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

Size: px
Start display at page:

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

Transcription

1 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 the volume of fluid (VOF) multiphase model. The 6DOF UDF is used to calculate the motion of the moving body which also experiences a buoyancy force as it hits the water (modeled using the VOF model). Gravity and the bouyancy forces drive the motion of the body and the dynamic mesh. This tutorial demonstrates how to do the following: Use 6DOF solver to calculate motion of the moving body. Use VOF multiphase model to model the buoyancy force experienced by the moving body. Set up and solve the dynamic mesh case. Create TIFF files for graphic visualization of the solution. Postprocess the resulting data. Prerequisites This tutorial is written with the assumption that you have completed Tutorial 1 from ANSYS FLUENT 13.0 Tutorial Guide, and that you are familiar with the ANSYS FLUENT navigation pane and menu structure. Some steps in the setup and solution procedure will not be shown explicitly. In this tutorial, you will use the dynamic mesh model and the 6DOF model. If you have not used these models before, see Sections 11.3 Using Dynamic Meshes and Six DOF Solver Settings, respectively in the ANSYS FLUENT 13.0 User s Guide. Problem Description The schematic of the problem is shown in Figure 1. The tank is partially filled with water. A box is dropped into the water at time t = 0. The box is subjected to a viscous drag force and a gravitational force. When the box is immersed in water, it is also subjected to a buoyancy force. c ANSYS, Inc. November 24,

2 The walls of the box undergoes a rigid body motion and displaces according to the calculation performed by 6DOF solver. Whenever the box and its surrounding boundary layer mesh are displaced, the mesh outside the boundary layer is smoothed and/or remeshed. Figure 1: Schematic of the Problem Setup and Solution Preparation 1. Copy the files (6dof-mesh.msh.gz and 6dof 2d.c) to your working folder. 2. Create a subfolder (tiff-files) to store the tiff files for postprocessing purpose. 3. Use FLUENT Launcher to start the 2D version of ANSYS FLUENT. For more information about FLUENT Launcher see Section Starting ANSYS FLUENT Using FLUENT Launcher in ANSYS FLUENT 13.0 User s Guide. 4. Enable Double-Precision in the Options list. 5. Click the UDF Compiler tab and ensure that the Setup Compilation Environment for UDF is enabled. The path to the.bat file which is required to compile the UDF will be displayed as soon as you enable Setup Compilation Environment for UDF. If the UDF Compiler tab does not appear in the FLUENT Launcher dialog box by default, click the Show Additional Options >> button to view the additional settings. 2 c ANSYS, Inc. November 24, 2010

3 The Display Options are enabled by default. Therefore, after you read in the mesh, it will be displayed in the embedded graphics window. Step 1: Mesh 1. Read the mesh file (6dof-mesh.msh.gz). File Read Mesh... As the mesh file is read, ANSYS FLUENT will report the progress in the console. Step 2: General Settings 1. Define the solver settings. General Transient (a) Select Transient from the Time list. 2. Check the mesh (see Figure 2). General Check Figure 2: Mesh Display ANSYS FLUENT will perform various checks on the mesh and will report the progress in the console. Make sure the minimum volume reported is a positive number. c ANSYS, Inc. November 24,

4 Step 3: Models 1. Define the multiphase model. Models Multiphase Edit... (a) Select Volume of Fluid from the Model list to open Multiphase Model dialog box. (a) Ensure that Number of Eulerian Phases is set to 2. (b) Retain the default value of Courant Number. (c) Enable Implicit Body Force in the Body Force Formulation group box. (d) Click OK to close the Multiphase Model dialog box. 2. Enable the standard k-ɛ turbulence model. Models Viscous Edit... Step 4: User-Defined Functions Define User-Defined Functions Compiled... 4 c ANSYS, Inc. November 24, 2010

5 1. Click Add... for the Source Files. 2. Select 6dof 2d.c in the Select File dialog box. ANSYS FLUENT displays a Warning dialog box warning you to ensure that the UDF source files are in the same folder that contains the case and data files. Click OK. ANSYS FLUENT sets up the folder structure and compiles the code. The compilation is displayed in the console. 3. Click Load to load the UDF library. Step 5: Materials Materials Create/Edit Retain the properties of air. 2. Copy water-liquid (h2o<l>) from the FLUENT Database Modify the properties of water-liquid (h2o<l>). (a) Select user-defined from the Density drop-down list. i. Select water density::libudf from the User-Defined Functions dialog box. (b) Select user-defined from the Speed of Sound drop-down list. i. Select water speed of sound::libudf from the User-Defined Functions dialog box. (c) Click Change/Create and close the Create/Edit Materials dialog box. Step 6: Phases 1. Define the primary phase, water. Phases phase-1 Edit... c ANSYS, Inc. November 24,

6 (a) Enter water for Name. (b) Select water-liquid from the Phase Material drop-down list. (c) Click OK. 2. Similarly, define the secondary phase, air. Phases phase-2 Edit... 6 c ANSYS, Inc. November 24, 2010

7 Step 7: Boundary Conditions 1. Define the boundary conditions for tank outlet. Boundary Conditions tank outlet (a) Set the boundary conditions for the mixture phase. i. Ensure that mixture is selected from the Phase drop-down list and click Edit... ii. Select Intensity and Viscosity Ratio from the Specification Method drop-down list. iii. Enter 1% for Backflow Turbulence Intensity and 10 for Backflow Turbulent Viscosity Ratio. iv. Click OK to close the Pressure Outlet dialog box. (b) Set the boundary conditions for the air phase. i. Select air from the Phase drop-down list and click Edit... ii. Click the Multiphase tab and enter 1 for Backflow Volume Fraction. iii. Click OK to close the Pressure Outlet dialog box. Step 8: Operating Conditions Boundary Conditions Operating Conditions Retain pascal for Operating Pressure. 2. Enable Gravity. The dialog box expands to show additional inputs. 3. Enter m/s 2 for Gravitational Acceleration in the Y direction. c ANSYS, Inc. November 24,

8 4. Enable Specified Operating Density and retain the default setting of kg/m 3 for Operating Density. Step 9: Dynamic Mesh Setup 1. Set the dynamic mesh parameters. Dynamic Mesh (a) Enable Dynamic Mesh. (b) Enable Six DOF Solver. (c) Ensure that Smoothing is enabled. (d) Enable Remeshing from the Mesh Methods group box ans click Settings... i. Click Smoothing tab and set the Spring Constant Factor to 0.5. ii. Click Remeshing tab and set the remeshing parameters. 8 c ANSYS, Inc. November 24, 2010

9 A. Enter m for Minimum Length Scale and 0.13 m for Maximum Length Scale. The Minimum Length Scale and the Maximum Length Scale can be obtained from the Mesh Scale Info dialog box. Click on the Mesh Scale Info... button to open the Mesh Scale Info dialog box. B. Enter 0.5 for Maximum Cell Skewness. iii. Click OK to close Mesh Method Settings dialog box. Six DOF Solver Settings includes Gravitational Acceleration setting and the Write Motion History option. You already have set the Gravitational Acceleration in the Operating Conditions dialog box. If you want the motion history, enable Write Motion History and specify the File Name. c ANSYS, Inc. November 24,

10 2. Set up the moving zones. Dynamic Mesh (Dynamic Mesh Zones) Create/Edit... (a) Create the dynamic zone, moving box. i. Select moving box from the Zone Names drop-down list. ii. Ensure that Rigid Body is selected in the Type group box. iii. Ensure that test box::libudf is selected from the Six DOF UDF drop-down list. iv. Ensure that On is enabled in the Six DOF Solver Options group box. v. Click Create. ANSYS FLUENTwill create the dynamic zone moving box which will be available in the Dynamic Mesh Zones list. i. Similarly, create the dynamic zone, moving fluid by also enabling Passive from the Six DOF Solver Options group box. Ensure that you enable Passive from the Six DOF Solver Options group box. When Passive for the rigid body is enabled, ANSYS FLUENT does not take forces and moments on the zone into consideration. ANSYS FLUENTwill create the dynamic zone moving fluid which will be available in the Dynamic Mesh Zones list. 10 c ANSYS, Inc. November 24, 2010

11 (b) Close the Dynamic Mesh Zones dialog box. Step 10: Mesh Preview The purpose of the preview is to verify the quality of the mesh yielded by the mesh motion parameters. Since the flow is not initialized, the motion of the box will be vertical due to gravity. 1. Save the case file (6dof-init.cas.gz). File Write Case Display the mesh. Graphics and Animations Mesh Set Up Preview the motion. Dynamic Mesh Preview Mesh Motion... (a) Enter for Time Step Size. (b) Enter 1000 for Number of Time Steps. (c) Click Preview (see Figure 3). Figure 3: Mesh Motion at t = 0.5 s c ANSYS, Inc. November 24,

12 The motion is acceptable. (d) Close the Mesh Motion dialog box. 4. Exit ANSYS FLUENT without saving. Step 11: Solution 1. Start the 2D version of ANSYS FLUENT and read the case file (6dof-init.cas.gz). 2. Set the solution method parameters. Solution Methods (a) Ensure that SIMPLE is selected from the Scheme drop-down list. (b) Select Green-Gauss Node Based from the Gradient drop-down list. (c) Select Second Order Upwind for all the equations except Volume Fraction. (d) Retain the default discretization method of Geo-Reconstruct for Volume Fraction. 12 c ANSYS, Inc. November 24, 2010

13 3. Set the solution control parameters. Solution Controls (a) Enter 0.5 for Body Forces in the Under-Relaxation Factors group box. (b) Enter 0.8 for Turbulent Viscosity. (c) Retain the default values for other parameters. c ANSYS, Inc. November 24,

14 4. Initialize the solution. Solution Initialization (a) Enter m 2 /s 2 for Turbulent Kinetic Energy and m 2 /s 3 for Turbulent Dissipation Rate. (b) Enter 1 for air Volume Fraction. (c) Click Initialize. 5. Create an adaption register for patching. Adapt Region... (a) Set the Input Coordinates as follows: (b) Click Mark. (c) Close the Region Adaption dialog box. Parameters Values X Min (m), X Max (m) (-5, 5) Y Min (m), Y Max(m) (-5, -1.5) 14 c ANSYS, Inc. November 24, 2010

15 6. Patch the air volume fraction. Solution Initialization Patch... (a) Select air from the Phase drop-down list. (b) Select Volume Fraction from the Variable list. (c) Select hexahedron-r0 from the Registers to Patch list. (d) Retain 0 for Value. (e) Click Patch. (f) Close the Patch dialog box. 7. Enable the plotting of residuals. Monitors Residuals Edit... (a) Enter 400 for Iterations to Plot. (b) Click OK to close the Residual Monitors dialog box. c ANSYS, Inc. November 24,

16 8. Define a surface monitor for Y Velocity. Monitors (Surface Monitors) Create... (a) Enable Print to Console, Plot, and Write for surf-mon-1. (b) Retain the default setting of 2 for Window. (c) Enter 6dof yvel.out for File Name. (d) Select Flow Time from the X Axis drop-down list. (e) Select Time Step from the Every drop-down list. (f) Select Area-Weighted Average from the Report Type drop-down list. (g) Select Velocity... and Y Velocity from the Field Variable drop-down lists. (h) Select moving box from the Surfaces list and click OK to close the Surface Monitor dialog box. 16 c ANSYS, Inc. November 24, 2010

17 9. Set the auto save option. Calculation Activities (a) Enter 100 for Autosave Every (Time Steps) and click Edit... i. Enable Retain Only the Most Recent Files. ii. Set the Maximum Number of Data Files to 2. iii. Enter falling-box.gz for File Name. ANSYS FLUENTwill append the timestep number so that each file will have a unique filename. iv. Click OK to close the Autosave dialog box. 10. Save the hardcopy of display. File Save Picture... (a) Select TIFF from the Format list. (b) Ensure that Color is selected from the Coloring list. (c) Ensure that Raster is selected from the File Type list. (d) Enter 800 (pixels) for Width and 600 (pixels) for Height in the Resolution group box. (e) Click Apply and close the Save Picture dialog box. c ANSYS, Inc. November 24,

18 11. Execute commands for the animation setup. Calculation Activities (Execute Commands) Create/Edit... (a) Set the Defined Commands to 4. (b) Enable Active for all commands. (c) Enter 100 for Every and select Time Step from the When drop-down list. (d) Enter the commands as shown in the Execute Commands dialog box. Ensure to create the subfolder tiff-files before clicking the OK button. (e) Click OK to close the Execute Commands dialog box. 12. Display filled contour plots, enter the following command in the ANSYS FLUENT console. > display set contours filled-contours yes 13. Run the calculation. Run Calculation (a) Enter s for Time Step Size. (b) Enter for Number of Time Steps. (c) Set Max Iterations/Time Step to 50. (d) Click Calculate. Step 12: Postprocessing 1. Convert the TIFF files in the subfolder tiff-files to form an animation sequence for postprocessing purpose, using the software package like QuickTime or Fast Movie Player. The contours of volume fraction of water at different time steps are as shown in Figures 4 through c ANSYS, Inc. November 24, 2010

19 Figure 4: Contours at t = 0.25 s Figure 5: Contours at t = 0.5 s Figure 6: Contours at t = 0.75 s Figure 7: Contours at t = 1.0 s Figure 8: Contours t = 1.25 s Figure 9: Contours t = 1.5 s c ANSYS, Inc. November 24,

20 Figure 10: Contours at t = 1.75 s Figure 11: Contours at t = 2.0 s Figure 12: Contours of at t = 2.25 s Figure 13: Contours at t = 2.5 s Figure 14: Contours at t = 2.75 s Figure 15: Contours at t = 3.0 s 20 c ANSYS, Inc. November 24, 2010

21 Figure 16: Contours at t = 3.25 s Figure 17: Contours at t = 3.5 s Figure 18: Contours at t = 3.75 s Figure 19: Contours at t = 4.0 s Figure 20: Contours at t = 4.25 s Figure 21: Contours at t = 4.5 s c ANSYS, Inc. November 24,

22 Figure 22: Contours at t = 4.75 s Figure 23: Contours at t = 5.0 s Summary This tutorial demonstrated the setup and solution of a dynamic mesh case along with the 6DOF solver and the VOF multiphase model. The 6DOF UDF was used to calculate the motion of the box dropped into the water. The TIFF files created in the tutorial can be used to provide a graphic visualization of the solution. 22 c ANSYS, Inc. November 24, 2010

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: 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

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

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

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

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: 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

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

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

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

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: 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

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

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

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

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

Auto Injector Syringe. A Fluent Dynamic Mesh 1DOF Tutorial

Auto 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 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 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

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

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

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

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

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

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

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

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

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

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

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 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 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

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

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

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

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 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 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

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

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

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

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

Optimization of under-relaxation factors. and Courant numbers for the simulation of. sloshing in the oil pan of an automobile

Optimization of under-relaxation factors. and Courant numbers for the simulation of. sloshing in the oil pan of an automobile Optimization of under-relaxation factors and Courant numbers for the simulation of sloshing in the oil pan of an automobile Swathi Satish*, Mani Prithiviraj and Sridhar Hari⁰ *National Institute of Technology,

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

Advanced ANSYS FLUENT Acoustics

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 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

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

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

1 Thomas Chengattu MAE 494 November Project # 2: Transient Simulation using VOF Methods

1 Thomas Chengattu MAE 494 November Project # 2: Transient Simulation using VOF Methods 1 Thomas Chengattu Project # 2: Transient Simulation using VOF Methods INITIAL SET UP The initial set-up for all the geometries varied with respect to each tasks. The common similarities between these

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

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

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

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 02 Using the Discrete Phase Model (DPM)

Express Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM) Express Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM) Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry

More information

Workshop 3: Cutcell Mesh Generation. Introduction to ANSYS Fluent Meshing Release. Release ANSYS, Inc.

Workshop 3: Cutcell Mesh Generation. Introduction to ANSYS Fluent Meshing Release. Release ANSYS, Inc. Workshop 3: Cutcell Mesh Generation 14.5 Release Introduction to ANSYS Fluent Meshing 1 2011 ANSYS, Inc. December 21, 2012 I Introduction Workshop Description: CutCell meshing is a general purpose meshing

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

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

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 Training Seminar. Christopher Katinas July 21 st, 2017

FLUENT Training Seminar. Christopher Katinas July 21 st, 2017 FLUENT Training Seminar Christopher Katinas July 21 st, 2017 Motivation We want to know how to solve interesting problems without the need to build our own code from scratch GEMS has ~35 engineer-years

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

APPLIED COMPUTATIONAL FLUID DYNAMICS-PROJECT-3

APPLIED COMPUTATIONAL FLUID DYNAMICS-PROJECT-3 APPLIED COMPUTATIONAL FLUID DYNAMICS-PROJECT-3 BY SAI CHAITANYA MANGAVELLI Common Setup Data: 1) Mesh Proximity and Curvature with Refinement of 2. 2) Double Precision and second order for methods in Solver.

More information

Project 2 Solution. General Procedure for Model Setup

Project 2 Solution. General Procedure for Model Setup Project 2 Solution MAE598 Applied Computational Fluid Dynamics Shashank Kunjibettu General Procedure for Model Setup Step 1: Model the given component using design modeler Step 2: Meshing is done for the

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

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

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

SimCafe. ANSYS WB - Airfoil - Setup (Physics) Added by Benjamin J Mullen, last edited by Benjamin J Mullen on Apr 29, :18

SimCafe. ANSYS WB - Airfoil - Setup (Physics) Added by Benjamin J Mullen, last edited by Benjamin J Mullen on Apr 29, :18 Page 1 of 5 Search Cornell SimCafe Home Edit Browse/Manage Login Simulation > > ANSYS WB - Airfoil - Setup (Physics) Search ANSYS WB - Airfoil - Setup (Physics) Added by Benjamin J Mullen, last edited

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

CFD Simulation for Stratified Oil-Water Two-Phase Flow in a Horizontal Pipe

CFD Simulation for Stratified Oil-Water Two-Phase Flow in a Horizontal Pipe CFD Simulation for Stratified Oil-Water Two-Phase Flow in a Horizontal Pipe Adib Zulhilmi Mohd Alias, a, Jaswar Koto, a,b,* and Yasser Mohamed Ahmed, a a) Department of Aeronautics, Automotive and Ocean

More information

Offshore Platform Fluid Structure Interaction (FSI) Simulation

Offshore Platform Fluid Structure Interaction (FSI) Simulation Offshore Platform Fluid Structure Interaction (FSI) Simulation Ali Marzaban, CD-adapco Murthy Lakshmiraju, CD-adapco Nigel Richardson, CD-adapco Mike Henneke, CD-adapco Guangyu Wu, Chevron Pedro M. Vargas,

More information

EXPERIMENTAL VALIDATION OF STAR-CCM+ FOR LIQUID CONTAINER SLOSH DYNAMICS

EXPERIMENTAL VALIDATION OF STAR-CCM+ FOR LIQUID CONTAINER SLOSH DYNAMICS EXPERIMENTAL VALIDATION OF STAR-CCM+ FOR LIQUID CONTAINER SLOSH DYNAMICS Brandon Marsell a.i. solutions, Launch Services Program, Kennedy Space Center, FL 1 Agenda Introduction Problem Background Experiment

More information

Introduction to ANSYS SOLVER FLUENT 12-1

Introduction 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 information

RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent

RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent Gilles Eggenspieler Senior Product Manager 1 Morphing & Smoothing A mesh morpher is a tool capable of performing mesh modifications in order

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

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

Repairing a Boundary Mesh

Repairing a Boundary Mesh Tutorial 1. Repairing a Boundary Mesh Introduction TGrid offers several tools for mesh repair. While there is no right or wrong way to repair a mesh, the goal is to improve the quality of the mesh with

More information

Automotive Fluid-Structure Interaction (FSI) Concepts, Solutions and Applications. Laz Foley, ANSYS Inc.

Automotive Fluid-Structure Interaction (FSI) Concepts, Solutions and Applications. Laz Foley, ANSYS Inc. Automotive Fluid-Structure Interaction (FSI) Concepts, Solutions and Applications Laz Foley, ANSYS Inc. Outline FSI Classifications FSI Solutions FSI Modeling Approaches ANSYS Workbench for FSI System

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

Project #3 MAE 598 Applied CFD

Project #3 MAE 598 Applied CFD Project #3 MAE 598 Applied CFD 16 November 2017 H.P. Huang 1 Task 1 (a) Task 1a was to perform a transient analysis of a 2-D chamber that is initially filled with air, and has water flowing through the

More information

Stratified Oil-Water Two-Phases Flow of Subsea Pipeline

Stratified Oil-Water Two-Phases Flow of Subsea Pipeline Stratified Oil-Water Two-Phases Flow of Subsea Pipeline Adib Zulhilmi Mohd Alias, a, Jaswar Koto, a,b,*, Yasser Mohamed Ahmed, a and Abd Khair Junaidi, b a) Department of Aeronautics, Automotive and Ocean

More information

Dam removed at start of analysis. Air g = 9.8. Water SI units used. Water: Air: = 10, = Slip walls are used to model the basin.

Dam removed at start of analysis. Air g = 9.8. Water SI units used. Water: Air: = 10, = Slip walls are used to model the basin. Problem description It is desired to analyze the motion of water within a basin. Initially, the basin contains a dam, and the water is confined by the dam as shown. At the start of the analysis, the dam

More information

SIMULATION OF PROPELLER-SHIP HULL INTERACTION USING AN INTEGRATED VLM/RANSE SOLVER MODELING.

SIMULATION OF PROPELLER-SHIP HULL INTERACTION USING AN INTEGRATED VLM/RANSE SOLVER MODELING. SIMULATION OF PROPELLER-SHIP HULL INTERACTION USING AN INTEGRATED VLM/RANSE SOLVER MODELING. M.N.Senthil Prakash, Department of Ocean Engineering, IIT Madras, India V. Anantha Subramanian Department of

More information

CFD VALIDATION FOR SURFACE COMBATANT 5415 STRAIGHT AHEAD AND STATIC DRIFT 20 DEGREE CONDITIONS USING STAR CCM+

CFD VALIDATION FOR SURFACE COMBATANT 5415 STRAIGHT AHEAD AND STATIC DRIFT 20 DEGREE CONDITIONS USING STAR CCM+ CFD VALIDATION FOR SURFACE COMBATANT 5415 STRAIGHT AHEAD AND STATIC DRIFT 20 DEGREE CONDITIONS USING STAR CCM+ by G. J. Grigoropoulos and I..S. Kefallinou 1. Introduction and setup 1. 1 Introduction The

More information

NaysEddy ver 1.0. Example MANUAL. By: Mohamed Nabi, Ph.D. Copyright 2014 iric Project. All Rights Reserved.

NaysEddy ver 1.0. Example MANUAL. By: Mohamed Nabi, Ph.D. Copyright 2014 iric Project. All Rights Reserved. NaysEddy ver 1.0 Example MANUAL By: Mohamed Nabi, Ph.D. Copyright 2014 iric Project. All Rights Reserved. Contents Introduction... 3 Getting started... 4 Simulation of flow over dunes... 6 1. Purpose of

More information

Ryian Hunter MAE 598

Ryian Hunter MAE 598 Setup: The initial geometry was produced using the engineering schematics provided in the project assignment document using the ANSYS DesignModeler application taking advantage of system symmetry. Fig.

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

Introduction to ANSYS FLUENT Meshing

Introduction to ANSYS FLUENT Meshing Workshop 04 CAD Import and Meshing from Conformal Faceting Input 14.5 Release Introduction to ANSYS FLUENT Meshing 2011 ANSYS, Inc. December 21, 2012 1 I Introduction Workshop Description: CAD files will

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

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

Heat transfer and Transient computations

Heat transfer and Transient computations Lecture Heat transfer and Transient computations 12-1 Introduction to TRANSIENT calculation 10-2 Motivation Nearly all flows in nature are transient! Steady-state assumption is possible if we: Ignore transient

More information

Workbench Tutorial Flow Over an Airfoil, Page 1 ANSYS Workbench Tutorial Flow Over an Airfoil

Workbench Tutorial Flow Over an Airfoil, Page 1 ANSYS Workbench Tutorial Flow Over an Airfoil Workbench Tutorial Flow Over an Airfoil, Page 1 ANSYS Workbench Tutorial Flow Over an Airfoil Authors: Scott Richards, Keith Martin, and John M. Cimbala, Penn State University Latest revision: 17 January

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

Swapnil Nimse Project 1 Challenge #2

Swapnil Nimse Project 1 Challenge #2 Swapnil Nimse Project 1 Challenge #2 Project Overview: Using Ansys-Fluent, analyze dependency of the steady-state temperature at different parts of the system on the flow velocity at the inlet and buoyancy-driven

More information

Flow Sim. Chapter 16. Airplane. A. Enable Flow Simulation. Step 1. If necessary, open your ASSEMBLY file.

Flow Sim. Chapter 16. Airplane. A. Enable Flow Simulation. Step 1. If necessary, open your ASSEMBLY file. Chapter 16 Airplane Flow Sim A. Enable Flow Simulation. Step 1. If necessary, open your ASSEMBLY file. Step 2. If necessary, turn on Flow Simulation, click the flyout of Options on the Standard toolbar

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

STAR-CCM+ User Guide 6922

STAR-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 information

Kratos Multi-Physics 3D Fluid Analysis Tutorial. Pooyan Dadvand Jordi Cotela Kratos Team

Kratos Multi-Physics 3D Fluid Analysis Tutorial. Pooyan Dadvand Jordi Cotela Kratos Team Kratos Multi-Physics 3D Fluid Analysis Tutorial Pooyan Dadvand Jordi Cotela Kratos Team Kratos 3D Fluid Tutorial In this tutorial we will solve a simple example using GiD and Kratos Geometry Input data

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

Flow Sim. Chapter 14 P-51. A. Set Up. B. Create Flow Simulation Project. Step 1. Click Flow Simulation. SolidWorks 10 Flow Sim P-51 Page 14-1

Flow Sim. Chapter 14 P-51. A. Set Up. B. Create Flow Simulation Project. Step 1. Click Flow Simulation. SolidWorks 10 Flow Sim P-51 Page 14-1 Chapter 14 A. Set Up. P-51 Flow Sim Step 1. If necessary, open your ASSEMBLY file. Step 2. Click Tools Menu > Add-Ins. Step 3. In the dialog box, scroll down to Flow Simulation and place a check in the

More information