figure (43) shows the acceleration when FORM= 5 is used and when the structural mesh is either 5 mm or 9 mm. Like the previous figure, this figure shows that a significantly higher acceleration is shown for the 5 mm mesh than for the 9 mm mesh. Figures (40)-(43) show that the choice of mesh size affects the acceleration more than the choice of SPH approximation. The acceleration phase at impact for the accelerations calculated by the SPH method is approximately 5 ms which is closer to the experimental acceleration phase than the acceleration phase calculated by the mesh-based method in LS-DYNA, seen in Figure (38).

(45)

Figure 40: The acceleration when the structural mesh is 5 mm. The angle of impact is 30◦.

(46)

Figure 42: The acceleration when FORM= 0. The angle of impact is 30◦.

Figure 43: The acceleration when FORM= 5. The angle of impact is 30◦.

The Figures that correspond to Figures (40)-(43), but for an impact angle of 45◦are attached in Appendix. The graphs in these figures show a similar behaviour as the graphs in the figures for the 30◦impact angle. Though, the figures for the 45◦impact angle show that the choice of mesh size and SPH approximation does not affect the acceleration as much as the figures for the 30◦ impact angle show.

(47)

6.3 Comparison between the CFD methods

Note that the numerically calculated accelerations presented in this section are calculated in the global coordinate system. When comparing the CFD methods, the acceleration in the global y-direction of the whole body retrieved from the different CFD methods are compared. Theoretically, the body should have an acceleration of -9.81 m/s2 in the global y-direction as it falls freely in the beginning of the run/simulation. When the body hits the surface, a spike of the acceleration should be seen that drops quickly to a constant value.

Figures (44) and (45) show the acceleration of the whole body from the mesh-based one-way and two-way FSI in ANSYS and from the mesh-based two-way FSI in LS-DYNA. The acceleration curves for ANSYS have been retrieved by taking the ANSYS calculated curve of the force acting on the body in global y-direction and dividing the values on this curve with the mass of the body (force divided by mass gives acceleration). Results from the simulations where the coarse fluid mesh is used and from simulations where the fine fluid mesh is used are shown in the figures. Figure (44) shows the accelerations from the drop with impact angle 30◦ and Figure (45) shows the accelerations from the drop with impact angle 45◦. Some numerical instabilities can be seen in the beginning of the curves that show the acceleration calculated by ANSYS.

Study of a Body Subjected to a Vertical Drop into Water – Experiment and Simulations