Advanced ANSYS FLUENT Acoustics

Size: px
Start display at page:

Download "Advanced ANSYS FLUENT Acoustics"

Transcription

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

2 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 ANSYS, Inc. November 7,

3 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 ANSYS, Inc. November 7,

4 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,

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

6 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 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 = Done ANSYS, Inc. November 7,

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

8 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 ANSYS, Inc. November 7,

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

10 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 ANSYS, Inc. November 7,

11 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 for Density 2. Retain the default value of e-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 ANSYS, Inc. November 7,

12 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 Pa for the Operating Pressure 2011 ANSYS, Inc. November 7,

13 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 ANSYS, Inc. November 7,

14 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,

15 Step 7: Solution Controls Solution Solution Controls 1. Set the Relaxation Factor for Pressure to 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 ANSYS, Inc. November 7,

16 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 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,

17 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 ANSYS, Inc. November 7,

18 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 ANSYS, Inc. November 7,

19 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,

20 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,

21 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 = Velocity = 69.2 Length = (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 ANSYS, Inc. November 7,

22 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 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 ANSYS, Inc. November 7,

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

24 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 ANSYS, Inc. November 7,

25 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,

26 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,

27 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,

28 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 ANSYS, Inc. November 7,

29 Step 9: Aeroacoustics Calculation (continued) 5. Set the acoustics model constants Problem Setup Models Acoustics (a) Retain Far-Field Density at 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 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,

30 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,

31 Step 9: Aeroacoustics Calculation (continued) i. Increase Number of Receivers to 2. ii. For the receiver-1 coordinates, enter 0 m for X-Coord., m (35D) for Y-Coord., and 0 for Z- Coord. iii. For the receiver-2 coordinates, enter 0 m for X-Coord., 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,

32 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,

33 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,

34 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,

35 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,

36 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 = e-005) = e+002 Note: The maximum frequency plotted is f = 1/[2(2Dt)] = 50 khz, as expected. Figure 8. Spectral analysis of pressure signal for receiver ANSYS, Inc. November 7,

37 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,

38 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,

39 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,

40 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,

41 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,

42 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 receiver ANSYS, Inc. November 7,

43 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 ANSYS, Inc. November 7,

44 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 Final Report for NASA Contract NAS ANSYS, Inc. November 7,

Modeling Supersonic Jet Screech Noise Using Direct Computational Aeroacoustics (CAA) 14.5 Release

Modeling Supersonic Jet Screech Noise Using Direct Computational Aeroacoustics (CAA) 14.5 Release Modeling Supersonic Jet Screech Noise Using Direct Computational Aeroacoustics (CAA) 14.5 Release 2011 ANSYS, Inc. November 7, 2012 1 Workshop Advanced ANSYS FLUENT Acoustics Introduction This tutorial

More information

Using a Single Rotating Reference Frame

Using a Single Rotating Reference Frame Tutorial 9. Using a Single Rotating Reference Frame Introduction This tutorial considers the flow within a 2D, axisymmetric, co-rotating disk cavity system. Understanding the behavior of such flows is

More information

Modeling External Compressible Flow

Modeling External Compressible Flow Tutorial 3. Modeling External Compressible Flow Introduction The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a nonzero angle of attack. You will use the Spalart-Allmaras

More information

Calculate a solution using the pressure-based coupled solver.

Calculate a solution using the pressure-based coupled solver. Tutorial 19. Modeling Cavitation Introduction This tutorial examines the pressure-driven cavitating flow of water through a sharpedged orifice. This is a typical configuration in fuel injectors, and brings

More information

Tutorial 17. Using the Mixture and Eulerian Multiphase Models

Tutorial 17. Using the Mixture and Eulerian Multiphase Models Tutorial 17. Using the Mixture and Eulerian Multiphase Models Introduction: This tutorial examines the flow of water and air in a tee junction. First you will solve the problem using the less computationally-intensive

More information

Modeling Evaporating Liquid Spray

Modeling Evaporating Liquid Spray Tutorial 17. Modeling Evaporating Liquid Spray Introduction In this tutorial, the air-blast atomizer model in ANSYS FLUENT is used to predict the behavior of an evaporating methanol spray. Initially, the

More information

Tutorial: Hydrodynamics of Bubble Column Reactors

Tutorial: Hydrodynamics of Bubble Column Reactors Tutorial: Introduction The purpose of this tutorial is to provide guidelines and recommendations for solving a gas-liquid bubble column problem using the multiphase mixture model, including advice on solver

More information

Tutorial 2. Modeling Periodic Flow and Heat Transfer

Tutorial 2. Modeling Periodic Flow and Heat Transfer Tutorial 2. Modeling Periodic Flow and Heat Transfer Introduction: Many industrial applications, such as steam generation in a boiler or air cooling in the coil of an air conditioner, can be modeled as

More information

Solution Recording and Playback: Vortex Shedding

Solution Recording and Playback: Vortex Shedding STAR-CCM+ User Guide 6663 Solution Recording and Playback: Vortex Shedding This tutorial demonstrates how to use the solution recording and playback module for capturing the results of transient phenomena.

More information

Modeling Evaporating Liquid Spray

Modeling Evaporating Liquid Spray Tutorial 16. Modeling Evaporating Liquid Spray Introduction In this tutorial, FLUENT s air-blast atomizer model is used to predict the behavior of an evaporating methanol spray. Initially, the air flow

More information

Modeling Unsteady Compressible Flow

Modeling Unsteady Compressible Flow Tutorial 4. Modeling Unsteady Compressible Flow Introduction In this tutorial, FLUENT s density-based implicit solver is used to predict the timedependent flow through a two-dimensional nozzle. As an initial

More information

Tutorial: Riser Simulation Using Dense Discrete Phase Model

Tutorial: Riser Simulation Using Dense Discrete Phase Model Introduction The purpose of this tutorial is to demonstrate the setup of a dense discrete phase model (DDPM) with the example of 2D riser. DDPM is used for the secondary phase that has a particle size

More information

Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders

Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders Objective: The objective of this laboratory is to introduce how to use FLUENT to solve both transient and natural convection problems.

More information

Using Multiple Rotating Reference Frames

Using Multiple Rotating Reference Frames Tutorial 9. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive

More information

Use 6DOF solver to calculate motion of the moving body. Create TIFF files for graphic visualization of the solution.

Use 6DOF solver to calculate motion of the moving body. Create TIFF files for graphic visualization of the solution. Introduction The purpose of this tutorial is to provide guidelines and recommendations for setting up and solving a moving deforming mesh (MDM) case along with the six degree of freedom (6DOF) solver and

More information

Using Multiple Rotating Reference Frames

Using Multiple Rotating Reference Frames Tutorial 10. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive

More information

Non-Newtonian Transitional Flow in an Eccentric Annulus

Non-Newtonian Transitional Flow in an Eccentric Annulus Tutorial 8. Non-Newtonian Transitional Flow in an Eccentric Annulus Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D, turbulent flow of a non-newtonian fluid. Turbulent

More information

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

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

More information

Simulation of Flow Development in a Pipe

Simulation of Flow Development in a Pipe Tutorial 4. Simulation of Flow Development in a Pipe Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D turbulent fluid flow in a pipe. The pipe networks are common

More information

Compressible Flow in a Nozzle

Compressible Flow in a Nozzle SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 1 Compressible Flow in a Nozzle Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification Consider air flowing at high-speed through a

More information

Tutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow

Tutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow Tutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow Introduction This tutorial illustrates the setup and solution of the two-dimensional turbulent fluid flow and heat

More information

Express Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding

Express Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding Express Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry Oriented HPC Simulations,

More information

This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following:

This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following: Tutorial 22. Modeling Solidification Introduction This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following: Define a

More information

Module D: Laminar Flow over a Flat Plate

Module D: Laminar Flow over a Flat Plate Module D: Laminar Flow over a Flat Plate Summary... Problem Statement Geometry and Mesh Creation Problem Setup Solution. Results Validation......... Mesh Refinement.. Summary This ANSYS FLUENT tutorial

More information

Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil

Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 -

More information

Modeling Flow Through Porous Media

Modeling Flow Through Porous Media Tutorial 7. Modeling Flow Through Porous Media Introduction Many industrial applications involve the modeling of flow through porous media, such as filters, catalyst beds, and packing. This tutorial illustrates

More information

Aero-Vibro Acoustics For Wind Noise Application. David Roche and Ashok Khondge ANSYS, Inc.

Aero-Vibro Acoustics For Wind Noise Application. David Roche and Ashok Khondge ANSYS, Inc. Aero-Vibro Acoustics For Wind Noise Application David Roche and Ashok Khondge ANSYS, Inc. Outline 1. Wind Noise 2. Problem Description 3. Simulation Methodology 4. Results 5. Summary Thursday, October

More information

A B C D E. Settings Choose height, H, free stream velocity, U, and fluid (dynamic viscosity and density ) so that: Reynolds number

A B C D E. Settings Choose height, H, free stream velocity, U, and fluid (dynamic viscosity and density ) so that: Reynolds number Individual task Objective To derive the drag coefficient for a 2D object, defined as where D (N/m) is the aerodynamic drag force (per unit length in the third direction) acting on the object. The object

More information

Using the Eulerian Multiphase Model for Granular Flow

Using the Eulerian Multiphase Model for Granular Flow Tutorial 21. Using the Eulerian Multiphase Model for Granular Flow Introduction Mixing tanks are used to maintain solid particles or droplets of heavy fluids in suspension. Mixing may be required to enhance

More information

The purpose of this tutorial is to illustrate how to set up and solve a problem using the. Moving Deforming Mesh (MDM) using the layering algorithm.

The purpose of this tutorial is to illustrate how to set up and solve a problem using the. Moving Deforming Mesh (MDM) using the layering algorithm. Tutorial: Introduction The purpose of this tutorial is to illustrate how to set up and solve a problem using the following two features in FLUENT. Moving Deforming Mesh (MDM) using the layering algorithm.

More information

Tutorial: Modeling Liquid Reactions in CIJR Using the Eulerian PDF transport (DQMOM-IEM) Model

Tutorial: Modeling Liquid Reactions in CIJR Using the Eulerian PDF transport (DQMOM-IEM) Model Tutorial: Modeling Liquid Reactions in CIJR Using the Eulerian PDF transport (DQMOM-IEM) Model Introduction The purpose of this tutorial is to demonstrate setup and solution procedure of liquid chemical

More information

Grid. Apr 09, 1998 FLUENT 5.0 (2d, segregated, lam) Grid. Jul 31, 1998 FLUENT 5.0 (2d, segregated, lam)

Grid. Apr 09, 1998 FLUENT 5.0 (2d, segregated, lam) Grid. Jul 31, 1998 FLUENT 5.0 (2d, segregated, lam) Tutorial 2. Around an Airfoil Transonic Turbulent Flow Introduction: The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a non-zero angle of attack. You will use the

More information

Introduction to ANSYS CFX

Introduction to ANSYS CFX Workshop 03 Fluid flow around the NACA0012 Airfoil 16.0 Release Introduction to ANSYS CFX 2015 ANSYS, Inc. March 13, 2015 1 Release 16.0 Workshop Description: The flow simulated is an external aerodynamics

More information

Tutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing

Tutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing Tutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing Introduction The purpose of this tutorial is to demonstrate how to simulate a ball check valve with small displacement

More information

Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim

Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon

More information

Simulation of Turbulent Flow over the Ahmed Body

Simulation of Turbulent Flow over the Ahmed Body Simulation of Turbulent Flow over the Ahmed Body 58:160 Intermediate Mechanics of Fluids CFD LAB 4 By Timur K. Dogan, Michael Conger, Maysam Mousaviraad, and Fred Stern IIHR-Hydroscience & Engineering

More information

TUTORIAL#3. Marek Jaszczur. Boundary Layer on a Flat Plate W1-1 AGH 2018/2019

TUTORIAL#3. Marek Jaszczur. Boundary Layer on a Flat Plate W1-1 AGH 2018/2019 TUTORIAL#3 Boundary Layer on a Flat Plate Marek Jaszczur AGH 2018/2019 W1-1 Problem specification TUTORIAL#3 Boundary Layer - on a flat plate Goal: Solution for boudary layer 1. Creating 2D simple geometry

More information

Express Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing

Express Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing Express Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry Oriented HPC Simulations,

More information

Simulation of Laminar Pipe Flows

Simulation of Laminar Pipe Flows Simulation of Laminar Pipe Flows 57:020 Mechanics of Fluids and Transport Processes CFD PRELAB 1 By Timur Dogan, Michael Conger, Maysam Mousaviraad, Tao Xing and Fred Stern IIHR-Hydroscience & Engineering

More information

Flow in an Intake Manifold

Flow in an Intake Manifold Tutorial 2. Flow in an Intake Manifold Introduction The purpose of this tutorial is to model turbulent flow in a simple intake manifold geometry. An intake manifold is a system of passages which carry

More information

Introduction to CFX. Workshop 2. Transonic Flow Over a NACA 0012 Airfoil. WS2-1. ANSYS, Inc. Proprietary 2009 ANSYS, Inc. All rights reserved.

Introduction to CFX. Workshop 2. Transonic Flow Over a NACA 0012 Airfoil. WS2-1. ANSYS, Inc. Proprietary 2009 ANSYS, Inc. All rights reserved. Workshop 2 Transonic Flow Over a NACA 0012 Airfoil. Introduction to CFX WS2-1 Goals The purpose of this tutorial is to introduce the user to modelling flow in high speed external aerodynamic applications.

More information

Verification and Validation of Turbulent Flow around a Clark-Y Airfoil

Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1 Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 2 (ANSYS 19.1; Last Updated: Aug. 7, 2018) By Timur Dogan, Michael Conger,

More information

Simulation of Turbulent Flow over the Ahmed Body

Simulation of Turbulent Flow over the Ahmed Body 1 Simulation of Turbulent Flow over the Ahmed Body ME:5160 Intermediate Mechanics of Fluids CFD LAB 4 (ANSYS 18.1; Last Updated: Aug. 18, 2016) By Timur Dogan, Michael Conger, Dong-Hwan Kim, Maysam Mousaviraad,

More information

FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016

FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016 FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016 Note: These instructions are based on an older version of FLUENT, and some of the instructions

More information

Tutorial: Modeling Domains with Embedded Reference Frames: Part 2 Sliding Mesh Modeling

Tutorial: Modeling Domains with Embedded Reference Frames: Part 2 Sliding Mesh Modeling Tutorial: Modeling Domains with Embedded Reference Frames: Part 2 Sliding Mesh Modeling Introduction The motion of rotating components is often complicated by the fact that the rotational axis about which

More information

Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent

Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent MEGR 7090-003, Computational Fluid Dynamics :1 7 Spring 2015 Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent Rahul R Upadhyay Master of Science, Dept of Mechanical

More information

Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes

Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School

More information

Simulation of Turbulent Flow around an Airfoil

Simulation of Turbulent Flow around an Airfoil 1. Purpose Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew

More information

Verification of Laminar and Validation of Turbulent Pipe Flows

Verification of Laminar and Validation of Turbulent Pipe Flows 1 Verification of Laminar and Validation of Turbulent Pipe Flows 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 1 (ANSYS 18.1; Last Updated: Aug. 1, 2017) By Timur Dogan, Michael Conger, Dong-Hwan

More information

TUTORIAL#4. Marek Jaszczur. Turbulent Thermal Boundary Layer on a Flat Plate W1-1 AGH 2018/2019

TUTORIAL#4. Marek Jaszczur. Turbulent Thermal Boundary Layer on a Flat Plate W1-1 AGH 2018/2019 TUTORIAL#4 Turbulent Thermal Boundary Layer on a Flat Plate Marek Jaszczur AGH 2018/2019 W1-1 Problem specification TUTORIAL#4 Turbulent Thermal Boundary Layer - on a flat plate Goal: Solution for Non-isothermal

More information

Near Field and Far Field Prediction of Noise in and around a Loudspeaker: A Numerical and Experimental Investigation

Near Field and Far Field Prediction of Noise in and around a Loudspeaker: A Numerical and Experimental Investigation Near Field and Far Field Prediction of Noise in and around a Loudspeaker: A Numerical and Experimental Investigation M. Younsi, V. Morgenthaler ANSYS France SAS, France G. Kergourlay Canon CRF, France

More information

Using the Discrete Ordinates Radiation Model

Using the Discrete Ordinates Radiation Model Tutorial 6. Using the Discrete Ordinates Radiation Model Introduction This tutorial illustrates the set up and solution of flow and thermal modelling of a headlamp. The discrete ordinates (DO) radiation

More information

Revolve 3D geometry to display a 360-degree image.

Revolve 3D geometry to display a 360-degree image. Tutorial 24. Turbo Postprocessing Introduction This tutorial demonstrates the turbomachinery postprocessing capabilities of FLUENT. In this example, you will read the case and data files (without doing

More information

Supersonic Flow Over a Wedge

Supersonic Flow Over a Wedge SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 2 Supersonic Flow Over a Wedge Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification A uniform supersonic stream encounters a wedge

More information

Step 1: Create Geometry in GAMBIT

Step 1: Create Geometry in GAMBIT Step 1: Create Geometry in GAMBIT If you would prefer to skip the mesh generation steps, you can create a working directory (see below), download the mesh from here (right click and save as pipe.msh) into

More information

Simulating Sinkage & Trim for Planing Boat Hulls. A Fluent Dynamic Mesh 6DOF Tutorial

Simulating Sinkage & Trim for Planing Boat Hulls. A Fluent Dynamic Mesh 6DOF Tutorial Simulating Sinkage & Trim for Planing Boat Hulls A Fluent Dynamic Mesh 6DOF Tutorial 1 Introduction Workshop Description This workshop describes how to perform a transient 2DOF simulation of a planing

More information

Simulation and Validation of Turbulent Pipe Flows

Simulation and Validation of Turbulent Pipe Flows Simulation and Validation of Turbulent Pipe Flows ENGR:2510 Mechanics of Fluids and Transport Processes CFD LAB 1 (ANSYS 17.1; Last Updated: Oct. 10, 2016) By Timur Dogan, Michael Conger, Dong-Hwan Kim,

More information

Simulation of Turbulent Flow around an Airfoil

Simulation of Turbulent Flow around an Airfoil Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Pre-Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew Opyd, Dong-Hwan

More information

Steady Flow: Lid-Driven Cavity Flow

Steady Flow: Lid-Driven Cavity Flow STAR-CCM+ User Guide Steady Flow: Lid-Driven Cavity Flow 2 Steady Flow: Lid-Driven Cavity Flow This tutorial demonstrates the performance of STAR-CCM+ in solving a traditional square lid-driven cavity

More information

Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions. Milovan Perić

Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions. Milovan Perić Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions Milovan Perić Contents The need to couple STAR-CCM+ with other theoretical or numerical solutions Coupling approaches: surface and volume

More information

and to the following students who assisted in the creation of the Fluid Dynamics tutorials:

and to the following students who assisted in the creation of the Fluid Dynamics tutorials: Fluid Dynamics CAx Tutorial: Pressure Along a Streamline Basic Tutorial #3 Deryl O. Snyder C. Greg Jensen Brigham Young University Provo, UT 84602 Special thanks to: PACE, Fluent, UGS Solutions, Altair

More information

Appendix: To be performed during the lab session

Appendix: To be performed during the lab session Appendix: To be performed during the lab session Flow over a Cylinder Two Dimensional Case Using ANSYS Workbench Simple Mesh Latest revision: September 18, 2014 The primary objective of this Tutorial is

More information

Simulation of Turbulent Flow in an Asymmetric Diffuser

Simulation of Turbulent Flow in an Asymmetric Diffuser Simulation of Turbulent Flow in an Asymmetric Diffuser 1. Purpose 58:160 Intermediate Mechanics of Fluids CFD LAB 3 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University of Iowa C.

More information

Investigation of cross flow over a circular cylinder at low Re using the Immersed Boundary Method (IBM)

Investigation of cross flow over a circular cylinder at low Re using the Immersed Boundary Method (IBM) Computational Methods and Experimental Measurements XVII 235 Investigation of cross flow over a circular cylinder at low Re using the Immersed Boundary Method (IBM) K. Rehman Department of Mechanical Engineering,

More information

ANSYS AIM Tutorial Steady Flow Past a Cylinder

ANSYS AIM Tutorial Steady Flow Past a Cylinder ANSYS AIM Tutorial Steady Flow Past a Cylinder Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Solution Domain Boundary Conditions Start-Up

More information

The viscous forces on the cylinder are proportional to the gradient of the velocity field at the

The viscous forces on the cylinder are proportional to the gradient of the velocity field at the Fluid Dynamics Models : Flow Past a Cylinder Flow Past a Cylinder Introduction The flow of fluid behind a blunt body such as an automobile is difficult to compute due to the unsteady flows. The wake behind

More information

Middle East Technical University Mechanical Engineering Department ME 485 CFD with Finite Volume Method Fall 2017 (Dr. Sert)

Middle East Technical University Mechanical Engineering Department ME 485 CFD with Finite Volume Method Fall 2017 (Dr. Sert) Middle East Technical University Mechanical Engineering Department ME 485 CFD with Finite Volume Method Fall 2017 (Dr. Sert) ANSYS Fluent Tutorial Developing Laminar Flow in a 2D Channel 1 How to use This

More information

November c Fluent Inc. November 8,

November c Fluent Inc. November 8, MIXSIM 2.1 Tutorial November 2006 c Fluent Inc. November 8, 2006 1 Copyright c 2006 by Fluent Inc. All Rights Reserved. No part of this document may be reproduced or otherwise used in any form without

More information

Verification and Validation of Turbulent Flow around a Clark-Y Airfoil

Verification and Validation of Turbulent Flow around a Clark-Y Airfoil Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose 58:160 Intermediate Mechanics of Fluids CFD LAB 2 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University

More information

Fluent User Services Center

Fluent User Services Center Solver Settings 5-1 Using the Solver Setting Solver Parameters Convergence Definition Monitoring Stability Accelerating Convergence Accuracy Grid Independence Adaption Appendix: Background Finite Volume

More information

c Fluent Inc. May 16,

c Fluent Inc. May 16, Tutorial 1. Office Ventilation Introduction: This tutorial demonstrates how to model an office shared by two people working at computers, using Airpak. In this tutorial, you will learn how to: Open a new

More information

Tutorial: Heat and Mass Transfer with the Mixture Model

Tutorial: Heat and Mass Transfer with the Mixture Model Tutorial: Heat and Mass Transfer with the Mixture Model Purpose The purpose of this tutorial is to demonstrate the use of mixture model in FLUENT 6.0 to solve a mixture multiphase problem involving heat

More information

Analysis of an airfoil

Analysis of an airfoil UNDERGRADUATE RESEARCH FALL 2010 Analysis of an airfoil using Computational Fluid Dynamics Tanveer Chandok 12/17/2010 Independent research thesis at the Georgia Institute of Technology under the supervision

More information

LARGE EDDY SIMULATION OF VORTEX SHEDDING WITH TRIANGULAR CYLINDER AHEAD OF A SQUARE CYLINDER

LARGE EDDY SIMULATION OF VORTEX SHEDDING WITH TRIANGULAR CYLINDER AHEAD OF A SQUARE CYLINDER The Eighth Asia-Pacific Conference on Wind Engineering, December 10 14, 2013, Chennai, India LARGE EDDY SIMULATION OF VORTEX SHEDDING WITH TRIANGULAR CYLINDER AHEAD OF A SQUARE CYLINDER Akshoy Ranjan Paul

More information

Viscous Hybrid Mesh Generation

Viscous Hybrid Mesh Generation Tutorial 4. Viscous Hybrid Mesh Generation Introduction In cases where you want to resolve the boundary layer, it is often more efficient to use prismatic cells in the boundary layer rather than tetrahedral

More information

The Spalart Allmaras turbulence model

The Spalart Allmaras turbulence model The Spalart Allmaras turbulence model The main equation The Spallart Allmaras turbulence model is a one equation model designed especially for aerospace applications; it solves a modelled transport equation

More information

Isotropic Porous Media Tutorial

Isotropic Porous Media Tutorial STAR-CCM+ User Guide 3927 Isotropic Porous Media Tutorial This tutorial models flow through the catalyst geometry described in the introductory section. In the porous region, the theoretical pressure drop

More information

CFD Analysis of 2-D Unsteady Flow Past a Square Cylinder at an Angle of Incidence

CFD Analysis of 2-D Unsteady Flow Past a Square Cylinder at an Angle of Incidence CFD Analysis of 2-D Unsteady Flow Past a Square Cylinder at an Angle of Incidence Kavya H.P, Banjara Kotresha 2, Kishan Naik 3 Dept. of Studies in Mechanical Engineering, University BDT College of Engineering,

More information

Workbench Tutorial Minor Losses, Page 1 Tutorial Minor Losses using Pointwise and FLUENT

Workbench Tutorial Minor Losses, Page 1 Tutorial Minor Losses using Pointwise and FLUENT Workbench Tutorial Minor Losses, Page 1 Tutorial Minor Losses using Pointwise and FLUENT Introduction This tutorial provides instructions for meshing two internal flows. Pointwise software will be used

More information

Aerodynamic Study of a Realistic Car W. TOUGERON

Aerodynamic Study of a Realistic Car W. TOUGERON Aerodynamic Study of a Realistic Car W. TOUGERON Tougeron CFD Engineer 2016 Abstract This document presents an aerodynamic CFD study of a realistic car geometry. The aim is to demonstrate the efficiency

More information

NUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING

NUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING Review of the Air Force Academy No.3 (35)/2017 NUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING Cvetelina VELKOVA Department of Technical Mechanics, Naval Academy Nikola Vaptsarov,Varna, Bulgaria (cvetelina.velkova1985@gmail.com)

More information

Backward facing step Homework. Department of Fluid Mechanics. For Personal Use. Budapest University of Technology and Economics. Budapest, 2010 autumn

Backward facing step Homework. Department of Fluid Mechanics. For Personal Use. Budapest University of Technology and Economics. Budapest, 2010 autumn Backward facing step Homework Department of Fluid Mechanics Budapest University of Technology and Economics Budapest, 2010 autumn Updated: October 26, 2010 CONTENTS i Contents 1 Introduction 1 2 The problem

More information

and to the following students who assisted in the creation of the Fluid Dynamics tutorials:

and to the following students who assisted in the creation of the Fluid Dynamics tutorials: Fluid Dynamics CAx Tutorial: Channel Flow Basic Tutorial # 4 Deryl O. Snyder C. Greg Jensen Brigham Young University Provo, UT 84602 Special thanks to: PACE, Fluent, UGS Solutions, Altair Engineering;

More information

ANSYS FLUENT. Lecture 3. Basic Overview of Using the FLUENT User Interface L3-1. Customer Training Material

ANSYS FLUENT. Lecture 3. Basic Overview of Using the FLUENT User Interface L3-1. Customer Training Material Lecture 3 Basic Overview of Using the FLUENT User Interface Introduction to ANSYS FLUENT L3-1 Parallel Processing FLUENT can readily be run across many processors in parallel. This will greatly speed up

More information

8. BASIC TURBO MODEL WITH UNSTRUCTURED MESH

8. BASIC TURBO MODEL WITH UNSTRUCTURED MESH 8. BASIC TURBO MODEL WITH UNSTRUCTURED MESH This tutorial employs a simple turbine blade configuration to illustrate the basic turbo modeling functionality available in GAMBIT. It illustrates the steps

More information

ANSYS FLUENT. Airfoil Analysis and Tutorial

ANSYS FLUENT. Airfoil Analysis and Tutorial ANSYS FLUENT Airfoil Analysis and Tutorial ENGR083: Fluid Mechanics II Terry Yu 5/11/2017 Abstract The NACA 0012 airfoil was one of the earliest airfoils created. Its mathematically simple shape and age

More information

Prerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT, and that you have solved Tutorial 1.

Prerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT, and that you have solved Tutorial 1. Tutorial 22. Postprocessing Introduction: In this tutorial, the postprocessing capabilities of FLUENT are demonstrated for a 3D laminar flow involving conjugate heat transfer. The flow is over a rectangular

More information

CFD Analysis of a Fully Developed Turbulent Flow in a Pipe with a Constriction and an Obstacle

CFD Analysis of a Fully Developed Turbulent Flow in a Pipe with a Constriction and an Obstacle CFD Analysis of a Fully Developed Turbulent Flow in a Pipe with a Constriction and an Obstacle C, Diyoke Mechanical Engineering Department Enugu State University of Science & Tech. Enugu, Nigeria U, Ngwaka

More information

NUMERICAL MODELING AND EXPERIMENTAL EVALUATION OF AN HIGH-SPEED TRAIN PANTOGRAPH AERODYNAMIC NOISE

NUMERICAL MODELING AND EXPERIMENTAL EVALUATION OF AN HIGH-SPEED TRAIN PANTOGRAPH AERODYNAMIC NOISE NUMERICAL MODELING AND EXPERIMENTAL EVALUATION OF AN HIGH-SPEED TRAIN PANTOGRAPH AERODYNAMIC NOISE D. SIANO 1, M. VISCARDI 2, F. DONISI 2 P. NAPOLITANO 2 1 CNR (National Research Council of Italy) - Istituto

More information

High-Fidelity Simulation of Unsteady Flow Problems using a 3rd Order Hybrid MUSCL/CD scheme. A. West & D. Caraeni

High-Fidelity Simulation of Unsteady Flow Problems using a 3rd Order Hybrid MUSCL/CD scheme. A. West & D. Caraeni High-Fidelity Simulation of Unsteady Flow Problems using a 3rd Order Hybrid MUSCL/CD scheme ECCOMAS, June 6 th -11 th 2016, Crete Island, Greece A. West & D. Caraeni Outline Industrial Motivation Numerical

More information

CFD MODELING FOR PNEUMATIC CONVEYING

CFD MODELING FOR PNEUMATIC CONVEYING CFD MODELING FOR PNEUMATIC CONVEYING Arvind Kumar 1, D.R. Kaushal 2, Navneet Kumar 3 1 Associate Professor YMCAUST, Faridabad 2 Associate Professor, IIT, Delhi 3 Research Scholar IIT, Delhi e-mail: arvindeem@yahoo.co.in

More information

ANSYS AIM Tutorial Turbulent Flow Over a Backward Facing Step

ANSYS AIM Tutorial Turbulent Flow Over a Backward Facing Step ANSYS AIM Tutorial Turbulent Flow Over a Backward Facing Step Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Governing Equation Start-Up Geometry

More information

Problem description. The FCBI-C element is used in the fluid part of the model.

Problem description. The FCBI-C element is used in the fluid part of the model. Problem description This tutorial illustrates the use of ADINA for analyzing the fluid-structure interaction (FSI) behavior of a flexible splitter behind a 2D cylinder and the surrounding fluid in a channel.

More information

Chapter 24. Creating Surfaces for Displaying and Reporting Data

Chapter 24. Creating Surfaces for Displaying and Reporting Data Chapter 24. Creating Surfaces for Displaying and Reporting Data FLUENT allows you to select portions of the domain to be used for visualizing the flow field. The domain portions are called surfaces, and

More information

Large Eddy Simulation of Flow over a Backward Facing Step using Fire Dynamics Simulator (FDS)

Large Eddy Simulation of Flow over a Backward Facing Step using Fire Dynamics Simulator (FDS) The 14 th Asian Congress of Fluid Mechanics - 14ACFM October 15-19, 2013; Hanoi and Halong, Vietnam Large Eddy Simulation of Flow over a Backward Facing Step using Fire Dynamics Simulator (FDS) Md. Mahfuz

More information

µ = Pa s m 3 The Reynolds number based on hydraulic diameter, D h = 2W h/(w + h) = 3.2 mm for the main inlet duct is = 359

µ = Pa s m 3 The Reynolds number based on hydraulic diameter, D h = 2W h/(w + h) = 3.2 mm for the main inlet duct is = 359 Laminar Mixer Tutorial for STAR-CCM+ ME 448/548 March 30, 2014 Gerald Recktenwald gerry@pdx.edu 1 Overview Imagine that you are part of a team developing a medical diagnostic device. The device has a millimeter

More information

Cold Flow Simulation Inside an SI Engine

Cold Flow Simulation Inside an SI Engine Tutorial 12. Cold Flow Simulation Inside an SI Engine Introduction The purpose of this tutorial is to illustrate the case setup and solution of the two dimensional, four stroke spark ignition (SI) engine

More information

Recent developments for the multigrid scheme of the DLR TAU-Code

Recent developments for the multigrid scheme of the DLR TAU-Code www.dlr.de Chart 1 > 21st NIA CFD Seminar > Axel Schwöppe Recent development s for the multigrid scheme of the DLR TAU-Code > Apr 11, 2013 Recent developments for the multigrid scheme of the DLR TAU-Code

More information

STUDY OF FLOW PERFORMANCE OF A GLOBE VALVE AND DESIGN OPTIMISATION

STUDY OF FLOW PERFORMANCE OF A GLOBE VALVE AND DESIGN OPTIMISATION Journal of Engineering Science and Technology Vol. 12, No. 9 (2017) 2403-2409 School of Engineering, Taylor s University STUDY OF FLOW PERFORMANCE OF A GLOBE VALVE AND DESIGN OPTIMISATION SREEKALA S. K.

More information

Solver Basics. Introductory FLUENT Training ANSYS, Inc. All rights reserved. ANSYS, Inc. Proprietary

Solver Basics. Introductory FLUENT Training ANSYS, Inc. All rights reserved. ANSYS, Inc. Proprietary Solver Basics Introductory FLUENT Training 2006 ANSYS, Inc. All rights reserved. 2006 ANSYS, Inc. All rights reserved. 3-2 Solver Execution The menus are arranged such that the order of operation is generally

More information