2. Enable Airfoil Feature
We need to enable the Airfoil feature in the SimFlow launcher in the Advanced Settings section.
Go to Advanced Settings panel
Expand features list by clicking Manage Features
Choose Airfoil from the list and close the Advanced Settings panel
3. Create Case
Open SimFlow and create a new case named airfoil_naca_0012
Go to New panel
Provide name airfoil_naca_0012
Click Create Case
4. Import Geometry
Firstly we need to Download GeometryNaca0012
Go to Airfoil panel
Click Import Geometry
Select geometry file naca0012.dat
Click Open
5. Airfoil Meshing
Set Radius [m] to 25 meters
Set the following parameters accordingly
Surface Cell Thickness \({\sf [m]}\)2e-04
Min Surface Cell Length \({\sf [m]}\)2e-03
Max Surface Cell Length \({\sf [m]}\)8e-03Click Mesh to start the meshing process
6. Mesh
After creating a mesh, it will appear in the 3D window.
Click XZ View
Click Fit View to zoom the mesh
Change view projection from Perspective to Parallel
Zoom in the middle section of the mesh by using scroll mouse button
If you zoom in enough, airfoil shape should appear
7. Inspect Mesh Boundaries
Now we will check if the boundaries are set properly.
Inspect boundaries
8. Select Solver - SIMPLE
We want to analyze incompressible turbulent flow around the Airfoil. For this purpose, we will use the SIMPLE (simpleFoam) solver.
Go to Setup panel
Select Steady State filter
Select Incompressible filter
Pick SIMPLE (simpleFoam) solver
Select solver
9. Turbulence
We are going to use the standard \(k-\omega \; SST\) model to handle turbulence. This model gives very good agreement with experimental data and is commonly used for aerodynamics applications.
Go to Turbulence panel
Select RANS modeling
Select \(k-\omega \; SST\) model
10. Dicretization - Convection
Go to Discretization panel
Go to Convection tab
Select Linear Upwind for U (Velocity) parameter
11. Solution - Solvers (Pressure)
The calculations will be run until Residuals will drop down under 10 −6 . This criterion will guarantee high accuracy and will require more iteration. To make sure that the fluid solver will be able to capture very small changes in the flow, we need to make sure that the linear solvers for fluid flow equations will also be able to operate on very slight flow changes. To do this, we will change default solver tolerances.
Go to Solution panel
Expand list of options
Set Tolerance to 1e-07
12. Solution - Solvers (Velocity)
Go to U (Velocity) tab
Expand list of options
Set following parameters accordingly
Tolerance1e-07
Relative Tolerance1e-02
13. Solution - SIMPLE
Go to SIMPLE tab
Set Non-Orthogonal Corrections to 2
14. Solution - Residuals
Go to Residuals tab
Set following parameters accordingly
p1e-06
U1e-06
k1e-05
\(\omega\)1e-05
15. Parameter - U (Velocity)
It is handy to parameterize velocity value to be easily accessible in the further setup. To be able to compare the results with test results we should assume \(Re=6000000\). Based on the air viscosity \(\nu = 1.5 \cdot 10^{-5} \; m^2/s \) and chord \(c\approx 1 \;m\) we calculate the velocity from the equation: \(V=Re \cdot \frac{\nu}{c}\)
Go to Parameters panel
Define the name and formula of the new parameter
NameU
Formula6e6*(1.5e-5/1)Click Create Parameter
The newly created parameter will be shown in the parameters list
16. Boundary Conditions - Inlet (Flow)
Go to Boundary Conditions panel
Select inlet boudary
Change boundary character to Free Stream
Set to velocity type to Free Stream
Now we can use parameter U defined earlier
Freestream Value \({\sf [m/s]}\)U00
17. Boundary Conditions - Inlet (Turbulence)
Go to Turbulence tab
Set Mixing Length \({\sf [m]}\)0.07
18. Initial Conditions - Basic
Go to Initial Conditions panel
Set following initial conditions accordingly
UU00
k0.1
\(\omega\)100
\(\nu_t\)0.1
19. Initial Conditions - Potential
We will use the "Potential" initialization feature. This utility solves pseudo potential flow prior to actual calculations. This will give a better initial guess for velocity and pressure fields.
Go to Potential tab
Check Initialize Potential Flow
20. Monitors - Forces
Go to the Monitors panel
Go to the Forces tab
For Monitor Boundaries select lower tip upper
Check Monitor Coefficients
Define free stram velocity accordingly
\(U_\infty\) \({\sf [m/s]}\)U
21. Monitors - Create Slice
Additionally to observing force coefficients, we will display intermediate results on a section plane.
Go to Sampling tab
Add new Slice
Set the follwing parameters accordingly
Normal \({\sf [-]}\)010
Point \({\sf [m]}\)000Expand Fields menu. Choose p U k (pressure, velocity and turbulent kinetic energy) to be sampled on the section plane.
22. Run - Time Control
Go to Run panel
Set Number of Iterations to 5000
23. Run - Output
Go to Output tab
Set Interval [-] to 100
This controls when results are written to the hard drive. When slices are enabled this also applies to them. Each new result will be displayed at a specified interval.
24. Run - CPU
To speed up the calculation process increase the number of CPUs basing on your PC capability. The free version allows you to use only 2 processors in parallel mode. To get the full version, you can use the contact form to Request 30-day Trial
Estimated computation time for 2 processors: 15 minutes
Switch to CPU tab
Use parallel mode
Increase the Number of processors
Click Run Simulation button
25. Slice - View Velocity field
Change tab to Slices
Choose U (Velocity) field
Click Adjust range to data adjust color range to actually displayed data
26. Results - Force Coefficients
Change tab to Force Coefficients
Click Fit Axes
Select Lookup Data
Choose the last point from the chart
Read the Lift coefficient
27. Reset Simulation
If you want to change the angle of the attack, you should first reset the simulation in the run panel.
Go to Run Panel
Reset Simulation
28. Change Angle of Attack
In the Airfoil panel, we can now remesh the Airfoil change angle of attack. And then rerun the simulation.
Go to Airfoil panel
Change the Angle of attack for the desired value for example
Angle of Attack \({\sf [deg]}\)5Click Mesh button
29. Mesh - Second Case
After creating a mesh, it will appear in the 3D window.
Click XZ View
30. Run Second Simulation
Go to Run panel
Click Run Simulation button
31. Results Comparison With Experimental Data
You might repeat the above operations for different angles of attack, e.g: 5, 10 and 15 degrees. Next comparing them with the experimental data (NASA Langley, 1988) you should be able to obtain the following results.
