Workshop 2 Transonic Flow over a NACA 0012 Airfoil

1. Workshop 2Transonic Flow over a NACA 0012 Airfoil Introductory FLUENT Training

2. Goals The purpose of this tutorial is to introduce the user to good techniques for modelling flow in high speed external aerodynamic applications. Transonic flow will be modelled over a NACA 0012 airfoil for which experimental data has been published, so that a comparison can be made. The flow to be considered is compressible and turbulent. The solver used is the density based implicit solver, which gives good results for high speed compressible flows. The tutorial is carried out using FLUENT and CFD Post from within Workbench, but it could also be completed in standalone mode.

3. Start a workbench project Launch Workbench and save the new project as naca0012 in your working directory. Double-click or drag a FLUENT module from the component systems. Add a results module – double click or drag. Drag the mouse from cell A3 (Solution) to B2 (Results) to couple the modules.

4. Import a mesh that was generated in Gambit • Import the FLUENT mesh file (naca0012.msh). • Right click on cell A2 (setup) and select ‘import FLUENT case file’ • Change the ‘Files of type’ to “FLUENT mesh file” • Select the mesh file naca0012.msh • The FLUENT launcher will start. • Keep the default options. • Note that ‘2D’ has automatically been selected

5. Mesh FLUENT will launch in a new window. The mesh will read in and display, and the zones will be written out for the Workbench project.

6. Mesh • The mesh needs scaling, since it was created with lengths in mm. • Select General > Scale and observe the current domain extents. • Select ‘Mesh was created in mm’. • Press ‘Scale’ • Check that the domain extents are as expected. • Close the scale panel and select General > Check • Review the text window and check there are no errors. • Finally use ‘Report Quality’ to print out cell quality statistics.

7. Mesh Zoom in and examine the mesh. The maximum aspect ratio in this mesh is quite high (around 7000) This is acceptable because these cells are close to the airfoil wall surfaces. This is needed for the turbulence model being used, since it ensures the first grid point is in the viscous sublayer.

8. Solver • Select the steady-state density-based solver: • From ‘General’ in the tree select Type: Density-Based • Check time is steady • Turn on the energy equation. • This is needed because the flow is compressible and we will be using the ideal gas equation. • From ‘Models’ in the tree, select ‘Energy’ > Edit > and check box • Select the turbulence model to be used: • From ‘Models’ in the tree, select ‘Viscous’ and Edit • Choose the one-equation Spalart-Allmaras model. • Select strain/vorticity based production, then OK • This is a relatively simple turbulence model that has been shown to give good results for boundary layers subjected to adverse pressure gradients, particularly where there is no or only mild separation.

9. Materials • The properties to be used for the material ‘air’ need to be set. • Select ‘Materials’ from the model tree • Highlight ‘Air’ then Create/Edit • For Density, select ‘Ideal Gas’ • For Viscosity, select “Sutherland”, and accept the default settings for the 3 Coefficient method. • The Sutherland law for viscosity is well suited for high-speed compressible flow. For simplicity, we will leave Cp and Thermal Conductivity as constants. Ideally, in high speed compressible flow modeling, these should be temperature dependent as well. • Select Change/Create • Assign the material ‘air’ to the grid cells: • Select ‘Cell Zone Conditions’ • Highlight ‘fluid’ then ‘Edit’ • Observe ‘air’ is already selected.

10. Operating Conditions • Set the Operating Pressure to Zero: • Absolute pressure is the gauge pressure plus the operating pressure. • Setting zero operating pressure means that all pressures set in FLUENT will be absolute. This is the most common practice for compressible flows. • Select ‘Cell Zone Conditions > Operating Conditions • Set the Operating Pressure to Zero, then ‘OK’

11. Boundary Conditions • Set the upstream boundary conditions: • Select ‘Boundary Conditions’ > pressure-far-field-1 > edit • The pressure-far-field boundary type is applicable only when the density is calculated using the ideal-gas law. It is important to place the far-field boundary far enough from the object of interest. For example, in lifting airfoil calculations, it is not uncommon for the far-field boundary to be a circle with a radius of 20 chord lengths. • On the ‘Momentum’ tab, set the gauge static pressure to 73048 Pa • We need to input static pressure for a far-field boundary. We can calculate this from the total pressure, which was atmospheric at 101325 Pafor the wind-tunnel test. • In the case of a real external aerodynamic simulation, rather than a wind tunnel, the static pressure (at a given altitude) would actually be the same as the total pressure in the far field, because the air in the far field would be stationary. • We have already set the operating pressure to zero, sowe are now working in absolute pressure values. Hence the gauge static pressure input will be equal to the absolute static pressure value, which we will calculate to be 73048 Pa.

12. Boundary Conditions • Set the Mach Number to 0.7 and flow direction components as shown. • The angle of attack (α) in this numerical case is 1.53 deg. The x-component of the flow is cos α and the y-component is sin α. • It is common practice to adjust the numerical α from the experimental α in order to match the lift obtained in the wind tunnel, and then to determine the drag associated with this lift. This adjustment of α is carried out to counter the effects of the wind tunnel enclosure. • Set a reasonable boundary condition for the far field turbulence: • In reality the far-field air would be stationary. Wind tunnels attempt to replicate this by using filters and grids to obtain a low turbulence intensity at the inlet. • Select ‘Intensity and Length Scale’ • Set an intensity of 0.01% • Choose a length scale proportional to the boundary layer thickness. Based on an estimated maximum boundary layer thickness of 50mm*, a suitable length scale is 0.4 x 0.05m = 0.02m • * taken from a previous simulation

13. Boundary Conditions • Select the thermal tab. • The wind tunnel operating conditions for validation test data give the total temperature as T0 = 311 K • We can therefore calculate the static temperature to be 283.24 K

14. Boundary Conditions For both walls representing the airfoil, leave the default settings which correspond to a no-slip condition for momentum and adiabatic for thermal.

15. Reference Values • Set the reference values: These are not used in the actual solution, but are used for reporting coefficients, such as Cp. • Use the freestream conditions as a reference, so choose ‘compute from’ then select ‘pressure-far-field-1’ in the drop down list.Note the reference values for density, enthalpy, pressure, temperature,etc. will update from the freestream values you specified in the pressure-far-field-1 boundary. • Set the reference length (which is not updated from the far field boundary values). In this 2D case, we will use the airfoil chord length, of 1m.

16. Solution Methods • The CFD computation is now defined. However the solver settings need to be modified. These dictate how fast, stable and accurate (within the mesh and BC constraints) the solution will be. • Select Solution Methods in the LHS tree. • Keep the default settings for the implicit formulation and Roe-FDS flux type. • The explicit formulation is only normally used for cases where the characteristic time scale is of the same order as the acoustic time scale, for example the propagation of high Mach number shock waves. • The implicit formulation is more stable and can be driven much harder to reach a converged solution in less time.

17. Solution Methods • Change the gradient method to Green-Gauss Node Based. • This is slightly more computationally expensive than the other methods but is more accurate. • Select Second Order Upwind for flow and turbulence discretization. • To accurately predict drag, select the ‘Second Order Upwind’ schemes.

18. Solution Controls • The Courant number (CFL) determines the internal time step and affects the solution speed and stability. • The default CFL for the density-based implicit formulation is 5.0. It is often possible to increase the CFL to 10, 20, 100, or even higher, depending on the complexity of your problem. You may find that a lower CFL is required during startup (when changes in the solution are highly nonlinear), but it can be increased as the solution progresses. As we will be using automatic ‘solution steering’, the choice of CFL at this stage is not important for this case. Keep the default under-relaxation factors (URFs) for the uncoupled parameters.

19. Solution Monitors • Set up residual monitors so the convergence can be monitored • Monitors > Residuals > Edit • Make sure ‘plot’ is on • Turn off convergence checks by setting the criterion to ‘none’. This means that the calculation will not stop based on the residual plots convergence, but you can still see their progress.

20. Solution Monitors • Set up a monitor for the drag coefficient on the airfoil. • Select both wall zones and toggle on ‘Print’, ‘Plot’ and ‘Write’. • Remember that α is 1.53° so we need to use the force vector as shown. -Lift and drag are defined relative to the wind, not the airfoil. • Press OK, then follow the same process to setup a monitor for Lift. • The settings are identical except for the File Name (cl-history instead of cd-history) and the Force Vectors defined as shown here: You can specify which window FLUENT uses to display plots. For now, accept the defaults.

21. Solution Initialization Initialize the flow field based on the far-field boundary: Select Solution Initialization from the model tree Compute from > pressure-far-field-1 Press ‘Initialize’. Solution Steering enables the robust first order discretization in the early-stages of the computation, then blends to the more accurate second order schemes as the solution stabilizes. Select Run Calculation, and toggle on Solution Steering Change the flow type to transonic and keep default options Full-Multi-Grid Initialization will compute a quick, simplified solution based on a number of coarse sub-grids. This will then be used as a starting point for the main calculation. FMG can help to get a stable starting point.

22. Case Check • Check the case file and make sure there are no reported issues. • Use Run Calculation > Check Case • Any potential problems with the case setup will be raised in the case check panel if there are no problems this panel will not appear. In this case there is a recommendation to check the reference values for the force monitors. Since we have already set these we can ignore this warning. • Save the case file. • File > Save Project (if running under workbench)

23. Run Calculation Although the calculation is ready to compute, It is good practice (but not strictly necessary) to run the FMG and then check the coarse FMG solution before starting the main calculation iterations. Set the number of requested iterations to zero, and press ‘Calculate’.

24. Run Calculation Check the pressure and velocity contours to make sure that no spurious values are predicted. Go to ‘Graphics and Animations in the LHS tree, choose ‘Contours’ and ‘Set Up’

25. Run Calculation Choose Contours of Pressure > Static Pressure and ‘Filled’ Display. If you need to autoscale the display press <control> A Zoom in as required. Examine the min and max reported values. Repeat for Contours of Velocity> Mach Number.

26. Run Calculation There are no spurious results from the FMG, so proceed to the main calculation. Return to ‘Run Calculation’ in the LHS tree. Change the number of windows to three (for the residual, drag and lift monitors that we set up earlier). Request 900 iterations. ‘Calculate’

27. Run Calculation • After 900 iterations the calculation has fully converged. • Note that the CFL has been updated during the calculation in a number of stages, ramping up from 5 to 200 as we requested. This can be seen in the CFL window and the effect on the residuals is also evident. By the end of the calculation the residuals have converged well and are no longer changing. The drag and lift monitors are also stable.

28. Post Processing [FLUENT] • Select ‘Graphics and Animations’ in the LHS menu • Examine the contours of static pressure. • Turn off ‘Filled’ to just display the contour lines. • Adjust the Levels to increase the number of contour lines. The contour will display in the active window (click a window to activate). Alternatively, use the drop down menu to return the display to a single window as shown here

29. Post Processing [FLUENT] Plot contours of Velocity > Mach Number and notice that the flow is now locally supersonic.

30. Post Processing [FLUENT] Select ‘Plots’ in the LHS menu. Plot Pressure Coefficient along the top and bottom airfoil surfaces.

31. Post Processing [FLUENT] Compare experimental pressure coefficient plots which we can import and plot here alongside the numerical prediction. Click on ‘Load File’ and browse for the files in your directory.

32. Post Processing [FLUENT] Once loaded, plot the CFD and experimental Cp plots together. A good agreement can be seen.

33. Post Processing [FLUENT] • In order to obtain a good drag prediction, and for the turbulence model to work effectively, we need to have a mesh that is well resolved near to the wall, such that the first grid point is in the viscous sub-layer. Ideally we want a Y+ value of 1 or less. • Plot Turbulence > Y+, along both of the airfoil walls. • Deselect the Pressure Coefficient File Data. • We can see that this is achieved here, the max Y+ is 0.75

34. Post Processing [FLUENT] • Compare the predicted Cl and Cd against the experimental values. • From Reference 1 • Cl = 0.241 and Cd = 0.0079 • From the console window, we have predicted • Cl = 0.241 and Cd = 0.0083 • Again, good agreement can be seen.

35. Post Processing • Save the project from the FLUENT file menu . • Take the middle option ‘Continue after replacing settings file’) • Close FLUENT (File > Close FLUENT) • Additional post-processing will now be performed in CFD Post. • Return to the Workbench Project window. • Click on ‘Update Project’ and notice the Results panel update. • Right click on cell B2 (Results) and select edit. This will launch CFD Post.

36. Post Processing Note that CFD Post works in 3D, so a unit thickness will be added to the 2D airfoil, with symmetry side boundaries.

37. Post Processing • Insert a new Contour and accept the default name Contour 1 • Top menu > Insert > Contour • Choose the location as symmetry-1 • Choose the variable to be pressure and ‘Apply’ (zoom in)

38. Post Processing • A useful feature in CFD Post is the ability to compare two different sets of CFD data. • Verify that the file NACA0012-mach-0.5-conv.dat.gz is in your working directory. • File > Load Results – Browse to your working directory. • Under ‘Case options’ make sure ‘keep current cases loaded’ is checked. • Open the File NACA0012-mach-0.5-conv.dat.gz. • Click OK if an Information/Warning dialog box appears. • We now have two data sets loaded and can do a case comparison.

39. Post Processing Make sure that two windows are open, and select the respective cases in a different window. Lock the views so they are synchronised.

40. Post Processing Toggle on location ‘Symmetry 1’ in each case. Select ‘Contour 1’ and apply. We can compare the two pressure plots.

41. Post Processing Finally, we can plot the difference between the two. In the Outline view, double-click Case Comparison. The Case Comparison details view appears. Select Case Comparison Active and click Apply. A third viewport opens that displays the pressure difference between the two cases.

42. Summary In this tutorial we have used FLUENT within a Workbench project to compute the transonic, compressible flow over a naca0012 airfoil. We have imported a mesh that was generated in Gambit. We have used the density based solver with solution steering. We have compared the results to published experimental data and seen good agreement. We have seen how FLUENT can be linked to CFD Post in a Workbench project, and we have explored some of the features within CFD Post.

43. References T.J. Coakley, “Numerical Simulation of Viscous Transonic Airfoil Flows,” NASA Ames Research Center, AIAA-87-0416, 1987. C.D. Harris, “Two-Dimensional Aerodynamic Characteristics of the NACA 0012 Airfoil in the Langley 8-foot Transonic Pressure Tunnel,” NASA Ames Research Center, NASA TM 81927, 1981.