First steps in Aerodynamics
with CFX TASCflow
First, we load the Problem Directory-Mach0.2. Type in the shell window:cp -R /logiciels-mfn/CFX/LINUX/TASCflow/Examples/tutorials/sts/trnsonic/mach.2 .
There are five files in the directory mach.2:
bcf gci grd name.lun prm
The bcf file is the Boundary Conditions file.
The grd file is the Grid file.
The prm file is the Solver Parameters file.
To start CFX TASCflow, type in the shell window:
To select the problem directory, click Browse...button. After, click on CFX-TASCflow.
The first step of the preprocessing is to define the zones of the "Zone Manager"
and to create the grid in these zones. To simplify the study, we use a pre-existing grid.
Setting up Zones and Attributes
Two zones are defined:
-the BLADE_BLOCK zone is the blocked-off section, which represents the airfoil
-the FLUID zone represents the grid.
With the FLUID zone selected, we choose the physical properties of the flow.
In this example, we study a fluid flow with heat transfer. The flow is turbulent
In Models and Material Properties, we click the Turbulence... button to choose the
models of turbulence we use. In this example, we choose the k-epsilon model and
a High-Reynolds model near the wall.
After defining models, we click Materials button to select the used fluid.
In Current Working Fluid, we click Select button and choose a fluid (air in the example).
The physical properties like density, viscosity and specific heat are given by CFX.
We click Apply, then Ok in the "Material Properties" panel.
Finally, we click on Apply in tne "Zone Manager" panel.
Having defined the zones and physical properties of the flow and the fluid,
we set up the Boundary Conditions.
Creating Boundary Conditions
To create the Boundary Conditions, we click on PreProcess in the top menu bar and
we select the Boundary Conditions. In the "Boundary Conditions Manager", we can
define the Boundary Conditions. In this example, we have four types of Boundary Conditions:
-Symmetry Boundary Conditions
-Wall Boundary Conditions
-Inflow Boundary Conditions
-Outflow Boundary Conditions
For each boundary, we select Fluids, Energy and Turbulence
to choose the properties of the boundary condition.
In this example, we click Apply for each boundary condition.For the Outflow, we choose
"Applied as Face". When we click Apply, a "Command Line" window appear.
In the "Command Line" window, we type [55,20:21,1:2] and we hit the key
on the keyboard. After, we close the "Command Line" window.
Generating and Initial Guess
We click on PreProcess and we select Initial Guess Generator.
We click on Turbulence to define the Turbulence Initial Guess. In this example,
we choose 0.01 for the Turbulence Intensity and 0.02 for the Eddy Length Scale.
To define the solver parameters, we click on Solve and we select Solver Monitor.
In Solver Monitor Panel, we click Parameter button. For this example, we specify
the time step, the convergence criterion, the advection discretization scheme,
and the fluid properties.
Setting Solver Parameters
-the Fluid Time Step value
-the Number of time steps
-the Maximum residual value,
and we select:
-the Modified Linear Profile
-the Physical Advection Correction
After, we click on Additional Solver Parameters and we select Flow Solver Control and Pressure
to apply a pressure offset.
We clickOk in the "Additional Parameters" panel and Save in the "Solver Parameters" panel.
After, we click on File, Write PreProcessing to save this information.
Running the solver Monitor
Having defined the solver parameters, we click on Start in the Solver Monitor panel to
begin execution of the flow solver.
When the solver stops, we click on Exit button.
To visualize the results of the run, we click on File and select Load PostProcess, Full RSO.
In the "Vizualisation Object Manager" panel, we click on New... to create a new visualization object
We enter a name for the new visualization object (MACH in the example).
We set Type to Contour Plot. Then, we click on Ok.
In the "Contour Interface" panel, we click the Select... button to open
the "Region Manager". In the "Region Manager" panel, we click on New....
In the "New Region Name" panel,
we enter the name of the region MIDPOINT and we select the Type Nodal.
We click on Ok in the "New Region Name" panel.
After, we select the boundaries of the region with the values of I, J, K. We click Apply and Ok
In the "Contour Interface" panel, we click on Select... button
to choose the scalar to plot. For this example, we choose Mach. Then we click on Ok.
Finally, we select Lines and Visibility and we click
Apply to view the plot.