The following picture demonstrates what should be visible after importing the tutorial project:
1.1 Required CAD Preparation
You can see that there are two geometries in the imported project. The first one is called Drone Parts and the second one called Drone – Original. The original model shows the drone model with its four propellers:
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:
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.
A cylinder covering the propeller (blue). This cylinder will be used to create the region of cells rotating and the MRF concept.
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.
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 assignements 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:
First, select the corresponding two faces from the viewer (notice these are the ones that intersect with the drone).
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 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:
Select the Drone Parts geometry from the left panel.
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 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:
Click the ‘+’ button next to Boundary Conditions.
Select the proper type from the drop-down menu.
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:
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.
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.
Now assign the topological set Atmosphere to the boundary condition.
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:
Expand Advanced concepts.
Click the ‘+’ button next to rotating zones.
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:
Select Numerics from the tree at the left panel.
Set the Number of non-orthogonal correctors to 4.
The Simulation control parameters are left as default.
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:
Now we need to specify that the rotating zone volume corresponds to a cell zone, and not a different region. In order to create a cell zone, click the ‘+’ button next to Cell zones under Mesh at the left panel, then assign the Rotating Zone volume as shown in the picture:
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.
The following result plots were generated using the SimScale online post-processor, and they display the computed flow field around the drone due to the propeller rotation:
This plot shows the airflow velocity magnitude across a cutting plane, and black arrows for flow direction. Here the wake created by the propeller can be appreciated alongside the range of flow speed.
This second plot displays the air flow stream lines. It displays the vorticity and the speed variation.
You can analyze your results 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!
Strictly Necessary Cookies
Strictly Necessary Cookie should be enabled at all times so that we can save your preferences for cookie settings.
If you disable this cookie, we will not be able to save your preferences. This means that every time you visit this website you will need to enable or disable cookies again.