Fill out the form to download

Required field
Required field
Not a valid email address
Required field

Documentation

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.

flow visualization drone simulation mrf rotating zone
Figure 1: Flow visualization across the drone rotating propeller.

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:

imported project drone simulation mrf rotating zone
Figure 2: Imported project in the SimScale Workbench.

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:

drone geometry including the rotating zone cylinder simscale
Figure 3: The original drone body with its four impellers. Due to symmetry only one impeller will be simulated.

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:

symmetry model drone simulation mrf rotating zone
Figure 4: Modeled domain, symmetry, and cylinder for rotating region.

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:

geometry detail drone simulation mrf rotating zone
Figure 5: Detail of the geometrical volumes present in the model
  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.

You can also create the flow region using the CAD mode, or in your own CAD following the instructions in this page.

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:

topological entity sets drone simulation mrf rotating zone
Figure 6: Topological entity sets.

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:

creating topological entity set drone simulation mrf rotating zone
Figure 7: Creating a topological entity set.
  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.

naming topological entity set drone simulation mrf rotating zone
Figure 8: Name and finish the topological entity set creation.

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:

create simulation drone simulation mrf rotating zone
Figure 9: Creating a new simulation.
  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:

simulation library drone simulation mrf rotating zone
Figure 10: SimScale simulation library.

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:

materials library drone simulation mrf rotating zone
Figure 11: SimScale materials library.

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

materials properties drone simulation mrf rotating zone
Figure 12: Material parameters for air and assignment of the flow region.

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:

creating boundary condition drone simulation mrf rotating zone
Figure 13: Creating a boundary condition.
  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:

drone faces boundary condition drone simulation mrf rotating zone
Figure 14: Drone faces boundary condition.

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:

symmetry planes boundary condition drone simulation mrf rotating zone
Figure 15: Symmetry planes boundary conditions.

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.

creating a custom atmospheric boundary condition in simscale
Figure 16: Custom inlet-outlet boundary condition for the faces open to atmosphere.
  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:

creating rotating zone drone simulation mrf rotating zone
Figure 17: Creating a MRF rotating zone.
  1. Expand Advanced concepts.
  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:

setup of mrf rotating zone
Figure 18: Creating the MRF rotating zone.

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:

numerics parameters drone simulation mrf rotating zone
Figure 19: Numerics setup.
  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:

mesh parameters drone simulation mrf rotating zone
Figure 20: Mesh setup.

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:

creating simulation run drone simulation mrf rotating zone
Figure 21: Creating and starting a new simulation run.

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.

access to the post-processor
Figure 22: Click ‘Post-process results’ in your Run dialog or ‘Solution Fields’ under your run to access the post processor

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.
post-processor interface propeller
Figure 23: Make sure that the post-processor is at the last timestep and to remove all predefined filters
  • Hide the walls surrounding the drone by selecting them, right-clicking on the post-processor, and choosing ‘Hide selection’.
how to hide selections in simscale post-processor
Figure 24: Select the walls surrounding the drone, right-click on the mouse, and select ‘Hide selection’ to hide the walls.
  • Change the Coloring to ‘Pressure’ in the Filters panel to show the pressure distribution on the drone.
how to change visualized quantities
Figure 25: In the Filters panel, change the Coloring to ‘Pressure’.
  • 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 view button besides ‘Rotating Zone’ in the Mesh dialog.
pressure distribution on the surfaces of the drone
Figure 26: Pressure distribution on the surface of the drone ranging from -300 to 300 \(Pa\). The bottom surfaces of the propeller and the drone arm are high pressure zones.

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.
how to select particle traces in simscale post processor
Figure 27: Select ‘Particle Trace’ after clicking the ‘Add Filter’ button in the Filters panel.
  • Select the origin of the particle traces by clicking the pick position button icon beside Position and placing it at the bottom of the drone.
how to choose origins of the streamlines
Figure 28: Click the icon besides Position to choose the origin of the streamlines and place 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’.
particle traces settings
Figure 29: Change the #Seeds horizontally and #Seeds vertically to ’40’, so that there are 40 origin points vertically and horizontally. the Spacing and Sizing to ‘1e-3’.
  • 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 \(m/s\).
particle traces for drone simulation
Figure 30: Velocity streamlines through the drone ranging from 0 to 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.
first step to creating a cutting plane
Figure 31: Select ‘Cutting Plane’ after clicking the ‘Add Filter’ button in the Filters panel.
  • 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.
cutting plane settings for drone simscale
Figure 32: Replicate the cutting plane settings to create a cutting plane in the propeller region

The cutting plane will look similar to the figure below:

cutting plane post processor drones
Figure 33: Cutting plane along the propeller of a drone

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

Contents
Data Privacy