Documentation

External Aerodynamics around a vehicle

This short tutorial shows how to create a mesh and simulate external flow over a vehicle body.

Geometry Preparation

Make the geometry ‘CFD ready’:

  • The model should be completely closed solids.
  • Small features which don’t contribute to the flow need to be removed.

Link to tutorial project containing the geometry:

Import tutorial project into workbench

  • As a first step we need to create a new simulation. To create a simulation left click under the Geometries  and then on Create Simulation.

Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics

    Create simulation for starting off with meshing
  • This dialog box allows the user to select the simulation model. Click on ‘Incompressible’. 

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Select Incompressible flow simulation analysis

Simulation Settings

  • Incompressible analysis (This analysis type is used when the fluid density variations are negligible, often when Mach number is below 0.3 )
  • k-omega SST (This turbulence switches in between k-omega and k-epsilon models automatically, therefore it takes the advantage of both models.)
  • Steady-state (Due to the transient behavior of external flows, more accurate results can be achieved by transient simulation. Chose steady-state for a faster convergence)
Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
keep the default settings for the simulation setup

The default settings for the simulation are kept the same. Save the simulation model by clicking on the tick mark.

Mesh Generation

  •  Left click on the mesh icon to create a new mesh.
  • Choose the Hex-Dominant (only CFD) Algorithm.
  • Choose the External meshing option and Automatic sizing option
  • Specify the number of cores to 16
Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
Mesh settings for the geometry

 

BACKGROUND MESH BOX

  • An important parameter is the size of the base box, which is used as the surrounding fluid domain.
  • To change the size of the box click on Backgound mesh box expand geometry primitives under Mesh and change the coordinates of Base mesh Box as shown below

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Set up the coordinates of the background mesh box

Material Point

  • Material point: This is the parameter the algorithm uses to determine wether the mesh is created inside a shape or outside. In this case this point therefore lies within the base mesh box but outside the body.
  • Select the Material Point and give the coordinates as below:

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Set up the coordinates of the material point

Geometry Primitives

  • Now we create additional Geometry Primitives, to be used later for region refinements.
  • Click Geometry primitives and add new primitive of type Cartesian Box as shown in figures below.

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Adding new geometry primitives for region refinement

Region Refinement

  • Region refinements will refine the volume mesh cells based on the given refinement level.
  • Click on Refinements to add a new refinement and select region refinement.
  • Selecting internal means that only the mesh within the volume will be refined.
  • Under geometry primitive, select the name of the refinement region you created. The value of 0.02m defines the element size.

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Region refinement settings for the internal flow

Surface Refinement

  • In order to have a finer mesh over the surface of the body, we add surface refinement.
  • Click on Refinements to add a new refinement and select surface refinement.
  • Assign the body for surface refinement using the volume selection icon.
  • The settings for the surface refinement are shown below

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Surface refinement settings for the mesh

Boundary Layer Refinement

  • Select the  Inflate Boundary layer setting
Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
Boundary layer refinement settings for the mesh
  • keep the default settings in the dialog box
  • Select all the faces using for boundary layer refinement by using the Active box selection icon and dragging it over the entire volume.

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Select all the faces for boundary layer

Mesh Inspection

  • After the mesh generation we need to select the mesh as our domain of simulation.
  • The generated mesh is presented below. It has 1.5 million cells and 1.6 million nodes.

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Image of mesh showing the region refinement
  • On further zooming we can see the boundary layer refinement

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Boundary layers in the mesh
  • We can hide all the bounding faces to see the surface mesh refinement.

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Surface refinement on the body

Simulation Setup

Materials

Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
Assigning air for the flow in material settings

Assign the standard air material to the fluid domain as shown above.

Initial Conditions

Default values for initial condition parameters are usually enough. If these parameters estimated correctly, the solution will converge faster.

Boundary Conditions

Assign the following boundary conditions:

  • Velocity inlet: U_z = -63.7 m/s
  • Pressure outlet: P = 0 Pa
  • Vertical and top surfaces: Wall boundary, slip velocity condition
  • Ground: Wall boundary, Moving wall, U_z = -63.7 m/s
  • Symmetry surface: Symmetry boundary condition
Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
Image showing the boundary conditions

Leaving all other surfaces unassigned will mean that the default no-slip wall condition is applied. In the present case, this is physically correct.

Numerics

The default settings are usually suitable. Experienced users can use Manual settings for better convergence.

Simulation

The Simulation Control settings define the general controls over the simulation. The following controls should be applied:

  • Start time: 0 s
  • End time: 2000 s
  • Delta t: 1 s (Since this is a steady-state analysis, time variables define iteration number. 2000 iterations would be enough for external flow analysis.)
  • Write interval: 2000 timestep (in a steady-state analysis, only the final state of the system is important.)
  • The number of processors: 16 (Increase the number of processors according to the complexity of the model.)
  • Maximum runtime: 36000 s (Program will stop after 36000 seconds)

Result Control

To see the forces on the body, define Forces and Moments. Select the surfaces of the body.To see the drag coefficient of the body, define Forces and Moment Coefficients. Define the lift and drag directions, Freestream velocity, Reference length, and Reference area values and finally select the surfaces of the body.

Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
Result Control Settings for computing the forces on the body

Simulation Run

  • Create a new Simulation Run
  • There is usually a warning that certain surfaces will be set to wall boundary condition – this means that the unassigned faces will be set to walls and is totally normal.
  • The convergence plot after the simulation is shown below:

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Convergence plot showing the convergence of results
  • Click on ‘Solution Fields’ under Convergence Plot.
  • Click on Results and and select the option All velocity to see the velocity fields in the domain.

    Meshing, CFD, Simscale, External Flow Analsysis, Car Aerodynamics
    Velocity profile of the simualtion
Contents