External Aerodynamics using Standard Mesher
Copy the tutorial from here
This short tutorial shows how to create a mesh and simulate external flow over a vehicle body. The purpose of this guide is to show the user the basic workflow to create an external fluid dynamics study. It is not aimed for achieving accurate results.
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:
Flow Domain Extraction
Under Geometry operations, create an Enclosure. This will define the flow domain.
If the model is symmetric, consider symmetry to reduce computational time. Define the size of the domain sufficient enough to capture flow effects.
Figure below provides a general rule of thumb for dimension sizing.
Create a new simulation
Once the flow domain has been created, you can create an incompressible simulation analysis.
- 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.)
Assign the standard air material to the fluid domain.
Default values for initial condition parameters are usually enough. If these parameters are estimated correctly, the solution will converge faster.
Define the initial (U) Velocity with respect to the freestream velocity.
Assign the following boundary conditions:
- Velocity inlet: U_x = 63.7 m/s
- Pressure outlet: P = 0 Pa
- Vertical and top surfaces: Wall boundary, slip velocity condition
- Ground: Wall boundary, Moving wall velocity, U_x = 63.7 m/s
- Symmetry surface: Symmetry boundary condition (If your geometry is not symmetrical, skip this BC assignment)
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:
- End time: 1000 s
- Delta t: 1 s (Since this is a steady-state analysis, time variables define iteration number. 1000 iterations would be enough for external flow analysis.)
- Write interval: 1000 timestep (in a steady-state analysis, only the final state of the system is important.)
- The number of processors: Automatic (Professional users can manually change this. However, we recommend automatic assignment for optimal usage of computational power)
- Maximum runtime: 10000 s (Simulation will stop after 10000 seconds, even if the iterations are not completed)
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. By activating turbulence, you can see the y+ values on the surfaces at the end of the simulation.
- Use the default mesh settings. This is the most automated approach and is usually the best starting point. You can increase the fineness, if the cell size looks inconvenient.
To see the aerodynamic effects more accurately, refine the mesh around the object as well as in the wake region. Add a Region refinement.
Maximum edge length defines the biggest mesh size inside the region. Create a cartesian box, which covers the car and potential wake region.
- In order to have a finer mesh over the surface of the body, add surface refinement.
- Click on Refinements to add a new refinement and select surface refinement
- Select the surfaces of the body and assign a suitable maximum edge length
You can predict the suitable element size with respect to y+ value
- Create a new Simulation Run
- First, a mesh will be generated. After the mesh has completed simulation will start automatically.
- After simulation finishes, check the convergence. You can visit this knowledge base article to learn how to check convergence of a CFD simulation.
- If the recommended mesh settings are done correctly, the mesh should look as follows:
- Automatic boundary layers should be generated only on No-slip and Moving walls.
- Click on Results and select the option All velocity to see the velocity fields in the domain. All velocity stands for the magnitude of velocities in x, y, and z-axes.
This video shows how to visualize the velocity field, as well as streamlines.
Drag Force and Drag Coefficient can be seen under the Force plot and Force coefficients plots. Hiding the other parameters will zoom to the parameter of interest.