Back to all tutorials

Droplet - CFD Simulation SimFlow Tutorial

1. Introduction

The Droplet tutorial serves as an introduction to SimFlow. In this tutorial, we will present the simulation of free free-falling droplet into the tank (geometry created directly in SimFlow). This simulation considers a 2D analysis of a multi-phase (water + air), incompressible flow.

2. 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

3. Create Case

Open SimFlow and create a new case named droplet

  1. Click New
  2. Provide name droplet
  3. Click Create to open a new case

4. Meshing parameters

We will start by creating a 2D mesh. This can be accomplished by choosing the Plate type as the background mesh.

  1. Go to Hex Meshing panel
  2. Go to Base tab
  3. Select Plate as a Base Mesh Type
  4. Define minimum and maximum extend
    Min \({\sf [m]}\)00
  5. Define the number of divisions
  6. Change boundary type to wall for all background mesh boundaries
droplet 02 hex meshing

5. Start Meshing

We will start by creating a 2D mesh. This can be accomplished by choosing the Plate type as the background mesh.

Now we are ready to create our simple mesh.

  1. Go to Mesh tab
  2. Press the Mesh button to start meshing process
droplet 03 meshing

6. Mesh

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

  1. Click ViewXY or press CTRL+F1 to orient view plane
  2. Click Fit View to zoom the geometry
droplet 04 mesh view

7. Create Geometry - Droplet

To indicate the initial shape of the droplet we will use cylinder geometry.

  1. Go to Geometry panel
  2. Select Create Cylinder
  3. Change geometry name from cylinder_1 to droplet
  4. Set the origin
    Origin \({\sf [m]}\)0.250.4-0.1
  5. Set the cylinder dimensions
    Length \({\sf [m]}\)0.2
    Radius \({\sf [m]}\)0.025
droplet 05 droplet geometry

8. Create Geometry - Water

Additionally, we would like the droplet to fall down into the tank partially filled by water. To fill the bottom part of the domain with the water we will add another geometry.

  1. Add a new geometry by clicking Create Box
  2. Change geometry name from box_1 to water
  3. Set the origin and box dimensions
    Origin \({\sf [m]}\)00-0.1
    Dimensions \({\sf [m]}\)
droplet 06 water geometry

9. Create Geometry - Water Refinement

To be able to better resolve water behavior, we will create an area with a higher mesh resolution. To do this, we will add two more box geometries.

  1. Select Create Box
  2. Change geometry name from box_1 to water_refinement
  3. Set the origin and box dimensions
    Origin \({\sf [m]}\)00-0.1
    Dimensions \({\sf [m]}\)
droplet 07 water refinement geometry

10. Create Geometry - Droplet Refinement

The second refinement box will be located at the path of the falling droplet.

  1. Select Create Box
  2. Change geometry name from box_1 to droplet_refinement
  3. Set the origin and box dimensions
    Origin \({\sf [m]}\)0.20.3-0.1
    Dimensions \({\sf [m]}\)
droplet 08 droplet refinement geometry

11. Refine Mesh (I)

  1. Go to Mesh panel
  2. Expand the Options list next to default region
  3. Select Refine
droplet 09 refine regions

12. Refine Mesh (II)

  1. Check the refinement regions
  2. Uncheck the Z axis in Refinement Directions
  3. Click Refine
droplet 10 refine mesh

13. Display Mesh

Check the refinement region by hiding the geometries and displaying mesh.

  1. Click Graphic Object List
  2. Uncheck Geometry
To hide the Graphics Objects panel press the Esc key.
droplet 11 refine mesh check 2

14. Select Solver - Inter

To analyze water behavior we will use Inter (interFoam) solver. This solver 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
  5. Click Select button to confirm
droplet 12 select solver

15. Transport Properties - Water

Now we will define the transport properties for both fluids.

  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
droplet 13 transport prop water

16. Transport Properties - Air

Repeat this step for phase2 using air properties.

  1. Change phase name from phase2 to air
  2. Open Material Database
  3. Pick up air from the list
  4. Click Apply
droplet 14 transport prop air

17. Operating Conditions - Gravity

  1. Go to Operating Conditions panel
  2. Define gravitational acceleration along negative Y-axis
    g \({\sf [m/s^2]}\)0-9.810
droplet 15 operating conditions

18. Initial Conditions - Droplet

We will use the droplet geometry to select the region where water phase fraction should be initially applied.

  1. Go to Initial Conditions panel
  2. Switch to Patch tab
  3. Enable initialization on droplet
  4. Expand Fields list
  5. Select \(\alpha_{water}\) fraction for initialization
  6. Set initial value of \(\alpha_{water}\) to 1
droplet 16 initial condition droplet

19. Initial Conditions - Water

Repeat the step for water geometry.

  1. Enable initialization on water
  2. Expand Fields list
  3. Select \(\alpha_{water}\) fraction for initialization
  4. Set initial value of \(\alpha_{water}\) to 1
droplet 17 initial condition water

20. Monitors - Create Slice

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.

  1. Go to Monitors panel
  2. Switch to Sampling tab
  3. Select Create Slice
  4. Expand Fields list
  5. Check U and \(\alpha_{water}\)
droplet 18 monitor slice v2

21. Run - Time Controls

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 the Courant number. In our case, we will reduce the default Courant number for better stability and quality.

  1. Go to RUN panel
  2. Change Time Stepping to Automatic
  3. Set initial time step, time step limit and Courant number accordingly
    Initial \(\Delta t\) \({\sf [s]}\)5e-03
    Max \(\Delta t\) \({\sf [s]}\)0.1
    Max Co \({\sf [-]}\)0.5
droplet 19 run time controls

22. Run - Output

It is very important to control when results should be stored on the hard drive. This is especially important for the transient simulations where users are interested in the whole flow history saved as a collection of the snapshots.

  1. Switch to Output tab
  2. Set Write Control Interval [s] to 0.02
    (solver will store results on the hard drive every 0.02 second of the simulation)
  3. Click Run Simulation button
droplet 20 run output

23. Results

When calculations will begin SimFlow automatically will switch view to the Residuals tab, where we can observe the convergence of our simulation. This is very handy for steady-state simulations when we try reaching low residuals levels. In case of transient simulation, we would rather like to see how our flow develops as simulation time progress.

  1. Switch to Slices tab
  2. Choose alpha.water field
  3. Click Adjust range to data
  4. Play with an animation buttons to track the results of analysis
droplet 21 results

24. Advanced Postprocessing with ParaView

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.