We need to enable the Airfoil feature in the SimFlow launcher in the Advanced Settings section.
1. Go to Advanced Settings panel
2. Expand features list by clicking Manage Features
3. Choose Airfoil from the list and close the Advanced Settings panel
After opening SimFlow, we will create a new case named airfoil_naca_0012
1. Go to New panel
2. Provide name airfoil_naca_0012
3. Click Create Case
Firstly we need to Download Airfoil Geometry: naca0012.dat
1. Go to Airfoil panel
2. Click Import Geometry
3. Select geometry file naca0012.dat
4. Click Open
1. Set Radius [m] to 25 meters
2. Set the following parameters accordingly
Surface Cell Thickness [m] 2e-04
Min Surface Cell Length [m] 2e-03
Max Surface Cell Length [m] 8e-03
3. Click Mesh to start the meshing process
After creating a mesh, it will appear in the 3D window.
1. Click XZ View
2. Click Fit View to zoom the mesh
3. Change view projection from Perspective to Parallel
4. Zoom in the middle section of the mesh by using scroll mouse button
5. If you zoom in enough, airfoil shape should appear
Now we will check if the boundaries are set properly.
1. Inspect boundaries
We want to analyze incompressible turbulent flow around the Airfoil. For this purpose, we will use the SIMPLE (simpleFoam) solver.
1. Go to Setup panel
2. Select Steady State filter
3. Select Incompressible filter
4. Pick SIMPLE (simpleFoam) solver
5. Select solver
We are going to use the standard k-ω SST model to handle turbulence. This model gives very good agreement with experimental data and is commonly used for aerodynamics applications.
1. Go to Turbulence panel
2. Select RANS modeling
3. Select k-ω SST model
1. Go to Discretization panel
2. Go to Convection tab
3. Select Linear Upwind for U (Velocity) parameter
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.
1. Go to Solution panel
2. Expand list of options
3. Set Tolerance to 1e-07
1. Go to U (Velocity) tab
2. Expand list of options
3. Set following parameters accordingly
Tolerance 1e-07
Relative Tolerance 1e-02
1. Go to SIMPLE tab
2. Set Non-Orthogonal Corrections to 2
1. Go to Residuals tab
2. Set following parameters accordingly
p 1e-06
U 1e-06
k 1e-05
ω 1e-05
1. Go to Parameters panel
2. Define the name and formula of the new parameter
Name U
Formula 6e6*(1.5e-5/1)
3. Click Create Parameter
4. The newly created parameter will be shown in the parameters list
1. Go to Boundary Conditions panel
2. Select inlet boudary
3. Change boundary character to Free Stream
4. Set to velocity type to Free Stream
5. Now we can use parameter U defined earlier
Freestream Value [m/s] U 0 0
1. Go to Turbulence tab
2. Set Mixing Length [m] 0.07
1. Go to Initial Conditions panel
2. Set following initial conditions accordingly
U U 0 0
k 1e-1
ω 100
𝝂t 0.1
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.
1. Go to Potential tab
2. Check Initialize Potential Flow
1. Go to the Monitors panel
2. Go to the Forces tab
3. For Monitor Boundaries select lower tip upper
4. Check Monitor Coefficients
5. Define free stram velocity accordingly
U∞ [m/s] U
Additionally to observing force coefficients, we will display intermediate results on a section
plane.
1. Go to Sampling tab
2. Add new Slice
3. Set the follwing parameters accordingly
Normal [-] 0 1 0
Point [m] 0 0 0
4. Expand Fields menu. Choose p U k (pressure, velocity and turbulent kinetic energy) to be sampled on the section plane.
1. Go to Run panel
2. Set Number of Iterations to 5000
1. Go to Output tab
2. 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.
3. Run Simulation
1. Change tab to Slices
2. Choose U (Velocity) field
3. Click Adjust range to data adjust color range to actually displayed data
If you want to change the angle of the attack, you should first reset the simulation in the run panel.
1. Go to Run Panel
2. Reset Simulation
In the Airfoil panel, we can now remesh the Airfoil change angle of attack. And then rerun the simulation.
1. Go to Airfoil panel
2. Change the Angle of attack for the desired value for example
Angle of Attack [deg] 5 degrees
3. Click Mesh button
