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.
This is an external aerodynamics project, which analyses the airflow around the Ahmed Body to calculate the drag force and drag coefficient.
Import CAD geometry. The supported formats are STEP, IGES, STL, SolidWorks, Autodesk Inventor, Rhino, Parasolid and ACIS.
Once the CAD is imported make sure the scale of the model is correct. A scaling tool can be found under ‘Geometry Operations’ to rescale the model to the correct size if necessary.
Add a Simulation
- 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)
- Hex-Dominant (only-CFD) mesh algorithm (This is the most automated approach and is usually the best starting point.)
- External mesh mode
- Coarse mesh
- 32 processors
Use Coarse mesh and 32 processors as a starting point. Increase mesh Fineness and Number of processors according to the complexity of the model.
- Under Geometry Primitives define the dimensions of the Background mesh box, these will be the dimensions for your external air volume.
- Consider symmetry to reduce computational time.
The figure below provides a general rule of thumb for dimension sizing.
- Define the material point to be within the air
Alternatively, the external volume could be created using the ‘Enclosure’ geometry operation. This is applied before the meshing process.
To see the full aerodynamic effects more accurately, mesh around as well as the wake region of the objects should be refined. To achieve this, add necessary local refinements.
It is important to create a refinement region around the objects and extending behind them in order to capture wake behavior. The creation of this region is achieved by adding a new Geometry primitive and the shape can be optimized for the flow direction.
After creating the geometry for the region of interest, define the 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.
In CFD simulations, it is important to capture the velocity gradient on the walls correctly. To capture the boundary layer region in wall-bounded turbulent flows, inflation layer should be added to the mesh.
Add layers on the surfaces of the body. Inflation layer sizes are dependant on the mesh size on the surface. Add more layers to reduce the minimum thickness.
Add a surface refinement on the surfaces of the body.
Once the mesh is complete, check its quality with these two steps:
- Open the Meshing log and scroll down to the last few lines – use event log, reach support if there is an error
- Here no errors were detected. Please contact SimScale support for assistance on solving this issue.
The following picture represents the coarse automatic mesh after all the refinements.
Note that if setup tasks are not mentioned below then default values should be sufficient.
Assign the standard air material to the fluid domain. Here is a short video on how to assign Materials to different parts of the model. Materials in the product library can also be customized as necessary.
Default values for initial condition parameters are usually enough. If these parameters estimated correctly, the solution will converge faster. Define the initial (U) Velocity with respect to the flow.
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
Leaving all other surfaces unassigned will mean that the default no-slip wall condition is applied. In the present case, this is physically correct.
The default settings are usually suitable. Experienced users can use Manual settings for better convergence.
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: 32 (Increase the number of processors according to the complexity of the model.)
- Maximum runtime: 36000 s (Program will stop after 36000 seconds)
- 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.
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.
It is also a good idea to see the y+ (Dimensionless Wall Distance) value. Under Field calculations add Turbulence field calculation to see the y+. In case Wall functions are used, y+ values between 30 and 200 are recommended.
For a general overview of the SimScale’s online post-processing capabilities, the following documentation can be used: here.
The following video shows how the velocity field, as well as streamlines, can be shown:
Drag Force and Drag Coefficient can be seen under the Force plot and Force coefficients plots. Hide the unimportant parameters by clicking on them, to see the plot of interest.