Tutorial:Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
Introduction
This tutorial demonstrates how to model2D turbulent?ow across a circular cylinder using large eddy simulation(LES)and compute?ow-induced(aeroacoustic)noise using FLUENT’s acoustics model.
You will learn how to:
?Perform a2D large eddy simulation.
?Set parameters for an aeroacoustic calculation.
?Save acoustic source data for an acoustic calculation.
?Calculate acoustic pressure signals.
?Postprocess aeroacoustic results.
Prerequisites
This tutorial assumes that you are familiar with the 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,?rst read Chapter21,Predicting Aerodynamically Generated Noise,of the FLUENT6.2 User’s Guide
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
Problem Description
The problem considers turbulent air?ow over a2D circular cylinder at a free stream ve-locity(U)of69.2m/s.The cylinder diameter(D)is1.9cm.The Reynolds number based on the diameter is90,000.The computational domain(Figure1)extends5D upstream and 20D downstream of the cylinder.
U = 69.2 m/s D = 1.9 cm
Figure1:Computational Domain
Preparation
1.Copy the?le cylinder2d.msh to your working directory.
2.Start the2D version of FLUENT.
Approximately2.5hours 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 Step7and using the provided case and data?les.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT Step1:Grid
1.Read the grid?le cylinder2d.msh.
File?→Read?→Case...
As FLUENT reads the grid?le,it will report its progress in the console window.
Since the grid for this tutorial was created in meters,there is no need to rescale the grid.Check that the domain extends in the x-direction from-0.095m to0.38m.
2.Check the grid.
Grid?→Check
FLUENT will perform various checks on the mesh and will 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 grid.
Grid?→Reorder?→Domain
To speed up the solution procedure,the mesh should be reordered,which will substan-tially 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=32634/253=128.99
Done.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
4.Display the grid.
Display?→Grid...
(a)Display the grid with the default settings(Figure2).
Use the middle mouse button to zoom in on the image so you can see the mesh
near the cylinder(Figure3).
Figure2:Grid Display
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
Figure3:The Grid Around the Cylinder
Quadrilateral cells are used for this LES simulation because they generate less numerical di?usion than triangular cells.The cell size should be small enough to capture the relevant turbulence length scales,and to make the numerical di?usion 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?ner mesh near the cylinder wall.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT Step2:Models
1.Select the segregated solver with second-order implicit unsteady formulation.
De?ne?→Models?→Solver...
(a)Retain the default selection of Segregated under Solver.
(b)Under Time,select Unsteady.
(c)Under Transient Controls,select Non-Iterative Time Advancement.
(d)Under Unsteady Formulation,select2nd-Order Implicit.
(e)Under Gradient Option,select Node-Based.
(f)Click OK.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
2.Select the LES turbulence model.
The LES turbulence model is not available by default for2D calculations.You can make it available in the GUI by typing the following command in the FLUENT console window:
(rpsetvar’les-2d?#t)
De?ne?→Models?→Viscous...
(a)Under Model,select Large Eddy Simulation.
(b)Retain the default option of Smagorinsky-Lilly under Subgrid-Scale Model.
(c)Retain the default value of0.1for the model constant Cs.
(d)Click OK.
You will see a Warning dialog box,stating that Bounded Central-Di?erencing 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 aeroa-coustic noise can be predicted using LES simulations.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
Step3:Materials
You will use the default material,air,which is the working?uid in this problem.The default properties will be used for this simulation.
De?ne?→Materials...
1.Retain the default value of1.225for Density.
2.Retain the default value of1.7894e-05for Viscosity.
You can modify the?uid properties for air or copy another material from the database if needed.For details,refer the chapter Physical Poperties in the FLUENT User’s Guide.
Step4:Operating Conditions
De?ne?→Operating Conditions...
1.Retain the default value of101325Pa for the Operating Pressure.
Step5:Boundary Conditions
1.Retain the default conditions for the?uid.
De?ne?→Boundary Conditions...
(a)Under Zone,select?uid.
The Type will be reported as?uid.
(b)Click Set...to open the Fluid panel.
i.Retain the default selection of air as the?uid material in the Material Name
drop-down list.
ii.Click OK.
2.Set the boundary conditions at the inlet.
(a)Under Zone,select inlet.
The Type will be reported as velocity-inlet
(b)Click Set...to open the Velocity Inlet panel.
i.Set the Velocity Magnitude to69.2m/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 pertur-
bations at velocity inlets when using LES.It is assumed that all unsteadiness
is due to the presence of the cylinder in the?ow.
Modeling Flow-Induced (Aeroacoustic)Noise Problems Using FLUENT
3.Set the boundary conditions at the outlet.
(a)Under Zone ,select outlet .
The Type will be reported as pressure-outlet
(b)Click Set...to open the Pressure Outlet panel.
i.Con?rm that the Gauge Pressure is set to 0.
ii.Retain the default option of Normal to Boundary in the Back?ow Direction
Speci?cation 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.
Step 6:Quasi-Stationary Flow Field Solution
Before extracting the source data for the acoustic analysis,a quasi-stationary ?ow needs to be established.The quasi-stationary state will be judged by monitoring the lift and drag forces.
1.Set the solution controls.
Solve ?→Controls ?→Solution...
(a)Retain the default PISO scheme for Pressure-Velocity Coupling .
(b)Under Discretization ,select PRESTO!in the Pressure drop-down list.
PRESTO!is a more accurate scheme for interpolating face pressure values from
cell pressures.
准稳态
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
(c)Retain the default Bounded Central Di?erencing for Momentum.
For LES calculations on unstructured meshes,the Bounded Central Di?erencing
scheme is recommended for Momentum.
(d)Set the Relaxation Factor for Pressure to0.75.
(e)Retain the default Relaxation Factor for Momentum.
The pressure?eld is relaxed only during the initial transient phase.The Relax-
ation Factor for Pressure will be increased to1at a later stage.
(f)Click OK.
2.Initialize the solution.
Solve?→Initialize?→Initialize...
(a)Initialize the?ow from the inlet conditions by selecting inlet in the Compute From
drop-down list.
(b)Click Init to initialize the solution and click Close.
3.Enable the plotting of residuals.
Solve?→Monitors?→Residual...
(a)Select Plot under Options.
(b)Under Storage,enter10000Iterations.
(c)Under Plotting,enter20Iterations.
(d)Retain the default values for the other parameters and click OK.
4.Set the time step parameters.
Solve?→Iterate...
(a)Set the Time Step Size(s)to5e-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 of1.It is generally di?cult to know the proper
time step size at the beginning of a simulation.Therefore,an adjustment after
the?ow is established,is often necessary.For a given time step?t,the highest
frequency that the acoustic analysis can produce is f=1
2?t .For the time step size
selected here,the maximum frequency is100kHz.Typically in most aeroacoustic calculations,the maximum frequency obtained from the analysis is higher than the audible range of interest.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
(b)Click Apply.
5.Save the case and data?les(cylinder2d t0.00.cas.gz and cylinder2d t0.00.dat.gz).
File?→Write?→Case&Data...
Save the case and data?les before the?rst iteration.This will save you time in the event of user error or code divergence,where the case?le would have to be set up all over again.
6.Run the case for a few time steps before activating the force monitors.
Solve?→Iterate...
(a)Set the Number of Time Steps to20.
(b)Click Iterate.
The residual history will be displayed as the calculation proceeds.When the non-iterative time advancement scheme is used,by default,two residuals are plotted per time step.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
7.Enable the monitoring of the lift and drag forces.
Setting the force monitors after some initial transient state limits the range of the drag
coe?cient when starting from an impulse initial condition.
Solve?→Monitors?→Force...
(a)In the Coe?cient drop-down list,select Drag.
(b)In the Wall Zones list,select wall cylinder.
(c)Verify that the X and Y values under Force Vector are1and0,respectively.
(d)Under Options,select Plot to enable plotting of the drag coe?cient.
(e)Under Options,select Write to save the monitor history to a?le,cd-history will
be the default?le name.
If you do not select the Write option,the history information will be lost when
you exit FLUENT.
(f)Click Apply.
(g)In the Coe?cient drop-down list,select Lift.
(h)Under Force Vector,specify X and Y to be0and1,respectively.
(i)Under Options,select Plot to enable plotting of the lift coe?cient.
(j)Under Options,select Write to save the monitor history to a?le.This time, cl-history will be the default?le name.
(k)Close the panel.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
8.Set the reference values to be used in the lift and drag coe?cient calculation.
Report?→Reference Values...
(a)Set the values as shown in the table:
Parameter Value
Area0.019
Velocity69.2
Length0.019
(b)Retain the default values for the other parameters and click OK.
The reference area is calculated using the cylinder diameter,D,and the default depth of1m for2D problems.Adjust the reference area if a di?erent depth (Depth)value is used.
For the actual force coe?cient calculation,only the reference area,density and velocity are needed.The reference length(Length)will be needed later for the Strouhal number calculation.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
9.Overwrite the previously saved initial conditions(cylinder2d t0.00.cas.gz and
cylinder2d t0.00.dat.gz).
File?→Write?→Case&Data...
10.Advance the?ow in time until a quasi-stationary state is reached.
Solve?→Iterate...
(a)Set the Number of Time Steps to4000.
(b)Click Iterate.
The4000time steps will advance the?ow up to t=0.02s.At that time the bulk?ow
will have crossed 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 Figure4and Figure5,
respectively.Di?erences in the long-term?ow evolution can occur due to operating
system dependent round-o?errors.Once the lift and drag histories are su?ciently
oscillatory and periodic in nature,you are ready to set up the acoustics model and
perform the acoustic calculations.
Figure4:Lift Coe?cient History
11.Verify that the selected time step size is reasonable for the given mesh and?ow
condition.
Plot?→Histogram...
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
Figure5:Drag Coe?cient History
(a)Under Histogram of,select Velocity....
(b)From the Velocity...category,select Cell Courant Number.
(c)Set the value for Divisions to100.
(d)Click Plot and verify that the peak CFL value is less than3.5.The histogram
(Figure6)shows that most cells have a Cell Courant Number of less than1.
12.Save the case and data?les(cylinder2d t0.02.cas.gz and cylinder2d t0.02.dat.gz).
File?→Write?→Case&Data...
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
Figure6:A Histogram Displaying the Range of the CFL Number Step7:Aeroacoustics Calculation
1.De?ne the acoustics model settings.
De?ne?→Models?→Acoustics...
(a)Under Model,select Ffowcs-Williams&Hawkings.
(b)Under Options,select Export Acoustic Source Data.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
(c)Click the Sources...button.
This will open the Acoustic Sources panel.
i.Under Source Zones,select wall cylinder.
All relevant acoustic source data(i.e.pressure in this case)will be extracted from the wall cylinder surface.
ii.In the text-entry box for Source Data Root Filename,enter cylinder2d.
This is the?lename root of the index?le which will be created.The index ?le contains information about the source data?les that are created when you run the case.The index?le is automatically created with a.index?le extension.
iii.Under Write Frequency,enter2.
Depending on the physical time step size and the important time scales in the?ow,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
=50kHz.
2(2?t)
iv.Set the No.of Time Steps Per File to200.
The source data can be conveniently segmented into multiple source data ?les.This makes it easier to process partial sequences when calculating the receiver signals.A value of200for No.of Time Steps Per File means that each source data?le covers a time span of200time steps.With a Write Frequency of2,there are100data sets written into each source data?le.
v.Click Apply and Close.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
(d)Click OK to close the Acoustics Model panel.
2.Modify the solution controls.
Solve?→Controls?→Solution...
(a)Increase the Relaxation Factor for Pressure to1.
(b)Click OK.
3.Resume the calculation.
Solve?→Iterate...
(a)Retain the Number of Time Steps at4000.
(b)Click Iterate.
The additional4000time steps will advance the?ow up to t=0.04s.
At every second time step,a message will be displayed in the FLUENT console window
informing you that data is written to a source data?le(.asd?le extension).
4.Save the case and data?les(cylinder2d t0.04.cas.gz and cylinder2d t0.04.dat.gz).
File?→Write?→Case&Data...
5.Set the acoustics model constants.
De?ne?→Models?→Acoustics...
(a)Retain the Far-Field Density at1.225kg/m3.
The far-?eld density is the density of the?uid outside the computational domain,
i.e.the density of the?uid near the receivers.In most calculations it is the same
as the density within the computational domain.
(b)Use the default value of340m/s for the Far-Field Sound Speed.
(c)Leave the Reference Acoustic Pressure at2e-05Pa.
The reference acoustic pressure is used to calculate decibel values during postpro-
cessing.
(d)Set the Source Correlation Length to0.095m.That is equal to?ve cylinder
diameters.
The source correlation length is very important when performing aeroacoustic cal-
culations in2D.FLUENT assumes that the sound sources are perfectly correlated
over the speci?ed correlation length,and zero outside.That is,FLUENT internally
builds a source volume with a depth equal to the speci?ed correlation length and
neglects sources outside.In your practical2D application,you will have to esti-
mate the source correlation length;your obtained sound pressure levels will de-
pend on your input.That makes it di?cult to rely on2D calculations to obtain
absolute sound pressure levels.Therefore,you should use aeroacoustic2D simu-
lations primarily to observe trends.The source correlation length is not needed
for3D calculations.
(e)Click OK to close the panel.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
6.Calculate the acoustic signals.
Solve?→Acoustic Signals...
(a)Click the Receivers...button.
This will open the Acoustic Receivers panel.
Note that you can open the Acoustic Receivers panel also from the Acoustics Model and Acoustic Sources panels.
i.Increase the No.of Receivers to2.
ii.For the receiver-1coordinates,enter0m for X-Coord.,-0.665m(35D)for Y-Coord.,and0for Z-Coord.
iii.For the receiver-2coordinates,enter0m for X-Coord.,-2.432m(128D)for Y-Coord.,and0for Z-Coord.
Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT
iv.Retain the defaults for Signal File Name(receiver-1.ard and receiver-2.ard).
v.Click OK to close the Acoustic Receivers panel.
(b)Under Active Source Zones,select wall cylinder.
All source zones which were selected in the Acoustic Sources panel are now avail-
able under the Active Source Zones.In this tutorial,the sound sources are ex-
tracted 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)Under Source Data?les,select all?les available.
Selecting a subset of the available source?les is a convenient way to analyze
shorter sequences.It is important to select a contiguous set of source data?les.
(d)Under Receivers,select the two available receivers.
As soon as the source zones,source data?les,and receivers are selected,the
Compute/Write function becomes available.
(e)Click Compute/Write.
The FLUENT console window will con?rm that the source data?les are being
read and that the receiver signals are computed and written into receiver?les.
(f)Click Close to close the Acoustic Signals panel.
Step8:Aeroacoustic Postprocessing
1.Display the acoustic pressure signals at the two receiver locations.
Plot?→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 Files list.
Tutorial:Modeling Flow-Induced(Aeroacoustic)Noise Problems Using FLUENT Introduction This tutorial demonstrates how to model2D turbulent?ow across a circular cylinder using large eddy simulation(LES)and compute?ow-induced(aeroacoustic)noise using FLUENT’s acoustics model. You will learn how to: ?Perform a2D large eddy simulation. ?Set parameters for an aeroacoustic calculation. ?Save acoustic source data for an acoustic calculation. ?Postprocess aeroacoustic results. Prerequisites This tutorial assumes that you are familiar with the 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,?rst read Chapter21,Predicting Aerodynamically Generated Noise,of the FLUENT6.2 User’s Guide