Import CAD geometry. The supported formats are STEP, IGES, STL, SolidWorks, Autodesk Inventor, Rhino, Parasolid and ACIS.
Create new simulation
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.
Create simulation for starting off with meshing
This dialog box allows the user to select the simulation model. Click on ‘Incompressible’.
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)
The default settings for the simulation are kept the same. Save the simulation model by clicking on the tick mark.
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
BACKGROUND MESH BOX
An important parameter is the size of the background mesh box, which is used as the surrounding fluid domain.
The figure below provides a general rule of thumb for dimension sizing.
To change the size of the box click on Backgound mesh box expand geometry primitives under Mesh and change the coordinates of Background mesh Box as shown below
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:
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.
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.
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
Boundary Layer Refinement
Select the Inflate Boundary layer setting
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.
Now click on ‘Generate mesh’ in the meshing tab to generate the mesh.
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.
On further zooming we can see the boundary layer refinement
We can hide all the bounding faces to see the surface mesh refinement.
Assign the standard air material to the fluid domain as shown above.
Default values for initial condition parameters are usually enough. If these parameters estimated correctly, the solution will converge faster.
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: 16 (Increase the number of processors according to the complexity of the model.)
Maximum runtime: 36000 s (Program will stop after 36000 seconds)
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.
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:
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.
Zoom in on the backside of ahmed body to see the the wake region
The pressure field in the simulation is presented below
We can also trace the particles by clicking on the particle traces icon and using seed to pick faces on the outlet
Zooming in the body, we can see the reason why wakes are formed in the back.
Last updated: May 23rd, 2019
Did you find this article helpful?
How can we do better?
We appreciate and value your feedback.