Tutorial: Incompressible turbulent airflow around a front wing

In this tutorial, aerodynamic analysis of a F1 frontwing is presented. The flow around the wing is modeled as an incompressible, turbulent flow using a k-omega SST turbulence model. This tutorial is based on the first part of the SimScale F1 Simulation workshop series about aerodynamics.

Tutorial Link:

Import tutorial case into workbench


Import tutorial project

  • To start this tutorial, you have to import the tutorial project into your ‘Dashboard’ via the link above.
  • Once the ‘Work bench’ is open you will be in the ‘Geometries’ tab.
  • Click on the CAD model named “FrontWing” to load the CAD model in the viewer.
  •  The CAD model is displayed in the viewer like shown in the figure below
  • You can interact with the CAD model as in a normal desktop application

Create the flow domain

  • In order to calculate the flow around the frontwing, you need to create a new geometry for the flow region
  • You can do this using an enclosure. Therefore add the geometry operation “enclosure” to the Geometry HalfFrontwing, as shown in the following pictures.
Adding a geometry operation
  • Now you need to define the dimensions of the flow domain. We recommend you coose the settings as pictured in the figure below
  • Now press start, after a few minutes the closure is finished and you can create a new simulation
Creating an enclosure

Create a New Simulation

  • To create a new simulation click on the ‘+’ option next to the ‘Simulations’ tab
  • Select the ‘Incompressible Flow Analysis type and click ‘Ok’
  • After clicking ‘Ok’, a new tree will be automatically generated in the left panel with all the parameters and settings that are necessary to completely specify such an analysis.
  • All parts that are completed are highlighted with a green check. Parts that need to be specified have a red circle. While, the blue circle indicates an optional settings that does not need to be filled out
Creating a new simulation
  • k-omega SST is used for turbulence modelling
  • Since we are interested in a time invariant analysis the Steady-State option is activated
Defining the analysis type

Creating and assigning materials

  • Next, add the materials from the ‘Material Library’ . First, we start with clicking on sub-tree “Materials”, click on ‘+’ from the options panel as shown.
  • This pops-up a ‘Material Library’ from which we select “Air” and click on ‘Ok’. This will then load the standard properties for Air.
  • Then, assign the material to the domain and save.
Adding a new material
Assigning material to the domain

Defining the Initial Conditions

  • Next item is Initial conditions. Here you can specify the state of the fluid at the beginning of the simulation. We are using the following:
Variable Value Unit
pressure 0 m^2/s^2
velocity (x, y, z) (60, 0, 0) m/s
k 0.25 m^2/s^2
omega 1.8 1/s
Defining the initial conditions of the simulation

Boundary Conditions

  • The next item is the Boundary conditions. You can see an overview of the boundary conditions below.
Boundary condition overview
  • To create a boundary condition, click on the ‘+’ option next to the Boundary conditions and select the required boundary condition from drop down menu, as shown in figure
Creating new boundary conditions
  • For the inlet select the ‘Velocity Inlet’ boundary condition, specify the values shown in the figure below, assign ‘Inlet’ entity set for this boundary condition and click on save.
Assigning velocity inlet boundary condition
  • Next select a ‘pressure outlet’ boundary condition, set the parameters as shown below and assign this to the ‘Outlet’ entity set created earlier
Assigning pressure outlet boundary condition
  • Next select a ‘Symmetry’ boundary condition and assign this to the ‘Symmetry’ entity set created earlier
Assigning symmetry boundary condition
  • For the ‘Side-walls’, select the Slip type wall boundary condition as shown
Assigning boundary condition for solid walls
  • For ‘Floor’, select the moving wall boundary condition
Assigning floor boundary condition
  • Lastly, for ‘Front Wing’, select the No-slip wall boundary condition
Assigning wing surface boundary condition


  • The next item is Numerics. Here one can specify the numerical setup of the simulation.
  • For this tutorial case, it is necessary to change some of the default settings.
  • Change Properties and ‘Relaxation factors’ according to the figure.
Numerics-relaxation factors
  • Additionally we will tweak some settings of the linear solvers according to the figure below:
Solver Settings
  • Lastly change the following Divergence schemes.


Parameter Scheme
Divergence scheme for div(phi,U) bounded Gauss upwind
Divergence scheme for div(phi,k) bounded Gauss upwind
Divergence scheme for div(phi,omega) bounded Gauss upwind
  • Under Simulation control we can specify the global parameters of the simulation run
  • Since we are running a steady-state analysis, the time steps are only “quasi time steps”
  • Specify the values as shown in figure below.
Simulation control

Create a mesh

  • To create a mesh, select the mesh option
  • Give an appropriate name to the mesh like ‘FrontWing mesh’
  • We set the mesh operation type to “Hex-dominant parametric (CFD only)”.
Creating the mesh
  • Adjust the Bounding Box Discretization to define the base size of the mesh.
  • We use the following values:
Bounding Box Discretization Value
Number of cells in x direction 25
Number of cells in y direction 5
Number of cells in z direction 5
Setting the bounding box resolution
  • You can also increase the number of processors used for the meshing process from 1 to 32 to reduce the time for meshing
  • Save the mesh operation by clicking on ‘tick’ symbol
  • Under the geometry primitives, we specify the Background Mesh Box dimensions by the values shown in figure below
Setting the dimensions of the Background Mesh Box
  • Similalrly, change the “MaterialPoint” to (0, -1, 1)
  • Next, we define additional primitives of type ‘Cartesian Box’ that will be used for mesh refinement later on
  • Click on the ‘+’ option next to Geometry Primitives and select the Cartesian box from the drop down menu, as shown in figure
Creating Geometry Primitives
  • We add a total of 3 cartesian boxes that will be used to further refine the mesh. This will increase the result quality of the simulation and allow enable you to resolve the wake of the wing.
  • The first one is called Region1 and has the following values:


  • The second one is called Region2 and has the following values:

  • The third one is called Region3 and has the following values:

  • Now we move on to the “Mesh Refinements”.
  • To add a refinement click on the ‘+’ next to the Refinements and select the required refinement from the drop down menu
Creating a mesh refinement
  • Add a refinement of type “surface refinement” to control the cell size on top of the wing surfaces
  • Setup the values and properties as shown in figure below, and assign to the volume ‘solid_0’
Adding surface refinement to the wing surfaces
  • Next we add “region refinements” as follows.
  • The region refinements have levels 5, 6 and 7 to be very fine near the wing and coarse in the far field
  • Define region refinements with the refinement boxes you created earlier. The following values are used:
Refinement Region Level
Region_Ref_1 5
Region_Ref_2 6
Region_Ref_3 7
Level 5 region refinement for region 1
  • Similarly add level 6 for Region2 and level 7 for Region3 and save.
  • Next we add a set of finer layer cells on the wing surface by selecting ‘Inflate boundary layer’ option from the ‘Refinements’ drop down list shown earlier
  • Set the parameters as shown in figure below
  • Select all the faces of the wing using the box select option, and save
To capture the viscous flow boundary layer, we refine the cells close to the wing using a “Layer addition” refinement
  • Next, we add layer of cells at the bottom of the box, which will be the floor in the final simulation
  • Select the ‘Bounding Box Layer Addition’ from the refinements drop down menu
  • Set the Face to ‘Zmin’ to select the ground of the simulation
  • Set the remaining parameters as shown in figure
Creating a ground layer
  • Lastly, to resolve all edges we add a Feature refinement that will refine the cells close to the edges of the wing
  • Select the ‘Feature Refinement’ option from the ‘Refinements’ drop down menu
  • Set the parameters as shown below, and save
Add a refinement to all edges of the front wing
  • Now our meshing operation is ready to go – let’s start it
Start the mesh operation
  • After some time, the mesh will be finished and we can review it via the 3D viewer
Resulting Mesh
Reviewing the mesh

Start a simulation run

  • The last thing to do for running this simulation is to create a run.
  • The new run is created by clicking on the ‘+’ symbol next to ‘Simulation Runs’
  • Give a name to the run and start the run
Starting a new run


Once the simulation is finished, select the ‘Solution fields’ under the Run to post process the results on the platform. Or they can be downloaded and post-processed locally (e.g. with ParaView)

  • To view the streamlines through the front wing use the ‘Particle Tracer’ option
  • Set the parameters as shown in figures
Creating particle tracer
Parameters for the Particle tracer
  • Zoom in to visualize the flow over the front wing and shape of the wake formed
TUT-front wing-35
Flow over the from wing
  • Figure below shows a post processing image form paraview
download the results and post-process locally in Paraview

Data Privacy