Required field
Required field
Required field

# Tutorial: Drone Simulation Using Rotating Zones

This article provides a step-by-step tutorial for the flow simulation around a drone using rotating zones (the propeller) using the moving reference frame (MRF) modelling technique.

This tutorial teaches how to:

• Setup and run an incompressible flow simulation.
• Assign boundary conditions, material, and other models to the simulation.
• Mesh the geometry with the SimScale standard meshing algorithm.
• Set up a moving reference frame (MRF) rotating zone.

The typical SimScale workflow will be followed:

• Prepare the CAD model for the simulation.
• Set up the simulation.
• Set up the mesh.
• Run the simulation and analyze the results.

## 1. Prepare the CAD model and Select the Analysis Type

First of all, click the button below. It will copy the tutorial project containing the geometry into your own workbench.

The following picture demonstrates what should be visible after importing the tutorial project:

### 1.1 Required CAD Preparation: Rotating Zones

You can see that there are two geometries in the imported project. The first one is called Drone and the second one is called Volume Region. The drone model shows the body with its four propellers and a cylinder surrounding the region that will rotate:

An important optimization in the simulation is achieved by noticing that this model has two planes of symmetry. This means that we can get away with modelling only one-quarter of the geometry. This is performed in the creation of the bounding box, which covers the desired quarter as shown in the following picture:

A crucial aspect of the modelling is the creation of the cylinder for the rotating region. This cylinder should cover (with some margin) the faces that will be included in the rotation model. The one used in our case covers the drone propeller, and can be found by having a closer look at the Drone Parts geometry:

1. The flow region (gray), which models the volume filled by fluid. Notice that it has a void representing the space occupied by the drone structure and propellers, and that it uses the symmetry of the model as explained above.
2. A cylinder covering the propeller (blue). This cylinder will be used to create the region of cells rotating and the MRF concept.

Tip

You can better visualize the internal faces by changing the render mode to translucent surfaces. Do this by using the top bar at the viewer.

Important

In case you want to model your own drone, or any external rotating geometry for that matter, you should always follow the modelling convention outlined in this section: a flow region volume with the removed bodies and a cylinder around the rotating region.

### 1.2 Create the Topological Entity Sets

Topological entity sets are groups of faces so boundary conditions or other assignments can be done faster.

They can be found at the panel on the right side of the workbench:

Two of the needed sets are already provided in the project, but the set for the two symmetry planes is still missing. The picture below shows how to add it:

1. First, select the corresponding two faces from the viewer (notice these are the ones that intersect with the drone).
2. Click the ‘+’ icon next to Topological Entity Sets in the right panel.

In the pop-up dialog that appears, name the set ‘Symmetry’ and click Create new set.

### 1.3 Create the Rotating Zones Drone Simulation

Now we can start with the simulation setup. Follow the steps presented in the picture below to create a new simulation for our geometry:

1. Select the Drone Parts geometry from the left panel.
2. Click the Create Simulation button of the dialog

The simulation library window appears to select the appropriate simulation type:

Choose Incompressible and click Create Simulation. A new simulation tree will appear at the left panel and a pop-up with the simulation settings, which we will leave at the default values.

## 2. Set Up the Rotating Zones Simulation

### 2.1 Material Model

To define and assign a material, click the ‘+’ icon next to Materials. Doing so, the SimScale material library will pop up. Select Air from the materials library and click Apply:

The material properties window will appear. Assign the Flow Region volume and accept the selection with the check-mark button.

### 2.2 Boundary Conditions

Now we will define the boundary conditions. In order to create a boundary condition, follow the steps shown in the picture below:

1. Click the ‘+’ button next to Boundary Conditions.
2. Select the proper type from the drop-down menu.
3. Set up the physical parameters and assigned faces in the pop-up dialog (not shown in the picture).

Now apply this process for the following boundary conditions:

#### a. Drone Surface

For the drone faces, a no-slip wall condition is used.

Create a new boundary condition by following the instructions in figure 11 and select ‘Wall’. Now select the Drone topological entity set to assign it to the boundary condition. You can also rename the boundary condition to ‘Drone’.

Leave all parameters as default, as shown in the picture:

#### b. Symmetry Planes

For the symmetry planes, a Symmetry boundary condition is used.

Create it according to the steps presented in figure 11. Once the setup panel pops up, select the Symmetry entity set that was created before for the assignment.

The setup should look as shown in the picture:

#### c. Atmosphere

For the faces open to the atmosphere, a custom boundary condition will be used. Follow the same procedure as before to create a custom boundary condition.

1. As we do not know if the direction of flow at these faces will be inlet or outlet, it will allow the solver to automatically compute it. Therefore we select ‘pressure inlet-outlet’ for the (U) Velocity setup.
• Define ‘Total pressure’ for the gauge pressure option and assign 0 Pa, which corresponds to atmospheric pressure.
• We set the turbulence quantities, Turb. kinetic energy and specific dissipation rate to ‘zero gradient’, so that the solver calculates them.
2. Now assign the topological set Atmosphere to the boundary condition.
3. If you want you can also rename the boundary condition to ‘Atmosphere’ to keep an overview.

### 2.3 Propeller Rotation

To specify the rotating propeller in our model, a moving reference frame (MRF) rotating zone is employed. The following picture shows how to create it:

2. Click the ‘+’ button next to rotating zones.
3. Select MRF rotating zone from the list.

In the pop-up window, assign the Rotating Zone volume and set up the parameters as shown in the picture:

You can read more on the topic of MRF rotating zones at the corresponding documentation page:

### 2.4 Numerics and Simulation Control

For the numeric solver parameters, there is only one parameter that will be changed: The Number of non-orthogonality correctors. This will allow the solver to achieve a better solution for the tetrahedral mesh created by the SimScale standard mesher algorithm:

1. Select Numerics from the tree at the left panel.
2. Set the Number of non-orthogonal correctors to 4.

The Simulation control parameters are left as default.

## 3. Mesh

For the mesh setup, all settings are left as default, as we will make use of the SimScale standard mesh algorithm. You do not need to click Generate either, as the mesh will be computed as part of the simulation run:

Did you know?

It’s necessary to define cell zones in the mesh whenever we want to apply a specific property, such as a rotating motion, to a subset of cells.

The standard mesher algorithm automatically creates the necessary cell zones whenever Physics-based meshing is enabled. Since we are using physics-based meshing in this tutorial, the algorithm will take care of the cell zone definition.

If you are using a different mesher, you can learn alternative ways to define a cell zone in the rotating zones documentation page.

## 4. Start the Rotating Zones Simulation

Now that the simulation setup is complete, a new simulation run can be created to perform the computation. In order to do so, click the ‘+’ button next to Simulation Runs at the left panel. In the pop-up window, give a proper name to the run and click Start:

This computation takes about 36 minutes to be completed. If you can’t wait to see the results, at the end of the article you will find a link to the completed version of the project.

## 5. Post-Processing

After the simulation is finished, access the post-processor by clicking the ‘Post-process results’ button or ‘Solution Fields’ under your run.

### 5.1 Surface Visualization

One of the most important things to observe in the drone is the pressure distribution on the surfaces of the drone. Follow the steps below to show pressure on the surfaces of the drone:

• Make sure that you are at the last timestep of the simulation and no filters are applied.
• Hide the walls surrounding the drone by selecting them, right-clicking on the post-processor, and choosing ‘Hide selection’.
• Change the Coloring to ‘Pressure’ in the Filters panel to show the pressure distribution on the drone.
• As you can see, the pressure distribution is not informative for the shown range. Change the range of the scale in the legend to -300 to 300 $$Pa$$. To make the pressure distribution clearer hide the rotating zone by clicking the view symbol besides ‘Rotating Zone’ in the Mesh dialog.

As you can see from Figure 26, the highest pressures are on the arm of the drone which is due to the air pushed down by the propellers hitting the arm and on the bottom surface of the propellers causing lift generation.

### 5.2 Streamlines

We will continue showing the airflow through the propellers of the drone by using streamlines. See the steps below to create them:

• Click the ‘Add Filter’ button in the Filters panel and select ‘Particle Trace’. This will lead to the settings for the particle trace setup.
• Select the origin of the particle traces by clicking the icon beside Position and placing it at the bottom of the drone.
• Next, configure the streamlines so that it will be more clear. Change the #Seeds horizontally and #Seeds vertically to ’40’, so that there are 40 origin points vertically and horizontally. Change the Spacing and Sizing to ‘2.5e-4’.
• Since the velocity through the drone is in the range of 20-30 $$m/s$$, adjust the scale so that the maximum value is 25 $$m/s$$.

From Figure 30, it can be seen that the flow velocity accelerates when going through the drone and creates a swirl due to rotating movement of the propellers.

### 5.3 Cutting Plane

To comprehend the velocity contours in the areas of the propeller better, create a cutting plane by following the steps below:

• Click the ‘Add Filter’ button in the Filters panel and select ‘Cutting Plane’. This will show you the settings of the cutting plane.
• Change the position of the Orientation of the cutting plane to the ‘Y’ axis and the Position to coordinates: ‘0.6, 0.035, 0.6’. Slide the Vectors slider and change the Coloring of the vectors to a black ‘Solid color’. The Scale factor of the vectors should be ‘0.03’ with a Grid Spacing of ‘0.005’. Project the vectors onto the plane by sliding the slider beside Project vectors onto Plane.

The cutting plane will look similar to the figure below:

From Figure 33, we can see that the velocity is higher within the propeller rotating zone. Air being pushed towards the propeller center can also be observed as a result of pressure difference and it moves in rotation which is in accordance with the movement of the propellers.

You can analyze your results further with the SimScale post-processor. Have a look at our post-processing guide to learn how to use the post-processor.

Congratulations! You finished the drone with rotating zones tutorial!

Note

If you have questions or suggestions, please reach out either via the forum or contact us directly.

Last updated: May 20th, 2021