# Droplet - CFD Simulation

Source: https://help.sim-flow.com/tutorials/droplet
Last updated: 2026-10-14

[Video](https://help.sim-flow.com/tutorials/images/droplet.mp4)

## 1. Introduction

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

## 2. Download SimFlow

SimFlow is a general-purpose [CFD Software](https://sim-flow.com/download/cfd-simulation-software/)

To follow this tutorial, you will need the SimFlow free version. You may download it via the following link:
[Download SimFlow](https://sim-flow.com/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

![simflow-launcher](https://help.sim-flow.com/tutorials/images/launcher-droplet.png)

## 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 extent
   *Min \({\sf [m]}\)*`0``0`
   *Max \({\sf [m]}\)*`0.5``0.5`
5. Define the number of divisions
   *Division*`80``80`
6. Change boundary type to `wall` for all background mesh boundaries

![droplet 02 hex meshing](https://help.sim-flow.com/tutorials/images/droplet/droplet-02-hex-meshing.png)

## 5. Start Meshing

Now we are ready to create our simple mesh.

1. Go to `Mesh` tab
2. Press the **Mesh** button to start the meshing process

![droplet 03 meshing](https://help.sim-flow.com/tutorials/images/droplet/droplet-03-meshing.png)

## 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](https://help.sim-flow.com/tutorials/images/droplet/droplet-04-mesh-view.png)

## 7. Create Geometry - Droplet

To indicate the initial shape of the droplet, we will use a 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 \({\sf [m]}\)*`0.25``0.4``-0.1`
5. Set the cylinder dimensions
   *Length \({\sf [m]}\)*`0.2`
   *Radius \({\sf [m]}\)*`0.025`

![droplet 05 droplet geometry](https://help.sim-flow.com/tutorials/images/droplet/droplet-05-droplet-geometry.png)

## 8. Create Geometry - Water

Additionally, we would like the droplet to fall down into the tank partially filled with 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 \({\sf [m]}\)*`0``0``-0.1`
   *Dimensions \({\sf [m]}\)*`0.5``0.2``0.2`

![droplet 06 water geometry](https://help.sim-flow.com/tutorials/images/droplet/droplet-06-water-geometry.png)

## 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 \({\sf [m]}\)*`0``0``-0.1`
   *Dimensions \({\sf [m]}\)*`0.5``0.3``0.2`

![droplet 07 water refinement geometry](https://help.sim-flow.com/tutorials/images/droplet/droplet-07-water-refinement-geometry.png)

## 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 \({\sf [m]}\)*`0.2``0.3``-0.1`
   *Dimensions \({\sf [m]}\)*`0.1``0.2``0.2`

![droplet 08 droplet refinement geometry](https://help.sim-flow.com/tutorials/images/droplet/droplet-08-droplet-refinement-geometry.png)

## 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](https://help.sim-flow.com/tutorials/images/droplet/droplet-09-refine-regions.png)

## 12. Refine Mesh (II)

1. Check the refinement regions
   `droplet_refinement`
   `water_refinement`
2. Uncheck the **Z** axis in `Refinement Directions`
3. Click **Refine**

![droplet 10 refine mesh](https://help.sim-flow.com/tutorials/images/droplet/droplet-10-refine-mesh.png)

## 13. Display Mesh

Check the refinement region by hiding the geometries and displaying the 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](https://help.sim-flow.com/tutorials/images/droplet/droplet-11-refine-mesh-check-2.png)

## 14. Simulation Type

We want to analyze the behavior of a water droplet. For this purpose, we will use a transient simulation of two immiscible fluids (water and air) using the free-surface method.

![Simulation Panel](https://help.sim-flow.com/assets/images/go-to-simulation-panel@2x.png)

![Step 1](https://help.sim-flow.com/assets/images/solvers-selection/interFoam/01_multiphase@2x.png)

![Step 2](https://help.sim-flow.com/assets/images/solvers-selection/interFoam/02_free_surface@2x.png)

![Step 3](https://help.sim-flow.com/assets/images/solvers-selection/interFoam/03_immiscible@2x.png)

![Step 4](https://help.sim-flow.com/assets/images/solvers-selection/interFoam/04_2_fluids@2x.png)

![Step 5](https://help.sim-flow.com/assets/images/solvers-selection/interFoam/05_apply@2x.png)

## 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](https://help.sim-flow.com/tutorials/images/droplet/droplet-13-transport-prop-water.png)

## 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](https://help.sim-flow.com/tutorials/images/droplet/droplet-14-transport-prop-air.png)

## 17. Operating Conditions - Gravity

1. Go to `Operating Conditions` panel
2. Define gravitational acceleration along negative Y-axis
   *g \({\sf [m/s^2]}\)*`0``-9.81``0`

![droplet 15 operating conditions](https://help.sim-flow.com/tutorials/images/droplet/droplet-15-operating-conditions.png)

## 18. Initial Conditions - Droplet

We will use the `droplet` geometry to select the region where the 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](https://help.sim-flow.com/tutorials/images/droplet/droplet-16-initial-condition-droplet.png)

## 19. Initial Conditions - Water

Repeat the step for the *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](https://help.sim-flow.com/tutorials/images/droplet/droplet-17-initial-condition-water.png)

## 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 postprocessing can only be defined before starting calculations and cannot be changed later on.

1. Go to `Monitors` panel
2. Switch to `Sampling` tab
3. Select **Create Slice**
4. Set the origin to
   *Point \({\sf [m]}\)*`0.25``0.25``5e-03`
5. Expand **Fields** list
6. Check *U* and *\(\alpha_{water}\)*

![droplet 18 monitor slice v2](https://help.sim-flow.com/tutorials/images/droplet/droplet-18-monitor-slice-v2.png)

## 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](https://help.sim-flow.com/tutorials/images/droplet/droplet-19-run-time-controls.png)

## 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](https://help.sim-flow.com/tutorials/images/droplet/droplet-20-run-output.png)

## 23. Results

When calculations begin, SimFlow will automatically switch the 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 residual levels. In the case of a transient simulation, we would rather like to see how our flow develops as simulation time progresses.

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

![droplet 21 results](https://help.sim-flow.com/tutorials/images/droplet/droplet-21-results.png)

## 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 postprocessing techniques.

[Paraview CFD Tutorial - Advanced Postprocessing in ParaView](https://www.youtube.com/watch?v=5M6VgXyHB60&list=PLy7xPqn9xXckoD2gZgPpv8mrxillJ9PWU&index=21)