Truck aerodynamics simulation

Truck aerodynamics simulation

The truck aerodynamics simulation tutorial is completed using SimWorks, which is available to download for free. The tutorial assumes you are already familiar with some basic functionalities of SimWorks, therefore we recommend to complete first at least one of the base level tutorials available.

The objectives of this simulation are to evaluate the truck aerodynamics and the sensitivity of the simulation results on the outer domain dimensions. For this reason, we will complete the truck aerodynamics simulation with both a reduced size computational domain and with a larger one to see effect on the results.

As already seen in the previous tutorials, create a new simulation and load the truck.igs file renaming this simulation as Truck std domain.

truck aerodynamics simulation
Truck aerodynamics simulation showing the Cp0 around the truck - Simulation carried out with the free CFD simulation software SimWorks

Before starting the tutorial simply download SimWorks if you have not already and the tutorial geometry

Define the outer domain for the truck aerodynamics simulation

The first simulation will have a reduced size outer domain:

  1. Select the Regions tab in the simulation editor and define the box dimensions as 60 10 8
  2. Define the Origin as -10 0 4.2

This way the front face of the outer domain (OD) is roughly 0.5 truck lengths (chord) away from the geometry, while behind the truck there are further 2 chords.

Base mesh parameters

From the Mesh tab in the simulation editor window define the following mesh parameters:

  1. Define the base size as 2 
  2. Define the point in mesh location as -15 0 5 and its size as 0.5, the point will be shown in the geometry viewer, verify that is inside the OD but outside of the geometry
  3. In the Surface mesh group with all the truck parts define the Surface level as 0 5 (minimum refinement value is 0 and maximum 5) and the Edge level as 5
  4. Add a Refinement box clicking on the relevant icon in the Mesh tab in the Simulation editor window
  5. The refinement box will have a level of 2, a dimension of 30 5 6 and an origin of 0 0 3.2.

The reason to add a refinement box is to guarantee a smooth transition from the coarse OD base mesh (2 meters of base cell dimension) and improve the mesh resolution around the truck body. The geometry will create a wake and aerodynamic structures which need to be correctly captured. 

The base cell size level of 2 means that the characteristic base cell will be 2m /  \(2^2\) = 0.5 m. Meanwhile, on the surface of the truck we set the maximum resolution to level 5, therefore the surface mesh size will go down to 2m / \(2^5\) = 6.25 cm.

Boundary conditions definition

We will set a velocity of 25 m/s (corresponding to 90 km/h) normal to the inlet face of the OD and a constant pressure of 0 on the outlet face. You can define the boundary conditions using the SimWorks pre-processor. To do so, please show the Boundary conditions types layering in the layering menu as seen in previous tutorials:

  1. Select the Boundary conditions types layering in the layering menu 
  2. Set 25 m/s inlet velocity on the OD front face
  3. Define a 0 Pa pressure outlet at the outlet of the OD

Post-processing options

In the Setup tab, we need to set the reference values in order to correctly calculate the aerodynamic force coefficients.  In this case, please set the Reference area to 10.5 m,  the Reference length to 3 m and the Reference velocity to 25 m/s. 

In the Output tab, we want to create 50 planes in the x direction, between xmin of -15 and xmax 25, 30 planes in y direction between ymin of -3 and ymax of 3 and, finally, 30 planes in z direction between zmin of 0 and zmax of 5.


Complete the simulation

We recommend to run the simulation in parallel. For example, set the number of processors in the Setup tab to 4. Also, set the total number of iterations to  1000 step and then execute all the simulation phases sequentially: Setup, Mesh and Run.

Analyse the results

In the Simulation Manager, right click on the simulation and load the results with Fields → Load:

  1. Show a plane that intersect the truck in the middle in the direction normal to y, select Cp in the Variable tab and set the legend range from -1 to 1
  2. Select the line probing tool icon in the Fields window 
  3. Select two points near the OD inlet to evaluate the Cp. The actual max is 0.18
  4. As the flow reaches the stagnation point on the front face of the truck cabin, the Cp raises to 1 as expected
truck aerodynamics simulation Cp distribution

Clearly the max Cp value at the inlet of 0.18 is higher than the expected freestream value of 1 showing that the Cp overpressure is propagating upstream and the OD is too small to obtain reliable results.

Repeat the same visualisation but showing the total pressure coefficient Cp0, with a range from -1 to 1

The total pressure coefficient is defined as the sum of the static pressure and the dynamic pressure and represents the flow energy. In this case the maximum Cp0 on the inlet is around 1.18, when the theoretical value of a freestream flow should be 1. Again, this is a sign that the inlet is too close to the geometry, also because the truck geometry is showing a very high level of blockage.

Extended Outer Domain simulation

Now define a new simulation called truck_extended_domain following the exact steps as above but defining the OD with dimensions 140 12 15 and origin 10 0 7.7. Also update the refinement box dimensions to 40 7 8 and the Origin to 0 0 4.2: 

Extended Outer Domain simulations results

Now repeating the same analysis carried out for the standard outer domain size both for Cp and Cp0 keeping the same ranges as before:

Cp plot for the extended computational domain simulation
Cp0 (flow energy) plot ofr the extended computational domain simulation

Close to the inlet plane, the max Cp value is now 0.07 and the max Cp0 is 1.07. Both are much closer to the theoretical freestream values of 0 and 1, respectively. Clearly further extending the OD can improve those results, but it is important to find the right trade off between the simulation accuracy and the total number of cells, which leads to a longer simulation time.

Truck aerodynamics simulation results

The results obtained with the larger OD can be used to look at the truck aerodynamics in more detail. The Cp0 distribution (now with range between -1 and 1) shows that the truck produces a large wake and the region of low energy flow extends toward OD outlet. Using a line probe, it is possible to see that flow in the lower portion of the wake has lost roughly 30% of energy (minimum Cp0 value of 0.63):

It is possible to look in more detail on how the wake is affecting the truck aerodynamics using a combination of a plane normal to the y direction and one normal to x direction, placed downstream of the truck:

The picture above shows that the truck aerodynamic wake downstream of the body (1) is wider at the base (3) compared to the higher region (2) due to the effect of the losses introduced by the wheels and the truck underside. Aerodynamic losses are also building up on the top and sides of the truck from the very beginning of the geometry (4).

Finally, selecting Cp and defining a range from -2 to 0 (1) highlights the areas where the flow is accelerating. Regions of very low local Cp (2) can become critical from an aerodynamic viewpoint as these can create regions with strong negative pressure gradients. This occurs when the flow is moving in a direction where the pressure is increasing. If the raise of the pressure from the low Cp region towards the ambient pressure is very rapid, the boundary layer will not have enough energy to remain attached to the surface and the flow can be prone to separations:

Truck aerodynamics CD plot

On the last simulation it is now possible to evaluate the overall drag coefficient of the truck

  1. right click on the simulation results and select Plots–>Load, the Plot window will appear
  2. Select the Move graph icon to center every graph
  3. Zoom in the area of interest, which are the latest iterations where the simulation is fully converged
  4. It is possible to click on the Reset view icon to come back to the original view

The calculated drag coefficient of the truck is 0.715, this value and the flow field results are in line with the findings of experimental data and other CFD simulations available in literature

Try the free version of SimWorks or contact us to find out more