Ship Hull


1. Create Case

After opening SimFlow, we will create a new case named Boat

1. Go to New panel
2. Provide name Boat
3. Click Create Case

2. Import Geometry - Boat

Firstly we need to Download Geometry: Boat.step

1. Click Import Geometry
2. Select geometry file Boat.step
3. Click Open

3. Geometry - Boat

After importing geometry, it will appear in the 3D window.

1. Click Fit View to zoom in on the geometry.

4. Scale Geometry - Boat (I)

The model is defined in millimeters unit. We will scale it to the meters.

1. Expand the Options list for Boat
2. Select Scale

5. Scale Geometry - Boat (II)

1. Check Uniform options
2. Type Scaling Factors as 1e-03 and press Enter
3. Click Scale

6. Rotate Geometry - Boat (I)

We will rotate the model about X axis at 90 deg to orient the Z axis vertically.

1. Expand the Options list for Boat
2. Select Rotate

7. Rotate Geometry - Boat (II)

1. Set the following parameters accordingly

Axis [-] 1 0 0
Angle [deg] 90

2. Click Rotate

8. Create Geometry – Water

Additionally to the hull geometry, we will create a box that will be used to indicate the initial location of the water.

1. Select Create Box
2. Change geometry name from box_1 to water
(double click to edit name and press Enter to confirm)
3. Set the origin and box dimensions:
Origin[m] -11 -6 -3
Dimensions [m] 22 12 2.85

9. Create Geometry – Refinement

We need to refine the mesh near the water surface to increase the accuracy of the results. For this purpose, we will create also a refinement box.

1. Select Create Box
2. Change geometry name from box_1 to refinement
3. Set the origin and box dimensions:
Origin[m] -11 -6 -0.35
Dimensions [m] 22 12 0.4

10. Meshing Parameters - Boat

In order to create the mesh, we need to specify geometries options for the meshing process.

1. Go to Hex Meshing panel
2. Select Boat geometry
3. Enable Mesh Geometry
4. Enable Create Boundary Layer Mesh
5. Set Refinement to Min 4 Max 4
6. Set No. of Layers to 4

11. Meshing Parameters - Refinement

1. Click on the refinement geometry
2. Enable Refine Geometry
3. Set the refinement Level to 2

12. Base Mesh - Domain

Now, we will define the base mesh. The box geometry determines the background mesh domain. The model is symmetrical with respect to the XZ plane and we can take advantage of this fact. Using box dimensions we will choose only half of the required domain.

1. Go to Base tab
2. Set the size of the base mesh:
Min [m] -10 0 -2
Max [m] 10 5 1
3. Define the number of divisions
Division 55 14 13

13. Base Mesh - Boundaries

We need to assign individual names to each side of the base mesh. This will allow us to apply different conditions to each side.

1. Define boundary names and types accordingly
X- inlet patch
X+ outlet patch
Y- symmetry symmetry
Y+ symmetry symmetry
Z- bottom wall
Z+ top patch

14. Material Point

Material Point tells the meshing algorithm on which side of the geometry the mesh is to be retained. Since we are considering fluid outside the boat we need to place the material point outside the geometry.

1. Go to Point tab
2. Specify location inside base mesh but outside boat geometry
Material Point 0 2 0

You can specify the point location from the 3D view. Hold the Ctrl key and drag the arrows to the destination.

15. Start Meshing

We can define the count of the buffer cells between refinement levels. This parameter determines the width of the transition zone between refined and background mesh. Lowering this parameter will reduce the overall cells count.

1. Go to Mesh tab
2. Go to Settings
3. Set Cells Between Levels to 3
4. Press the Mesh button to start meshing process

16. Mesh

After the meshing process is finished the mesh should appear in the graphics window.

17. Select Solver

To analyze water behavior we will use Inter (interFoam) solver. This solver is designed to model two-phase flow with interface capturing capabilities.

1. Go to SETUP panel
2. Select Transient filter
3. Select Multiphase model filter
4. Pick Inter (interFoam) solver from the list
5. Select solver

18. Dynamic Mesh (I)

The dynamic mesh can be used for a simulation where the shape of the domain is changing. In our case, we will use dynamic mesh capabilities paired with a six degrees of freedom (6 DOF) solver. The 6DOF solver will predict the trajectory of a moving body using the aero or hydrodynamic forces and inertial properties assigned to a given boundary. During the analysis, the mesh will adjust to the new position of the body by moving nodes in the deformation region defined by the distance from the body.

1. Go to Dynamic Mesh panel
2. Choose Dynamic Mesh Type 6 DoF
3. Select the Boat geometry
4. Set the Inner Distance [m] to 0.2 for the deformation region
5. Set the boat mass properties:
Mass [kg] 120 (it is only half of the mass because of model symmetry)
Center of Mass [m] -1.1 0 -0.1385
Mom. Of Inertia [kg m2] 100 500 100
6. Set the Relaxation to 1

19. Dynamic Mesh (II)

It is possible to constrain boundary motion. We will allow the boat to move only in the Z-axis direction and rotate about Y-axis. We will also enable damping to improve the stability of the calculation.

1, 2. Set the constraints accordingly

Translation Constraint Line

Rotation Constraint Axis
Axis [-] 0 1 0

3, 4. Set the restraints accordingly

Linear Restraint Damper
Damping [Ns/m] 30

Angular Restraint Damper
Damping [Nms/m] 30

20. Turbulence

For the purpose of this tutorial, we will model the turbulence phenomenon using the k-ω SST model.

1. Go to Turbulence panel
2. Select RANS turbulence formulation
3. Select k-ω SST model

21. Transport Properties - Water

In order to define water and air properties, we go to the transport properties panel. We will use predefined fluids properties from the material database.

1. Go to Transport Properties panel
2. Change phase name from phase1 to water
3. Open Material Database
4. Pick up water from the list
5. Click Apply

22. Transport Properties - Air

Repeat previous step for phase2 using air properties. To assign material to the domain, the phase fraction parameter phase is used. The parameter determines the proportion of each fluid in the domain. The value of phase fraction varies in range from 0 to 1 where phase1=1 means that the whole domain is filled only with the phase1, while phase1=0 means that the domain is filled with the second phase.

1. Change phase name from phase2 to air
2. Open Material Database
3. Pick up air from the list
4. Click Apply

23. Solution - PIMPLE

For the purpose of the simulation we will change PIMPLE algorithm parameters to increase stability:

1. Go to Solution panel
2. Switch to the PIMPLE tab
3. Increase Outer Correctors to 3
4. Increase Non-Orthogonal Correctors to 2
5. Uncheck Momentum Predictor for stability

24. Simulation Parameters

The velocity magnitude will be used in multiple simulation settings. It is handy to parameterize velocity value to be easily accessible in the future.

1. Go to Parameters panel
2. Define new parameter
Name U
Formula 2
3. Press Enter or Create Parameter button
4. The newly created parameter will be shown in the parameters list.

25. Boundary Conditions – Bottom

In our simulation, the frame of reference will be associated with the boat and therefore we will simulate a fluid flow around the stationary boat. In order to properly represent ground in the boat frame of reference, we will enforce velocity at the bottom mesh boundary.

1. Go to Boundary Conditions panel
2. Select the bottom boundary
3. Change the Type of velocity to the Fixed Value
4. Set the Value [m/s] U 0 0

26. Boundary Conditions – Inlet (Flow)

We will model the inlet to the domain by assign the Inlet Velocity character. As an inlet velocity value we will use U parameter.

1. Select the inlet boundary
2. Set the Velocity Inlet character
3. Set the velocity Reference Value [m/s] to U

27. Boundary Conditions – Inlet (Phases)

Additionally to the flow conditions, it is required to choose the inlet phase. Initially, we will specify pure air. The water phase at the inlet will be patched later on by the water box geometry. Patching operation will modify the value parameter in a certain region and effectively we will get an inlet of two phases from a single boundary.

1. Switch tab to Phases
2. Set the type to Fixed Value

28. Boundary Conditions – Outlet (Flow)

For the outflow boundary we will use Outlet Phase Mean Velocity condition. This boundary condition adjusts the velocity for the given phase to achieve the specified mean velocity.

1. Select the oulet boundary
2. Set the Outflow character
3. Switch tab to Flow
4. Set the velocity type and mean value accordingly
U Type Outlet Phase Mean Velocity
U Umean[m/s] U

Note: After you change flow boundary condition the character will switch form Outflow to Custom. Do not change it back to Outflow afterwards.

29. Boundary Conditions – Outlet (Phases)

1. Switch tab to Phases
2, 3. Set the water parameters accordingly
water Type Variable Height
water Upper Bound [-] 1

30. Initial Conditions - Basic

Before we start simulation we need to define the initial state. We will use parameter U to initiate constant velocity in the domain. Phase fraction air=0 tells us that the whole domain is filled with the air by default.

1. Go to Initial Conditions panel
2. Set the velocity to U 0 0

31. Initial Conditions – Patch

Using the water geometry, we will overwrite the phase fraction value inside it. We will set the water to 1 to fill the patched geometry with the water.

1. Switch to Patch tab
2. Enable initialization on water geometry
3. ExpandFields list
4. Select water fraction for initialization
5. Set initial value of water to 1
6. Apply patch for Both cells and faces. This will override values at boundaries as well.

32. Monitors – Sampling

During calculation, we can observe intermediate results on a section plane. To add sampling data on a plane we need to define plane properties and also select fields that will be sampled. Note that runtime post-processing can only be defined before starting calculations and can not be changed later on.

1. Go to Monitors panel
2. Switch to Sampling tab
3. Select Create Slice
4. Set the slice normal vector alogn y-axis
Normal [-] 0 1 0
5. ExpandFields list
6. Check the velocity U
7. Check the water phase water

33. Monitors - Forces

Additionally, we will observe forces acting on the boat boundary.

1. Switch to Forces tab
2. Expand Monitored Boundaries list and check Boat

34. Run - Time Control

For any simulation, it is very convenient to let the solver automatically determine the proper time step value. To use this option we need to define time step constraints by providing the initial time step(adjusted by the solver during computations) and maximal time step value. Rest of the parameters we can leave the default.

1. Go to RUN panel
2. Set the Simulation Time [s] to 10
3. Change Time Stepping to Automatic
4. Set initial and maximum timesteps (solver will start computation with the initial value and adjust it in the next iterations not exceeding the maximum value)
Initial Δt [s] to 1e-04
Max Δt [s] to 1e-02

35. Run - Output

We can control how often results should be saved on the hard drive. Only this data will be available for postprocessing.

1. Switch to Output tab
2. Set the Write Control Interval [s] to 0.05
3. Click Run Simulation button

36. Postprocessing – ParaView

After computations are finished we can do complex visualization of our results with ParaView.

1. Go to POSTPROCESSING panel
2. Click on Run ParaView

37. ParaView - Load Results

Load the results into the program.

1. Turn on Toggle advanced properties
2. Uncheck option Decompose polyhedra
3. Click Apply to load results into ParaView

38. ParaView – Dynamic mesh

We will look at the dynamic mesh displacement. As we can see, the boat can move along Z-axis and rotate around Y-axis. The mesh at a distance of 0.2m from the boat is rigid and moves together with a boat. The mesh at the distance from 0.2m to 1m from the boat is able to move. Further than 1m from the boat, the mesh is non-deformable.

1. Select Surface with Edges from the representation toolbar list
2. Select pointDisplacement from the variable list
3. Click Rescale to Data Range
4. Play with an animation buttons to track the results of analysis.

39. ParaView – Reflect the results (I)

We have run the simulation with only half of the fluid domain. At the postprocessing step, we can reproduce the second part of the domain. For visualization purposes, we will reflect the results about the plane of symmetry.

1. Select the case Boat.foam
2. Extend the list of Filters from the top menu
3. Go to Alphabetical
4. Select Reflect from the list

40. ParaView – Reflect the results (II)

1. Choose the plane of the reflection Y min
2. Click Apply

41. ParaView – Water Surface

We will focus on the water-air interface behavior and observe the velocity map.

1. Select Clip from top menu
2. Change the clip type to Scalar
3. Select alpha.water from the scalar list
4. Click Refresh
5. Make sure Invert option is unchecked
6. Click Apply
7. Select the velocity U from the list
8. Click on Rescale to Custom Data Range
9. Set the range from 0 to 3
10. Confirm by clicking Rescale

42. ParaView – Boat Geometry (I)

To display the boat geometry, we will read the result file once again and load only the boat boundary.

1. Select Open from top menu
2. Choose the Boat.foam file from case folder
3. Press OK

43. ParaView – Boat Geometry (II)

1. Uncheck internalMesh from the Mesh Regions
2. Check the Boat
3. Press Apply

44. ParaView – Boat Geometry (III)

Similarly as before, we will reflect the boat geometry.

1. Select the new case name Boat.foam, go to Filters, extend Alphabetical and select Reflect from the list
2. Choose the plane of reflection Y min
3. Click Apply
4. Select the Solid Color from the list

45. ParaView – Results

1. Play with animation buttons to investigate the time history of the flow.

This website uses cookies to offer you the best experience online. By continuing to use our website, you agree to the use of cookies.