EP-704 ANSYS FLUENT Airfoil 2D Setup

Wikis > EP-704 ANSYS FLUENT Airfoil 2D Setup

4. Setup & Solution PROCEDURE


  • General
    • Click on Report Quality (Confirm that the values that appear are not close to the extremes that Fluent describes)
    • Click on Check
  • Models
    • DCLK (double click) on Viscous
      • Model = k-omega (2 eqn)
      • k-omega Model = SST
    • Materials
      • DCLK on air under Fluid
        • Use the default properties already there, or change the properties to match a desired temperature.
      • Cell Zone Conditions
        • Click on the cell zone (there should only be one).
        • Confirm that Type is set to fluid.
      • Boundary Conditions (if names used are not the same, look for corresponding names)
        • DCLK on inlet
Momentum Velocity Specification Method Components
Reference Frame Absolute
X-Velocity (m/s) 7.785564

The velocity will components will depend on the axes’ orientation and the angle of attack.

Y-Velocity (m/s) 0
  • DCLK on outlet
Momentum Gauge Pressure (pascal) 0
  • DCLK on all walls to confirm they are Stationary, No-Slip Walls with 0 Thermal properties.
  • Reference Values
    • By setting Compute from to inlet, Fluent will automatically set the appropriate values for density, viscosity, and temperature.
Compute from outlet
Reference Values Area (m^2) 1

Use the appropriate planform area. (With chord length of 1m, it is recommended to keep the area at 1m^2)

Length (m) 1

Use the appropriate chord length of the airfoil.



  • Solution Methods
Pressure-Velocity Coupling Scheme COUPLED
Spatial Discretization Gradient Least Squares Cell Based
Pressure Second Order
Momentum Second Order Upwind
Turbulent Kinetic Energy Second Order Upwind
Specific Dissipation Rate Second Order Upwind
  • Refer to notes and course material to choose appropriate scheme and discretization methods.
  • Solution Controls
    • These values should be changed case by case, but the defaults seem to be sufficient for the procedure-specific example.
  • Monitors
    • Click on Create under Residuals, Statistic and Force Monitors > Drag…
Options Print to Console checked
Plot checked
Force Vector X 1

Force Vector should be determined depending on the angle of attack.

Y 0
Z 0
Surfaces wing

Or choose surfaces that form the airfoil.

  • Click on Create under Residuals, Statistic and Force Monitors > Lift…
Options Print to Console checked
Plot checked
Force Vector X 0

Force Vector should be determined depending on the angle of attack.

Y 1
Z 0
Surfaces wing

Or choose surfaces that form the airfoil.

  • Click on Create under Surface Monitors
Report Type Area-Weighted Averaged
Options Print to Console checked
Plot checked
Field Variable Pressure
Total Pressure
Surfaces wing

Or choose surfaces that form the airfoil.

  • The pressure plot will be used to see that values are stabilizing while solving.
  • Note that Cd and Cl calculated while solving may not be true coefficients because the solver uses the Area input in the Reference section.
  • Click on Convergence Manager… under Convergence Monitors
    • Set Stop Criterion and other parameters to check for convergence of the coefficients. These values are also should be decided according to the behavior of the problem.704-06
  • Solution Initialization
    • Click Initialize (while Hybrid Initialization is chosen)
    • Choose Standard Initialization
Compute from inlet
Reference Frame Absolute
Initial Values X Velocity (m/s) 7.785564

The velocity will components will depend on the axes’ orientation, the angle of attack, and desired Reynold’s number.

Y Velocity (m/s) 0
Z Velocity (m/s) 0
  • Click Initialize
  • Calculation Activities
    • Autosave Every (Iterations) = 50 (can be changed to 0 or another value if needed)
  • Run Calculation
    • Number of Iterations = 1000
    • Click Check Case. There should be no recommendations that appear.
    • File > Save Project
    • Click Calculate
    • Click 703-05 and choose an option to show all of the plots as the solver is solving. The window should show something similar to the screenshot below.704-07
    • Check on the residuals to see that they decrease monotonically and the other plots to see that they reach a steady value. In general, residuals should be below 1e-4 to confirm convergence. However, the matter of convergence is problem-dependent, so the other values, such as drag coefficient, need to be monitored in addition to the residuals. Small oscillations in the variables may occur due to the characteristics of the flow, and so identifying convergence will be subject to individual judgment.
    • If the solver is not converging it is a good idea to decrease the Courant number (you may or may not have this depending on the solver scheme) and relaxation factors bit by bit to help the solver converge.
    • The example case took about 80 iterations to converge.
    • File > Save Project


Results (and CFD-Post)

  • Plots > DCLK on XY Plot
Y Axis Function Turbulence…
Wall Yplus
Plot Direction X 1
Y 0
Z 0
X Axis Function Direction Vector
Surfaces wing

Or choose surfaces related to the subject.

  • Click Plot and a plot like the one below should show. Yplus is a dimenionless value that shows how far the first grid point is from a wall and is important to consider when working with drag and turbulence. Since a significant majority of the Y+ values (especially the wings) are less than 11, it is considered satisfactory for accurate calculations that resolve the boundary layer. Same criterion can be applied to different cases. You can either screenshot this or use the camera button.704-08
  • Reports > DCLK on Forces
    • Select wing (or corresponding zones) for Wall Zones and click Print.
    • Change the direction vector appropriately and click Print
  • There are numerous analyses and graphics you can produce within Fluent. Search notes and researches for methods to obtain needed renderings and data.
  • File > Export > Case & Data… > Save with appropriate name to represent this case.
    • This can be used to compare different cases later on.
  • Close ANSYS Fluent


  • Double click on the Results cell to open CFD-Post
    • Use screenshot or to capture images.
    • Switch to the Expressions tab and enter these expressions (Right click on Expressions > New). Remember that expressions are case sensitive. (These expressions are for
drag force_y@wing

Or use appropriate names for the subject

lift force_x@wing
cop X (areaInt_y(Pressure*X)@wing) /lift
cop Y (areaInt_z(Pressure*Y)@wing) / drag
wing area areaInt_y(if(Normal Y > 0,1,0))@wing

This is not exactly necessary as we know the area we assumed is 1m2, so use appropriate values.

coef drag drag*2/(massFlowAve(Density)@inlet *(massFlowAve(Velocity)@inlet)^2*wing area)
coef lift lift*2/(massFlowAve(Density)@inlet*(massFlowAve(Velocity)@inlet)^2*wing area)
  • There are many other functions in CFD-Post and should be researched and used according to needs.


5. Mesh Independence Study

  • whether the solution depends on the mesh or not should be checked. These are the steps to take:
    • Make sure initial mesh converges.
    • Refine the mesh (generally 1.5 times the initial size)
    • Run solver again
    • Compare results
    • Repeat steps 1 to 4 until results become acceptably close.

**It is recommended that you plot the results against the number of cells for each mesh to see where the change in solution is acceptably low.