Getting started with CFD packages. OpenFOAM R and FLUENT R

Transcription

1 Getting started with CFD packages OpenFOAM R and FLUENT R

2 Copyright c 2015

3 Contents I Automotive 1 Ahmed Body CREO R Geometry OpenFOAM R Structure Case File Mesh Generation Case Setup High Performance Computing Grid Decomposition Potential Run Monitoring your Job Convergence check techniques: ParaView R Pre-processing Post Processing Mesh Refinement Analysis Validation and Verification Useful links 49 II Aerospace 2 Onera M6 Wing Geometry 53

4 2.2 ANSYS ICEM CFD Mesh Generation Meshing journey FLUENT R Case Setup Monitoring your job Post Processing Mesh Refinement Analysis Validation and Verification Useful links File scripts Force Coefficients Graphs: Pressure Probes Graphs Residuals Graphs

5 List of Tables 1.1 General OpenFOAM R case folder General blockmeshdict file Comparison between MPI and openmp turnaround time for the simulations Calculated y+ values for the coarse grid

6

7 List of Figures 1.1 Step 2, defining a new part Step 3, sketching the front part, Step 4, extruding the front part Step 5, rounding the nose Step 7, sketching (left) and extruding the middle part (middle). Then, drawing the zones to accommodate the stilts and colouring it as blue Step 7, sketching and extruding the rear part Step 7, sketching and extruding the stilts Step 8, starting an assembly mode Step 9, Importing the.prt files by clicking on the assemble icon Step 9, Combining all the parts together Step 10, Saving as.stl Step 11, specifying the number of vertices and the encoding type Mesh generation composition in OpenFOAM R Output of the surfacecheck command in the terminal Shows how to open the blockmeshdict in a text editor from the terminal Ways to find the dimensions of the computational domain Ways to create the computational domain General block topology of the blockmesh utility The Ahmed body is placed in the correct spot in the boundary stack. But, rotated 90 counter-clockwise Correction procedure; rotation step (top) and translation step (bottom) Automatic mesh generation functionality in OpenFOAM R Meshing strategy in OpenFOAM R My final mesh of the Ahmed body, it consist of 2,766,483 cells and 2,280,483 points Regions of varying cells densities; Ahmed body (left), xz-symmetry plane (right) unbalanced computational domain from different orientations; xz-axis (left), yz-axis (middle) and xy-axis (right) Balanced computational domain from different orientations; xz-axis (left), yz-axis (middle) and xy-axis (right) xz-symmetry plane showing no layer growth; minimumthickness=3 (left), =0.08 (right) Cells at the bottom rear end of the car; bad cell (left), good cell (right) Boundary layers within y+ in the range of 40<y+< Second mesh generated in OpenFOAM R The molecular viscosity value as seen in the transportproperties file Mesh decomposition in OpenFOAM R Adjusting the camera view

8 1.34 xz-symmetry plane showing the U-magnitude plots for the steady RANS simulation of mesh xz-symmetry plane showing the U-magnitude plots for the steady RANS simulation Transient DDES results of the velocity flow fields at: t 1 = s (left), t 2 =4000.3s (middle), t 3 =4000.4s (right) Transient DDES results of the velocity flow fields at: t 4 = s (left), t 5 =4000.6s (middle), t 6 =4000.7s (right) Transient DDES results of the velocity components at t 6 = 0.7s xz-symmetry plane showing Pressure Density plots for the steady RANS (top) simulation and transient DDES (bottom) Velocity plots showing the vortex at (00mm) from the rear end, Lienhart results (left)[lienhart-paper ], steady RANS (middle), transient DDES at t = 7s (right) Velocity plots showing the vortex at (80mm) from the rear end, Lienhart results (left)[lienhart-paper ], steady RANS (middle), transient DDES at t = 7s (right) Velocity plots showing the vortex at (200mm) from the rear end, Lienhart results (left)[lienhart-paper ], steady RANS (middle), transient DDES at t = 7s (right) Velocity plots showing the vortex system at (500mm) from the rear end, Lienhart results (left)[lienhart-paper ], steady RANS (middle), transient DDES at t = 7s (right) Velocity plots on the symmetry wall and the stream lines, and Pressure Density plots on the surface of the Ahmed body for the steady RANS (upper) and the transient DDES (lower) Velocity plots on the stream lines, yz-slices, ground and far-side Pressure plots on the glyph vectors, velocity plots on the yz-slices, ground and far-side Velocity contours over the range (0 U 72) Velocity plots on the symmetry wall and y+ plots on the surface of the Ahmed body for RANS simulation Velocity contours of mesh y+ plots of mesh Force coefficients for the RANS and DDES simulations, measurement results obtained from [openfoam-ws ] Importing the M6 geometry into ICEM CFD The M6 geometry file passed all tolerance checks First mesh generated in ICEM CFD; enclosure (top left), symmetrical+wing (top middle), wing (top right), wing+symm (bottom left), prism layers at leading and trailing edge (bottom middle and right respectively) Second mesh generated in ICEM CFD; enclosure (all top), wing+symm (bottom left), wing tip (bottom middle) and wing (bottom right) Second mesh generated in ICEM CFD; enclosure (all top), wing+symm (bottom left), wing tip (bottom middle) and wing (bottom right) Third mesh generated in ICEM CFD; far-side (top left), inlet (top middle), ground (top right), symmetry plane (bottom left), symm. near aerofoil (bottom middle) and wing (bottom right) Fourth mesh generated in ICEM CFD; far-field (top left), inlet (top middle), symmetry plane (top right), symm. near aerofoil (bottom left and middle) and wing (bottom right) th mesh generated in ICEM th mesh generated in ICEM; view from upper surface (left), view from trailing edge (right) A fine mesh Defining names for the different patches in the.stl file and the determining the bounding refinement boxes Castellated mesh generation parameters part 1 of Castellated mesh generation parameters part 2 of Surface-recovering snapping parameters

9 15 Boundary-layers addition parameters Mesh quality controls parameters This file lies in /case_folder/0/initialconditions This file lies in: /case_folder/0/include/fixedinlet This file lies in: /case_folder/0/include/sidestoppatches Velocity foam file Pressure foam file ν t foam file ν foam file ν file for DDES simulation ν Sgs f ile f orddes Descriptive dictionary showing the settings of different mesh-cutting scenarios A sample of a file script used for submitting jobs on Apocrita Force Coefficients graphs for the Spalart-Allmaras simulation Force Coefficients graphs for the Spalart-Allmaras simulation of mesh Pressure probes graphs for the Spalart-Allmaras simulation Residual graphs for the Spalart-Allmaras simulation Residual graphs for the Spalart-Allmaras simulation of mesh 2. first run 3000 iterations (left), further 2000 iterations (right). Total iterations=

10

11 I Automotive 1 Ahmed Body CREO R 1.2 OpenFOAM R 1.3 High Performance Computing 1.4 Monitoring your Job 1.5 ParaView R 1.6 Validation and Verification 1.7 Useful links

12

13 1. Ahmed Body 1.1 CREO R Presented in this section a guidance through exporting the so-called Ahmed model geometry from CREO R package into separate patches and in.stl format. Assuming that most of the student here at QMUL are well trained in using CREO R in sketching complex shapes. There might be an alternative way to carry out any of the following tasks in CREO R. Nevertheless, this can give you an overview of how I managed to prepare the geometry for my project. The following steps were carried out in CREO R 2.0. The following steps are compatible with other CREO R versions (i.e. Student version and Pro E), the only difference is the GUI (graphical user interface) Geometry 1. Launch CREO R parametric. 2. File New Part OK. 3. Sketch the part with the correct dimensions as in figure. 4. Extrude the part as in figure Round the part as in figure Save as.prt. 7. Repeat steps 2, 3, 4 and 6 for the middle, rear-end and stilts as shown in figure File New Assembly Name. as shown in figure Click on assemble front part and repeat this step for the rest as in figures File save as type stereolithography (*.stl), as shown in figure Export one patch at a time; Click on include the stilts ASCII Reduce the step size and the chord height as shown in figure Repeat the previous step for the other parts. 13. Check in every.stl file that the 1st line starts with solid partname and the last line ends with endsolid partname. 14. Merge all the.stl files into one; by writing the following command in a terminal: 1 Importing the stilts is challenging, I did it this way because I could not find an alternative way to export the stl as multi-patches. The importance of having the stilts as a separate patch will be seen later.

14 14 Chapter 1. Ahmed Body cat front. stl middle. stl rearend. stl stilts. stl > ahmedbody25. stl 15. Copy ahmedbody25.stl into an OpenFOAM R case folder See table Convert the dimensions of the geometry file from (mm) to (m) using the following command: surfacetransformpoints - scale ( ) ahmedbody25. stl ahmed - meters. stl 17. Check the geometry file for any illegal triangles and if there is a hole, by typing the following command in a terminal: surfacecheck constant / trisurface / ahmed - meters. stl In case of any failure in the geometry file; you can fix and repair it using Meshlab R. This open-source software can be downloaded from here meshlab/ and the tutorials for treating the failures in the geometry can be found here tinyurl.com/ou37p5w, and Figure 1.1: Step 2, defining a new part. Figure 1.2: Step 3, sketching the front part,.

15 Figure 1.3: Step 4, extruding the front part. Figure 1.4: Step 5, rounding the nose. Figure 1.5: Step 7, sketching (left) and extruding the middle part (middle). Then, drawing the zones to accommodate the stilts and colouring it as blue.

16 Figure 1.6: Step 7, sketching and extruding the rear part. Figure 1.7: Step 7, sketching and extruding the stilts. Figure 1.8: Step 8, starting an assembly mode

17 Figure 1.9: Step 9, Importing the.prt files by clicking on the assemble icon. Figure 1.10: Step 9, Combining all the parts together. Figure 1.11: Step 10, Saving as.stl

18 Figure 1.12: Step 11, specifying the number of vertices and the encoding type.

19 1.2 OpenFOAM R OpenFOAM R Open-source Field Operation And Manipulation is a free software for numerical analysis of fluids (i.e. CFD) which is written in C++. More info can be found by visiting this website Structure Case File An OpenFOAM folder should have the files shown in table 1.1. Files Function 0: Time directory~initial conditions of flow parameters. U and p Should ALWAYS be there. ν and ν t Should be there in case of Spalart-Allmaras. ν, ν t and ν sgs Should be there in case of DES. constant: Mesh files and solver settings directory. \polymesh Computational domain files. blockmeshdict User-defined dimensions and patches. \trisurface Geometry files. CAD_FIle.stl Written in ASCII and exported to.stl format. turbulenceproperties Switch the turbulence on/off. transportproperties Fluid properties. RASProperties or LESProperties Turbulence modelling approach. system: Integration, discretisation and iteration directory. controldict run time, CFL number, t. fvschemes Discretisation schemes. fvsolution Solver type. snappyhexmeshdict mesh features parameters. decomposepardict Cut the mesh for parallel running. Table 1.1: General OpenFOAM R case folder Mesh Generation Meshing in OpenFOAM R can be carried out through HELYX-OS by making use of the notes found here or through the terminal by using the utilities SnappyHexMesh and blockmesh. In order to apply SnappyHexMesh to the case folder; there should be a geometry file written in ASCII and exported to.stl format and a computational domain that bounds the geometry which is created using blockmesh utility. This can be represented in figure Computational Domain In order to create a correct computational domain; you need to make use of figures 1.16, 1.17 and Then, check the following procedure: 1. Take a note of the dimensions of the boundary stack and the position of the geometry from the inlet. 2. Take a note of the bounding box of your geometry; by typing the following command line in a terminal and the output will be similar to figure surfacecheck constant / trisurface / File_ name. stl 3. Determine the bounding box of the computational domain relative to the position of your geometry.

20 20 Chapter 1. Ahmed Body Mesh Generation Utility in OpenFOAM R SnappyHexMesh Computational domain Geometry written in ASCII and exported to.stl blockmesh Figure 1.13: Mesh generation composition in OpenFOAM R Figure 1.14: Output of the surfacecheck command in the terminal. 4. Fill in the blockmeshdict 2 by making use of figures 1.15 and 1.18 and table 1.2. Figure 1.15: Shows how to open the blockmeshdict in a text editor from the terminal. 5. Run the following command in the terminal that orders OpenFOAM R to generate your computational domain: blockmesh 6. Visualise your computational domain and import the geometry file in ParaView R Does the geometry lies in the correct position in the computational domain? If yes then tick this box. Otherwise, follow figure If you are not sure of where it is. Then, please check table If you are using your own linux machine, type the following command line $> parafoam &. However, if you are on apocrita then you need to type this first $> foamtovtk/ Then, download the VTK folder and the.stl file Directory on your machine Import both files to ParaView R. 4 Try to make the cell aspect ratio constant in all directions. For more info, the reader is encouraged to read the consecutive part about meshing the Ahmed body.

21 1.2 OpenFOAM R 21 To specify your computational domain no Is it a benchmark case? yes Research paper. search: Ercoftac Case name Defined under the computational setup or the wind tunnel dimensions section. Take a note! Figure 1.16: Ways to find the dimensions of the computational domain. Problem 1.1 The object is contained inside the computational domain. But, not placed in the right orientation as shown in figure Solution: 1. Visualise the boundary stack in ParaView R by typing blockmesh in the terminal. 2. Import the geometry file into ParaView R (File open geometry.stl). 3. See what s wrong; as in figure Then, plan a correction method. 4. Rotate the geometry by 90 in the clockwise direction by typing the following line 5. Then, see figure 1.20.: surfacetransformpoints - rollpitchyaw (90 0 0) geometry. stl rotatedgeometry. stl 5. Find the current position of the body by typing the following command in a terminal. surfacecheck constant / trisurface / geometry. stl 6. Translating vector = final position (To) - the current position (From). 7. Type the following line in the terminal: surfacetransformpoints - translate ( translated vector ) rotatedgeometry. stl translatedgeometry. stl. 8. Repeat steps 1 and 2 (and the output is shown in figure 1.20). Exercise 1.1 Try an alternative correction procedure to problem 1.1. hint: Don t change the orientation of the geometry but rather modify the blockmeshdict. 5 Where geometry.stl is the current name of the geometry file while rotatedgeometry.stl is a user defined file name.

22 22 Chapter 1. Ahmed Body Bounding box of your geometry Determine the vertices of the computational domain You can do it! Fill in the blockmeshdict Run it! Visualise paraview no Correct position? Yes Well Done! Figure 1.17: Ways to create the computational domain. 7 Top 4 Side 6 Outlet 2 5 Inlet 3 Ground 1 0 Figure 1.18: General block topology of the blockmesh utility.

23 1.2 OpenFOAM R 23 blockmeshdict Function converttometers 1; Assuming that you converted the cad.stl file to m. vertices Vertices for a single block as shown in figure ( ( ) coordinates of vertex 0. ( ) coordinates of vertex 1. ( ) coordinates of vertex 2. ( ) coordinates of vertex 3. ( ) coordinates of vertex 4. ( ) coordinates of vertex 5. ( ) coordinates of vertex 6. ( ) coordinates of vertex 7. ); blocks ( hex ( ) Specify the number of cells for the defined block(s). Hexahedral mesh block with correctly ordered vertices as in figure (24 8 6) Number of cells in x, y and z directions respectively 4. simplegrading (1 1 1) ); edges ( ); Difference in the refinement between the beginning and end cells for all directions. 1 means uniform spacing. Leave it as it is; for a single block as shown in figure patches Define 6 patches as shown in figure ( patch inlet ( ( ) ) patch outlet ( ( ) ) wall ground ( ( ) ) symmetry sides ( ( ) ( ) ) symmetry top ( ( ) ) ); Symmetry means that half the domain is modelled. Table 1.2: General blockmeshdict file. Figure 1.19: The Ahmed body is placed in the correct spot in the boundary stack. But, rotated 90 counter-clockwise.

24 24 Chapter 1. Ahmed Body Figure 1.20: Correction procedure; rotation step (top) and translation step (bottom).

25 1.2 OpenFOAM R 25 Ahmed Body SnappyHexMesh Castellated Snap mesh to surface Layers addition Base mesh Refine base mesh Remove unused cells Figure 1.21: Automatic mesh generation functionality in OpenFOAM R Presented in this part a general overview of the different processes undertaken by the snappyhexmesh utility. The mesh generation is decomposed into three main stages as shown in figure Followed by a prepared copy of a snappyhexmeshdict which are shown in figures 11, 12, 13, 14, 15 and 16. Castellated Mesh: is the first process undertaken by the mesher; where the user has to define the refinement regions and the level of refinement depends on the type of simulations. In this case, two boxes of very high gradient were defined at the rear end to cover the wake. Then, two boxes of varying densities covered the whole car. Snapping stage: resolves the sharp edges of the geometry according to the skewness level and the max. orthogonality scales set by the user. Layers addition: The last process undertaken by the mesher; where the user has to specify the number of boundary layers, the minimum thickness of the first cell away from the wall (y), the stretching ratio (expansionratio) and the ratio of the height of the final layer cell to its width (finallayerthickness). Strategies for choosing a reasonable y for simulating a viscous flow: 1. Interested in the linear sublayer where 0 y + 5? This choice is very expensive. Deactivate the layer addition process in the snappyhexmeshdict. Specify a box near the wall with high level of refinement. 2. Interested in the log-layer, where 30 y + 60? OpenFOAM R contains a variety of wall functions; that are compatible with specific turbulence modelling approaches. Activate the layer addition process. Calculate the minimum thickness of the first cell near the wall using any yplus calculator found online. 1. Resolve the sharp edges of the geometry. By typing the following command: surfacefeatureextract - includedangle writeobj constant / trisurface / geometryfile. stl geometry 2. Run the automatic mesher; by typing the following command: snappyhexmesh - overwrite

26 26 Chapter 1. Ahmed Body Meshing strategy in OpenFOAM R can be summarised in figure 1.22: (1) Specify mesh quality parameters Thank him a lot! yes Run mesher Quality check yes checkmesh utility paraview Satisfied? No yes Set the case Ask your supervisor for help! No Any similarity? Check on the forum cfd-online.com No Any similarity to the problems covered here? Figure 1.22: Meshing strategy in OpenFOAM R Preceding Work Before attempting the meshing stage; one should know the flow physics over the Ahmed body. You are encouraged to read the paper by Gillieron et al which can be downloaded from here As the flow hits the car, a high pressure gradient was captured at the nose. A separation line (Kelvin Helmholtz) was observed by Gillieron et al. at the top side of the nose. Then, the fluid travels with constant momentum alongside the middle part. As the flow at the top side reaches the rear-end, the momentum suddenly drops, and fluid re-attached alongside the hatch part generating swirling vortices. At the same time, the flow at the bottom rear end will generate a smaller vortices which is opposite in direction to the vortices generated from the flow at the top side. As a consequence, the vortices will combine together resulting in an unsteady flow.. Own mesh: In order to capture the flow separation; 3 boxes of refinement were specified in the snappyhexmeshdict one at the frontal nose, hatch-side and the wake. In addition, a very small refinement box was added near the bottom right rear-end of the car to capture the small vortices coming from the bottom side. As shown in figure Figure 1.23: My final mesh of the Ahmed body, it consist of 2,766,483 cells and 2,280,483 points.

27 1.2 OpenFOAM R 27 Problem 1.2 The cells on the body are not balanced and separated by regions of high density cells. As a consequence, the layers will grow badly as shown in figure Figure 1.24: Regions of varying cells densities; Ahmed body (left), xz-symmetry plane (right). Solution: The problem is due to the unbalance of the aspect ratio of cells in the x,y and z directions as shown in figure Balancing the number of cells in the x, y and z directions will solve this problem as shown in figure Figure 1.25: unbalanced computational domain from different orientations; xz-axis (left), yz-axis (middle) and xy-axis (right). Figure 1.26: Balanced computational domain from different orientations; xz-axis (left), yz-axis (middle) and xy-axis (right). Problem 1.3 The layers did not grow at all as in figure Solution: This might be due to two reasons; either the minimumthickness was chosen greater than 1.0 or chosen smaller than 0.1. By choosing a value between this range (i.e. minimumthickness=0.4) the layers will grow as in figure Problem 1.4 There is a very bad cell at the bottom rear end of the car as in figure Those bad cells can influence the solution and result in non-physical results. Solution: By changing the number of cells in the computational domain so that the cell aspect ratio is 1 : 1 : 1. The overall cells will be stretched or compressed accordingly. Problem 1.5 Y+ is in the wrong range, less than 10 boundary layers, underestimated stretching ratio. This might result in non-physical results.

28 28 Chapter 1. Ahmed Body Figure 1.27: xz-symmetry plane showing no layer growth; minimumthickness=3 (left), =0.08 (right). Figure 1.28: Cells at the bottom rear end of the car; bad cell (left), good cell (right). Figure 1.29: Boundary layers within y+ in the range of 40<y+<70.

29 1.2 OpenFOAM R 29 Meshing journey Presented in this part some of the attempts I went through before arriving at my final mesh Attempt 1.1 Attempt 1.2 The second mesh generated using snappyhexmesh. The mesh consist of 1,562,813 cells and 1,307,831 nodes. Figure 1.30: Second mesh generated in OpenFOAM R Case Setup In order to proceed further in this section; you should check the following procedures first: 1. Determine the turbulence at the inflow boundaries. Specify the molecular viscosity ν from the definition of the Reynolds number Re = U L ν (1.1) Where U is the mean velocity of the object with respect to the fluid flow. L is the characteristic length. Specify the turbulent viscosity using the following relation: ν t = β ν (1.2) Where β = 100 and is constant for Re 100,000. Specify the modified kinematic viscosity ν at the free-stream, using the following relation: ν = 5ν (1.3) Use ν=0 at the wall. 2. Determine the time step: Recall that the CFL number is a dimensionless ratio (briefly how much of the transport solution can travel one cell width in one second); which can be expressed mathematically as: CFL = u t x Where t is the time step, x is the cell width and is a grid characteristic 6 How many iterations? (1.4) 6 For a transient solution; you need to resolve the eddy with 4 time-step. More info is available online ;-)

30 30 Chapter 1. Ahmed Body 3. Scenarios for solution convergence? Request lift and drag coefficients. Specify the spots to place pressure probes. 4. Specify the finite volume schemes? Steady state or transient solution? 1st or 2nd order solution? 5. Specify the solver that you will be using? SIMPLE or PISO or PIMPLE? Setting the case using GUI HELYX-OS 1. Launch HELYX from a terminal../ HELYX -OS.sh & 2. Import your case folder: Open Path to your case folder Open. 3. Make sure there is no errors. 4. Switch to the Case setup tab. 5. Set the solution modelling: (a) Time steady. (b) Flow incompressible. (c) Turbulence model Spalart-Allmaras 6. Set the materials: (a) ρ = (b) Dynamic viscosity = (c) Kinematic viscosity = Set the Boundary Conditions: (a) Inlet: i. Velocity: Type fixed value and U x = 40. ii. Pressure: zero gradient. (b) Outlet: i. Velocity: Type inletoutlet. Inlet value ( ). ii. Pressure: Type fixed value. Value 0.0 (c) Ground & Ahmed body patches: i. Patch type wall. Momentum Type Fixed. Wall Type No-slip. (d) Sides and Top i. Patch type symmetry. 8. Set the numerical schemes: (a) Advection: i. U: first run Upwind-1st order. Then, switch to bounded linear upwind 2nd O. ii. nutilda: first run Upwind-1st order. Then, switch to bounded linear upwind 2nd O. (b) Laplacian: i. Non-orthogonal corrections: Set the Solver Settings: (a) Non-orthogonal correctors = 0. (b) Residual control = (c) Relaxation factor 7 : i. U = 0.7 ii. p=0.3. iii. ν=0.7 7 The sum of the relaxation factor values of the velocity and pressure should equal to 1.

31 1.2 OpenFOAM R Set the Run-time controls: (a) Start from 8 : start time 0.0 (b) End-time 9 : 5000 (c) Data Writing: i. Write Control 10 A. Time step every 500 iteration. 11. Set the Field Initialisation: (a) U: Fixed value (40 0 0). (b) p: Fixed value 0.0 (c) ν: Fixed value (d) Click initialise Run the simulations in series: (a) Switch to Solver tab Run. Setting the case manually in the terminal Presented in this part a general view of the case setup. Starts by going through the dictionary files, setting the boundary and initial conditions. A quick introduction to discretization schemes and solver control. Finally, how to start the simulation in serial and parallel. (Setting the case in OpenFOAM R flow chart to be placed here...) RANS The initial and boundary conditions dictionary files can be copied from the tutorials folders that are pre-installed in OpenFOAM R, a suitable case is the motorbike one. The initial and boundary conditions for this case can be copied using the following command: cp -r $FOAM_ TUTORIALS / incompressible / simplefoam / motorbike /0. org path_ to_ your_ case_ folder / // This command copies the time directory folder to your own case folder. cp -r 0. org 0 // This command renames the 0. org to 0 The solver settings, fvschemes and the RANS-settings files that are vital for running this simulation are available in some of the tutorials folders that are pre-installed in OpenFOAM R, a suitable case that runs Spalart-Allmaras can be found if you typed the following command: cd $FOAM_ TUTORIALS / incompressible / simplefoam / airfoil2d / Now, you need to copy the finite volume files (i.e. discretisation schemes and the solver type), run time file, RANS-settings files to your own case folder by running the following commands on at a time in a terminal respectively: cp system / fvschemes / your_ case_ folder_ directory / system cp system / fvsolutions / your_ case_ folder_ directory / system cp system / controldict / your_ case_ folder_ directory / system cp constant / RASProperties / your_ case_ folder_ directory / constant cp constant / transportproperties / your_ case_ folder_ directory / constant The molecular viscosity value can be changed in the transportproperties file as shown in figure Click on the drop-down arrow to see other options. Choose Start time if you haven t run the simulations before. Or latesttime if you already ran it and haven t converged and would like to run few more iterations. 9 The number of iterations to run. 10 After how many iterations would you like OpenFOAM R to store the data. 11 In case, you already ran few iterations and would like to start from initial conditions rather than starting from the latest calculated conditions.

32 32 Chapter 1. Ahmed Body Figure 1.31: The molecular viscosity value as seen in the transportproperties file. DDES Setting the velocity (U), pressure (p) and turbulent viscosity (ν t ) is the same as in figures 20 and 21 respectively. Now, we are left with two unset viscosity variables ( ν and ν Sgs ) which can be set by copying the nut file twice and renaming one as nusgs and the second as nutilda as follows: cp 0/ nut 0/ nusgs cp 0/ nut 0/ nutilda

33 1.3 High Performance Computing High Performance Computing Multiprocessing computing can be classified into MPI and openmp. MPI - Parallel computing. - Communications between processors - One process runs on one core - Point-to-point operation where each processor runs one process (i.e. calculation of one cell) then passes the solution to another processor in an iterative method. OpenMP Table 1.3: Comparison between MPI and openmp OpenFOAM R just support MPI jobs. Thus, if you tried to run your job using openmp it will crash. Submitting a parallel job onto Apocrita, can be as follows: 1. Connect to the apocrita server using the command: ssh -X username@login.hpc.qmul.ac.uk 2. Copy and paste your password from the sent to you by the cluster admin 12. Now, you arrived at the front-end which is the receptionist. From here you will request the number of nodes, cores and the period you need to accommodate your job for. Followed by the type of work (simulation type, decomposing your mesh etc...) that you want the supercomputer to run all written in commands as in figure 27. Then, this request will be passed on to the back-end which will place your job in a queue (batch) till there is an empty slot to accommodate your job as described by Dr. J-D. Müller in one of his lectures. 3. Generate your case folder as described in section If you have OpenFOAM R installed on your box. Then, you can prepare the case on your laptop, hence, upload it onto Apocrita using: scp -r -p directory_casefolder/folder_name QMuserID@login.hpc.qmul.ac.uk:folderName 4. Change your directory from the current one to the case folder cd case_ folder_ name 5. Write a file script specifying the amount of virtual memory, the run time etc... Or Copy the following lines if you want to mesh your geometry: #!/ bin /sh # $ - cwd -V // Set the working directory for the job to the current directory # $ - pe openmpi 1 // Ordering a whole node. # $ -l h_rt =10:0:0 // Do you want your simulation to run for 10 hrs? # $ -l h_vmem =24 G // Requesting 24 Gb of RAM ( as 1 node =12 cores =24 Gb) # $ -m base // Get an at the Beginning of the job, Alert, Something that I might have forgotten and as it Ends. # $ -M _ address // Your address where the base can be sent to. # $ -N Job_ name // User - defined job name. blockmesh // Generate the virtual wind tunnel. surfacefeatureextract - includedangle writeobj constant / trisurface / geometryfile. stl geometry // resolve the sharp edges 12 To paste any thing in the terminal; use ctrl+shift+v instead of the recognised ctrl+v. You are advised to change your password by typing passwd in the terminal

34 34 Chapter 1. Ahmed Body decomposepar // Order OpenFOAM to generate your mesh on a number of processors. foamjob - parallel - screen snappyhexmesh - overwrite // Terminate the parallel meshing process reconstructparmesh - mergetol 1e -6 - constant // reconstructing your mesh. ls -d processor * xargs -i rm - rf./ $1 // delete the processor files. checkmesh // check if your mesh has failed certain criteria. foamtovtk // convert your mesh into a Paraview friendly format. (a) Now that you meshed your geometry, you should visualise it in ParaView R as discussed in section 6. (b) If you want to run the solver on apocrita, then copy the following lines: #!/ bin /sh # $ - cwd -V // Set the working directory for the job to the current directory # $ - pe openmpi 1 // Ordering a whole node. # $ -l h_rt =10:0:0 // Do you want your simulation to run for 10 hrs? # $ -l h_vmem =24 G // Requesting 24 Gb of RAM ( as 1 node =12 cores =24 Gb) # $ -m base // Get an at the Beginning of the job, Alert, Something that I might have forgotten and as it Ends. # $ -M _ address // Your address where the base can be sent to. # $ -N Job_ name // User - defined job nam decomposepar // Distribute your mesh and the time fields among n processors. mpirun - np 12 simplefoam - parallel // Run your simulation on 12 cores using the simplefoam solver. reconstructpar // reconstruct your case. ls -d processor * xargs -i rm - rf./ $1 // delete the processor files. yplusras // Calculate the y+ incase of using any RANS approach. foamtovtk // This format is easily imported to Paraview. Try to avoid the following mistakes when writing a file script: Ending any of your commands with &. This means that you ordered your job to run in the background of the node so the Sun Grid Engine would probably kill your job. 2. Redirecting your job to a log file is un-necessary. By default the Sun Grid Engine (queueing system) will create two files; an output file job_name.o and an error file job_name.e. 3. Following your mpirun command. Write the number of cores that you are getting from one node (i.e. in case of small nodes it is 12 cores). If you wrote a number >12 (i.e. 16). Still you will have your job running. But, your job will be slowed down as a result of 2 processes running on 4 cores. For more information and alternative ways on how to write a file-script you can visit this website: Grid Decomposition Presented in this sub-section an overview of the different mesh decomposition methods in OpenFOAM R as shown in figure In order to decompose your mesh, please complete the following steps: 1. Copy the decomposepardict file to your case_folder/system. The data inside this file can be found in this report s appendix or from the motorbike tutorial case folder which can be found in the following directory: 13 Thanks to the IT-research and support team for their clarification in writing a correct file script.

35 1.3 High Performance Computing 35 $FOAM_ TUTORIALS / incompressible / simplefoam / motorbike / system / decomposepardict 2. Edit the decomposepardict by choosing a suitable mesh decomposition method and specifying the number or the order of cuts as illustrated in figure Type the following command to start the mesh cutting process: decomposepar After running your parallel simulation; you may want to reconstruct your mesh for postprocessing. This is a one step which can be done by typing the following command: reconstructpar Grid Decomposition Methods in OpenFOAM R Simple Hierarchical Scotch/Metis Manual Similar concept. Different configuration. Applied for simulation running over cores with varying performance Figure 1.32: Mesh decomposition in OpenFOAM R A good source worth considering is this link and if you got time on your hands (i.e. 68 minutes and 36 seconds) then why not considering watching these tutorials and tinyurl.com/ozsydkm.

36 36 Chapter 1. Ahmed Body Potential Run Why potential run? 1.4 Monitoring your Job Convergence check techniques: Force Coefficients The force coefficients are useful in checking the degree of convergence of the solution. But, this function is not calculated automatically with the simulation, you need to order OpenFOAM R to do so; which can be done adding few lines at the end of the controldict file. Those lines are as follows: functions forcecoeffs type forcecoeffs ; functionobjectlibs ( " libforces. so" ); outputcontrol timestep ; // instead of timestep, you can try runtime. timeinterval 1; log yes ; // The calculations will be produced in a separate. dat file. patches ( " ahmed_.*" ); // name of the patches where you want to calculate the forcecoeffs. pname p; UName U; rhoname rhoinf ; // Indicates incompressible log true ; rhoinf 1.225; // Redundant for incompressible liftdir (0 0 1); // z- component dragdir (1 0 0); // x- component CofR ( ); // Axle midpoint on ground pitchaxis (0 1 0); maguinf 40; // free stream velocity lref 1.044; // Wheelbase length Aref 0.112; // Estimated The lift and drag coefficients can be found in the postprocessing folder in the main case directory (i.e. case_directory/postprocessing/forcecoeffs/start_times/forcecoeffs.dat, where start_times are the numbers when you started the simulation). During the simulation you can view the force coefficients to check the degree of unsteadiness in the solution using either two ways: 1. Type the following command to view the last few lines of the force coefficients: tail -n 500 postprocessing / forcecoeffs /0/ forcecoeffs. dat 2. Plot the force coefficients on the go using gnuplots (an opensource package that is preinstalled in most linux packages; and is the most efficient way to plot any graph from the command-line): (a) Order gnuplots to extract the force coefficients from its directory relative to your current directory (i.e. if you are currently in the main case folder then the force coefficients are there case_directory/postprocessing/forcecoeffs/start_times/forcecoeffs.dat):

37 1.4 Monitoring your Job 37 Open a text editor, by typing the name of the editor (in this case its nano which is a very simple and light text editor), followed by the file name: nano forcecoeffs Copy the few lines into the file you just created: set logscale y set key bottom right set xlabel " Simulationtime [ s]" set ylabel " forcecoeff [ -]" set title " Plot of forcecoeffs over simulationtime " set grid plot " postprocessing / forcecoeffscyl /0/ forcecoeffs. dat " using ($1):( $4) with lines title " lift_coeff ",\ " postprocessing / forcecoeffscyl /0/ forcecoeffs. dat " using ($1):( $3) with lines title " drag_coeff " pause 1 reread If you became familiar with using gnuplots, you can replace the first line in the previous script to define the x and y range so instead of set logscale y you can write the following lines : set yr [0:1] set xr [1:100] where 0 y 1 and 1 x 100. You can specify any range you want! (b) Type the command that will plot your graph instantly: gnuplot forcecoeffs (c) To close this window; press ctrl+c in the terminal. An example of the force coefficients plots is illustrated in figure 28 for the iterations (50, 100, 500 and 4000) of the own RANS simulation. Residuals Plotting the residuals using gnuplots will follow the same main steps as plotting the force coefficients. However, the only difference is the file name and the lines that you will need to copy into that file: i.e. set logscale y set title " Residuals " set ylabel Residual set xlabel Iteration plot " < cat solver_ output_ file grep Solving for Ux cut -d - f9 tr -d, " title Ux with lines,\ " < cat solver_ output_ file grep Solving for Uy cut -d - f9 tr -d, " title Uy with lines,\ " < cat solver_ output_ file grep Solving for Uz cut -d - f9 tr -d, " title Uz with lines,\ " < cat solver_ output_ file grep Solving for omega cut -d - f9 tr -d, " title omega with lines,\ " < cat solver_ output_ file grep Solving for k cut -d - f9 tr -d, " title k with lines,\ " < cat solver_ output_ file grep Solving for p cut -d - f9 tr -d, " title p with lines,\ " < cat solver_ output_ file grep Solving for nutilda cut -d - f9 tr -d, " title nutilda with lines pause 1 reread

38 38 Chapter 1. Ahmed Body If you are using your own linux box to run the simulations. Then, the solver_output_file can be requested before running the simulation by typing: simplefoam > log & On the other hand, if you are running your simulation on Apocrita. Then, you do not have to request a log file. Because, the sub grid engine will output four files. One of them is the log file. In both ways, you will have to replace solver_output_file with log (in case you are using your linux box) or with the output file name from apocrita (i.e. in most cases it will look something like this Job_name.o ). An example of the residual plots is illustrated in figure 31 for the iterations (50, 100, 500 and 4000) of the own RANS simulation. Probes A useful way to check for convergence, is by placing pressure probes in the regions where separation occurs. In the separation region (i.e. wake of the car) the solution is unsteady and fluctuates rigorously. You will need to copy the few lines to the end of the controldict file before the last curly bracket that belongs to the functions and not the forcecoeffs. I assume you previously copied the forcecoeffs function. probes type probes ; functionobjectlibs (" libsampling. so"); enabled true ; outputcontrol timestep ; outputinterval 1; fields ( p ); probelocations ( ( ) // define your own probe locations ( ) ( ) ( ) ( ) ( ) ); Viewing the calculated pressure probes is a similar process to viewing the force coefficients as previously discussed. To plot the pressure probes; you can copy the following lines into a file then type the command gnuplot file_name: set logscale y set key bottom right set xlabel " Simulationtime [ s]" set ylabel " Probes [ -]" set title " Plot of Probes over simulationtime " set grid plot " postprocessing / probes /0/ p" using ( $1):( $2) with lines title " ( ) ",\ " postprocessing / probes /0/ p" using ( $1):( $3) with lines title " ( ) ",\ " postprocessing / probes /0/ p" using ( $1):( $4) with lines title " ( ) ",\

39 1.5 ParaView R 39 pause 1 reread " postprocessing / probes /0/ p" using ( $1):( $5) with lines title " ( ) ",\ " postprocessing / probes /0/ p" using ( $1):( $6) with lines title " ( ) ",\ " postprocessing / probes /0/ p" using ( $1):( $7) with lines title " ( ) " An example of the pressure probes plots is illustrated in figure 30 for the iterations (50, 100, 500 and 4000) of the own RANS simulation. 1.5 ParaView R Pre-processing y+ check The y + can be checked manually before running the simulation. By doing the following steps: 1. Import your mesh into paraview. 2. Extract one cell and view its axis, then take a note of the height of this cell (y). 3. Calculate the y+ using the following equation: y + = y ν u τ (1.5) where ν is the molecular viscosity (i.e. ν = m 2 /s). u τ is the friction velocity and is defined as: u τ = U Re f c f 2 (1.6) Where U Re f is the velocity of the air relative to the car, and c f is the skin friction coefficient; which can approximated for a flat plate as follows: c f 0.074Re 0.2 L (1.7) A constraint for the previous equation is that < Re L < n Post Processing Presented in this sub-section the technique in carrying out the post-processing of the simulation results in ParaView R. There are few points that should be taken into account when comparing plots of the same quantities, which are: 1. Use the same legend range, which is done by: (a) Click toggle color legend visibility icon; to view the default range set for the chosen property. (b) Click on edit color map icon Rescale to custom range icon (set the min. and max.). 2. Use the same camera view, which can be done by: 3. Click Adjust camera Configure Name first view click current view OK Close. as shown in figure Save the screenshots from ParaView R, which can be done by: (a) File Save screenshot. (b) Override Color Palette, drop down menu choose Print Print.

40 40 Chapter 1. Ahmed Body Figure 1.33: Adjusting the camera view. Figure 1.34: xz-symmetry plane showing the U-magnitude plots for the steady RANS simulation of mesh2. Velocity Profiles Mesh 2 results: xz-symmetry plane: xz-symmetry plane: Velocity magnitude: Velocity components: The velocity vector components can be plotted by changing the default settings from the drop down menu: The surface vectors in figure 1.39 were plotted by following the tutorial in this website http: //goo.gl/57tlwj. yz-symmetry plane plots Presented in this section the technique of plotting surface vectors along the yx-symmetry plane: 1. Click on the case file in the pipeline browser (make it visible).

41 1.5 ParaView R 41 Figure 1.35: xz-symmetry plane showing the U-magnitude plots for the steady RANS simulation. Figure 1.36: Transient DDES results of the velocity flow fields at: t 1 = s (left), t 2 =4000.3s (middle), t 3 =4000.4s (right) Figure 1.37: Transient DDES results of the velocity flow fields at: t 4 = s (left), t 5 =4000.6s (middle), t 6 =4000.7s (right) Figure 1.38: Transient DDES results of the velocity components at t 6 = 0.7s 2. Filters menu Common Slice. 3. Set the origin so that you specify the x-coordinate. While, the y- and z-coordinates are set to zero Apply. 4. Filters Alphabetical Surface Vectors. Select input U. Constraint Mode Parallel. Apply. 5. Filters Common Glyph. Vectors U. Glyph type Arrow. Scale Mode off.

42 42 Chapter 1. Ahmed Body Figure 1.39: xz-symmetry plane showing Pressure Density plots for the steady RANS (top) simulation and transient DDES (bottom). Set Scale Factor check Edit box Maximum number of points (Do your judgement). Coloring pressure (point). Figure 1.40: Velocity plots showing the vortex at (00mm) from the rear end, Lienhart results (left)[lienhart-paper ], steady RANS (middle), transient DDES at t = 7s (right) Figure 1.41: Velocity plots showing the vortex at (80mm) from the rear end, Lienhart results (left)[lienhart-paper ], steady RANS (middle), transient DDES at t = 7s (right)

43 1.5 ParaView R 43 Figure 1.42: Velocity plots showing the vortex at (200mm) from the rear end, Lienhart results (left)[lienhart-paper ], steady RANS (middle), transient DDES at t = 7s (right) Figure 1.43: Velocity plots showing the vortex system at (500mm) from the rear end, Lienhart results (left)[lienhart-paper ], steady RANS (middle), transient DDES at t = 7s (right)

44 44 Chapter 1. Ahmed Body Stream lines The velocity stream lines were plotted as follows: 1. In the pipeline browser click on the eye next to the case file (make it visible). 2. Filter menu Stream tracer. Vectors U. Integration direction Both (forward and backward). Integration type Runge-Kutta 4-5. Set the maximum streamline length to the highest value in the fixed range given. Seed type High resolution line source. Tick Show line. Set point 1 to the minimum bounding box of the car, while point 2 to the maximum bounding box of the car. resolution 100. Representation Surface. Figure 1.44: Velocity plots on the symmetry wall and the stream lines, and Pressure Density plots on the surface of the Ahmed body for the steady RANS (upper) and the transient DDES (lower). Computational Time: Grid Simulation Wall-clock time; hh:mm:ss coarse Max Vmem 14 S-A 3:57: GB 4,000 DDES 45:00: ,000 No. of iterations Table 1.4: turnaround time for the simulations. 14 Maximum amount of virtual memory

45 1.5 ParaView R 45 Figure 1.45: Velocity plots on the stream lines, yz-slices, ground and far-side. Figure 1.46: Pressure plots on the glyph vectors, velocity plots on the yz-slices, ground and far-side.

46 46 Chapter 1. Ahmed Body Mesh Refinement Analysis Presented in this subsection a guess method used in the mesh refinement analysis which is based on plotting the velocity contours as shown in figures You need to refine in the regions of: 1. High gradient; where the contours are perpendicular to the surface: Front nose. Rear end. 2. Flow separation. You Do not need to refine in the regions of: 1. Low gradient, where the contours are tangent to the surface: The middle part of the Ahmed model (cuboid), where the flow travels with constant momentum. This is why the mesh is coarse compared to the nose and the rear end. Far-fields (i.e. inlet, outlet, far-sides and top.) y + plots PLotting the y + over the mesh is useful in checking the regions where the y + falls below the range at which the wall function in OpenFOAM R is activated (i.e. 30 < y + < 300) which in turn could be used for mesh refinement analysis. But, this utility is not calculated automatically with the simulation, you need to order OpenFOAM R to do so; which is usually done by the end of any RANS simulation with activated wall functions, by typing: yplusras In case of running any LES approach, then type: yplusles In figure 1.48, the y + falls below 30 at the regions of low velocity, where separation takes place so the mesh was highly refined there (centre of nose and rear end). Apart from this, the average satisfy the range at which the wall function is activated which is shown in table 1.5. Grid minimum y+ maximum y+ average y+ Coarse Table 1.5: Calculated y+ values for the coarse grid.

47 1.5 ParaView R 47 Figure 1.47: Velocity contours over the range (0 U 72).

48 48 Chapter 1. Ahmed Body Figure 1.48: Velocity plots on the symmetry wall and y+ plots on the surface of the Ahmed body for RANS simulation. Plotting the y + as shown figure 1.48 was done as follows: 1. From the terminal, in the case directory type foamtovtk this command will convert the calculated flow quantities into a VTK file. 2. Type parafoam &, this will open ParaView R in a new window. 3. View all mesh parts Apply. 4. Filter menu Common Slice. To be able to cut the plane in the xz-symmetry, you have to enter the coordinates. Here I used the origin as ( ) which lies at the centre of the computational domain, then, I specified the normal to be (0 1 0) which will apply a longitudinal cut perpendicular to the y axis. 5. File Open VTK ahmed_body_endtime.vtk. This will import the car into the symmetry plane. Mesh 2 refinement analysis Figure 1.49: Velocity contours of mesh 2. Mesh 3 refinement analysis Figure 1.50: y+ plots of mesh 2.

49 1.6 Validation and Verification Validation and Verification C D C L Force Coefficients measurement RANS DDES Figure 1.51: Force coefficients for the RANS and DDES simulations, measurement results obtained from [openfoam-ws ] - Plot velocity over line using GIMP. Comparison between computational and experimental. 1.7 Useful links Presented in this section a number of very useful URLs for learning and using OpenFOAM R and ParaView R. 1. Tommaso Luchhini, Running OpenFOAM R in parallel, Politecnico Di Milano, tinyurl.com/qzv5x3b. 2. Artur Lidtke, Meshing in OpenFOAM R, University of Southampton, com/odavyc3. 3. Nilsson H., Petit O., Pre-processing in OpenFOAM R, mesh generation, Chalmers University of Technology, 4. Hrvoje Jasak, OpenFOAM R : Open Platform for CFD and Complex Physics Simulations,Wikki Ltd, United Kingdom, 5. Silva G., Arima G., Sousa F., Mesh Generation in OpenFOAM R with SnappyHexMesh, tinyurl.com/q25n9ja. 6. Nagy J., Introductory videos to CFD and OpenFOAM R, 7. Mesh Generation with the blockmesh utility 8. Brief introduction to OpenFOAM R 9. All OpenFOAM R utilities from the user guide, Meshing through HELYX-OS, Comments of the senior members, Mesh decomposition, Johnson G., Visualization with ParaView R, The university of Texas At Austin, Texas Advanced Computing Center,

50

51 II Aerospace 2 Onera M6 Wing Geometry 2.2 ANSYS ICEM CFD 2.3 FLUENT R 2.4 Post Processing 2.5 Validation and Verification 2.6 Useful links

52

53 2. Onera M6 Wing 2.1 Geometry The geometry was prepared by Mateusz Gugala 1 in Unigraphics NX R. Thanks to him for sharing it. In addition, Mateusz Gugala has shared how he created the geometry in the aforementioned software, such as: 1. Download the airfoil data points of the tip and root of the Onera M6. 2. Import the root airfoil points into the CAD system. 3. Remove the trailing edge point, so that you end up having a blunt trailing edge as can be seen in this picture See problem () for further explanation as why doing this step is worth considering for a better mesh quality. 4. Do not close the blunt trailing edge now. 5. Repeat the second step for the tip by scaling the root. 6. Blend the tip with the root. 7. Close the blunt trailing edge. 8. Export the geometry file to a STEP format. 2.2 ANSYS ICEM CFD The geometry was imported into ICEM CFD as illustrated in figure 2.1. Then, I would suggest that you follow some steps (Starting the project steps and step 1 all) from the ANSYS ICEM CFD Tutorial Manual (15.0, November 2013) for the tetra/prism mesh in a fin configuration. You will find LMB and RMB these are the short hand for left and right mouse button respectively Mesh Generation Presented in this subsection the process of setting up the mesh parameters for the M6 case, as follows: 1 PhD student, School of Engineering and Material Science

54 54 Chapter 2. Onera M6 Wing Figure 2.1: Importing the M6 geometry into ICEM CFD. 1. Assuming that you did Step 1 from the ANSYS ICEM CFD Tutorial Manual arriving at a geometry as shown in figure 2.2, which did not have any tolerance problem (if there was any tolerance problem, then the edges would be coloured in blue or yellow, and the tolerance is kept to the minimum when repairing the geometry). 2. Click on the Mesh tab Global Mesh Setup. 3. Set the scale factor to 1 and the seed size to The global element seed size is large when compared to the Ansys tutorials. Because, this geometry was not scaled to meters but, rather left as mm which is the default scaling in most CAD packages. 4. Mesh type All Tri, mesh method Patch Dependent. 5. Volume meshing parameters tetra/mixed, tetra/mixed meshing Delaunay. 6. Under the Mesh tab, click on Part Mesh Setup. Maximum size specifies the maximum size of each cell in the selected area. For the far-field patches (i.e. top, ground, far-side, inlet and outlet); choose a high value which will result in a coarse, since there is not much information being transferred there other than the free-stream value and we are not interested in this,. For the Symmetry patch (i.e. patch where the wing is fixed); choose a value smaller than for the farfield by a factor of 1.2. For the Wing parts: Leading edge; choose a very small value (this should be 1.5k less than the value specified to the far-field). Trailing edge; choose a slightly higher value ( 10 times higher than for the leading edge). Tip; choose a slightly higher value than the leading edge ( 5 times greater). Upper and lower surfaces; double the value specified for the trailing edge. Roots; make it 50 times greater than the value specified for the leading edge. Tetra size ratio specifies to how much each cell can grow with respect to its neighbouring ones.

55 2.2 ANSYS ICEM CFD 55 A value of 1.2 was only specified to few patches, such as: Upper and lower wing surfaces (i.e. span). Symmetry plane. Tip. Height is the minimum thickness of the first prism layer. This can be specified using a y+ calculator or manually (as described in the case of the Ahmed model, see section or any y+ calculator found online, here is one Height ratio is the stretching ratio; which is the ratio of two adjacent boundary layers (further/nearer). This can be calculated automatically in ICEM CFD, as follows: Mesh setup Prism meshing parameters: Growth law exponential. Specify the rest. Then, click on compute params. Num layers specifies the number of boundary layers ( 10-12). Just for the wing parts, make sure to tick their prism boxes in the part mesh setup. Figure 2.2: The M6 geometry file passed all tolerance checks. Exporting the mesh from ICEM to.msh file to be able to import it in FLUENT R. 1. Click on output tab. Select solver Choose ANSYS FLUENT R from the drop down menu apply. Click on write input icon (from the output tab) and save. Exit ICEM CFD Meshing journey Attempt 2.1 Presented here, the very first mesh I generated in ICEM CFD for the m6. By looking at figure 2.3, the mistakes I did were: Fine computational domain. (It should be much coarser.) Created prism layers before having a smooth mesh. (Adding boundary layers should be the last step.) Coarse leading and trailing edge. (I should have clustered a bit more into the leading and trailing edges.) Poor prism layers at trailing edge. (the wing geometry has a sharp edge. For a good quality there should be a blunt edge. For a better quality, a rounded trailing edge instead.) Attempt 2.2 Presented here, the second mesh I created in ICEM CFD after receiving the feedback

56 56 Chapter 2. Onera M6 Wing Figure 2.3: First mesh generated in ICEM CFD; enclosure (top left), symmetrical+wing (top middle), wing (top right), wing+symm (bottom left), prism layers at leading and trailing edge (bottom middle and right respectively). from Dr. J-D. Müller and Mr. Mateusz Gugala. By looking at figure 2.5. The mistakes in this mesh are: Leading edge still coarse. (The number of points should be doubled there.) Farfield still fine. (I should have increased the maximum size of the cells there.) The area where the wing meets the symmetry should not be refined. (I should ve avoided drawing density lines in this region.) The centre of the wing should be more coarser. The rate to which the mesh is coarsened from the wing is high. (It should be lower.) Figure 2.4: Second mesh generated in ICEM CFD; enclosure (all top), wing+symm (bottom left), wing tip (bottom middle) and wing (bottom right).

57 2.2 ANSYS ICEM CFD 57 Figure 2.5: Second mesh generated in ICEM CFD; enclosure (all top), wing+symm (bottom left), wing tip (bottom middle) and wing (bottom right). Attempt 2.3 Presented here, the third mesh generated in ICEM CFD. Infer from figure 2.6, the mistakes are: Symmetry plane is slightly fine. (It should be more coarser though.) The growth rate of the cells near the aerofoil (at the symmetry plane) is still high. (The tetra size ratio should be in the range of ) Figure 2.6: Third mesh generated in ICEM CFD; far-side (top left), inlet (top middle), ground (top right), symmetry plane (bottom left), symm. near aerofoil (bottom middle) and wing (bottom right). Attempt 2.4 Presented here, the fourth mesh generated in ICEM CFD. Infer from figure 2.9, the mistakes are: High mesh growth rate at the wing. (It should be reduced so that the cells coarsens slowly towards the outer boundaries.)

58 58 Chapter 2. Onera M6 Wing The nibbled edge at the trailing edge of the wing. (The basic spacing of the nodes should be improved.) The leading edge is below that standard threshold in terms of the number of nodes. (The number of nodes should be doubled.) The size of elements at the wing surface are a bit higher than the standard threshold of the element size. (Decrease the size of elements by a factor of ) The growing ratio is still high at the wing surface patch. (Reduce the tetra size ratio to 1.2.) Trailing edge is coarse. (It should be refined by a factor of than the current scale.) Figure 2.7: Fourth mesh generated in ICEM CFD; far-field (top left), inlet (top middle), symmetry plane (top right), symm. near aerofoil (bottom left and middle) and wing (bottom right). Attempt 2.5 Presented here the fifth mesh generated in ICEM CFD; the feedback from Dr. J-D. Müller and Mr. Mateusz Gugala are as follows: The wing tip is still coarse. (It should be refined.) The growth rate should be adjusted. (Change the tetra size ratio to 1.2) Attempt 2.6 Presented here the sixth mesh generated and the final one which is shown in figure Figure 2.8: 5th mesh generated in ICEM.

59 2.3 FLUENT R 59 Figure 2.9: 6th mesh generated in ICEM; view from upper surface (left), view from trailing edge (right) Attempt 2.7 The final attempt is just the refined version of mesh 6 and is shown in figure It contains 776,741 cells and nodes. Figure 2.10: A fine mesh 2.3 FLUENT R Presented in this section, the procedure of setting the case for an Euler run Case Setup 1. Import the mesh generated in ICEM CFD into FLUENT R. File Read mesh. 2. Check your mesh quality. Mesh Check.