Fluid Dynamics Software Lab. Flow past an airfoil

Transcription

1 Second Summer School on Embodied Intelligence Simulation and Modelling within Embodied Intelligence 27 June - 1 July 2011, Zürich, Switzerland Dr Asimina Kazakidi Foundation for Research and Technology Hellas (FORTH) Heraklion 70013, Crete, Greece kazakidi@ics.forth.gr URL: June 2011

2 Abstract This Software Lab aims to introduce computational fluid dynamic techniques, through the use of the open-source numerical code Open- FOAM ( the open-source visualization software ParaView ( and the data plotting software Gnuplot (www. gnuplot.info). For this purpose, the flow past an airfoil is considered, as a standard study for the aerodynamic design of aircrafts. An analysis of the influence of the flow incidence angle (angle of attack) on the lift force coefficient will give an appreciation of the aircraft stall (terminology explained in the document), which can be relevant to the design of efficient robotic systems and robotic control strategies. 1 Introduction Studying the flow past an airfoil, particularly for a prototype, is critical in the aerodynamic design of aircrafts. The shape of the airfoil, the boundary conditions, and the drag and lift forces generated on the airfoil are important in identifying the performance characteristics of the airfoil during flight. Similar principles can be applied to hydrofoils (artificially-made in boats or naturallyfound in aquatic animals). 1.1 Problem description Consider fluid flowing past an airfoil (Fig.1). The free stream velocity, V, is 26 m/sec and the angle of attack, α, is initially 0 o. The chord length (C) is 1 m (Fig.2). The density, ρ, is 1 kg/m 3 and the kinematic viscosity, ν, is 1 5 m 2 /sec. Visualize case with ParaView. Set boundary conditions and solver parameters. Run with OpenFOAM solver for α=0 o and analyze. Rotate mesh and solve for other angles of attack. Examine the drag and lift force coefficients vs. α. Which is the critical angle of attack for this airfoil?? Figure 1: Angle of attack and forces acting on an airfoil 2

3 1.2 Forces acting on an airfoil Drag: in the direction of the free stream velocity (Fig.1). Lift: perpendicular to the direction of the free stream velocity (Fig.1). Thrust: force generated through the reaction of accelerating a mass of fluid, in the opposite direction from the accelerated fluid. Weight: the force on an object due to gravity. 1.3 Terminology Airfoil: the cross-sectional shape of an aircraft wing. Aircraft stall: a reduction in the lift coefficient as angle of attack increases. Angle of attack (or flow incidence angle), α: the angle between the free stream velocity and the chord line of the airfoil (Fig.1). Critical angle of attack: the angle of attack which produces maximum lift coefficient. Leading Edge Upper Camber Mean Camber Trailing Edge Lower Camber Chord "C" Figure 2: Terminology used for airfoils 2 Pre-processing 2.1 Inspect mesh with ParaView - Open a Terminal window - Change to the airfoil directory cd Desktop/CFDLab/airfoil/ - Copy the entire airfoil 00 case directory into a new case directory, named airfoil ** (where ** is a numerical value for the angle of attack you will examine) cp -rf airfoil 00/ airfoil **/ - Change to the airfoil ** case directory cd airfoil **/ ls It is always a good practice to view the mesh before running the case for any errors. The mesh can be viewed in ParaView, the post-processing tool supplied 3

4 with OpenFOAM. It is started by typing from within the case directory, in the terminal, the command: parafoam ParaView has opened the airfoil **.OpenFOAM. - Select the Patch Names and all the Mesh Parts in the bottom left side of the GUI windown, leaving the Volume Fields empty - Click the Apply button to load the geometry into ParaView - At the top of the GUI window, press on the arrow adjacent to Outline and choose Surface With Edges - Zoom, Pan, and Rotate the geometry to see the airfoil and the boundaries (check default or change mouse functions from Edit > Settings > Render View > Camera; you can also change the Background Color to white from Edit > Settings > Colors) What type of mesh is used for this geometry? What is the size and shape of the computational domain? What type of boundaries are used and how are they labeled? Quadrilateral cells are used here because they can be stretched easily to account for different flow gradient magnitudes in different directions. A half-circle was chosen to represent the upstream (inlet) boundary because it has no discontinuities in slope, enabling the construction of a smooth mesh in the interior of the domain. The upstream boundary was placed away from the airfoil to minimize effects on the flow and therefore have more accurate boundary condition. - Note the names for the boundaries and close ParaView, or otherwise, go back to the Terminal window and press Ctrl+Z, then write bg to keep ParaView open in the background 2.2 Rotate mesh by α - Within the airfoil ** case directory, rotate the mesh by α degrees transformpoints -yawpitchroll ( α 0 0) - Inspect the rotated mesh with parafoam (like before) 2.3 Set boundary and initial conditions - Change to folder 0/ - Move the file p0 to p, and U0 to U mv p0 p mv U0 U 4

5 - In a text editor (emacs, gedit, vi etc), open the file U - Between the brackets for the boundaryfield add the velocity conditions for each of the domain boundaries as follows: 23 inlet1 24 { 25 type freestream; 26 freestreamvalue uniform (26 0 0); 27 } inlet2 30 { 31 type freestream; 32 freestreamvalue uniform (26 0 0); 33 } outlet 36 { 37 type freestream; 38 freestreamvalue uniform (26 0 0); 39 } airfoil 42 { 43 type fixedvalue; 44 value uniform (0 0 0); 45 } frontandbackplanes 48 { 49 type empty; 50 } - Save and close the U file - In a text editor (emacs, gedit, vi etc), open the file p - Between the brackets for the boundaryfield add the pressure conditions for each of the domain boundaries: 23 inlet1 24 { 25 type freestreampressure; 26 } inlet2 29 { 30 type freestreampressure; 31 } outlet 34 { 5

6 35 type freestreampressure; 36 } airfoil 39 { 40 type zerogradient; 41 } frontandbackplanes 44 { 45 type empty; 46 } - Save and close the p file - Change to folder system/ of the case directory - Open the file controldict and set the following solver parameters: 26 endtime 50; 27 deltat 1; 32 writeinterval 10; - Add the following Reference Values at the end of the controldict file (this is to calculate the drag, lift and moment force coefficients acting on the airfoil) 49 functions 50 { forces 51 { 52 type forcecoeffs; 53 functionobjectlibs ( libforces.so ); 54 outputcontrol timestep; 55 outputinterval 1; 56 //Patches to sample 57 patches 58 ( 59 airfoil 60 ); 61 //Name of fields 62 pname p; 63 UName U; 64 rhoname rhoinf; 65 //Dump to file 66 log true; 67 //Reference density of fluid 68 rhoinf 1; 69 //(Centre of Rotation) Origin for moment calculations 70 CofR ( ); 71 //Direction for lift 72 liftdir (0 1 0); 73 //Direction for drag 74 dragdir (1 0 0); 6

7 75 //Pitching moment axis 76 pitchaxis ( 0 0 1); 77 //Free stream velocity magnitude 78 maguinf 26; 79 //Reference length 80 lref 1; 81 //Reference area 82 Aref 1; 83 } 84 } - Save and close the controldict file 3 Processing 3.1 Run the case - Change back to the main folder of the case airfoil ** Which OpenFOAM solver should you run for this case? - Check the name of the solver in the application field of the controldict file in the system folder more system/controldict - Ctrl+C - Run the solver simplefoam 3.2 Check solution convergence - Open Gnuplot gnuplot - Plot the lift force coefficient plot./forces/0/forcecoeffs.dat using 1:3 w l Is the solution converged? It is crucial to ensure convergence of the numerical solution to the exact solution. The time evolution of the drag, lift, and moment coefficients can give such information. Initially, the values of the force coefficients will fluctuate, as a result of the fluctuation of the numerical solution. It is safe to say the solution has converged when the force coefficients have also converged and show a sustained behavior, e.g. reach a constant value, be periodic etc. However, these coefficients are defined globally and their convergence may not apply to all points of the domain; some points may be more likely to have greater variation 7

8 and need to be specified individually. - Exit gnuplot exit 3.3 Re-run the case - Open the controldict file in the system directory and set the endtime value to 500 (i.e. for longer time) - Re-run the case with simplefoam - Check solution convergence with Gnuplot (like before) Is the solution converged? 4 Post-processing 4.1 Visualize results - Open parafoam and load the case by selecting all the Mesh Parts and Volume Fields - Select Surface instead of Outline at the top of the GUI window - Pan and zoom on the airfoil and from the top-right of the GUI deselect Show Center - At the left side of the GUI, press Refresh Times - From top-left of the GUI, press the arrow adjacent to Solid Color and select p - From the top-far-left, turn the Color Legend visible - Press the adjacent button to edit the Color Map. Press Choose Preset and select HSV from Blue to Red. Press OK, Make Default, Close. - From the top-center of the GUI, press Play. - Change the field to U, then back to p again and press Play What are the pressure and velocity distributions around the airfoil? - Activate the Stream Tracer icon (eight button from the left, at the fourth row of options, or else from Filters > Alphabetical > Stream Tracer) - Slide the bar down in the Object Inspector field and under at the Seed Type replace Point Source with Line Source - Choose the following Point Point Resolution 21 - Press Apply - Select with the mouse the airfoil **.OpenFOAM in the Pipeline Browser - Activate the Slice icon (fourth button from the left, at the fourth row of options, or else from Filters > Alphabetical > Slice) and choose 8

9 Origin Normal Press Apply What is the streamline pattern around the airfoil? What is the pressure and velocity distribution? 4.2 Find the lift coefficient value - Close ParaView - Read the force coefficient file from the forcecoeffs.dat file within the forces/0/ directory What is the value of the lift force coefficient for this angle of attack? You need to get the converged mean value of the lift coefficient (the last value could do for this Lab, since variance is small). 4.3 Find the critical angle of attack - Create a file lift.dat (e.g. emacs lift.dat) and write in a column the angles of attack studied during this Lab (α from 0 o to 20 o degrees, by 2 o ) - Next to the value of α that you examined, add the value you found for the lift force coefficient - Fill the values of C L for the rest of α examined by the other groups during this Lab. E.g. for 0 o, C L is 0.369: Save, close the file and open Gnuplot - Plot the file you just created plot./lift.dat w l Which is the critical angle of attack for this airfoil?? 5 Conclusions In this Software Lab, the OpenFOAM, ParaView and Gnuplot open-source software were used to introduce some aspects of computational fluid dynamic analysis. The flow past an airfoil was considered and the influence of the angle of attack on the lift force coefficient was determined. This analysis may be relevant to identifying the performance characteristics of robotic systems and improving their design and control strategies. Further reading G.K. Batchelor, An Introduction to Fluid Dynamics, Cambridge University Press; D.J. Tritton, Physical Fluid Dynamics, Oxford University Press;