Advanced ANSYS FLUENT Acoustics

Workshop Modeling Flow-Induced (Aeroacoustic) Noise 14.5 Release Advanced ANSYS FLUENT Acoustics 2011 ANSYS, Inc. November 7, 2012 1

Introduction This tutorial demonstrates how to model 2D turbulent flow across a circular cylinder using large eddy simulation (LES) and compute flow-induced (aeroacoustic) noise using ANSYS FLUENT's acoustics model. This tutorial demonstrates how to do the following: Perform a 2D large eddy simulation Set parameters for an aeroacoustic calculation Save acoustic source data for an acoustic calculation Calculate acoustic pressure signals. Postprocess aeroacoustic results. 2011 ANSYS, Inc. November 7, 2012 2

Prerequisites This tutorial assumes that you are familiar with the ANSYS FLUENT interface and that you have a good understanding of basic setup and solution procedures. Some steps will not be shown explicitly. In this tutorial you will use the acoustics model. If you have not used this feature before, first read: Chapter 15, Aerodynamically Generated Noise, of the ANSYS FLUENT 14.5 Theory Guide, and Chapter 23, Predicting Aerodynamically Generated Noise, of the ANSYS FLUENT 14.5 User's Guide Note: Approximately 2.5 hours of CPU time is required to complete this tutorial. If you are interested exclusively in learning how to set up the acoustics model, you can reduce the computing time requirements considerably by starting at Step 9 and using the provided case and data files. 2011 ANSYS, Inc. November 7, 2012 3

Problem Description The problem considers turbulent air flow over a 2D circular cylinder at a free stream velocity (U) of 69.2 m/s. The cylinder diameter (D) is 1.9 cm. The Reynolds number based on the diameter is 90,000. The computational domain (Figure 1) extends 5D upstream and 20D downstream of the cylinder. U = 69.2 m/s D = 1.9 cm Figure 1. Computational domain 2011 ANSYS, Inc. November 7, 2012 4

Preparation 1. Copy the file cylinder2d.msh.gz to your working directory 2. Start the 2D double-precision version of ANSYS FLUENT 14.5 2011 ANSYS, Inc. November 7, 2012 5

Step 1: Mesh 1. Read the mesh file cylinder2d.msh.gz File Read Mesh As FLUENT reads the mesh file, it will report its progress in the console window. Since the mesh for this tutorial was created in meters, there is no need to rescale the mesh. Check that the domain extends in the x-direction from -0.095 m to 0.38 m. 2. Check the mesh Mesh Check FLUENT will perform various checks on the mesh and report the progress in the console window. Pay particular attention to the reported minimum volume. Make sure this is a positive number. 3. Reorder the mesh Mesh Reorder Domain To speed up the solution procedure, the mesh should be reordered, which will substantially reduce the bandwidth and make the code run faster. FLUENT will report its progress in the console window: Reordering domain using Reverse Cuthill-McKee method: zones, cells, faces, done. Bandwidth reduction = 32634/252 = 129.50 Done. 2011 ANSYS, Inc. November 7, 2012 6

Step 1: Mesh (continued) 4. Display the mesh Results Graphic and Animation Mesh Set Up... 2011 ANSYS, Inc. November 7, 2012 7

Step 1: Mesh (continued) (a) Display the grid with the default settings (Figure 2) Use the middle mouse button to zoom in on the image so you can see the mesh near the cylinder (Figure 3) Figure 2. Mesh Display Figure 3. Mesh around the cylinder Quadrilateral cells are used for this LES simulation because they generate less numerical diffusion than triangular cells. The cell size should be small enough to capture the relevant turbulence length scales, and to make the numerical diffusion smaller than the subgrid-scale turbulence viscosity. The mesh for this tutorial has been kept coarse in order to speed up the calculations. A high quality LES simulation will require a finer mesh near the cylinder wall. 2011 ANSYS, Inc. November 7, 2012 8

Step 2: Models 1. Select the pressure-based transient solver Problem Setup General 2011 ANSYS, Inc. November 7, 2012 9

Step 2: Models (continued) 2. Select the LES turbulence model The LES turbulence model is not available by default for 2D calculations. It can be made available in the GUI by typing the following command in the console window: (rpsetvar 'les-2d? #t) Problem Setup Models Viscous (a) Select Large Eddy Simulation under Model (b) Retain the default option of Smagorinsky-Lilly under Subgrid-Scale Model (c) Retain the default value of 0.1 for the model constant Cs (d) Click OK You will see a Warning dialog box, stating that Bounded Central-Differencing is default for momentum with LES/DES. Click OK The LES turbulence model is recommended for aeroacoustic simulations because LES resolves all eddies with scales larger than the grid scale. Therefore, wide band aeroacoustic noise can be predicted using LES simulations. 2011 ANSYS, Inc. November 7, 2012 10

Step 3: Materials Setup and Solution You will use the default material, air, which is the working fluid in this problem. The default properties will be used for this simulation. Problem Setup Materials Fluid Air 1. Retain the default value of 1.225 for Density 2. Retain the default value of 1.7894e-05 for Viscosity You can modify the fluid properties for air or copy another material from the database if needed. For details, refer to the Chapter 8, Physical Properties, in the ANSYS FLUENT 14.5 User's Guide. 2011 ANSYS, Inc. November 7, 2012 11

Step 4: Cell Zone Conditions Problem Setup Cell Zone Conditions 1. Select fluid 2. Click Edit... to open the Fluid panel. i. Retain the default selection of air as the fluid ii. material in the Material Name drop-down list Click OK 3. Click Operating Conditions... to open the Operating Conditions panel Retain the default value of 101325 Pa for the Operating Pressure 2011 ANSYS, Inc. November 7, 2012 12

Step 5: Boundary Conditions Problem Setup Boundary Conditions 1. Set the boundary conditions at the inlet a) Select inlet under Boundary Conditions The Type will be reported as velocity-inlet b) Click Edit... to open the Velocity Inlet panel i. Set the Velocity Magnitude to 69.2 m/s ii. Retain the default No Perturbations in the Fluctuating Velocity Algorithm drop-down list, and click OK This tutorial does not make use of FLUENT's ability to impose inlet perturbations at velocity inlets when using LES. It is assumes all unsteadiness is due to the presence of the cylinder in the flow. 2. Set the boundary conditions at the outlet a) Select outlet under Boundary Conditions The Type will be reported as pressure-outlet b) Click Edit... to open the Pressure outlet panel i. Confirm that the Gauge Pressure is set to 0. ii. Retain the default option of Normal to Boundary in the Backflow Direction Specification Method drop-down list, and click OK The top and bottom boundaries are set to symmetry boundaries. No user input is required for this boundary type. 2011 ANSYS, Inc. November 7, 2012 13

Step 6: Solution Methods Solution Solution Methods 1. Retain default Least Squares Cell Based under Gradient 2. Select PRESTO! under Pressure discretization PRESTO! is a more accurate scheme for interpolating face pressure values from cell pressures 3. Retain default Bounded Central Differencing under Momentum For LES calculations on unstructured meshes, the Bounded Central Differencing scheme is recommended for Momentum. 4. Select Second Order Implicit under Transient Formulation 5. Check Non-Iterative Time Advancement option 6. Select Fractional Step Method as Pressure-Velocity Coupling scheme 2011 ANSYS, Inc. November 7, 2012 14

Step 7: Solution Controls Solution Solution Controls 1. Set the Relaxation Factor for Pressure to 0.7 2. Retain the default Relaxation Factor of 1.0 for Momentum The pressure field is relaxed only during the initial transient phase. The Relaxation Factor for Pressure will be increased to 1 at a later stage. 3. Click on Advanced... and go to Expert tab. This will show Non-Iterative Solver Controls Panel. Retain default values. 2011 ANSYS, Inc. November 7, 2012 15

Step 8: Quasi-Stationary Flow Field Solution Before extracting the source data for the acoustic analysis, a quasi-stationary flow needs to be established. The quasi-stationary state will be judged by monitoring the lift and drag forces. 1. Initialize the solution Solution Solution Initialization (a) Initialize the flow from the inlet conditions by selecting inlet in Compute From dropdown list. (b) Click Initialize to initialize the solution 2. Enable the plotting of residuals Solution Monitors Residuals Edit... (a) Select Plot under Options (b) Enter 10000 under Iterations to Store (c) Enter 20 for Iterations under Iterations to Plot (d) Retain the default values for the other parameters and click OK 2011 ANSYS, Inc. November 7, 2012 16

Step 8: Quasi-Stationary Flow Field Solution (continued) 3. Set the time step parameters Solution Run Calculation Set the Time Step Size (s) to 5e-6 The time step size required in LES calculations is governed by the time scale of the smallest resolved eddies. That requires the local Courant-Friedrichs-Lewy (CFL) number to be of an order of 1. It is generally difficult to know the proper time step size at the beginning of a simulation. Therefore, an adjustment is often necessary after the flow is established. For a given time step Dt, the highest frequency that the acoustic analysis can produce is f = 1/(2Dt). For the time step size selected here, the maximum frequency is 100kHz. Typically in most aeroacoustic calculations, the maximum frequency obtained from the analysis is higher than the audible range of interest. 2011 ANSYS, Inc. November 7, 2012 17

Step 8: Quasi-Stationary Flow Field Solution (continued) 4. Save the case and data files: cylinder2d t0.00.cas.gz and cylinder2d t0.00.dat.gz File Write Case & Data... Save the case and data files before the first iteration. This will save you time in the event of user error or code divergence, where the case file would have to be set up all over again 5. Run the case for a few time steps before activating the force monitors Solution Run Calculation (a) Set the Number of Time Steps to 20 (b) Click Calculate The residual history will be displayed as the calculation proceeds. When the noniterative time advancement scheme is used, by default, two residuals are plotted per time step. 2011 ANSYS, Inc. November 7, 2012 18

Step 8: Quasi-Stationary Flow Field Solution (continued) 6. Enable the monitoring of the lift and drag forces: Setting the force monitors after some initial transient state limits the range of the drag coefficient when starting from an impulse initial condition. Solution Monitors (a) Select Drag, and click Edit... (b) Select wall_cylinder in the Wall Zones list (c) Verify that the X and Y values under Force Vector are 1 and 0, respectively. (d) Select Plot under Options to enable plotting of the drag coefficient (e) Select Write under Options to save the monitor history to a file; cd-history will be the default file name Note: If you do not select the Write option, the history information will be lost when you exit FLUENT (f) Click OK 2011 ANSYS, Inc. November 7, 2012 19

Step 8: Quasi-Stationary Flow Field Solution (continued) 6. Enable the monitoring of the lift and drag forces (continued): Solution Monitors (g) Select Lift, and click Edit... (h) Select wall_cylinder in the Wall Zones list (i) Verify that the X and Y values under Force Vector are 0 and 1, respectively (j) Select Plot under Options to enable plotting of the lift coefficient (k) Select Write under Options to save the monitor history to a file; cl-history will be the default file name (l) Click OK 2011 ANSYS, Inc. November 7, 2012 20

Step 8: Quasi-Stationary Flow Field Solution (continued) 7. Set the reference values to be used in the lift and drag coefficient calculation Problem Setup Reference Values (a) Set the values as listed below: Area = 0.019 Velocity = 69.2 Length = 0.019 (b) Retain the default values for the other parameters The reference area is calculated using the cylinder diameter, D, and the default depth of 1 m for 2D problems. Adjust the reference area if a different depth (Depth) value is used. For the actual force coefficient calculation, only the reference area, density and velocity are needed. The reference length (Length) will be needed later for the Strouhal number calculation. 2011 ANSYS, Inc. November 7, 2012 21

Step 8: Quasi-Stationary Flow Field Solution (continued) 8. Overwrite the previously saved initial conditions: cylinder2d t0.00.cas.gz and cylinder2d t0.00.dat.gz File Write Case & Data... 9. Advance the flow in time until a quasi-stationary state is reached Solution Run Calculation (a) Set the Number of Time Steps to 4000 (b) Click Calculate The 4000 time steps will advance the flow up to t=0.02 s. At that time the bulk flow will cross the computational domain about three times. The residual history, lift and drag force histories will be displayed as the calculation proceeds. The lift and drag histories should be similar to those in Figure 4 and Figure 5, respectively. Differences in the long-term flow evolution can occur due to operating system dependent round-off errors. Once the lift and drag histories are sufficiently oscillatory and periodic in nature, you are ready to set up the acoustics model and perform the acoustic calculations. 2011 ANSYS, Inc. November 7, 2012 22

Step 8: Quasi-Stationary Flow Field Solution (continued) Figure 4. Lift coefficient history Figure 5. Drag coefficient history 2011 ANSYS, Inc. November 7, 2012 23

Step 8: Quasi-Stationary Flow Field Solution (continued) 10.Verify that the selected time step size is reasonable for the given mesh and flow condition: Results Plots Histogram Set Up... (a) Select Velocity... under Histogram of (b) Select Cell Courant Number from the Velocity... category (c) Set the value for Divisions to 100 (d) Click Plot and verify that the peak CFL value is less than 3.5. The histogram (Figure 6) shows that most cells have a Cell Courant Number of less than 1 Figure 6. Histogram displaying the range of the CFL number 11. Save the case and data files: cylinder2d t0.02.cas.gz and cylinder2d t0.02.dat.gz File Write Case & Data... 2011 ANSYS, Inc. November 7, 2012 24

Step 9: Aeroacoustics Calculation 1. Define the acoustics model settings: Problem Setup Models Acoustics Edit... (a) Select Ffowcs-Williams & Hawkings under Model (b) Select Export Acoustic Source Data in ASD Format under Options 2011 ANSYS, Inc. November 7, 2012 25

Step 9: Aeroacoustics Calculation (continued): (c) Click Define Sources... button to open the Acoustic Sources panel i. Select wall_cylinder under Source Zones All relevant acoustic source data (i.e. pressure) will be extracted from the wall cylinder surface ii. Enter cylinder2d in the text-entry box for Source Data Root Filename This is the filename root of the index file which will be created. The index file contains information about the source data files that are created when you run the case. The index file is automatically created with a.index file extension 2011 ANSYS, Inc. November 7, 2012 26

Step 9: Aeroacoustics Calculation (continued): (c) iii. Enter 2 under Write Frequency Depending on the physical time step size and important flow time scales, it is not necessary to write the acoustic source data at every time step. In this tutorial, the source data is coarsened (in time) by a factor of two. Thus, the highest possible frequency the acoustic analysis can generate is reduced to f = 1/[2(2Dt)] =50 khz iv. Set Number of Time Steps Per File to 200 The source data can be conveniently segmented into multiple source data files. This makes it easier to process partial sequences when calculating the receiver signals. A value of 200 for Number of Time Steps Per File means that each source data file covers a time span of 200 time steps. With Write Frequency of 2, there are 100 data sets written into each source data file v. Click Apply and Close Click OK to close Acoustics Model panel 2011 ANSYS, Inc. November 7, 2012 27

Step 9: Aeroacoustics Calculation (continued) 2. Modify the solution controls: Solution Solution Controls Increase the Relaxation Factor for Pressure to 1 3. Resume the calculation Solution Run Calculation (a) Retain the Number of Time Steps at 4000 (b) Click Calculate The additional 4000 time steps will advance the flow up to t=0.04 s At every second time step, a message will be displayed in the console window informing you that data is written to a source data file (.asd file extension) 4. Save the case and data files: cylinder2d t0.04.cas.gz and cylinder2d t0.04.dat.gz File Write Case & Data... 2011 ANSYS, Inc. November 7, 2012 28

Step 9: Aeroacoustics Calculation (continued) 5. Set the acoustics model constants Problem Setup Models Acoustics (a) Retain Far-Field Density at 1.225 kg/m3 The far-field density is the density of the fluid outside the computational domain, i.e. the density of the fluid near the receivers. In most calculations it is the same as the density within the computational domain. (b) Use the default value of 340 m/s for Far-Field Sound Speed (c) Retain Reference Acoustic Pressure at 2e-05 Pa The reference acoustic pressure is used to calculate decibel values during postprocessing (d) Set the Source Correlation Length to 0.095 m. It is equal to five cylinder diameters The source correlation length is very important when performing aeroacoustic calculations in 2D. FLUENT assumes that sound sources are perfectly correlated over the specified correlation length, and zero outside. It internally builds a source volume with a depth equal to the specified correlation length and neglects sources outside. In your practical 2D application, you will have to estimate the source correlation length; your obtained sound pressure levels will depend on your input. That makes it difficult to rely on 2D calculations to obtain absolute sound pressure levels. Therefore, you should use aeroacoustic 2D simulations primarily to observe trends. The source correlation length is not needed for 3D calculations. (e) Click OK to close the panel 2011 ANSYS, Inc. November 7, 2012 29

Step 9: Aeroacoustics Calculation (continued) 6. Calculate the acoustic signals Solution Run Calculations Acoustic Signals... (a) Click the Receivers... button to open the Acoustic Receivers panel Note that you can open the Acoustic Receivers panel also from the Acoustics Model and Acoustic Sources panels 2011 ANSYS, Inc. November 7, 2012 30

Step 9: Aeroacoustics Calculation (continued) i. Increase Number of Receivers to 2. ii. For the receiver-1 coordinates, enter 0 m for X-Coord., -0.665 m (35D) for Y-Coord., and 0 for Z- Coord. iii. For the receiver-2 coordinates, enter 0 m for X-Coord., -2.432 m (128D) for Y-Coord., and 0 for Z- Coord. iv. Retain the defaults for Signal File Name (receiver-1.ard and receiver-2.ard) v. Click OK to close the Acoustic Receivers panel 2011 ANSYS, Inc. November 7, 2012 31

Step 9: Aeroacoustics Calculation (continued) (b) Select wall_cylinder under Active Source Zones All source zones which were selected in the Acoustic Sources panel are now available under the Active Source Zones. In this tutorial, the sound sources are extracted from only one zone. It is important to select the source zones consistently if redundant source zones were selected in the Acoustic Sources panel (c) Select all files available under Source Data Files Selecting a subset of the available source files is a convenient way to analyze shorter sequences. It is important to select a continuous set of source data files (d) Select the two available receivers, under Receivers As soon as the source zones, source data files, and receivers are selected, the Compute/Write function becomes available. (e) Click Compute/Write Console window will confirm that the source data files are being read and that the receiver signals are computed and written into receiver files (f) Click Close to close the Acoustic Signals panel 2011 ANSYS, Inc. November 7, 2012 32

Step 10: Aeroacoustic Postprocessing 1. Display the acoustic pressure signals at the two receiver locations: Results Plots File (a) Click Add... in the File XY Plot panel This will open the Select File panel where you can now select receiver-1.ard and receiver- 2.ard from the file list (b) Click OK to close the Select File panel 2011 ANSYS, Inc. November 7, 2012 33

Step 10: Aeroacoustic Postprocessing (continued) (c) Click Plot to display the receiver signals (Figure 7). Modify the line and marker styles as necessary, using the Curves panel You will notice a shift in time of approximately 5e-3 s for the signal at the second receiver. Receiver-2 is farther away from the source surface and the sound will therefore arrive later. Also notice that the signal at receiver-2 is weaker due to the increased distance and geometrical attenuation. Figure 7. Acoustic pressure signals 2011 ANSYS, Inc. November 7, 2012 34

Step 10: Aeroacoustic Postprocessing (continued) 2. Perform a spectral analysis of the receiver signals: Results Plots FFT (a) Select Process Receiver under Process Options to activate the Receiver list If the Ffowcs Williams and Hawkings (FW-H) acoustics model is used and the receiver signals have been calculated, then the signals are directly available for postprocessing. As an alternative, the receiver data can be loaded manually from files by using Process File Data option under Process Options (b) Select receiver-1 from the Receiver list (c) Select Sound Pressure Level (db) from the Y Axis Function drop-down list (d) Select Frequency (Hz) from the X Axis Function drop-down list 2011 ANSYS, Inc. November 7, 2012 35

Step 10: Aeroacoustic Postprocessing (continued) (e) Click Plot FFT to plot the sound pressure spectrum for receiver-1 (Figure 8) The overall sound pressure level (OASPL) is printed to the console window: Overall Sound Pressure Level in db (reference pressure = 2.000000e-005) = 1.133193e+002 Note: The maximum frequency plotted is f = 1/[2(2Dt)] = 50 khz, as expected. Figure 8. Spectral analysis of pressure signal for receiver-1 2011 ANSYS, Inc. November 7, 2012 36

Step 10: Aeroacoustic Postprocessing (continued) (f) Click Axes... This will open the Axes - Fourier Transform panel i. Deselect Auto Range for the X Axis ii. Manually set the Maximum for Range to 5000 iii. Click Apply and Close the panel 2011 ANSYS, Inc. November 7, 2012 37

Step 10: Aeroacoustic Postprocessing (continued) (g) Replot the sound pressure spectrum for receiver-1 (Figure 9). The spectrum peaks at about 900 Hz Note: The spectral resolution is only about 50 Hz, since the receiver signal was calculated for a short period only (approximately 0.02 s). For a sampled signal of length T, the spectral resolution is 1/T. You may increase the spectral resolution by running the simulation longer in time before recalculating the receiver signals Figure 9. Spectral analysis of pressure signal for receiver-1 at a reduced frequency range 2011 ANSYS, Inc. November 7, 2012 38

Step 10: Aeroacoustic Postprocessing (continued) (h) Select the Strouhal Number from the X Axis Function drop-down list Reset the Maximum for the x-axis Range to 1 in the Axes - Fourier Transform panel (i) (j) Replot the sound pressure spectrum as a function of the Strouhal Number. The spectrum peaks at a Strouhal Number of about 0.25 (Figure 10) If the Strouhal number calculation does not seem correct, verify that the correct values are specified in the Reference Values panel Repeat the spectral analysis for receiver-2 by selecting receiver-2 from the Receiver list. You should expect an OASPL of about 102 db for receiver-2 Figure 10. Spectral analysis of pressure signal for receiver-1 as a function of Strouhal number 2011 ANSYS, Inc. November 7, 2012 39

Step 10: Aeroacoustic Postprocessing (continued) 3. Plot the power spectral density of the lift force history to see that the observed peaks in the receiver spectrum match the dominant frequency in the lift force history: Results Plots FFT (a) Select Process File Data under Process Options (b) Click Load Input File... and select the lift monitor file (cl-history) (c) Select Power Spectral Density from the Y Axis Function drop-down list (d) Select Strouhal Number from the X Axis Function drop-down list (e) Verify that the Maximum for the x-axis Range in the Axes - Fourier Transform panel is 1 (f) Click Plot/Modify Input Signal... to open the Plot/Modify Input Signal panel. It lets you modify and plot the signal before the Fourier Transform is applied i. Select Clip to Range and set the Min value for X Axis Range to 0.02 Without clipping the temporal range, the complete lift monitor history would be analyzed including the initial transient state leading up to the quasistationary state ii. Click Apply/Plot and Close to return to the Fourier Transform panel 2011 ANSYS, Inc. November 7, 2012 40

Step 10: Aeroacoustic Postprocessing (continued) Since the x-axis range was manually set for the spectral plot, you will not see the proper range when plotting the modified signal. You will need to temporarily reset the range if you want to plot the input signal 2011 ANSYS, Inc. November 7, 2012 41

Step 10: Aeroacoustic Postprocessing (continued) (g) Click Plot FFT to plot the power spectral density for the lift monitor history (Figure 11). The spectrum peaks at a Strouhal number of about 0.25 As indicated in Step 7, 2D aeroacoustic predictions depend strongly on the selected source correlation length. As a consequence, the results can be fine-tuned to be in better agreement with experimental data. Table 1 compares the obtained OASPL values with experimental values reported by Revell et al [1]. Reasonable agreement is found for the correlation length of 5D. Table 1: Dependence of predicted OASPL on specified source correlation lengths (L = 2.5D, 5D, 10D) 2.5D 5D 10D Experiment Figure 11. Spectral analysis of lift force history receiver-1 107.3 113.3 119.3 117 receiver-2 96.0 102.0 108.0 100 2011 ANSYS, Inc. November 7, 2012 42

Summary This tutorial demonstrated the use of ANSYS FLUENT's acoustics model to calculate the far-field sound signals generated by the flow over a 2D cylinder. You have learned how to set up the relevant parameters, save the acoustic source data, calculate, and postprocess the acoustic pressure signals. The main computational efforts are spent calculating the time dependent turbulent flow. It is therefore advisable to export the sound sources during the flow calculation. This allows you to recalculate the acoustic signals for different receivers or model parameters with minimal computational costs. The tutorial demonstrated the use of the Ffowcs Williams and Hawkings acoustics tool on a 2D case. You have seen that it is difficult to obtain absolute SPL predictions in 2D due to the need to estimate the correlation length of the turbulent flow structures in the spanwise direction. This difficulty does not exist when solving 3D acoustics problems. 2011 ANSYS, Inc. November 7, 2012 43

References [1] Revell, J.D., Prydz, R.A., and Hays, A.P., Experimental Study of Airframe Noise vs. Drag Relationship for Circular Cylinders, Lockheed Report 28074, Feb. 1977. Final Report for NASA Contract NAS1-14403. 2011 ANSYS, Inc. November 7, 2012 44