Modeling Supersonic Jet Screech Noise Using Direct Computational Aeroacoustics (CAA) 14.5 Release
|
|
- Arleen Jenkins
- 5 years ago
- Views:
Transcription
1 Modeling Supersonic Jet Screech Noise Using Direct Computational Aeroacoustics (CAA) 14.5 Release 2011 ANSYS, Inc. November 7, Workshop Advanced ANSYS FLUENT Acoustics
2 Introduction This tutorial demonstrates how to model screech tone noise radiated by an axisymmetric supersonic jet using direct computational aeroacoustics (CAA) in ANSYS FLUENT This tutorial demonstrates how to do the following: Perform axisymmetric simulation of a steady-state supersonic jet flow using realizable k-e turbulence model with model constants modified for free jet flows Calculate unsteady flow and acoustic near field by direct CAA using unsteady realizable k-e turbulence model Save acoustic data at nearfield microphone location for further spectral analysis Postprocess flowfield and aeroacoustic results 2011 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 direct CAA method. 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 27 hours of CPU time on a single 32-bit Windows machine is required to complete this tutorial. It will take only 2.5 hours on 8 parallel nodes! If you are interested exclusively in learning how to set up the steady-state and direct CAA models, you can reduce the computing time requirements considerably by skipping Steps 9 (converging steady-state run), and Steps 11 (time-marching unsteady simulation) and using the provided case and data files to postprocess results at Step ANSYS, Inc. November 7,
4 Problem Description Supersonic jet noise has three main components: 1. Broadband shock-associated noise 2. Turbulent mixing noise 3. Screech tones Screech tones radiate at discrete frequencies. They are generated by a feedback loop 1,2 (Figure 1): A quasi-periodic shock-cell structure is formed in the core of an imperfectly expanded jet. At the nozzle exist, jet shear layer is thin and receptive to external excitations. Acoustic disturbances impinge on the nozzle lip and excite instability waves, which then propagate downstream and grow as they extract energy from the meanflow. At the fourth or fifth shock cell, amplitude of the instability wave becomes large enough to interact with the shock-cell structure. This unsteady interaction generates acoustic waves which propagate, in part, upstream outside the jet, and excite another excitation of the jet mixing layer at the nozzle lip. This generates a new instability wave, and closes the feedback loop nozzle feedback acoustic waves shock cells instability waves Figure 1. Screech tone feedback loop 1 Powell, A., On the Mechanism of Choked Jet Noise, Proceedings of the Physical Society, London, Vol. 66, 1953, pp Shen, H., and Tam, C. K. W., Numerical Simulation of the Generation of Axisymmetric Mode Jet Screech Tones, AIAA Journal, Vol. 36, No. 10, 1998, pp ANSYS, Inc. November 7,
5 Problem Description The problem considers turbulent air flow associated with Mach 1.2 cold jet emitted from 1 diameter round nozzle with thick lip. Nozzle geometry and flow conditions are from experiments of Ponton and Seiner Microphone locations Jet flow Nozzle lip Figure 1. Nozzle geometry 3 Ponton, M. K., and Seiner, J. M., The Effect of Nozzle Exit Lip Thickness on Plume resonance, Journal of Sound and Vibration, Vol. 154, Issue 3, 1992, pp ANSYS, Inc. November 7,
6 Preparation 1. Copy the file mesh-caa-jet-screech.msh.gz to your working directory 2. Start the 2D double-precision version of ANSYS FLUENT ANSYS, Inc. November 7,
7 Setup and Solution Step 1: Mesh 1. Read the mesh file mesh-caa-jet-screech.msh.gz File Read Mesh As FLUENT reads the mesh file, it will report its progress in the console window. 2. The mesh was created in inches, and it needs to be rescaled Mesh Scale (a) Select Convert Units under Scaling (b) Select in under Mesh Was Created In (c) Click Scale once (d) Check Domain Extents: Xmin (m) = , Xmax (m) = 25.4 Ymin (m)= 0, Ymax (m) = (e) Click Close 3. 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 2011 ANSYS, Inc. November 7,
8 Setup and Solution Steady-State Flow Step 1: Mesh (continued) 4. Display the mesh Results Graphic and Animation Mesh Set Up ANSYS, Inc. November 7,
9 Setup and Solution Steady-State Flow Step 1: Mesh (continued) (a) Display the grid with the default settings (Figure 3). Use the middle mouse button to zoom in on the image so you can see the mesh at the nozzle (Figure 4) Figure 3. Mesh Display Figure 4. Mesh at the nozzle exit Hybrid quad-tri mesh is used in this simulation. Structured quad cells are used to resolve the jet plume up to 20 nozzle diameters downstream. Tri cells are used in the far field. The cell size should be small enough to adequately resolve excitations of the jet shear layer at the nozzle lip, development of shear layer instability waves, shock cell structure in the nozzle core and nearfield propagation of screech acoustic waves ANSYS, Inc. November 7,
10 Step 2: Models Setup and Solution Steady-State Flow 1. Select the pressure-based steady-state axisymmetric solver Problem Setup General Note: pressure-based solver is used in this simulation to take advantage of higher order QUICK discretization scheme for the density, momentum, energy and turbulence equations on structured meshes 2011 ANSYS, Inc. November 7,
11 Setup and Solution Steady-State Flow Step 2: Models (continued) 2. Select realizable k-e turbulence model Problem Setup Models Viscous (a) Select k-epsilon under Model (b) Select Realizable under k-epsilon Model (c) Retain Standard Wall Functions under Near Wall Treatment (d) Modify model constants as: C2-Epsilon = 2.02 TKE Prandtl Number = TDR Prandtl Number = Energy Prandtl Number = This modification follows Ref. [4] which proposed a set of new constants for the standard k-e model designed specifically for predicting turbulent jet flows (e) Click OK 4 Thies, A., and Tam, C. K. W., Computation of Turbulent Axisymmetric and Nonaxisymmetric Jet Flows Using the K- model, AIAA Journal, Vol. 34, No. 2, 1996, pp ANSYS, Inc. November 7,
12 Step 3: Materials Setup and Solution Steady-State Flow You will use the default material, air, which is the working fluid in this problem. Air is modeled as ideal compressible gas Problem Setup Materials Fluid Air 1. Change the density formulation to ideal-gas Energy equation will be turned on automatically. The message Note: Enabling energy equation as required by material density method, will be printed in the console window 2. Change the viscosity formulation to sutherland, and accept Three Coefficient Method with default constants 3. Click Change/Create You can modify the fluid properties for air or copy another material from the database if needed. For details, refer to the Chapter 8, Physical Properties, in the ANSYS FLUENT 14.5 User's Guide 2011 ANSYS, Inc. November 7,
13 Setup and Solution Steady-State Flow Step 4: Cell Zone Conditions Problem Setup Cell Zone Conditions 1. Select air i. Click Edit... to open the Fluid panel ii. Retain the default selection of air as the fluid material in the Material Name drop-down list iii. Click OK 2011 ANSYS, Inc. November 7,
14 Setup and Solution Steady-State Flow Step 4: Cell Zone Conditions Problem Setup Cell Zone Conditions 2. Select air-lam i. Click Edit... to open the Fluid panel, and check Laminar Zone Small fluid region just at the nozzle exit is modeled as laminar (Figure 5). This is necessary to augment excitation of mixing layer instability waves. The rest of the fluid is modeled as turbulent air. ii. Click OK 3. Click Operating Conditions... to open the Operating Conditions panel Set Operating Pressure to 0 Turbulent zone Laminar zone Figure 5. Mesh at the nozzle exit showing location of the laminar zone 2011 ANSYS, Inc. November 7,
15 Setup and Solution Steady-State Flow 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 pressure-inlet b) Click Edit... to open the Pressure Inlet panel, and select Momentum tab i. Set the Gauge Total Pressure (pascal) to 242,496.5 ii. Set Supersonic/Initial Gauge Pressure (pascal) to 127,360 These settings are based on isentropic relationships, they correspond to fully expanded jet Mach number equal to 1.2 iii. Retain Normal to Boundary under Direction Specification Method iv. Select Intensity and Hydraulic Diameter under Turbulence Specification Method, and set Turbulent Intensity (%) = 0.1, and Hydraulic Diameter = Low level of turbulence is assumed at the nozzle exit c) Select Thermal tab in the Pressure Inlet panel i. Set Total Temperature (K) to 300 K For cold jets, total temperature is equal to the ambient static temperature 2011 ANSYS, Inc. November 7,
16 Setup and Solution Steady-State Flow Step 5: Boundary Conditions (continued) Problem Setup Boundary Conditions 2. Set the boundary conditions at the pressure outlet a) Select far-field under Boundary Conditions The Type will be reported as pressure-outlet b) Click Edit... to open the Pressure Outlet panel, and select Momentum tab i. Set the Gauge Pressure (pascal) to 100,000 ii. iii. Retain Normal to Boundary under Backflow Direction Specification Method Select Intensity and Viscosity Ratio under Turbulence Specification Method, and set Backflow Turbulent Intensity (%) = 1, and Viscosity Ratio = 2 c) Select Thermal tab in the Pressure Outlet panel i. Set Backflow Total Temperature (K) to 300 K Note: pressure-based coupled solver will be used in this simulation. Non-reflective outlet boundary condition option is not compatible with the pressure-based solver. To avoid spurious reflection of acoustic waves off the outlet boundary, the outlet is placed about 500 acoustic wavelengths away from the noise source, and a very coarse mesh with the mesh size Dx much larger than the acoustic wavelength L is applied in the far field (Dx / L = 25) to assure acoustic waves are fully dissipated by numerical viscosity before reaching the outlet boundary 2011 ANSYS, Inc. November 7,
17 Setup and Solution Steady-State Flow Step 5: Boundary Conditions (continued) Problem Setup Boundary Conditions 3. Set the boundary conditions at walls a) Select wall-back under Boundary Conditions The Type will be reported as wall b) Click Edit... to open the Wall panel, and select Momentum tab i. Select Specified Shear under Shear Condition, and set Shear Stress X- and Y- components to 0 Walls in this simulation are modeled as slip walls since the primary physics of screech noise generation is driven by free-stream jet flow structures, and wall turbulence does not contribute to the generation of screech noise c) Select Thermal tab in the Wall panel, and retain default settings of zero heat flux 2011 ANSYS, Inc. November 7,
18 Setup and Solution Steady-State Flow Step 5: Boundary Conditions (continued) Problem Setup Boundary Conditions 4. Copy setting for the wall-back to other walls a) Click Copy... below Boundary Conditions to open the Copy Conditions panel i. Select wall-back under From Boundary Zone ii. Select mic1, mic2, wall-lip and wall-lip-lam under To Boundary Zone, click Copy, and OK 2011 ANSYS, Inc. November 7,
19 Setup and Solution Steady-State Flow Step 6: Solution Methods Solution Solution Methods 1. Select Coupled under Pressure-Velocity Coupling Scheme This will activate pressure-based coupled solver 2. Select Green-Gauss Node Based under Gradient 3. Select Second Order under Pressure 4. Select QUICK for all other equations: Density, Momentum, Turbulent Kinetic Energy, Turbulent Dissipation Rate, and Energy 2011 ANSYS, Inc. November 7,
20 Setup and Solution Steady-State Flow Step 7: Solution Controls Solution Solution Controls 1. Set the Courant Number to Set the Explicit Relaxation Factors for Momentum and Pressure to Set Under-Relaxation Factor of 0.25 for Density 4. Retain default settings of Under-Relaxation Factors for other equations: Body Forces = 1.0 Turbulent Kinetic Energy = 0.8 Turbulent Dissipation Rate = 0.8 Turbulent Viscosity = 1.0 Energy = ANSYS, Inc. November 7,
21 Setup and Solution Steady-State Flow Step 8: Solution Initialization 1. Initialize the solution Solution Solution Initialization (a) Initialize the flow with values shown here Gauge Pressure (pascal) = 100,000 Axial Velocity (m/s) = 0 Radial Velocity (m/s) = 0 Turbulent Kinetic Energy (m2/s2) = 0.1 Turbulent Dissipation Rate (m2/s3) = 6 Temperature (K) = 300 (b) Click Initialize to initialize the solution 2011 ANSYS, Inc. November 7,
22 Setup and Solution Steady-State Flow Step 8: Solution Initialization (continued) 2. Run Full Multigrid (FMG) initialization (a) In the console window, which is also called Text User Interface (TUI), type: solve initialize set-fmg-initialization (b) Hit Enter on the keyboard to move down trough FMG settings. Change only: set FMG courant-number = 0.15 enable FMG verbose? yes (c) Run FMG initialization by typing in TUI: fmg-initialization yes This will provide an initial approximate solution (Figure 6) 3. Enable the plotting of residuals Solution Monitors Residuals Edit... (a) Select Plot and Print to Console under Options (b) Uncheck Check Convergence for all equations (c) Keep other setting at defaults, and click OK 2011 ANSYS, Inc. November 7, Figure 6. Contours of Mach number after FMG initialization 4. Write case and data files: run-screech-steady-fmg.cas.gz and run-screech-steady-fmg.dat.gz File Write Case & Data...
23 Setup and Solution Steady-State Flow Step 9: Steady-State Solution 1. Iterate the solution Solution Run Calculations (a) Set Number of Iterations to 200 and Calculate After 200 iterations, residuals will drop three orders of magnitude (Figure 7). Contours of converged steady-state Mach number distribution are shown in Figure 8 Note: it will take about 16 minutes of CPU time to finish the steady-state run on a single Windows processor. You can reduce the computing time requirements by skipping to Step ANSYS, Inc. November 7,
24 Setup and Solution Steady-State Flow Step 9: Steady-State Solution (continued) Figure 7. Convergence of residuals Figure 8. Contours of Mach number 2. Write case and data files: run-screech-steady.cas.gz and run-screech-steady.dat.gz File Write Case & Data ANSYS, Inc. November 7,
25 Setup and Solution Transient Flow Step 10: Transient Case Setup 1. Read in converged steady-state results from the previous step: run-screech-steady.cas.gz and run-screech-steady.dat.gz File Read Case & Data Change Time formulation to Transient in Problem Setup General 3. Change Transient Formulation to Second Order Implicit in Problem Setup Solution Methods 2011 ANSYS, Inc. November 7,
26 Setup and Solution Transient Flow Step 10: Transient Case Setup (continued) 4. Modify solution controls Solution Solution Controls (a) Set the Courant Number to 1e+15 (b) Set all other relaxation factors to 1.0 These are recommended Solution Controls settings when running transient pressure-based coupled solver Note: in the pressure-based coupled solver, the value 1/CFL, where CFL stands for Courant number, acts as an implicit relaxation factor for coupled continuity and momentum system of equations. Setting CFL to a very large number equals to removing implicit relaxation from the coupled equations 2011 ANSYS, Inc. November 7,
27 Setup and Solution Transient Flow Step 10: Transient Case Setup (continued) 5. Define Custom Field Function for pressure perturbations over its mean value: Define Custom Field Functions... (a) Select Pressure... and Static Pressure under Field Functions, and click Select (b) Click mouse pointer over keypad numbers to complete the function definition: p (c) Enter a new name pa under New Function Name, and click Define 2011 ANSYS, Inc. November 7,
28 Setup and Solution Transient Flow Step 10: Transient Case Setup (continued) 6. Enable the monitoring of static pressure perturbations at two microphone locations on the nozzle lip: Solution Monitors (a) Click Create... Under Surface Monitors (b) Change Name to mic1 (c) Select Area-Weighted Average under Report Type (d) Select Custom Field Functions... and pa under Field Variable (e) Select mic1 under Surface (f) Uncheck Print to Console and check Plot under Options (g) Check Write and specify File Name: mic1.out (h) Select Flow Time under X Axis (i) Select Get Data Every 1 Time Step (j) Click OK 2011 ANSYS, Inc. November 7,
29 Setup and Solution Transient Flow Step 10: Transient Case Setup (continued) (k) Repeat these steps to define the other monitor at mic2 surface: 2011 ANSYS, Inc. November 7,
30 Setup and Solution Transient Flow Step 10: Transient Case Setup (continued) 7. Set the time step parameters Solution Run Calculation (a) Set the Time Step Size (s) to 5e-6 (b) Set Number of Time Steps to 2000 (c) Set Max Iterations/Time Step to 10 Based on experimental data, expected fundamental screech tone frequency, f, is about 7 khz. Temporal discretization should provide 20 or more time steps per period of oscillation. This defines the maximum time step as Dt max = 1/(20*f) = 7.14e-06 sec 8. Write case and data files: run-screech-unsteady-0.00.cas.gz and run-screech-unsteady-0.00.dat.gz File Write Case & Data ANSYS, Inc. November 7,
31 Setup and Solution Transient Flow Step 11: Transient Run 1. Run the transient simulation Solution Run Calculation Click Calculate to time-march the solution to a time-periodic state The solution will advance to t = 0.01 sec by the end of the run 2. Write case and data files: run-screech-unsteady-0.01.cas.gz and run-screech-unsteady-0.01.dat.gz File Write Case & Data... Note: it will take about 26 hours of CPU time to finish the run on a single 32-bit Windows processor. You can reduce the computing time requirements considerably by skipping to Step 12 Parallel run on 8 compute 64-bit processors will take only 2.3 hours! 2011 ANSYS, Inc. November 7,
32 Setup and Solution Step 12: Aeroacoustic Postprocessing 1. Read in transient results from the previous step: run-screech-unsteady-0.01.cas.gz and run-screech-unsteady-0.01.dat.gz File Read Case & Data Display contours of Mach number: Results Graphics and Animations Contours (a) Select Contours of Velocity and Mach Number (b) Check Filled, Node Values, Global Range and Auto Range under Options (c) Click Display Display Views (a) Select axis and axis:001 under Mirror Planes (b) Click Apply (c) Zoom in to the region at the nozzle inlet (Figure 10b) 2011 ANSYS, Inc. November 7,
33 Setup and Solution Step 12: Aeroacoustic Postprocessing (continued) Figure 10a. Contours of Mach number: steady-state simulation Figure 10b. Contours of Mach number: transient simulation Note the difference between steady-state (Figure 10a) and transient (Figure 10b) Mach number distribution. Steady-state solution significantly suppresses the shock cell structure in the jet plume 2011 ANSYS, Inc. November 7,
34 Setup and Solution Step 12: Aeroacoustic Postprocessing (continued) 3. Display contours of static pressure perturbations: Results Graphics and Animations Contours (a) Select Contours of Custom Field Functions... and pa (b) Uncheck Global Range and set Min = -300 and Max = 300 (c) Uncheck Clip to Range and click Display sound waves Sound waves of the screech tone propagate predominantly in the upstream direction Figure 11. Contours of static pressure perturbations 2011 ANSYS, Inc. November 7,
35 Setup and Solution Step 12: Aeroacoustic Postprocessing (continued) 4. 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 mic1.out and mic2.out from the file list (b) Click OK to close the Select File panel 2011 ANSYS, Inc. November 7,
36 Setup and Solution Step 12: Aeroacoustic Postprocessing (continued) (c) Click Plot to display the microphone signals (Figure 12). Modify the line and marker styles as necessary, using the Curves panel. Modify the X axis to show the signal over the time rage of s. Modify legends using Change Legend Entry button in File XY Plot menu Figure 12. Acoustic pressure signals at two microphone locations on the nozzle lip 2011 ANSYS, Inc. November 7,
37 Setup and Solution Step 12: Aeroacoustic Postprocessing (continued) 5. Activate Ffowcs-Williams & Hawkings (FWH) acoustics model : Problem Setup Models Acoustics Edit... (a) Select Ffowcs-Williams & Hawkings under Model, retain default settings, and click OK This step is required only to make Sound Pressure Level available for FTT spectral analysis. However, FWH model will not be used to predict noise propagation 2011 ANSYS, Inc. November 7,
38 Setup and Solution Step 12: Aeroacoustic Postprocessing (continued) 6. Perform spectral analysis of the receiver signals: Results Plots FFT (a) Click Load Input Files..., change Files of Type to All Files in Select File window and select mic1.out (b) Select Sound Pressure Level (db) from the Y Axis Function drop-down list (c) Select Frequency (Hz) from the X Axis Function drop-down list 2011 ANSYS, Inc. November 7,
39 Setup and Solution Step 12: Aeroacoustic Postprocessing (continued) (d) Click Plot FFT to plot the sound pressure spectrum for mic1 (Figure 13) 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/[2Dt] = 100 khz, as expected. Figure 13. Spectral analysis of pressure signal for mic ANSYS, Inc. November 7,
40 Setup and Solution Step 12: Aeroacoustic Postprocessing (continued) (e) 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 iii. Set Precision to 0 iv. Click Apply and Close the panel 2011 ANSYS, Inc. November 7,
41 Setup and Solution Step 12: Aeroacoustic Postprocessing (continued) (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 Without clipping the temporal range, the complete pressure signal history would be analyzed including the initial transient state leading up to the quasiperiodic state ii. Click Apply/Plot and Close to return to the Fourier Transform panel 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 Setup and Solution Step 12: Aeroacoustic Postprocessing (continued) (g) Click Plot FFT to plot the sound pressure spectrum for mic1 (Figure 14a). The spectrum peaks at about 7000 Hz (h) Repeat above steps to plot the sound pressure spectrum for mic2 (Figure 14b) (a) screech tone (b) screech tone Figure 14. Spectral analysis of pressure signals at (a) mic1, and (b) mic2 microphone locations. Note: only the fundamental frequency of screech tones is resolved in this simulation, higher order harmonics are not resolved 2011 ANSYS, Inc. November 7,
43 Comparison with Test Data l/d j SPL (db) Screech tones of low supersonic jets are characterized by two axisymmetric screech modes A 1 and A 2. Mach numbers at which transition from one mode to another takes place may vary from experiment to experiment because of sensitivity of jet screech mechanism to specifics of experimental set-up. Figure 15a shows comparison of calculated screech wavelengths with experimental measurements. Numerically predicted wavelengths follow very closely the experimentally measured A 1 mode curve. Figure 15b shows favorable comparison between predicted and experimentally measured amplitudes of fundamental screech modes at two microphone locations at the nozzle lip. Note: Data points at other Mach numbers were obtained by re-running the tutorial cases with different pressure inlet settings A1 - experiment A2 - experiment A1 - CFD A M j Figure 15a. Wavelengths of fundamental screech modes 2011 ANSYS, Inc. November 7, microphone at r = 0.662" M j Figure 15b. Amplitudes of fundamental screech modes A1 - experiment A2 - experiment A1 - CFD
44 Summary This tutorial demonstrated the use of ANSY FLUENT's direct CAA capabilities to calculate near-field radiation of jet screech tones by an axisymmetric supersonic jet. You have learned how to set up the relevant parameters, record acoustic data at microphone locations, calculate, and postprocess the acoustic pressure signals. Calculated sound pressure level and frequency are in favorable agreement with experimental data. The main computational efforts are spent calculating the time dependent turbulent flow ANSYS, Inc. November 7,
Advanced ANSYS FLUENT Acoustics
Workshop Modeling Flow-Induced (Aeroacoustic) Noise 14.5 Release Advanced ANSYS FLUENT Acoustics 2011 ANSYS, Inc. November 7, 2012 1 Introduction This tutorial demonstrates how to model 2D turbulent flow
More informationCalculate 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 informationModeling 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 informationCompressible 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 informationSimulation 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 informationUsing 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 informationModeling 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 informationExpress 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 informationModeling 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 informationTutorial: 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 informationTransition 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 informationTutorial 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 informationModeling 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 informationNon-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 informationThis 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 informationTutorial 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 informationA 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 informationUse 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 informationSimulation 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 informationModeling 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 informationUsing 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 informationUsing 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 informationGrid. 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 informationTutorial: 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 informationSupersonic 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 informationUsing 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 informationTutorial: 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 informationAero-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 informationThe 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 informationLab 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 informationFlow 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 informationTutorial 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 informationExpress 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 informationThe 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 informationIntroduction 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 informationIntroduction 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 informationVerification 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 informationSimulation 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 informationSolution 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 informationSimulation 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 informationExpress 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 informationTutorial: 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 informationUsing 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 informationVerification 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 informationNear 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 informationVerification 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 informationSimulation 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 informationModule 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 informationNovember 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 informationExpress 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 informationTutorial: 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 informationTUTORIAL#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 informationLab 8: FLUENT: Turbulent Boundary Layer Flow with Convection
Lab 8: FLUENT: Turbulent Boundary Layer Flow with Convection Objective: The objective of this laboratory is to use FLUENT to solve for the total drag and heat transfer rate for external, turbulent boundary
More informationSTAR-CCM+ User Guide 6922
STAR-CCM+ User Guide 6922 Introduction Welcome to the STAR-CCM+ introductory tutorial. In this tutorial, you explore the important concepts and workflow. Complete this tutorial before attempting any others.
More informationIsotropic 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 informationc 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 informationTUTORIAL#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 informationWorkbench 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 informationProblem 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 informationANSYS AIM Tutorial Compressible Flow in a Nozzle
ANSYS AIM Tutorial Compressible Flow in a Nozzle Author(s): Sebastian Vecchi Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Pre-Analysis Start-Up Geometry Import Geometry Mesh
More informationNumerical and theoretical analysis of shock waves interaction and reflection
Fluid Structure Interaction and Moving Boundary Problems IV 299 Numerical and theoretical analysis of shock waves interaction and reflection K. Alhussan Space Research Institute, King Abdulaziz City for
More informationIntroduction To FLUENT. David H. Porter Minnesota Supercomputer Institute University of Minnesota
Introduction To FLUENT David H. Porter Minnesota Supercomputer Institute University of Minnesota Topics Covered in this Tutorial What you can do with FLUENT FLUENT is feature rich Summary of features and
More informationSimulation 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 informationCoupled Analysis of FSI
Coupled Analysis of FSI Qin Yin Fan Oct. 11, 2008 Important Key Words Fluid Structure Interface = FSI Computational Fluid Dynamics = CFD Pressure Displacement Analysis = PDA Thermal Stress Analysis = TSA
More informationMiddle 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 informationCold 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 informationThe 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 informationTutorial: 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 informationSimulation 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 informationSimulating 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 informationCOMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS
COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS Dr W. Malalasekera Version 3.0 August 2013 1 COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE
More informationCoupling 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 informationNumerical Analysis of a Blast Wave Using CFD-CAA Hybrid Method
Numerical Analysis of a Blast Wave Using CFD-CAA Hybrid Method In Cheol Lee * and Duck-Joo Lee. Korea Advanced Institute of Science and Technology, Daejeon, 305-701, Republic of Korea Sung Ho Ko and Dong
More informationMcNair Scholars Research Journal
McNair Scholars Research Journal Volume 2 Article 1 2015 Benchmarking of Computational Models against Experimental Data for Velocity Profile Effects on CFD Analysis of Adiabatic Film-Cooling Effectiveness
More informationRevolve 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 informationSolver 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 informationIntroduction to C omputational F luid Dynamics. D. Murrin
Introduction to C omputational F luid Dynamics D. Murrin Computational fluid dynamics (CFD) is the science of predicting fluid flow, heat transfer, mass transfer, chemical reactions, and related phenomena
More informationANSYS AIM Tutorial Flow over an Ahmed Body
Author(s): Sebastian Vecchi Created using ANSYS AIM 18.1 ANSYS AIM Tutorial Flow over an Ahmed Body Problem Specification Start Up Geometry Import Geometry Enclose Suppress Mesh Set Mesh Controls Generate
More informationFlat-Plate As stated earlier, the purpose of the flat-plate study was to create an opportunity for side-by-side comparison of ÒfastÓ RNG and
Chapter Six: Comparison of Turbulence Models Performance Comparisons There are a number of criteria by which to judge turbulence models. One criterion sometimes important to mathematicallyminded model
More informationSolidWorks Flow Simulation 2014
An Introduction to SolidWorks Flow Simulation 2014 John E. Matsson, Ph.D. SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following websites
More informationSimulation 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 informationFaculty of Mechanical and Manufacturing Engineering, University Tun Hussein Onn Malaysia (UTHM), Parit Raja, Batu Pahat, Johor, Malaysia
Applied Mechanics and Materials Vol. 393 (2013) pp 305-310 (2013) Trans Tech Publications, Switzerland doi:10.4028/www.scientific.net/amm.393.305 The Implementation of Cell-Centred Finite Volume Method
More informationFLUENT 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 informationS-ducts and Nozzles: STAR-CCM+ at the Propulsion Aerodynamics Workshop. Peter Burns, CD-adapco
S-ducts and Nozzles: STAR-CCM+ at the Propulsion Aerodynamics Workshop Peter Burns, CD-adapco Background The Propulsion Aerodynamics Workshop (PAW) has been held twice PAW01: 2012 at the 48 th AIAA JPC
More informationANSYS 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 informationAn Introduction to SolidWorks Flow Simulation 2010
An Introduction to SolidWorks Flow Simulation 2010 John E. Matsson, Ph.D. SDC PUBLICATIONS www.sdcpublications.com Schroff Development Corporation Chapter 2 Flat Plate Boundary Layer Objectives Creating
More informationCOMPUTATIONAL FLUID DYNAMICS USED IN THE DESIGN OF WATERBLAST TOOLING
2015 WJTA-IMCA Conference and Expo November 2-4 New Orleans, Louisiana Paper COMPUTATIONAL FLUID DYNAMICS USED IN THE DESIGN OF WATERBLAST TOOLING J. Schneider StoneAge, Inc. Durango, Colorado, U.S.A.
More informationFluent 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 informationPrerequisites: 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 informationInvestigation of mixing chamber for experimental FGD reactor
Investigation of mixing chamber for experimental FGD reactor Jan Novosád 1,a, Petra Danová 1 and Tomáš Vít 1 1 Department of Power Engineering Equipment, Faculty of Mechanical Engineering, Technical University
More informationStream Function-Vorticity CFD Solver MAE 6263
Stream Function-Vorticity CFD Solver MAE 66 Charles O Neill April, 00 Abstract A finite difference CFD solver was developed for transient, two-dimensional Cartesian viscous flows. Flow parameters are solved
More informationNUMERICAL 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 informationAxial Channel Water Jacket Cooling
28 November 2017 Motor-CAD Software Tutorial: Axial Channel Water Jacket Cooling Contents 1. Description... 1 2. Setting up the housing and axial channels... 2 3. Setting the water jacket fluid and flow
More informationAuto Injector Syringe. A Fluent Dynamic Mesh 1DOF Tutorial
Auto Injector Syringe A Fluent Dynamic Mesh 1DOF Tutorial 1 2015 ANSYS, Inc. June 26, 2015 Prerequisites This tutorial is written with the assumption that You have attended the Introduction to ANSYS Fluent
More informationWall thickness= Inlet: Prescribed mass flux. All lengths in meters kg/m, E Pa, 0.3,
Problem description Problem 30: Analysis of fluid-structure interaction within a pipe constriction It is desired to analyze the flow and structural response within the following pipe constriction: 1 1
More informationDevelopment of an Integrated Computational Simulation Method for Fluid Driven Structure Movement and Acoustics
Development of an Integrated Computational Simulation Method for Fluid Driven Structure Movement and Acoustics I. Pantle Fachgebiet Strömungsmaschinen Karlsruher Institut für Technologie KIT Motivation
More informationDYNAMIC ANALYSIS OF A GENERATOR ON AN ELASTIC FOUNDATION
DYNAMIC ANALYSIS OF A GENERATOR ON AN ELASTIC FOUNDATION 7 DYNAMIC ANALYSIS OF A GENERATOR ON AN ELASTIC FOUNDATION In this tutorial the influence of a vibrating source on its surrounding soil is studied.
More informationIntroduction to ANSYS SOLVER FLUENT 12-1
Introduction to ANSYS SOLVER FLUENT 12-1 Breadth of Technologies 10-2 Simulation Driven Product Development 10-3 Windshield Defroster Optimized Design 10-4 How Does CFD Work? 10-5 Step 1. Define Your Modeling
More informationEXPLICIT AND IMPLICIT TVD AND ENO HIGH RESOLUTION ALGORITHMS APPLIED TO THE EULER AND NAVIER-STOKES EQUATIONS IN THREE-DIMENSIONS RESULTS
EXPLICIT AND IMPLICIT TVD AND ENO HIGH RESOLUTION ALGORITHMS APPLIED TO THE EULER AND NAVIER-STOKES EQUATIONS IN THREE-DIMENSIONS RESULTS Edisson Sávio de Góes Maciel, edissonsavio@yahoo.com.br Mechanical
More informationModeling & Simulation of Supersonic Flow Using McCormack s Technique
Modeling & Simulation of Supersonic Flow Using McCormack s Technique M. Saif Ullah Khalid*, Afzaal M. Malik** Abstract In this work, two-dimensional inviscid supersonic flow around a wedge has been investigated
More information