Ship Hull - CFD Simulation SimFlow Tutorial

In this tutorial, you’ll discover how to simulate mesh deformation in SimFlow. An instance of this is the transformation of a 6DOF mesh, which results from the forces acting on a ship’s hull while it sails. The simulation considers a two-phase flow consisting of water and air, as well as Dynamic Mesh functionality with applied constraints.

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

Open SimFlow and create a new case named Boat

Firstly we need to Download GeometryBoat. The geometry will be imported in the same units as it was exported to the STEP format.

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

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

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

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.

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

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.

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

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.

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.

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

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

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

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.

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.

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

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.

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.

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

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

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.

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.

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.

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.

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 \(\alpha_{air}=0\).

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.

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.

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

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.

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

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.

Once the computations have been completed, we can perform advanced visualization of the results using ParaView.

Load the results into the program.

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.

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.

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

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

Similarly as before, we will reflect the boat geometry.