Sloshing Tank - CFD Simulation CFD Software Tutorial

In this tutorial, we will explore the phenomenon of water sloshing inside a cistern during braking. This occurs due to the inertial force that pushes the water. We will conduct two analyses: the first one will involve studying the tank without any support structure, while the second one will involve analyzing the tank with internal baffles. You will learn how to simulate rigid body motion and model an internal 2D wall within the mesh. Finally, we will compare the forces acting on the cistern for both cases and plot them on one chart.

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 sloshing tank no baffles

Firstly we need to Download GeometriesBaffle_1Baffle_2Tank

Although the baffles are not involved in the first simulation we will import them at this stage. We can omit them when creating the first mesh and include them in the second simulation.

The STL format does not contain the unit information which are defined during the geometry export. If we do not know the exported unit, we can estimate it based on the total size of the model. The size is displayed next to Geometry size label. In our case, the default unit meter is correct.

Inside the tank, there are two baffles. To view the baffles we will reduce tank opacity.

The imported geometry is made up of a single surface. We need to split it into multiple faces for further processing.

To make sharp edges visible, we will use Extract Features operation. These edges will indicate additional mesh refinement regions.

In order to create the mesh, we need to specify geometries options used during the meshing. In this tutorial, we will analyze two configurations: with and without baffles. We will start with the tank itself and skip baffles for now.

Now we will define the base mesh. The box geometry determines the background mesh.

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

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

Everything is now configured and ready to be meshed.

After the meshing is finished the mesh will appear in the graphics window. The mesh should consist of only a single boundary.

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

To model tank deceleration we will use a dynamic mesh feature. The dynamic mesh allows transforming mesh by moving its nodes. There are several types of mesh deformation available. In this tutorial, we will use the Rigid type to model mesh translation as a whole.

The external file displacement.dat stores the motion data that we will import to SimFlow. The data describes deceleration from the initial velocity 11.853 m/s to 0 m/s within 5 s .

Download Filedisplacement.dat

In the turbulence panel, enable turbulence modeling and select Raynolds Averaged Navier Stokes (RANS). For the purpose of this tutorial, we will model the turbulence phenomenon using the \(k{-} \varepsilon\) model.

In the transport properties panel we will define water and air properties. We will leave the default values for phase1 (water) and phase2 (air). To assign each of the materials to the domain, the phase fraction parameter \(\alpha_{phase}\) is used. The parameter determines the proportion of each fluid in the given point in space. The phase fraction value varies in range from 0 to 1, where \(alpha_{phase1}=1\) denotes phase1, while \(alpha_{phase1}=0\) denotes remaining fluid - the second phase.

The mesh consists of only one tank wall boundary. For this boundary, we will apply the velocity that matches the initial velocity of the tank.

Before we will set the initial condition we need to define the water region. For this purpose, we will create a box that will indicate the initial location of water.

Before we will start the calculation we need to define the fluid state at the time zero. We will specify velocity to be equal to -11.853 m/s which corresponds to the initial tank velocity. Phase fraction \(\alpha_{water} =0\) tells us that the whole domain is filled with air by default.

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 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 variables that will be sampled. Note that runtime post-processing can only be defined before starting calculations and can not be changed later on.

In order to track the sloshing force on the tank boundary, we will use the force monitor.

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), maximal time step value and Courant number.

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

To speed up the calculation process, take advantage of parallel computing and increase the number of CPUs based on your PC’s capability. The free version allows you to use only one processor (serial mode). To get the full version, you can use the contact form to Request 30-day Trial

Estimated computation time for serial mode: 1,5 hours

Slices tab appears next to Residuals. Under this tab, we can preview results on the defined slice planes. The results preview is available during the calculation and we can track it on a regular basis. The newly calculated time step will be actualized automatically as long as the time selector points to the latest time step.

Additional force tab appears next to Slices . Under this tab, we can view force plots. The results preview is available during the calculation and we can use it to track the progress of the simulation as well.

We will use this simulation as a starting point for the second configuration. To do so we will save the current model under a new name without the results.

After saving, we will open a new case.

In the new case, we will add the baffles inside the tank. The baffles geometries are already loaded in SimFlow but have not been used yet. We can just turn them on and remesh the model.

Repeat these steps for the second baffle.

We will use the same base mesh setup so we can go directly to the meshing step.

We have already defined the initial velocity of the tank. Now, we need to assign the velocities to the remaining walls. We will copy the boundary conditions from the tank to the others.

Previously fluid was acting only on the tank boundary. In the current mesh, we have additional walls that should participate in force calculation as well.

Finally, we can run the simulation using the same parameters as previously.

We can view the results on the slice.

Under the force tab, we will display the resultant force acting on a tank caused by fluid deceleration. We will add the results from the previous simulation (without the baffles) and compare them on the same chart.

New data series will be added to the chart. We will hide the unnecessary data series for clarity.

We will leave only the sloshing force (force along X direction).

Finally, we can compare the results from both configurations. We can see that the peak force was reduced by 30% by using baffles.

This concludes the tutorial, covering all the aspects we intended to showcase. To create a finely tuned presentation of the results, you may take advantage of the seamless integration with ParaView. You can easily open simulation results in ParaView with a single click from SimFlow.

In ParaView, you can perform typical and advanced postprocessing tasks such as displaying streamlines, contour plots, vector fields, line or time plots, and calculating volume or surface integrals.

To familiarize yourself with the ParaView capabilities, it’s worth checking out our video tutorial, Paraview CFD Tutorial - Advanced Postprocessing in ParaView, in which we demonstrate some of the most commonly used post-processing techniques.

Paraview CFD Tutorial - Advanced Postprocessing in ParaView