The second part of the tutorial continues with the subsequent ANSYS Mechanical simulation steps:

Transcription

1 Tutorial: Simulation of aero-vibro-acoustic phenomena using ANSYS Fluent and ANSYS Mechanical. Test case: Noise inside a cavity with a vibrating wall, caused by the external turbulent flow. Introduction This tutorial demonstrates the workflow of a combined usage of the CFD software ANSYS Fluent and the vibration and acoustics simulation tools of ANSYS Mechanical, in order to calculate the cabin noise caused by the turbulent flow outside of a vehicle. The ANSYS Mechanical solver computes the broad-band noise in the frequency domain, by performing the harmonic response analysis in a frequency sweep over the whole spectrum. The tutorial first demonstrates how to do the following using ANSYS Fluent: Prepare a 3D scale-resolving simulation of the separated turbulent flow past an obstacle. Set up the export of the wall pressure signals on the external side of a plate, which separates the flow domain and the enclosed acoustics domain. Perform the transient flow calculation. Compute the Fourier transform of the wall pressure signals, visualize its results in different frequency bands, and export fields of the complex Fourier amplitudes in the CGNS format. The second part of the tutorial continues with the subsequent ANSYS Mechanical simulation steps: Set up a harmonic response analysis in ANSYS Workbench. Define the acoustics properties of the air cavity using the ACT Acoustics extension. Import the structural plate mesh and map the real and imaginary components of the pressure from the CGNS files. Perform the frequency sweep vibro-acoustic analysis of the plate and the acoustic cavity from 20 to 500 Hz. Postprocess the plate deformations and the sound pressure levels at given locations in the acoustic cavity. Prerequisites This tutorial assumes that you are familiar with the ANSYS Fluent and Mechanical user interfaces and understand basic setup and solution procedures. Some steps will not be shown explicitly. In this tutorial you will use the Delayed DES (DDES) turbulence model. If you have not used this feature before, it is recommended that you read Chapter Detached Eddy Simulation (DES) of the Fluent 16.0 Theory Guide (as needed), and Section Setting Up DES with the SST k- Model of the Fluent 16.0 User s Guide.

2 In order to set up the vibro-acoustic harmonic analysis, you must first install the ACT Acoustics extension. For more information regarding the Application Customization Toolkit, refer to the ANSYS Workbench Application Customization Toolkit Developer's Guide. The extension can be downloaded from the Customer Portal using the following link: From the Workbench project page, use the Install Extension option of the Extensions menu to install the downloaded wbex file of the extension: Extensions Install Extension Note: Depending on the number of CPU cores used for the flow simulation, approximately 1 day is required to compute the results from the initialization. To learn the workflow, you can skip the DDES simulation and use the provided case, data, and pressure signal files (ASD files) for the remaining steps. Problem Description The problem considers turbulent air flow over a rectangular obstacle, which is mounted on a flat solid wall, as shown in Figure 1. The obstacle dimensions L x L y L z are 0.1 m 0.3 m 0.2 m.

3 U = 40 m/s Figure 1. Computational Domains for the Flow and the Vibro-Acoustic Simulations The inlet velocity of 40 m/s is applied with a block profile. Constant pressure is specified at the outlet boundary. The side planes and the top plane are the symmetry planes. A part of the wall downstream of the obstacle, which is shown in gray color in Figure 1., represents a 3mm-thick glass plate. This plate is firmly fixed along its contour and vibrates due to the flow pressure fluctuations. The vibration amplitude, however, is very small and does not influence the airflow above the plate. A rectangular closed cavity under the plate has the dimensions L x L y L z of 1 m 0.5 m 1 m and represents the vehicle cabin. Except for the upper glass plate, its other five walls are rigid. Two microphones are installed inside the cavity at its XY-symmetry plane, 25 cm below the plate at x=0.5 m and x=0.75 m, where x=0 corresponds to the beginning of the cavity. Setting Up and Performing the Flow Simulation This section explains how to set up and run a simulation of the time-dependent turbulent flow using ANSYS Fluent. If you are only interested in learning about the harmonic analysis of vibro-acoustics in

4 the cavity, you can skip this section and proceed with the next section Setting Up and Performing the Vibro-Acoustic Harmonic Response Analysis. The CGNS files, which are created at the end of this section and contain the spectrum fields of the flow pressure on the glass plate surface, are supplied with the tutorial materials (see files plate_pressure_spectrum.cgns and plate_pressure_spectrum_[1-5].cgns). These files are then imported by the ANSYS Mechanical software. Stage 1: Mesh In this stage, you will import a single-block hexahedral orthogonal mesh for the flow simulation. This mesh is supplied as an ASCII file in PATRAN Neutral format (mesh.out). You will use the Mark region tool to separate cells and create the obstacle. The same tool is then used to split the bottom boundary in the two parts, according to Figure 1. The result of Stage 1 is saved in the case file mesh.cas, which is provided with the tutorial materials. You have the option of skipping this stage and proceeding with Stage Copy the file mesh.out to your working directory. 2. Start the 3D double-precision version of Fluent. 3. Import the mesh file mesh.out, containing an orthogonal mesh of N x N y N z = = 432,000 hexahedral cells: File Import PATRAN Neutral 4. Check the mesh: Mesh Check Fluent will perform various checks on the mesh and will report the progress in the console. Verify that the flow domain extents are -0.5m<x<1m, 0<y<1m, -0.5m<z<0.5m, and the minimum cell volume as well as the minimum face area is positive. 5. Display the mesh to see the domain boundaries xmin, ymin, zmin from inside: Display Mesh Select xmin, ymin, zmin, as shown in Figure 2. Figure 3. depicts the imported mesh. This mesh does not yet have an obstacle, which is shown in Figure 1. and which is necessary to create a strongly turbulent separated flow. Also, the bottom boundary ymin must be split into two parts. The obstacle can be created using the Delete Cell Zone capability of Fluent. A zone to delete can be separated from the imported mesh by marking the appropriate cells using the Mark tool provided for the region adaption, as explained below.

5 Figure 2. Mesh Display Dialog Box 6. Mark a region to create the obstacle: Figure 3. Imported Mesh Adapt Region In the Region Adaption dialog box that opens, specify a hex-region: -0.1m<x<0, 0<y<0.3m, -0.1m<z<0.1m, as shown in Figure 4. Then click the Mark button.

6 Figure 4. Creating a Region for the Obstacle Note that the following message is displayed in the console: 6000 cells marked for refinement, 0 cells marked for coarsening Additional cells might have been marked because of the requirements of the adaption algorithms. 7. Separate the cell zone according to the marked region: Mesh Separate Cells In the Separate Cell Zones dialog box that opens (Figure 5.), select Mark from the Options list, as well as a register and a cell zone (there is only one register and one cell zone in this case). Then click the Separate button. Figure 5. Separate Cell Zones Dialog Box Figure 6. Delete Cell Zones Dialog Box The console reports on separating zone 1 into two zones, with 426,000 and 6,000 cells. It also provides information about the newly created face zones. Note the name of the new cell zone: solid-7:014.

7 8. Delete the cell zone, which corresponds to the obstacle: Mesh Zone Delete In the Delete Cell Zones dialog box that opens (Figure 6.), select the new cell zone and click the Delete button. 9. Mark a region to separate the ymin boundary into two parts along the line x=0 (see Figure 1.). Proceed as explained in step 6. above and mark a hex-region 0<x<1m, 0<y<1m, -0.5m<z<0.5m. 10. Separate face zone ymin using the region, which was created in the previous step: Mesh Separate Faces In the Separate Face Zones dialog box that opens (Figure 7.), select Mark from the Options list, as well as the second register and face zone ymin. Then click the Separate button. Figure 7. Separate Cell Zones Dialog Box Figure 8. Merge Zones Dialog Box 11. Merge the two parts of the obstacle boundary into one face zone for convenience: Mesh Merge In the Merge Zones dialog box that opens (Figure 8.), select zone type wall on the left and the appropriate zone names on the right. In case of uncertainty, display the mesh zones as done in step 5. Click the Merge button. The name of the combined zone will be displayed in the console. 12. Save the case file mesh.cas with the prepared mesh: File Write Case Stage 2: Initial RANS Calculation In this stage you will set up and start a short steady-state simulation with the RANS turbulence model, in order to develop the initial fields for the further scale-resolving transient simulation. The result of Stage 2 is saved in the case and data files rans.cas and rans.dat, which are provided with the tutorial materials. You have the option of skipping this stage and proceeding with Stage 3. The run time of the simulation in this stage is about 5 minutes on a single processor.

8 13. If you have skipped Stage 1 or have exited Fluent after Stage 1, then make sure that the file mesh.cas is in your working directory, start the 3D double-precision version of Fluent, and read the case file mesh.cas: File Read Case 14. Select the pressure-based solver for a steady flow simulation in the General task page. 15. In the Cell Zone Conditions task page, change the type of the single present cell zone from solid to fluid, and in the pop-up Fluid dialog box rename this zone from solid-7 to fluid. Make sure that air with constant properties (density of kg/m 3 and viscosity of kg/m/s) is selected as the zone material in the Fluid dialog box. The flow Mach number is slightly above 0.1, so the compressibility effects may be neglected. 16. In the Models task page, select the Viscous Laminar item in the models list and click the Edit button. In the Viscous Model dialog box that opens, select k-omega (2 eqn) and in the k-omega Model group box select SST. Leave the Energy model selector at Off. 17. Switch to the Boundary Conditions task page. Currently all face zones, except for default_interior-7, are of the type wall. Edit the boundary condition types according to the Problem Description section at the beginning of this document. Also change the face zone names for convenience. Use the display mesh tool Display Mesh when you are uncertain about the location of a particular face zone. Edit the face zone types and names according to the following list: Inlet plane (old name xmin ): Type = velocity-inlet; Zone Name = inlet; Momentum tab: Velocity Specification Method = Magnitude, Normal to Boundary; Velocity Magnitude = 40 m/s; Supersonic/Initial Gauge Pressure = 0 Pa; Turbulence group box: Specification Method = Intensity and Viscosity Ratio; Turbulent Intensity = 1%; Turbulent Viscosity Ratio = 10. Outlet plane (old name xmax ): Type = pressure-outlet; Zone Name = outlet; Momentum tab: Gauge Pressure = 0 Pa; Backflow Direction Specification Method = Normal to Boundary; Turbulence group box: Specification Method = Intensity and Viscosity Ratio; Turbulent Intensity = 1%; Turbulent Viscosity Ratio = 10. Left side plane (old name zmin ): Type = symmetry; Zone Name = left. Right side plane (old name zmax ): Type = symmetry; Zone Name = right. Top plane (old name ymax ): Type = symmetry; Zone Name = top. Obstacle surface (old name default_interiour-7:010 or similar): Type = wall; Zone Name = brick; Momentum tab: Wall Motion = Stationary Wall; Shear Condition = No Slip.

9 Bottom plane upstream of the obstacle (old name ymin ): Type = wall; Zone Name = wall; Momentum tab: stationary no-slip wall (same as above). Bottom plane downstream of the obstacle (old name ymin:017 or similar): Type = wall; Zone Name = plate; Momentum tab: stationary no-slip wall (same as above). 18. The Operating Conditions parameters, which are accessible from the Cell Zone Conditions and Boundary Conditions task pages via the button Operating Conditions, are to be left at the default state: Operating Pressure = Pa (1 atm), no gravity. 19. In the Reference Values task page, specify the reference values for the proper normalization of the lift and drag coefficients, as well as other possible outputs: Area = 0.06 m 2, Density = kg/m 3, Length = 0.2 m, Pressure = 1960 Pa, Velocity = 40 m/s, Viscosity = kg/m/s. 20. In the Solution Methods task page, select the following options: Pressure-Velocity Coupling group box: Scheme = Coupled; Spacial Discretization group box: Gradient = Green-Gauss Cell Based; Pressure = Linear; Momentum = Second Order Upwind; Turbulent Kinetic Energy = First Order Upwind; Specific Dissipation Rate = First Order Upwind; and leave all parameters in the Solution Controls task page at their default values. 21. Reorder the mesh: Mesh Reorder Domain To speed up the solution procedure, the mesh should be reordered, which will reduce the bandwidth and make the code run faster. >> Reordering domain using Reverse Cuthill-McKee method: zones, cells, faces, done. Bandwidth reduction = 4800/4200 = 1.14 Done. 22. In the Solution Initialization task page, select Standard Initialization from the Initialization Methods list, and then specify the following initial values: Gauge Pressure = 0 Pa, X Velocity = 40 m/s, Y Velocity = Z Velocity = 0 m/s, Turbulent Kinetic Energy = 0.24 m 2 /s 2, Specific Dissipation Rate = /s. Click the Initialize button. 23. Save the case file under the name rans.cas : File Write Case 24. In the Run Calculation task page, set the number of iterations equal to 50 and launch the calculation by clicking the Calculate button. This calculation takes 5 to 10 minutes on a single CPU and is not supposed to converge to a steady state, as a steady state does not exist for this

10 separated flow at the Reynolds number of half a million even with the RANS turbulence model. The purpose is simply to develop a better initialization for the following scale-resolving transient flow simulation. 25. After completion of the RANS calculation, save the case and the data files under the names rans.cas and rans.dat (the data file name is not requested, but generated automatically): File Write Case & Data Stage 3: Scale-Resolving Simulation of a Transient Flow In this stage you will set up and run a scale-resolving transient simulation using the DDES turbulence model. This simulation is performed in two runs. During the first 1000 time steps, the transient solution with the resolved turbulent vortices is being developed to a statistically established state. After that, the transient statistics and the transient export of the wall pressure are activated, and the DDES calculation is continued for the further 9000 time steps. The overall calculation time is around 5 hours on a 16-core machine. The result of Stage 3 is saved in the case and data files ddes cas and ddes dat, as well as in the transient wall pressure files plate.index and plate1000.asd-plate9001.asd, which are provided with the tutorial materials. You have the option of skipping this stage and proceeding with Stage 4 to learn the Fourier postprocessing. 26. If you have skipped Stage 2, then copy the files rans.cas and rans.dat to your working directory. If you continue from Stage 2, then restart Fluent on a multi-processor machine. The files, which are provided with this test case, have been computed on a 16-core machine using 14 mesh partitions. Start the 3D double-precision parallel version of Fluent, and read the case and data files rans.cas and rans.dat: File Read Case & Data 27. In the General task page, select Transient from the Time list. 28. In the Models task page, edit the Viscous model. Change it from k-omega to Detached Eddy Simulation (DES), and select the RANS Model SST k-omega. Activate the DES Option Delayed DES, and select the Shielding Function DDES. 29. In the Solution Methods task page, select the following options: Non-Iterative Time Advancement method; Pressure-Velocity Coupling group box: Scheme = Fractional Step; Spacial Discretization group box: Gradient = Green-Gauss Cell Based; Pressure = Linear; Momentum = Bounded Central Differencing; Turbulent Kinetic Energy = First Order Upwind; Specific Dissipation Rate = First Order Upwind; Transient Formulation : Second Order Implicit;

11 and leave the under-relaxation factors in the Solution Controls task page at their default values. 30. In the Monitors task page, create the drag and lift force monitors. For both force monitors select the wall zone brick, activate the Print to Console, Plot, and Write options. Specify the file names cd-history.out and cl-history.out, as well as the Force Vector components {X=1, Y=Z=0} and {Y=1, X=Z=0} for the drag and the lift monitor, respectively. Using the Surface Monitors tool in the Monitors task page creates several wall pressure monitors in the separated zone behind the obstacle. In the provided files, the four monitors are located at x=0.1 m, x=0.2 m, x=0.5 m, and x=0.9 m along the symmetry line z=0 of the plate boundary. Enable the Print to Console, Plot, and Write options with X Axis = Flow Time, Get Data Every 1 Time Step, Average Over (Time Steps) = 1, Report Type = Vertex Average, Field Variable = Static Pressure. Use the New Surface tool in this dialog box to create points. 31. In the Calculation Activities task page, specify Autosave Every (Time Steps) = 500. Click the Edit button, and in the Autosave dialog box that opens select Each Time from the Save Associated Case Files list, enable the Retain Only the Most Recent Files option with Maximum Number of Data Files = 1, and specify the File Name = ddes. 32. In the Run Calculations task page, specify the Time Step Size = 0.25e-3, which results in a Courant number of around one or less throughout most of the domain. 33. Save the case and the data files under the names ddes.cas and ddes.dat. 34. In the Run Calculations task page, specify Number of Time Steps = 1000 and start the calculation by clicking the Calculate button. This calculation will develop resolved turbulent vortices and prepare a statistically established transient solution. On a 16-core machine it takes about 30 minutes. 35. In the Models task page, select Acoustics and click the Edit button. In the Acoustics Model dialog box that opens, enable the Export Acoustic Source Data in ASD Format option, as shown in Figure 9., left. The abbreviation ASD stands for Acoustic Source Data. Figure 9. Acoustics Model Dialog Box and Acoustic Sources Dialog Box

12 This ASD export feature was originally implemented to store the transient fields of variables, which are necessary to compute the acoustic sources for the Ffowcs Williams Hawkings integral method (pressure on walls; pressure, velocity, and density on permeable surfaces). The same feature is naturally suited to store the transient distribution of pressure on the selected wall zones for the following Fourier postprocessing. To select the wall zones, click the Define Sources button. In the Acoustic Sources dialog box that opens, select the plate zone in the Source Zones list, as shown in Figure 9., right. Specify the Source Data Root File Name as plate or any other name, set the Write Frequency to 1 to store each time step, and set the Number of Time Steps per File to With these settings, each ASD file exported for this case will have a size of about 37 MB; this information is output to the Fluent console after your click the Apply button. 36. In the Run Calculation task page, select the option Data Sampling for Time Statistics with the Sampling Interval = 1. Click the Sampling Options button and make sure that the Flow Shear Stresses and the Wall Statistics options are enabled. 37. Save the case and the data files under the names ddes-developed.cas and ddesdeveloped.dat. These files are also supplied with the tutorial materials. 38. Continue the transient simulation for another 9000 steps with the activated transient export of the wall pressure to the ASD files and time statistics. This run of Fluent takes approximately 5 hours on a 16-core machine. Fluent will store the final simulation state in the case and data files ddes cas and ddes dat. These files are also provided with the tutorial materials. Stage 4: Fourier Postprocessing of the Wall Pressure Field and Export of the Wall Pressure Spectra to CGNS Files for ANSYS Mechanical In this stage, you will perform the Fourier postprocessing of the exported transient wall pressure files using the FFT tool of Fluent. The resulting fields of the complex Fourier amplitudes will be exported to the CGNS files for ANSYS Mechanical. These CGNS files are provided with the tutorial materials, so you have the option of skipping this stage and proceeding with the next section Setting Up and Performing the Vibro-Acoustic Harmonic Response Analysis. 39. If you have skipped Stage 3, then copy the files ddes cas and ddes dat, as well as the transient wall pressure files plate.index and plate1000.asd-plate9001.asd, to your working directory. The Fourier postprocessing for this small case does not necessarily need a multi-processor machine and can be performed in serial. The data file is not required for the Fourier postprocessing of the wall pressure field, because the input pressure signals for FFT are read from the ASD files. However, you can use the results from the data file for the visualization of the turbulent flow around the obstacle. Start the 3D double-precision version of Fluent, and either read the case and data files ddes cas and ddes dat, or read the case file ddes cas alone and then perform the initialization to enable the contour plotting in Fluent: File Read Case & Data

13 or, if you only wish to postprocess the wall pressure histories from the ASD files: File Read Case and then Solve Initialization and with the selected initialization method Standard Initialization and arbitrary initial values click the Initialize button. 40. Since the FFT of wall pressure fields is a beta-feature in ANSYS Fluent 16.0, enable beta feature access by typing the following command in the Fluent console: > define beta-feature-access yes yes 41. In the Run Calculation task page, click the Acoustic Sources FFT button. A Acoustic Sources FFT dialog box opens (Figure 10.), with the four tabs Read ASD Files Compute FFT Fields Write CGNS Files FFT Surface Variables 42. Begin with the first tab Read ASD Files, which is shown in Figure 10. In the Active Source Zones selection list, select the face zone plate, which is the only zone in the current case, where the transient export of wall pressure has been performed. In the Source Data Files selection list, select all available ASD files. Click the Read button. The console output informs you about the read data: Overall 9000 timesteps have been read

14 Figure 10. Acoustic Source FFT Dialog Box 43. Change to the Compute FFT Fields tab, Figure 11. Values shown in the middle Spectral Resolution group box inform you about the statistical properties, which depend on the sampling rate (simulation time step) and the signal length (simulation time). These values will change if you enable the Clip Time to Range option in the left Sampling Data group box, reduce the signals by omitting certain time at the beginning or at the end or both (entry fields Min and Max ), and click the Re-Estimate Spectral Resolution button. The right upper selection list allows you to specify a window function using the same choices that are offered to plot the single signal FFT under the Plots task page. For our current purpose, use the full signals and the Hanning window, which are the standard settings. Click the Compute button to start the FFT calculation, which in this small case takes only several seconds. 44. After the two previous obligatory steps, you can write the computed fields of the complex Fourier amplitudes in the CGNS binary files (using the Write CGNS Files tab), and/or create spectral surface variables to visualize them in Fluent (using the FFT Surface Variables tab). The computed fields of the Fourier spectra are stored in a big memory array denoted here as the storage area. This memory is allocated by Fluent dynamically when you read the pressure signals from the ASD files (see step 42. above). If you read data for all face zones available in the ASD files, and if they are the wall zones, then the size of the allocated storage area is equal to the total size of the ASD files being read. Since the same or a slightly less amount of data is produced by FFT, the same storage area is re-used to store the Fourier spectra. So the Fourier spectra displaces the original time signals in memory, which are not kept after the FFT has been computed. Therefore, if you wish to re-compute FFT using the Clip Time to Range tool or a different window function (both in the Compute FFT Fields tab, step 43. above), you have first to de-allocate the storage area by clicking the Clean up storage area button at the bottom left part of the dialog box, and then re-read the pressure histories from the ASD files. De-allocation of

15 the potentially very large storage area is also recommended, when you complete your use of the Acoustic Sources FFT tool and either proceed to the other postprocessing work or continue your transient simulation without re-starting Fluent. Figure 11. Compute FFT Fields Tab 45. Change to the Write CGNS Files tab (Figure 12.). Figure 12. Write CCGNS Files Tab

16 Here you select in the Processed Source Zones list the desired zones for the CGNS export (only one zone plate exists in this case). You can reduce the exported spectrum data using the Reduce Frequency Series option and specifying the frequency range (minimum and maximum frequencies), as well as the frequency step (in the Number of Frequencies to Skip integer field). The latter must be used with care, and only if really needed, because the Fourier amplitudes in the broadband noise spectrum depend on the frequency resolution. By skipping frequencies from the exported spectrum (i.e., exporting every other Fourier mode), you will artificially coarsen the frequency resolution. However, the exported amplitudes will not be automatically re-scaled for the increased frequency step, but will retain their originally computed values. Pressure spectra, which result from the scale-resolving flow simulations, may contain thousands of frequencies. Together with the dense surface meshes, this can result in a very large amount of data to export. The total size of the disk space required to store fields of the complete spectra is approximately equal to the total size of the ASD files containing the wall pressure histories. Therefore, the wall pressure spectra are written to a series of CGNS files according to the Number of Frequencies per File field. It is recommended to select an appropriate value for this field to avoid extremely large output files, as well as a high number of very small files. The total number of frequencies in the spectrum can be seen in the Compute FFT Fields tab as Number of Modes (see Figure 11.). For the current case, specify 1000 frequencies per file. Finally, you can specify a root name for the exported CGNS files in the Fourier Transform File Name Root field. If you, for example, select the root name plate_pressure_spectrum, as suggested in Figure 12., then after clicking the Write button Fluent will create in your working directory the following set of files: plate_pressure_spectrum.cgns plate_pressure_spectrum_1.cgns plate_pressure_spectrum_2.cgns plate_pressure_spectrum_3.cgns plate_pressure_spectrum_4.cgns plate_pressure_spectrum_5.cgns plate_pressure_spectrum.flst 5.0 MB 74.1 MB 74.1 MB 74.1 MB 74.1 MB 21.6 MB 78.0 KB If you leave the root name field empty, the files will be called cgns, 1.cgns,, 5.cgns, flst. The first CGNS file without a number in its name contains the mesh data, as well as the links to all the other CGNS files, which in turn contain the spectrum fields with 1000 modes per file. The CGNS links work like the file links in the UNIX file system: in order to import spectra in ANSYS Mechanical, you have to specify only the name of the first file. All other files will be imported automatically if they reside in the same directory. The file with the extension flst is an ASCII file, which contains the list of the exported frequencies for your information. 46. Change to the FFT Surface Variables tab (Figure 13). Here you can create new Fluent variables using the computed spectrum fields, which reside in the storage area. These variables will be defined only on those wall face zones, where the Fourier transformation has been computed. On the other face zones they will show zero values. Created variables can be used for any kind of further postprocessing in Fluent, typically for the contour plotting or for the export to CFD-Post.

17 Figure 13. FFT Surface Variables Tab Variables may either characterize the individual Fourier modes (select Set of Modes in the Modes/Frequency Bands drop-down list), or the frequency bands, each representing a range of frequencies (other choices in the drop-down list). The three types of frequency bands available in Fluent 16.0 are: Octave Bands proportional bands corresponding to the standard technical octaves 1/3 Octave Bands proportional bands corresponding to the standard technical thirds Constant Width Bands user-defined equidistant bands The Spectrum Property drop-down list shows the type of variables created according to the selected choice in the Modes/Frequency Bands drop-down list. For a set of modes, the created variables are the real and the imaginary parts of the complex Fourier amplitudes, one pair of variables per specified mode. For the frequency bands, the created variables are the surface pressure level (SPL) fields in decibels. The transformation to the decibel units is done by default, using the standard acoustic reference pressure value of Pa. This value can be changed by going to the Models task page and editing the acoustics model. If you select the Ffowcs- Williams & Hawkings model before creating the variables, you will be able to change the reference acoustic pressure at the right bottom part of the Acoustics Model dialog box. The currently allowed number of variables allows you to simultaneously keep SPL for all octave and octave third bands, as well as SPL for up to 20 constant width bands and the real and imaginary amplitudes for up to 20 individual frequencies. The SPL variables for the octave and the octave thirds include the band central frequency in their names (for example SPL for Octave Band at 250Hz (db) or SPL for 1/3-Octave Band at 1.25kHz (db) ). As for the user-defined frequencies and constant width bands, their variables are simply numbered from 0 to 19. In order to provide you with the information about the meaning of each such variable, Fluent

18 outputs a table in the console. For example, if you select Modes/Frequency Bands = Set of Modes and order the following set of frequencies in the input entries, as shown in Figure 14.: Frequency Min = 40 Hz, Frequency Max = 800 Hz, Number of Modes to Skip = 20, then the created variables will be called Pressure Spectrum Re 0, Pressure Spectrum Im 0, Pressure Spectrum Re 1, Pressure Spectrum Im 1, Pressure Spectrum Re 19, Pressure Spectrum Im 19, and the console output will be: Creating variables for 20 modes from Hz to Hz every Hz. f( 0) = Hz f( 1) = Hz f( 2) = Hz f( 3) = Hz f( 4) = Hz f( 5) = Hz f( 6) = Hz f( 7) = Hz f( 8) = Hz f( 9) = Hz f(10) = Hz f(11) = Hz f(12) = Hz f(13) = Hz f(14) = Hz f(15) = Hz f(16) = Hz f(17) = Hz f(18) = Hz f(19) = Hz Variables for frequencies above Hz are not created, because the limit of 20 modes has been reached. You can analyze more than 20 individual modes or constant width bands, if you process them by portions of 20 items and delete the processed variables by selecting them in the Existing Variables selection list and clicking the Remove Selected Variables button (see Figure 14.). Clicking the Clean up Storage Area button on the left side of the dialog box not only deallocates the spectrum storage array, but also removes all created variables.

19 Figure 14. Creating and Removing Variables for a Set of Individual Modes 47. Create and visualize different surface variables to see the footprints of the turbulent vortices in the different frequency ranges. In the sufficiently resolved spectrum, the band SPL are invariant with respect to the processed sampling time, which is not true for the complex Fourier amplitudes of the individual Fourier modes in the broadband spectrum. Therefore, the band SPL values are more appropriate for the comparison with the reference data (see SPL for the different octaves in Figures 15. and 16.). As to the individual Fourier modes, their amplitudes allow you see the required surface mesh resolution for ANSYS Mechanical (see the pattern at 500 Hz in Figure 17.).

20 Figure 15. Contours of SPL for the Octave at 16 Hz, db Units Figure 16. Contours of SPL for the Octave at 2 khz, db Units

21 Figure 17. Contours of the Real Part of the Fourier Amplitude at 500 Hz, Pa Units Setting Up and Performing the Vibro-Acoustic Harmonic Response Analysis This section covers the vibro-acoustic harmonic response of the plate and the acoustic cavity. The geometry containing the plate and the acoustic cavity (named Cabin.agdb) is provided in ANSYS DesignModeler format. The CGNS files plate_pressure_spectrum.cgns and plate_pressure_spectrum_[1-5].cgns exported from Fluent (as described previously in step 45.) will be imported and used as a load to excite the plate over the frequency range of interest (20 to 500 Hz). Stage 1: ACT Acoustics Extension Loading Before starting the setup of the frequency sweep harmonic analysis, it is required to load the ACT Acoustics extension, which will be used for the definition of the acoustic cavity properties and the import of the CGNS files. For more information related to the Act Acoustics extension, please refer to the training lectures provided along with the extension when you download it. 48. Start a new Workbench session. From the Workbench project page Extensions menu, select the Manage Extensions option: Extensions Manage Extensions

22 A dialog box will open displaying all of the ACT extensions available for this session. Check the box corresponding to the Acoustics extension to load it for the current Workbench session. Figure 18. Extensions Manager Dialog Box If you don t see the Acoustics extension in the displayed list, it means it has not been installed yet. In that case go to the Install Extension option available in the Extensions project page menu to install the wbex file of the extension: Extensions Install Extension Stage 2: Glass Material Properties Definition Before opening the Mechanical application, the material properties of the glass will be defined in the Engineering Data module (the properties of the acoustic cavity will be defined later in Mechanical). 49. In the Workbench project page, select a Harmonic Response system and double-click it to insert it in the project schematic: Figure 19. Workbench Project Page Schematic 50. Double-click the Engineering Data cell of the created system to enter in the material properties definition module. In the Outline of Schematic dialog box, choose Click here to add a new material and name it Glass :

23 Figure 20. Outline of Schematic Engineering Data Dialog Box 51. In the Toolbox dialog box, select the Density property of the Physical Properties submenu, drag and drop it on the Glass material. Repeat these steps for the Isotropic Elasticity property of Linear Elastic submenu. The inserted material properties are displayed in the Properties of Outline pane: Figure 21. Glass Material Properties Definition 52. Define the following material properties values for the Glass material in the Properties of Outline pane: Density: 2500 kg m^-3 Young s Modulus: MPa Poisson s Ratio: Close the Engineering Data tab to return to the project schematic: Figure 22. Closing the Engineering Data Tab

24 Stage 3: Mesh During this step the Cabin.agdb geometry file will be imported, then the plate and the acoustic cavity will be meshed using the Mechanical application. The geometry consists of a multibody part, containing the plate and the acoustic cavity made of several bodies, so a single conformal mesh will be generated. 54. Right-click on the geometry cell of the created system, select Import Geometry, and browse to select the Cabin.agdb geometry file: Figure 23. Importing the Geometry File 55. Right-click on the Model cell, and select the Edit option to open the Mechanical application: Figure 24. Opening the Mechanical Application 56. As can be seen in Figure 17., the plate mesh must be fine enough to properly capture the pressure distribution that is going to be mapped from the CGNS files onto the structural mesh. The pressure mapping process will retrieve the CFD pressure values at each frequency and will map them on surface elements created on the top side of the plate. One pressure value will thus be applied per surface element facet, so to reduce the number of nodes of the model you will use linear elements (without midside nodes). To that end, select Mesh in the tree outline. In the Advanced submenu of the Details view, drop the midside nodes: Mesh Advanced Element Midside Nodes Dropped

25 Figure 25. Dropping Element Midside Nodes 57. Because the plate is modeled as a thin solid body here, it will be meshed with Solid Shell elements (SOLSH190 elements) well suited for thin to moderate thick shells. To that end, select Mesh in the tree outline; right-click it to insert a Method : Mesh RMB>Insert Method Select the plate body and define the following properties: Method: Sweep Src/Trg Selection: Automatic Thin Free Face Mesh Type: All Quad Element Option: Solid Shell Figure 26. The Sweep Method for Meshing the Plate with Solid Shell Elements 58. To control the mesh refinement of the plate, you will insert edge sizing controls on the plate top face edges. Right-click Mesh and insert a first Sizing object: Mesh RMB>Insert Sizing

26 Select the plate top face edges aligned with Z axis and located at x=0 m and x=1 m, and set the following options: Type: number of Divisions Number of Divisions: 60 Behavior: Hard Bias Type: No Bias Figure 27. Edge Divisions along the Z Axis Insert another Sizing object to control the plate divisions along the X axis. Because the CFD mesh (and therefore the pressure being mapped) is finer at x=0 m than at x=1 m, you will also use a progressive expansion of the mesh along the X axis. Select the plate top face edges located at z=-0.5 m and z=0.5 m and aligned with X axis and set the following options: Type: number of Divisions Number of Divisions: 80 Behavior: Hard Bias Type: Bias Factor: 5 You will see the expansion direction isn t properly defined because the two edges don t have the same orientation as illustrated in Figure 28.:

27 Figure 28. Improper Expansion Direction To switch the expansion direction of the edge located at z=0.5 m, edit the Reverse Bias property and select this last edge. Then for both edges, smaller elements are requested at x=0 m than x=1 m: Figure 29. Proper Expansion Direction 59. The plate is rectangular, so it can easily be meshed with mapped elements. To do this, right-click Mesh, insert a Face Meshing object, and select the top face of the plate: Mesh RMB>Insert Face Meshing

28 60. You now need to insert mesh objects to control the mesh refinement of the acoustic cavity. When using an acoustic element, it is recommended that you use 12 linear elements per wave length. You thus need to ensure this criterion is satisfied for the highest frequency of interest (500 Hz). Because the speed of sound in air is equal to 343 m.s -1, we can then identify the maximum acoustic element size: You will therefore use an element size of 0.05 m. e = λ 12 = c f 12 = = 0.057m To that end, right-click Mesh and insert a Sizing object, select the eight acoustic bodies located at the bottom of the cavity (the buffer body between those eight and the plate will be used to create the mesh transition between the fine plate mesh and the coarser acoustic elements) and input the following properties: Type: Element Size Element Size: 5e-2 m Behavior: Hard Figure 30. Acoustic Bodies Sizing 61. In order to ensure that the mesh transition between the plate and the acoustic bodies at the bottom of the cavity is meshed with a maximum of hexahedrons elements, you will use a Hex Dominant method. Right-click Mesh, insert a Method, select the upper acoustic body of the air cavity, and use the following settings: Method: Hex Dominant Element Midside Nodes: Use Global Setting Free Face Mesh Type: Quad/Tri

29 Figure 31. Hex Dominant Method 62. You can now generate the mesh by right-clicking the Mesh tree object and selecting Generate Mesh : Mesh RMB>Generate Mesh The generated mesh contains approximatively nodes. Figure 32. Vibro-Acoustic Mesh

30 Stage 4: Harmonic Response Setup 63. The analysis settings of the harmonic response will now be defined to specify the frequency range and the solution method. To do so, select the Analysis Settings object in the tree outline and set the following settings in the Options submenu: Range Minimum: 20 Hz Range Maximum: 500 Hz Solution Method: Full Figure 33. Analysis Settings The Full resolution method is chosen here because this is currently the only resolution method supported to import and map the CFD pressure from the CGNS files. It is also worth noting that the Frequency Spacing and Solution Intervals values aren t important here, because they will be ignored during the resolution. Indeed, when CGNS files are imported, the solver performs the resolution for all frequencies between the Range Minimum and the Range Maximum contained in those files (1030 frequencies). However, for an easier postprocessing it is recommended that you use a Solution Intervals value that is equal or higher than the number of frequencies to be resolved. 64. The model is going to be resolved for an important number of frequencies, so decrease the size of the generated solution files by selecting the Output Controls submenu of the Analysis Settings and choosing the following options: Stress: No Strain: No Nodal Forces: No General Miscellaneous: Yes (this is required if you want to be able to postprocess the mapped CFD pressure, otherwise set the value to No) Figure 34. Output Controls

31 65. Introduce the damping of the glass by selecting the Damping Controls submenu of the Analysis Settings and specifying a Constant Damping Ratio of 0.01: Figure 35. Damping Controls 66. You will now request the saving of the solver database, in order to postprocess the sound pressure level at the microphones locations after the resolution. Select the Analysis Data Management submenu of Analysis Settings, and set Save MAPDL db to Yes: Figure 36. Analysis Data Management 67. You now need to define the properties of the acoustic air cavity. To that end, right-click the Harmonic Response tree object and insert an Acoustic Body. You can also insert it from the Acoustics toolbar. Note that if the toolbar isn t available, it means the ACT Acoustics extension hasn t been installed, so you will need to return to the Prerequisites section. After inserting the Acoustic Body, select the nine acoustic bodies of the cavity and use the following properties: Mass Density: kg.m -3 Sound Speed: m.s -1 Acoustic-Structural Coupled Body Options: Coupled With Symmetric Algorithm

32 Figure 37. Acoustic Body Properties Note the default mass density and sound speed values are used. The Acoustic-Structural Coupled Body Options allows you to specify that you are performing a vibroacoustic analysis: the interaction of the fluid and the structure at a mesh interface causes the acoustic pressure to apply a force to the structure, and the structural motions produce an effective fluid load. For more information regarding strongly coupled vibro-acoustic analysis, see the Acoustics Analysis Guide section of the Mechanical APDL documentation (help/ans_acous/ans_acous.html). 68. The four sides of the plate are considered fixed, so right-click the Harmonic response analysis and insert a Displacement support. Select the four lateral side faces of the plate and set a value of 0 for all displacement components: Figure 38. Displacement Support 69. The last step of the setup consists of importing the CFD CGNS files, so that you can map the pressure on the top face of the plate. To that end, right-click the Harmonic response analysis

33 and insert a CFD Pressure mapping object. It can also be inserted from the Tools menu of the Acoustics toolbar. Then select the top face of the plate and select the plate_pressure_spectrum.cgns file (the other parameters are left to the default values): Figure 39. CFD Pressure Mapping 70. The analysis can now be resolved by clicking the Solve upper toolbar button. If needed, you can modify the resolution properties (Number of cores, GPU acceleration) beforehand in the Solve Process Settings dialog box, accessible from Tools menu. For more information, see the Understanding Solving section of the Mechanical User s Guide (help/wb_sim/ds_using_solve_handlers.html): Tools Solve Process Settings Advanced Note: The elapsed time of the resolution is dependent on the solve process settings and the hardware configuration used. 71. When the resolution is finished, you can right-click the Solution tree object to insert a Deformation result scoped on the plate body to postprocess the displacement of the plate at a given frequency: Figure 40. Plate Deformation at 20 Hz, mm Units

34 Figure 41. Plate Deformation at 500 Hz, mm Units 72. It is also possible to use the same procedure to insert a Fluent Mapped Pressure displaying the resulting mapped pressure, to ensure the plate mesh was fine enough to capture the pressure distribution properly: Figure 42. Mapped Pressure at 20 Hz, Pa Units Figure 43. Mapped Pressure at 500 Hz, Pa Units

35 73. Finally, you can insert two Acoustic Time_Frequency Plot objects to display the sound pressure level function of the frequency at x=0.5, y=-0.25, z=0 (using named selection Microphone1 ) and at x=0.75, y=-0.25, z=0 (using named selection Microphone2 ): Figure 44. Microphones SPL Results Figure 45. SPL at Microphone1, db Units

36 Figure 46. SPL at Microphone2, db Units Note: The acoustic sound pressure level is calculated as follows (p ref = 2e-5 Pa): L SPL 2 2 p preal p rms 10log 10log 2 2 p ref 2 pref 2 imag ( db)