Fill out the form to download

Required field
Required field
Not a valid email address
Required field
Required field
  • Set up your own cloud-native simulation in minutes.

  • Documentation

    Tutorial: Incompressible Turbulent Airflow Around a Spoiler

    This article provides a step-by-step tutorial for the flow simulation around a GT car rear spoiler using the incompressible turbulent flow analysis type.

    incompressible turbulent airflow simscale
    Figure 1: Flow visualization across the spoiler


    This tutorial teaches how to:

    • Set up and run an incompressible turbulent flow simulation.
    • Assign boundary conditions, material, and other models to the simulation.
    • Mesh the geometry with the SimScale standard meshing algorithm.

    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 shows the geometry used for the simulation. It corresponds to a typical car spoiler, installed to increase the downforce in the rear axis:

    project workbench flow around a spoiler
    Figure 2: Workbench view 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 Original Spoiler and the second one is named Spoiler – Flow Region. The original model shows the geometry of the solid part to be analyzed:

    geometry model flow around a spoiler
    Figure 3: Model of the spoiler to be analyzed

    The Spoiler – Flow Region part contains the virtual wind tunnel representing the volume of air around the spoiler. Notice that, as the spoiler is symmetric, we simulate only one-half of the geometry to optimize simulation resources.

    The image below shows how the bounding box dimensions were chosen, relative to the chord length of the spoiler, \(L = \) 0.25 \(m\).

    extracted flow region flow around a spoiler
    Figure 4: Model and dimensions of the flow region around the spoiler; notice the usage of the symmetry.


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

    changing render mode workbench
    Figure 5: The viewer toolbar contains several visualization options, including render modes.

    You can check the details of the flow volume creation by selecting the Spoiler – Flow Region geometrical object item on the left, and clicking the ‘CAD mode’ icon:

    access cad mode flow around a spoiler
    Figure 6: Parameters of the enclosure creation operation

    The CAD mode environment will open, with the performed operations shown under History:

    cad model simscale
    Figure 7: CAD mode for the flow volume creation.

    In CAD mode, two operations were performed:

    1. External flow volume, to create the flow region (virtual wind tunnel), and
    2. Delete bodies, to remove the spoiler part from the model

    The details of the operations can be seen below:

    setting the face parameters within the simscale platform
    Figure 8: Parameters for the external flow volume operation

    As this is an incompressible analysis, only the flow volume is necessary to run the simulation. Therefore, the spoiler volume is deleted with the operation below:

    delete body operation cad mode
    Figure 9: Settings from the Delete bodies operation

    To exit from CAD mode, simply click on ‘Exit’ on the top-right corner.

    1.2 Create Saved Selections

    Saved selections are groups of faces used for boundary conditions or other assignments. By using them, the simulation setup can be done faster.

    For the simulation setup, we will use the Spoiler – Flow Region geometry. After selecting the geometry, you will find pre-defined saved selections on the right-hand side panel:

    saved selections flow around a spoiler
    Figure 10: Saved selections to help with the simulation setup

    Five of the needed sets are already provided in the template project, but the set for the flow inlet face is still missing. The picture below shows how to add it:

    creating a new saved selections flow around a spoiler
    Figure 11: Creating Saved Selections
    1. First, select the corresponding faces from the viewer (notice this is the one just in front of the spoiler).
    2. Click the ‘+’ icon next to Saved Selections in the scene tree.

    In the pop-up dialog that appears, name the set “Inlet” and click ‘Create new selection’.

    naming of a new saved selections flow around a spoiler
    Figure 12: Name and create the saved selections.

    1.3 Create the Simulation

    Now we can start with the simulation setup. Follow the steps shown in Figure 6 and click the ‘Create Simulation’ button located at the bottom right of the panel. The simulation library window appears to select the appropriate simulation type:

    simulation library flow around a spoiler
    Figure 13: SimScale simulation type widget

    Choose ‘Incompressible’ and click on ‘Create Simulation’.

    2. Set Up the Simulation

    A new simulation tree will appear on the left-hand side of the Workbench. The first entry of the simulation tree is the global settings of the simulation. For this tutorial, please keep the default values:

    simulation parameters flow around a spoiler
    Figure 14: Simulation global parameters

    From the Turbulence models available, this tutorial uses ‘k-omega SST’. For more details about its implementation, please check this page.

    2.1 Material

    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 flow around a spoiler
    Figure 15: SimScale materials library

    The material properties window will appear. The Flow Region volume is automatically selected because it is the only one present in the model. Therefore, please accept the selection by clicking on the checkmark.

    material definition, flow around a spoiler
    Figure 16: Material parameters for air and assignment of the flow region

    2.2 Boundary Conditions

    The image below contains an overview of the boundary conditions from this tutorial:

    boundary conditions overview, CFD analysis of a spoiler
    Figure 17: Boundary conditions overview for the spoiler tutorial

    To create a boundary condition, follow the steps shown in the picture below:

    creating boundary condition, flow around a spoiler
    Figure 18: 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 assign faces in the pop-up dialog (not shown in the picture).

    Now apply this process for the following boundary conditions:

    a. Spoiler Surface

    For the spoiler surfaces, a no-slip wall condition is used.

    Following the instructions in Figure 18, select ‘Wall’. Now, select the Spoiler saved selections to assign it to the boundary condition – You can also rename the boundary condition to ‘Spoiler’.

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

    spoiler boundary condition, simulation of flow around a spoiler
    Figure 19: Spoiler faces boundary condition

    b. External Walls

    For the External Walls, please create another ‘Wall’ boundary condition. Once the setup panel pops up, select the ‘External Walls’ entity set that was created before for the assignment. The Velocity definition is Slip, allowing non-zero velocity in the tangent direction:

    slip velocity for external walls in spoiler tutorial
    Figure 20: External walls boundary condition

    c. Inlet

    For the flow inlet face, a velocity inlet boundary condition will be used. Follow the same procedure as before to create a ‘Velocity inlet’ boundary condition and assign the ‘Inlet’ entity set.

    Set up the dialog as shown in the picture:

    inlet boundary condition
    Figure 21: Flow inlet boundary condition

    Define a fixed value velocity of ’10 \(m/s\)’ in the y-direction \((U_y)\).

    d. Outlet

    For the flow outlet face, a pressure outlet boundary condition will be used. Follow the same procedure as before to create a ‘Pressure outlet’ boundary condition and assign the ‘Outlet’ entity set.

    flow outlet boundary condition, spoiler cfd analysis
    Figure 22: Flow outlet boundary condition

    This tutorial uses the default settings for the pressure outlet condition.

    e. Floor

    For the floor below the spoiler, a moving wall boundary condition will be used. Create another ‘Wall’ boundary condition, and assign the ‘Floor’ entity set to it:

    floor boundary condition
    Figure 23: Floor boundary condition

    Select ‘Moving wall’ for (U) Velocity and assign ’10 \(m/s\)’ to the y-direction.

    f. Symmetry

    Finally, for the symmetry plane, create a ‘Symmetry’ boundary condition, assigning the ‘Symmetry’ saved selections.

    Set up the parameters as shown in the picture below:

    symmetry boundary condition
    Figure 24: Floor boundary condition

    3. Simulation Control

    One important setup in order to help the simulation achieve good results and converge faster is the Potential flow initialization. Toggle it on inside the Simulation Control tab, as shown in the figure:

    simulation control panel potential flow initialization
    Figure 25: Activate the ‘Potential flow initialization’ to achieve better results.

    4. Mesh

    For this tutorial, we are using the hex-dominant automatic mesher. Click on ‘Mesh’ from the simulation tree and define the global settings as follows. You can rename it as Hexahedral Mesh:

    mesh setting automatic hex-dominant global
    Figure 26: Global meshing settings for the Hex-dominant meshing tool.

    Do not generate the mesh just yet – click on the blue checkmark and save.

    Before generating the mesh, we want to set a mesh refinement to capture the wake more accurately. Therefore we will create a region refinement:

    creating a new region refinement in the simscale hex donimant mehser
    Figure 27: Adding a Region refinement.

    Click on the ‘+’ button next to Refinements and select ‘Region refinement’. This opens the settings panel.

    region refinement settings for meshing
    Figure 28: Region refinement settings

    Set the Maximum edge length to ‘0.01 \(m\)’ and click on ‘+’ button to create a ‘Cartesian box’ geometry primitive for the volume assignment:

    creating a cartesian box
    Figure 29: Creating a Cartesian box to refine the cells within this volume

    Define the following dimensions for the Cartesian box in meters as shown in the picture above.

    • Minimum x: ‘0’ \(m\)
    • Minimum y: ‘-0.1’ \(m\)
    • Minimum z: ‘-0.2’ \(m\)
    • Maximum x: ‘0.55’ \(m\)
    • Maximum y: ‘1.5’ \(m\)
    • Maximum z: ‘0.2’ \(m\)

    After saving the cartesian box settings, you are redirected to the region refinement settings. Assign the cartesian box that you just created. This ensures that all the cells within this box will have a maximum edge length of 0.01 \(m\).

    cartesian box assignment for region refinement of spoiler using hex mesh
    Figure 30: Assigning the newly created cartesian box for the region refinement of the wake behind the spoiler

    Save the settings and go back to the Mesh tab in the simulation tree and hit ‘Generate’ to create the mesh.

    After around 30 to 40 minutes, you will see this mesh:

    mesh from the spoiler tutorial
    Figure 31: Generated Hexahedral mesh

    Alternative Meshing Algorithms

    SimScale also offers other meshing algorithms, such as the Standard mesher, that works well for external aerodynamic applications. Please see this tutorial for airflow simulation around a vehicle for more details.

    5. Start the Simulation

    Now that the simulation setup is complete, a new simulation run can be created. For this, click the ‘+’ button next to Simulation Runs in the simulation tree. In the pop-up window, give a proper name to the run and click ‘Start’:

    creating simulation run flow around a spoiler
    Figure 32: Creating and starting a new simulation run

    This computation takes about an hour. 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.

    6. Post-Processing

    You can visualize your results by using SimScale’s online post-processor. We will visualize the pressure distribution on the spoiler, create a cutting plane, and animate the streamlines of the flow around the spoiler.

    6.1 Pressure Distribution

    One of the results of interest is the pressure distribution on the surface of the spoiler. Follow the steps below to visualize the same:

    • When entering the post-processor for the first time, check if you are at the last time step of the simulation and there are no pre-defined filters. Also, change the Coloring of Parts Color to ‘Pressure’.
    post-processor interface
    Figure 33: Make sure that you are at the last time and choose ‘Pressure’ as the Coloring of the model
    • The next step is to hide the enclosure. To do this, select the 6 external boundaries of the flow domain, and right-click on the viewer to ‘Hide the selection’:
    how to hide selected faces
    Figure 34: Hiding enclosure around the spoiler. To make the enclosure faces show again, you can right-click and select ‘Show all’.
    • After hiding the enclosure, you will get a clear visualization of the pressure distribution on the spoiler similar to the figure below:
    pressure on the spoiler
    Figure 35: Pressure distribution on a spoiler and highest at surfaces directly facing the flow

    Figure 35 shows high-pressure contours on the top of the spoiler. Given the low-pressure regions under the spoiler, this combination results in downforce.

    6.1 Cutting Planes

    A cutting plane can also be used to better understand the turbulence around the spoiler and its characteristics. To create a cutting plane, select ‘Cutting plane’ from the Filters panel.

    Next, place the cutting plane at the mid-section of the spoiler. Click on the arrow to the left of Position and set the values to ‘0.1, 1.5, 0.4’. Keep the Orientation normal to the ‘x-axis’. Switch Coloring to ‘Turbulent Kinetic Energy’. Finally, show the velocity vectors by sliding the toggle beside Vectors and changing the Coloring to black Solid color.

    turbulence kinetic energy field and velocity vectors around a spoiler on a cutting plane
    Figure 36: Cutting plane showing turbulence kinetic energy field around a spoiler and velocity vectors

    Here, we can see turbulence starts to occur when the flow hits the wing and is at its highest under and at the trailing edge of the wing.

    6.3 Streamlines and Animation

    Another result of interest is visualizing the streamlines around the spoiler. Follow the steps below to show the streamlines and animate them:

    how to choose particle trace entry position
    Figure 37: Creating a new particle traces filter. The seed face represents the origin of the traces.
    1. From the top filters ribbon, choose ‘Particle Trace’
    2. Make sure that the Pick Position selector is on
    3. Choose a seed for the particle traces at the inlet, just in front of the spoiler

    At this point, you can configure your particle traces so that the streamlines show relevant pictures. Change the number of particle traces by changing the values in #Seeds horizontally to ’50’ and #Seeds vertically to ‘8’. Change the Spacing to ‘1e-2’ and the Size to ‘1e-3’. Hide the walls of the fluid domain to see the streamlines around the spoiler. Finally, change the Coloring in Parts color to some contrasting white or grey solid color.

    particle trace settings
    Figure 38: Change the #Seeds horizontally to ’50’ and #Seeds vertically to ‘8’, the Spacing to ‘1e-2’ and the Size to ‘1e-3’

    After creating the particle trace filter, it is possible to animate it with an Animation filter. Please use the filter ribbon on the top to create a new ‘Animation’ filter. The Animation type will be ‘Particle Trace’.

    After the animation filter is set, you can press the play button playbutton to animate the traces:

    Animation 1: Flow streamlines around the spoiler with tip vortices at the trailing edge of the spoilers

    Animation 1 displays the airflow streamlines. The generated tip vortices, the up-wash, and the low speed close to the surface (blue portions of the streamlines) can be appreciated from the images.

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

    Congratulations! You finished the tutorial!


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

    Last updated: October 13th, 2023