Introduction to CFX

Introduction to CFX

اسلاید 1: Workshop 2 Transonic Flow Over a NACA 0012 Airfoil.Introduction to CFX

اسلاید 2: GoalsThe purpose of this tutorial is to introduce the user to modelling flow in high speed external aerodynamic applications.In this case the flow over a NACA 0012 airfoil at an angle of attach of 1.49° will be simulated and the lift and drag values will be compared to published results. These results were taken with a Reynolds number of 9x106 and a chord length of 1m.*The airfoil is travelling at Mach 0.7 so the simulation will need to account for compressibility as well as turbulence effects. To reduce the computational cost, the mesh will be made up of a 2D slice through the airfoil (one element thick).*NASA TM 81927 Two-Dimensional Aerodynamic Characteristics of the NACA 0012 Airfoil in the Langley 8-Foot Transonic Pressure Tunnel 1981. Harris, C. D.

اسلاید 3: Start a Workbench projectLaunch WorkbenchSave the new project as naca0012 in your working directoryDrag a Fluid Flow (CFX) module from the Analysis Systems section of the Toolbox onto the Project SchematicIn the Project Schematic right-click on the Mesh cell and select Import Mesh FileSet the file filter to FLUENT Files and select NACA0012.mshWith the mesh file imported the Geometry cell will not be needed so it is removed from the Fluid Flow module.Note that you could have dragged Component System > CFX onto the Project Schematic, as in the first workshop. The mesh would then be imported after starting CFX-Pre.

اسلاید 4: Mesh ModificationOpen CFX-pre by right-clicking on the Setup cell and selecting EditAfter CFX-Pre has opened the mesh can be examined and it is clear that the scale is incorrect as the airfoil chord is 1000 m rather than 1 m, indicating the mesh was built in mm rather than m. This can be fixed using the mesh transformation options.Right-click on Mesh in the Outline tree and select Transform MeshChange the Transformation to ScaleLeave the method to Uniform and enter a Uniform Scale of 0.001Click OKSelect the Fit View icon from the Viewer toolbarZoom in further to see the airfoil

اسلاید 5: Mesh Modification The mesh has been built to have a single boundary around the entire outer edge. This needs to be split into inlet and outlet regions. While it is better to create the correct mesh regions when generating the mesh, CFX-Pre can be used to modify the mesh regions.Right-click Mesh in the Outline tree and select Insert > Primitive RegionClick on the Start Picking buttonFrom the drop down selection menu select Flood Select (see image to the right)In the viewer select any element from the front curved boundaryThe flood fill will select all cells where the change in angle is less than 30°Click in the Move Faces To field and type InletClick OKInletOutlet

اسلاید 6: Mesh Modification The remaining section will now be renamed “Outlet”. Expand the Mesh section of the tree so the list of Principal 2D Regions is visible. Note that this list now contains the location InletClick on the region pressure far field 1 to confirm it is the region representing the outletIt will be highlighted in the ViewerRight-click on pressure far field 1 and select Rename. Change the name to Outlet

اسلاید 7: Domain SetupUsually the option to automatically generate domains is active, this can be checked by editing Case Options > General in the Outline tree.Check that Automatic Default Domain is active the click OK. Right-click on Default Domain in the Outline tree and rename it to FluidDouble-click on Fluid to edit the domain settings

اسلاید 8: Domain SetupThis case involves high speed aerodynamics so it is important to include compressibility.It is important to set the correct operating pressure so that the intended Reynolds number is achieved. The simulation will take place at 288 [K] in air; this allows the speed of sound to be calculated. This can then be converted into a free-stream velocity using the Mach number. Using the definition for Reynolds number the fluid density can be obtained, which can then be used to determine the operating pressure for the simulation, assuming an ideal gas.c =Speed of soundR=Gas Constantγ =Ratio of specific heatsT=Temperatureu= Free-stream velocityM=Mach numberRe=Reynolds numberμ= Dynamic viscosity ρ= Density

اسلاید 9: Domain SetupIn the Fluid domain Basic Settings tab:Set the Material to Air Ideal GasSet the Reference Pressure to 56867 [Pa]Make sure you change set the unitsMove to the Fluid Models tabSet the Heat Transfer Option to Total EnergyThis is required for compressible simulationsEnable Incl. Viscous Work TermThis includes viscous heating effectsSet the Turbulence Option to Shear Stress TransportClick OK

اسلاید 10: Boundary ConditionsAn outlet relative pressure of 0 [Pa] will now be applied. This pressure is relative to the operating pressure of 56867 [Pa].Absolute Pressure = Reference Pressure + Relative PressureRight-click on the domain Fluid in the Outline tree and select Insert > Boundary, naming the boundary OutletChange the Boundary Type to Outlet and check that the location is set to OutletMove to the Boundary Details tab and set the Mass and Momentum option to Average Static Pressure with a value of 0 [Pa]Click OKThe sides of the domain will use symmetry conditions since this is a 2D simulation.Insert a Symmetry boundary called Sym Left, at the location sym leftInsert a Symmetry boundary called Sym Right, at the location sym right

اسلاید 11: Boundary Conditions The mesh has been constructed so that the airfoil is at 0° angle of attack. To apply the required angle of 1.49° the flow direction at the inlet must be adjusted. The values will be created using expressions.Right-click on Expression in the tree and select Insert > Expression. Call it Uinf.Set the Definition to 238.12 [m s^-1] then click ApplyAll expressions must have the appropriate dimensionsIn the expression editor add the following expressions by right-clicking on Expressions and selecting Insert > ExpressionAOA = 1.49[deg]Ux = Uinf*cos(AOA)Uy = Uinf*sin(AOA)Return to the main Outline tree

اسلاید 12: Boundary ConditionsRight-click on Fluid and insert a boundary called InletThe Boundary Type should be set to Inlet by default and a Location of Inlet should also be selected by defaultMove to the Boundary Details tabChange the Mass and Momentum option to Cart. Vel. ComponentsEnter the U, V and W values as Ux, Uy and 0 [m s^-1]Use the Expression icon to allow the Ux and Uy expressions to be enteredSet Static Temperature = 288 [K]Click OK

اسلاید 13: Boundary ConditionsThe Viewer indicates the locations of the inlet and outlet boundaries. Note that the arrows do not represent the applied flow direction.The final boundary condition is the wall around the airfoil. This should already exist as Fluid Default.Edit Fluid Default to check that only the wall bottom and wall top regions remain in the default boundaryClick CloseRename Fluid Default to Airfoil

اسلاید 14: MonitorsFor this simulation the lift and drag are the quantities of interest, so monitor points will be added to track their values and ensure they reach a steady value. The lift and drag coefficients will be created using expressions. Remember that the free-stream flow is offset from the x-direction so the forces will have to be adjusted to account for the angle of attack. Enter the following expressions, or select File > Import > CCL and load the file Airfoil.ccl. If loading the CCL file, use the Append option as shownFy=force_y()@AirfoilFx=force_x()@AirfoilLift =cos(AOA)*Fy-sin(AOA)*FxDrag =cos(AOA)*Fx +sin(AOA)*FyDenom=0.5*massFlowAve(Density)@Inlet*Uinf^2*1[m]*0.1[m]cL=Lift/DenomcD=Drag/Denom

اسلاید 15: MonitorsEdit Output Control from the Outline tree and go to the Monitor tabCheck the Monitor Options boxClick on the Add New Item icon and name it CLSet the Option to Expression and enter cLThis is the monitor point for the Coefficient of Lift. Note that all names and expressions are case sensitive, so the monitor point is named “CL” and it refers to the expression named “cL”.Add a new item called CD and set it to the expression cDThis is the Coefficient of DragClick OK

اسلاید 16: Solver ControlOpen the Solver Control section from the Outline treeIncrease the Max. Iterations to 200Change the Timescale Factor from 1 to 10A larger timescale can accelerate convergence, but too large a timescale will cause the solver to failSet the Residual Target to 1e-6This is a tighter convergence criteria and is discussed further belowClick OKThis case is now ready to run so click on File > Save Project then close the CFX-Pre window to return to the main Workbench window

اسلاید 17: Running the SimulationIn Workbench right-click on Solution and select UpdateAfter the solver has started right-click on Solution again and select Display MonitorsThis will open the Solver Manager and allow the residuals and monitors to be viewedCheck through all of the residuals and monitor values. The values of CD and CL become steady after about 50 iterations. You can click the Stop button from the toolbar to stop the run at this point.In the Solver Manager the User Points tab displays the monitor points setup in the Output Control section of CFX Pre. This will include the values of CL and CD. These should converge to a steady value before the convergence criteria is met. Otherwise the run should be extended. Many cases will be converged when an RMS residual level of 1e-4 is reached. For this case this is inadequate since the lift and drag had not reached steady values when the residuals were at 1e-4, hence a tighter convergence criteria was used.

اسلاید 18: Monitor ValuesBefore exiting the Solver Manager the converged values of CL and CD can be viewed by clicking on the monitor lines.The values extracted should be CL=0.236 and CD=0.0082. These values compare well to published values* of CL=0.241 and CD=0.0079.Now close the solver and return to the Workbench window.*AIAA-87-0416 Numerical Simulation of Viscous Transonic Airfoil Flows 1987. Thomas J Coakley, NASA AMES Research Centre.

اسلاید 19: Post-processingRight-click in the Results cell and select Edit to open CFD-Post. The results should automatically be loadedThis case required a large domain to allow the boundary conditions to be imposed without a large artificial restriction on the flow. However during post-processing the main interest will be in the flow close to the airfoil.Click on the Z-axis in the bottom right corner of the Viewer to orientate the viewUse the box zoom (right mouse button) so the Viewer displays the region around the airfoil

اسلاید 20: Post-processingWhen looking at the flow around an airfoil, plots of several variables can be of interest such as velocity, pressure and Mach number.In the tree turn on the visibility of Sym Left by clicking in the check boxDouble-click on Sym Left to bring up the details sectionUnder the Colour tab change the mode to Variable and select Velocity using the Global Range, then click ApplyNotice that the maximum velocity is around 350 [m/s]. This is higher than the sonic speed of 340 [m/s] calculated earlier for free-stream conditions.

اسلاید 21: Post-processingTo plot the Mach number a contour plot will be used so the supersonic region can clearly be identified.Select Insert > Contour or click on the contour icon Accept the default name then set Locations to Sym Left and the Variable to Mach NumberChange the Range to User Specified and enter 0 to 1.1 as the rangeSet # of Contours to 12, then click ApplyTurn of the Visibility of Sym Left so that the previous velocity plot is hiddenTry plotting other variables such as Pressure or Density, use the Local or Global Range when limits are not known

اسلاید 22: Post-processingTo plot the pressure coefficient distribution around the airfoil a polyline is needed to represent the airfoil profile and a variable needs to be created to give CP.Create a Polyline using Location > Polyline from the toolbarChange the Method to Boundary IntersectionSet Boundary List to AirfoilSet Intersect With to Sym Left and then click ApplyTurn off visibility of the previous created Contour plot to see the PolylineA line will be created around one end of the airfoil. For full 3D cases XY planes can be create at various span locations and used to extract Polylines.

اسلاید 23: Post-processingMove to the Expressions tab and right-click to create a new expression named cP with the definition: Pressure/(0.5*massFlowAve(Density)@Inlet*Uinf^2) Move to the Variables tab and right-click to create a new variable named CP.Set the Method to Expression and select cP. Click OK.

اسلاید 24: Post-processingA chart showing the pressure distribution around the airfoil will now be created.Insert a chart using Insert > Chart or selecting In the General tab leave the type as XYMove to the Data Series tab and enter a new series. Set the location to Polyline 1Move to the X Axis tab and change the variable to XMove to the Y Axis tab and change the variable to CPClick Apply and the chart is generatedThese values can be compared with experimental results.**AIAA-87-0416 Numerical Simulation of Viscous Transonic Airfoil Flows 1987. Thomas J Coakley, NASA AMES Research Centre.

اسلاید 25: Post-processingReturn to the Data Series tab and change the name to CFXInsert a new series and give it the name ExperimentChange the Data Source to File and select the file CP.csvOn the Line Display tab, set Line Style to None and Symbols to Rectangle. Also ensure that Symbol Colour is a different colour from the currently plotted CFX lineClick Apply and both data series are drawn

اسلاید 26: SummaryThe workshop has covered:Loading an existing meshScaling the meshGenerating New Regions from existing 2D PrimitivesSetting up and running a high speed compressible flow simulation over an airfoilExtracting lift and drag forces and comparing with experimental dataExamining the flow patterns around the airfoilComparing the pressure distribution to experimental values

اسلاید 27: Scope for further work.This simulation is a good match to experimental work but further steps could be taken if required, including:Refining the mesh, particularly in the wake region.Applying a transition model to account for the small region of laminar flow around the nose of the airfoil.Adding additional airfoil features such as a finite thickness trailing edge that will be used on all “real airfoils”. Simulating the whole wing to account for spanwise variations.Adding more features to a simulation will usually increase the computational cost, so one of the most important step in any simulation is to decide which features need to be included and which can be left out.