1. Download SimFlow
SimFlow is a general purpose CFD Software
To follow this tutorial, you will need SimFlow free version, you may download it via the following link:
Download SimFlow
2. Create Case
Open SimFlow and create a new case named Boat
Go to New panel
Provide name Boat
Click Create Case

3. Import Geometry - Boat
Firstly we need to Download GeometryBoat. The geometry will be imported in the same units as it was exported to the STEP format.
Click Import Geometry
Select geometry file
Boat.step
Click Open

4. Preview Geometry - Boat
After importing geometry, it will appear in the 3D window.
Click Fit View to zoom in on the geometry.

5. Rotate Geometry - Boat (I)
We will rotate the model about X axis at 90 deg to orient the Z axis vertically.
Expand the Options list for
Boat
Select Rotate

6. Rotate Geometry - Boat (II)
Set the following parameters accordingly
Axis \({\sf [-]}\)100
Angle \({\sf [deg]}\)90Click Rotate

7. Create Geometry - Water
Additionally, to the hull geometry, we will create a box that will be used to indicate the initial water location.
Select Create Box
Change geometry name from
box_1
to water
double click to edit name and press Enter to confirmSet the origin and box dimensions:
Origin \({\sf [m]}\)-11-6-3
Dimensions \({\sf [m]}\)22122.85

8. 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.
Select Create Box
Change geometry name from
box_1
to refinementSet the origin and box dimensions
Origin \({\sf [m]}\)-11-6-0.35
Dimensions \({\sf [m]}\)22120.4

9. Meshing Parameters - Boat
In order to create the mesh, we need to specify geometries options for the meshing process.
Go to
Hex Meshing
panelSelect
Boat
geometryEnable Mesh Geometry
Enable Create Boundary Layer Mesh
Set
Refinement
toMin 4
Max 4
Set
No. of Layers
to 4

10. Meshing Parameters - Refinement
Click on the
refinement
geometryEnable Refine Geometry
Set the refinement
Level
to 2

11. 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.
Go to
Base
tabSet the size of the base mesh:
Min \({\sf [m]}\)-100-2
Max \({\sf [m]}\)1051Define the number of divisions
Division551413

12. 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.
Define boundary names and types accordingly
X-
inlet
patch
X+
outlet
patch
Y-
symmetry
symmetry
Y+
symmetry
symmetry
Z-
bottom
wall
Z+
top
patch

13. 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.
Go to
Point
tabSpecify location inside base mesh, but outside boat geometry
Material Point020
You can specify the point location from the 3D view. Hold the Ctrl key and drag the arrows to the destination. |

14. Meshing Settings
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.
Go to
Mesh
tabGo to
Settings
Set
Cells Between Levels
to 3

15. Start Meshing
In this step we will initiate the meshing process.
In the meshing panel you may indicate how many CPUs would you like to use for this process. Please note that if you are using SimFlow free version you may only use serial meshing, and you may not create meshes larger than 200'000 nodes.
If you would like to test full version Request 30-day Trial
Go to
CPU
tabPress the Mesh button to start meshing process

16. Mesh
After the meshing process is finished, the mesh will appear in the graphics window.

17. Select Solver - Inter
To analyze water behaviour we will use Inter (interFoam) solver. This solver is designed to model two-phase flow with interface capturing capabilities.
Go to
SETUP
panelSelect Transient filter
Select
Multiphase
model filterPick
Inter
(interFoam) solver from the listSelect 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 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.
Go to
Dynamic Mesh
panelChoose
Dynamic Mesh Type
6 DoFSelect the
Boat
geometrySet the
Inner Distance [m]
to 0.2 for the deformation regionSet the boat mass properties
Mass \({\sf [kg]}\)120
Center of Mass \({\sf [m]}\)-1.10-0.1385
Mom. Of Inertia \({\sf [kg m2]}\)100500100Set the
Relaxation
to 1
We use only half of the mass because of model symmetry |

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.
2 Set the constraints accordingly
Translation Constraint
Line
Rotation Constraint
Axis
Axis \({\sf [-]}\)0103 Set the restraints accordingly
Linear Restraint
Damper
Damping \({\sf [Ns/m]}\)30
Angular Restraint
Damper
Damping \({\sf [Nms/m]}\)30

20. Turbulence
For the purpose of this tutorial, we will model the turbulence phenomenon using the k-ω SST model.
Go to
Turbulence
panelSelect
RANS
turbulence formulationSelect \(k {-} \omega \; SST\) model

21. Transport Properties - Water
In order to define water and air, we need to go to the transport properties panel, and use predefined fluids properties from the material database.
Go to
Transport Properties
panelChange phase name from
phase1
to waterOpen Material Database
Pick up
water
from the listClick Apply

22. Transport Properties - Air
Repeat previous step for phase2 using air properties.
To assign material to the domain, the phase fraction parameter \(\alpha_{phase}\) 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 \(\alpha_{phase 1}=1\) means that the whole domain is filled only with the phase1, while \(\alpha_{phase 1}=0\) means that the domain is filled with the second phase.
We will assign \(\alpha_{phase}\) parameter in the later steps.
Change phase name from
phase2
to airOpen Material Database
Pick up
air
from the listClick Apply

23. Solution - PIMPLE
For the purpose of the simulation we will change PIMPLE algorithm parameters to increase stability:
Go to
Solution
panelSwitch to the
PIMPLE
tabIncrease
Outer Correctors
to 3Increase
Non-Orthogonal Correctors
to 2Uncheck
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.
Go to
Parameters
panelDefine new parameter
NameU
Formula2Press Enter or Create Parameter button
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.
Go to
Boundary Conditions
panelSelect the
bottom
boundaryChange the
Type
of velocity to theFixed Value
Set the Value \({\sf [m/s]}\)U00

26. Boundary Conditions - Inlet (Flow)
To model the inlet to the domain, we will assign the Inlet Velocity character and use the value of the "U" parameter as the inlet velocity value.
Select the
inlet
boundarySet the Velocity Inlet character
Set the velocity
Reference Value [m/s]
to U

27. Boundary Conditions - Inlet (Phases)
In addition to setting the flow conditions, selecting the inlet phase is also necessary.
Initially, we will specify pure air as the inlet phase. 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.
Switch tab to
Phases
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.
Select the
oulet
boundarySet the
Outflow
characterSwitch tab to
Flow
Set the velocity type and mean value accordingly
U
Type
Outlet Phase Mean Velocity
U
Umean \({\sf [m/s]}\)U
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)
Switch tab to
Phases
3 Set the \(\alpha_{water}\) parameters accordingly
\(\alpha_{water}\)Type
Variable Height
\(\alpha_{water}\) Upper Bound \({\sf [-]}\)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. The domain will initially be filled entirely with air, as indicated by a phase fraction \(\alpha_{air}=0\).
Go to
Initial Conditions
panelSet the velocity to U00

31. Initial Conditions - Patch
Using the water
geometry, we will overwrite the phase fraction value inside it. We will set the \(\alpha_{water}\) to 1
to fill the patched geometry with the water.
Switch to
Patch
tabEnable initialization on
water
geometryExpand Fields list
Select \(\alpha_{water}\) fraction for initialization
Set initial value of \(\alpha_{water}\) to 1
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 after the simulation has started.
Go to
Monitors
panelSwitch to
Sampling
tabSelect Create Slice
Set the slice normal vector align y-axis
Normal \({\sf [-]}\)010Expand Fields list
Check the velocity
U
Check the water phase \(\alpha_{water}\)

33. Monitors - Forces
Additionally, we will observe forces acting on the boat boundary.
Switch to
Forces
tabExpand
Monitored Boundaries
list and checkBoat

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.
Go to
RUN
panelSet the
Simulation Time [s]
to 10Change
Time Stepping
toAutomatic
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 \(\Delta t\) \({\sf [s]}\)1e-04
Max \(\Delta t\) \({\sf [s]}\)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.
Switch to
Output
tabSet the
Write Control
Interval [s]
to 0.05

36. Run - CPU
The calculation of this simulation is very time-consuming, due to the dynamic mesh and 2 phase model. To speed up the calculation process we recommend using at least 8 cores for this tutorial.
If you are using SimFlow free version (which allows only for 2 CPUs) you can use the contact form to Request 30-day Trial
Estimated computation time for 2 CPUs is over 5 hours.
Switch to
CPU
tabUse
parallel
modeIncrease the
Number of processors
Click Run Simulation button

37. Postprocessing - ParaView
Once the computations have been completed, we can perform advanced visualization of the results using ParaView.
Go to
POSTPROCESSING
panelClick on Run ParaView

38. ParaView - Load Results
Load the results into the program.
Turn on Toggle advanced properties
Uncheck option
Decompose polyhedra
Click Apply to load results into ParaView

39. 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 0.2 m from the boat is rigid and moves together with a boat. The mesh at the distance from 0.2 m to 1 m from the boat is able to move. Further than 1 m from the boat, the mesh is non-deformable.
Select
Surface with Edges
from the representation toolbar listSelect
pointDisplacement
from the variable listClick Rescale to Data Range
Play with an animation buttons to track the results of analysis

40. ParaView - Reflect the results (I)
During the simulation, only one half of the fluid domain was used. However, during the post-processing stage, we can replicate the second half of the domain.
To produce a visualization that is symmetrical, we will reflect the results across the plane of symmetry.
Select the case
Boat.foam
Extend the list of
Filters
from the top menuGo to
Alphabetical
Select
Reflect
from the list

41. ParaView - Reflect the results (II)
Choose the plane of the reflection
Y min
Click Apply

42. ParaView - Water Surface
We will focus on the water-air interface behaviour and observe the velocity map.
Select Clip from top menu
Change the clip type to
Scalar
Select
alpha.water
from the scalar listClick Refresh
Make sure
Invert
option is uncheckedClick Apply
Select the velocity
U
from the listClick on Rescale to Custom Data Range
Set the range from 0 to 3
Confirm by clicking Rescale

43. ParaView - Boat Geometry (I)
To display the boat geometry, we will read the result file once again and load only the boat boundary.
Select Open from top menu
Choose the
Boat.foam
file from case folderPress OK

44. ParaView - Boat Geometry (II)
Uncheck
internalMesh
from theMesh Regions
Check the
Boat
Press Apply

45. ParaView - Boat Geometry (III)
Similarly as before, we will reflect the boat geometry.
Select the new case name
Boat.foam
, go toFilters
, extendAlphabetical
and selectReflect
from the listChoose the plane of reflection
Y min
Click Apply
Select the
Solid Color
from the list

46. ParaView - Results
Play with animation buttons to investigate the time history of the flow.
