4. Setup & Solution PROCEDURE
Setup
 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 = komega (2 eqn)
 komega 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
 DCLK on air under Fluid
 DCLK (double click) on Viscous
Momentum  Velocity Specification Method  Components 
Reference Frame  Absolute  
XVelocity (m/s)  7.785564
The velocity will components will depend on the axes’ orientation and the angle of attack. 

YVelocity (m/s)  0 
 DCLK on outlet
Momentum  Gauge Pressure (pascal)  0 
 DCLK on all walls to confirm they are Stationary, NoSlip 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
 Solution Methods
PressureVelocity 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 procedurespecific 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  AreaWeighted 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.
 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 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.
 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 1e4 to confirm convergence. However, the matter of convergence is problemdependent, 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 CFDPost)
 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.
 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 CFDPost
 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 1m^{2}, 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 CFDPost 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.