Solution Recording and Playback: Vortex Shedding

Size: px
Start display at page:

Download "Solution Recording and Playback: Vortex Shedding"

Transcription

1 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. The particular scenario being modeled is that of incompressible water flowing over a cylinder with diameter D = 0.01 m. Under the correct conditions, vortices are formed and shed from the cylinder in a regular pattern. The free-stream velocity is 0.15 m/s and the flow is laminar with a Reynolds number (Re) of 75. A report, monitor and plot will be set up to display the lift forces acting on the cylinder. The predicted Strouhal number and shedding frequency can be determined from this graph and compared to results obtained by Daily et al.[216]. A 2D volume mesh of a simple cylinder in a fluid domain is provided for this tutorial, the dimensions of which are shown below. Prerequisites To complete this tutorial, you need to be familiar with the following techniques: Techniques Associated Tutorial The STAR-CCM+ workflow Introduction Using visualization tools, Introduction scenes and plots

2 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6664 Importing the Mesh Start up STAR-CCM+ in a manner that is appropriate to your working environment and create a New Simulation. Save the new simulation to disk with the file name vortexshedding.sim We will begin by importing the volume mesh. Select File > Import > Import Volume Mesh from the menu. The Open dialog will appear. Navigate to the /doc/tutorials/simpleflow subdirectory of your STAR-CCM+ installation directory and select vortexsheddingdomainmesh.ccm A geometry scene is automatically created after the mesh has been successfully imported. The boundaries have been pre-defined, so no further action is required. Create a mesh scene and examine the 2D mesh. Selecting Physics Models A physics continuum was added to the object tree when the volume mesh was imported. We will select the physics models required to run this case.

3 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6665 The fluid used in this tutorial is water, and the flow is incompressible and laminar. Vortex shedding is a periodic phenomenon and will require the use of a transient solver. Rename the Continua > Physics 1 continuum to Fluid. Right-click on the Fluid > Models node and choose Select models... The Fluid Model Selection dialog will guide you through the model selection process. Select the following models: Implicit Unsteady from the Time box. Liquid from the Material box. Coupled Flow from the Flow box. Constant Density from the Equation of State box. Laminar from the Viscous Regime box. Click Close. The selected models are shown in the Fluid > Models node in the object tree. Modifying Material Properties and Setting Initial Conditions Modify the material properties of water, so that the correct Reynolds number is obtained. Within the Fluid continuum, select the Models > Liquid > H2O > Material Properties > Density > Constant node and set its Value property to

4 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding kg/m^3 Select the Dynamic Viscosity > Constant node and set its Value property to 2.0E-5 Pa-s Set the initial conditions so that the simulation will begin with the fluid in a state of motion. Select the Fluid > Initial Conditions > Velocity > Constant node. In the Properties window, set the Value property to [0.15, 0.0, 0.0] m/s Setting Boundary Conditions Set the required velocity at the inlet boundary. Select the Regions > Fluid_Domain > Boundaries > Inlet > Physics Conditions > Velocity Specification node. In the Properties window,

5 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6667 set the Method property to Components. Select the Inlet > Physics Values > Velocity > Constant node and set its Value property to [0.15, 0.0, 0.0] m/s Save the simulation. Creating a Scalar Scene Create a scalar scene displaying vorticity. This will be used to visualize the solution while the simulation is running. Create a new scalar scene. Click on the scene/plot button located above the object tree.

6 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6668 Select the Displayers > Scalar 1 > Scalar Field node. In the Properties window set the Function property to Vorticity > Magnitude. In the same window, set the following properties: Property Value Min 0 Max 28 Clip Off Select the Displayers > Scalar 1 node. In the Properties window, set the Contour Style property to Smooth Filled. Click on the simulation button to return to the STAR-CCM+ simulation object tree. We will add an annotation displaying solution time to the scene. Expand the Tools > Annotations node and drag the Solution Time node

7 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6669 into the scene. The Solution Time annotation is added to the bottom left of the scene. Preparing the Lift Plot We will monitor the lift that the cylinder wall is experiencing. This will be used to determine the period of oscillation for the vortex shedding. First create a report: Right-click on the Reports node and select New Report > Force Coefficient. Rename the new plot to Coefficient of Lift. In the Properties window of the CoefficientofLift node, do the following: Set the Reference Velocity to 0.15 m/s Set the Reference Area to 0.01 m^2 Set the Force Option to Pressure. Set the Direction to [0.0, 1.0, 0.0] Click to the right of the Parts property. In the object selection dialog, tick

8 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6670 the checkbox next to Regions > Fluid_Domain > Cylinder. The completed Properties window is shown below. Create a monitor and plot from this report. Right-click on the CoefficientofLift node and select Create Monitor and Plot from Report.

9 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6671 A new monitor and plot is added to the Monitors and Plots nodes respectively. We will now modify the monitor so that the data is plotted against time; the default setting would plot the data against iterations. Select the Monitors > Coefficient of Lift Monitor node. In the Properties window, set the Trigger property to Time Step. Open the Coefficient of Lift Monitor Plot by right-clicking on its node in the object tree and selecting Open. Modifying Solver Settings Modify the solver settings to more appropriate values for this case.

10 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6672 Select the Solvers > Implicit Unsteady node. In the Properties window, set the Time-Step to 0.02 s In the same window, set the Temporal Discretization to 2nd-order. Select the Solvers > Coupled Implicit node and set its Courant Number property to 100 Setting Up Stopping Criteria Reduce the number of inner iterations for each time step and extend the maximum time the solver will be allowed to run. Select the Stopping Criteria > Maximum Inner Iterations node and set its Maximum Inner Iterations property to 15 Select the Stopping Criteria > Maximum Physical Time node and set its Maximum Physical Time property to 8 s Save the simulation Setting Up the Solution History File Create a new solution history (.simh) file and use it to store selected solution data at specified time intervals.

11 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6673 Right-click on the Solution Histories node and select New... The Save dialog appears. Choose a location where you would like to store the solution history file. Enter vortexsheddingdata.simh as the name of the solution history file. Click Save.

12 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6674 A new sub-node containing the name of the solution history file is added to the object tree below the Solution Histories node. The red asterisk next to this node means that data will be actively written to the file when the simulation runs. Choose what data to save to the solution history file. As this is a vortex shedding case it would be appropriate to store the results for pressure, velocity and vorticity. Select the Solution Histories > vortexsheddingdata node. In the Properties window, click on the (property customizer) button next to the Scalar Functions property. The Scalar Functions dialog appears. Use the > (Add selected) button to select the following items: Pressure Velocity

13 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6675 Vorticity The selections are added to the right-hand side column, as shown below. Click OK to close the dialog. Set the frequency with which the selected data will be written to the solution history file. We would like the data to be written every time step. Select the Solution Histories > vortexsheddingdata > Update node and set its Update Policy property to Time Step. Select the Update > Update Frequency node. In the Properties window,

14 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6676 ensure that the Number of Time Steps property is set to 1 Return to the Solution Histories > vortexsheddingdata node. A summary of the properties for the solution history file is shown in the Properties window. The Auto-record property will, when ticked, record the data to the solution history file at the required intervals. If you do not want to record the data when the solver is running, simply clear this checkbox. The Regions property is automatically populated with all regions in the simulation. In cases with multiple regions, you may remove regions by clicking to the right of the Regions property and clearing the checkbox next to the region you want to remove. The Path property displays the relative path to the simulation history file. The States property displays the number of saved states stored in the selected solution history file; currently this is displaying 0 as the solver has not yet run. Save the simulation. Running the Simulation The simulation is now ready to be run. Click on the (Run) button. While the simulation is running you can click on the tabs at the top of the Graphics window to switch between the plot and the scene. The Residuals display will be created automatically and shows the progress of the solvers. The simulation will continue until the physical time of the simulation reaches 8 seconds. While the simulation is running, the Current Solution sub-node under the Solution View node displays the current Iteration, Time Step, and Solution Time. The selected data is saved to the solution history file at every time step. While the simulation is running, select the Scalar Scene 1 tab at the top of the Graphics window to visualize the solution. When the simulation has finished running, click on the (Save) button.

15 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6677 Visualizing the Results The scalar scene after 8 s is shown below.

16 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6678 The Coefficient of Lift monitor plot is shown below. Validating the Results From the scalar scene and the monitor plot, it is clear that vortex shedding is occurring. The Strouhal number (St) is commonly used when describing oscillating flows and is defined as: fd St = U Where f is the frequency of vortex shedding, D is the cylinder diameter, and U is the free-stream velocity. In this case, the Strouhal number is given as 0.15 by Daily et al. [216]. The theoretical frequency of vortex shedding is therefore calculated as 2.25 Hz, which gives a period of seconds. The predicted period of shedding can be obtained by zooming into the last two troughs of the monitor plot. Click on the (Toggle Plot Zoom) button in the Plot toolbar.

17 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6679 Drag a box around the last two troughs on the plot, as shown below.

18 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6680 The resulting plot is shown below. Click on the scene/plot button. Select the Coefficient of Lift Monitor Plot > Axes > X Axis > Grid node. In the Properties window, set the Spacing property to 0.02 Click on the simulation button.

19 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6681 The enlarged scale on the X axis makes it possible to measure the period. The predicted period is shown to be approximately 0.44 seconds. Note that a relatively large time step was used for this tutorial resulting in a limited number of data points in the plot. If you want more accurate results and a smoother plot, the time step should be reduced. There is a difference of less than 1% between the predicted period and the reference period, which is good agreement for this case. The corresponding predicted frequency of 2.27 Hz is also in good agreement with the theoretical frequency of vortex shedding of 2.25 Hz. Creating a Recorded Solution View The solution history file contains all the data that was specified in the previous part of the tutorial. Solution views are used to interrogate this data and make it available for post-processing. Properties of the solution view set the point in the solution history at which data is read. Data is read into a separate representation linked to the solution view. Select the Solution Histories > vortexsheddingdata node. The number of

20 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6682 states stored in the solution history file is displayed next to the States property. 400 states are stored in the solution history file. We will create a solution view to access the states. Right-click on the Solution Histories > vortexsheddingdata node and select Create Recorded Solution View.

21 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6683 A new sub-node, vortexsheddingdata_view, is added to the Solution Views node. The properties of the solution view node control the data shown by the representation associated with it. An additional representation linked to this view was added to the object tree under the Representations node. This representation stores solution data from the solution history file. Click on the Scalar Scene 1 tab in the Graphics window. Drag and drop the Solution Views > vortexsheddingdata_view node onto a

22 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6684 blank area in the scene window.

23 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6685 The scene is shown below. This scene corresponds to the data stored in the solution history file for the first time step. We will now adjust the solution time to display the solution data at 1.3 seconds. Select the Solution Views > vortexsheddingdata_view node. In the Properties window, click to the right of the Solution Time property. A slider bar will appear. Here you can drag the slider to change the physical time of the solution being displayed in the scene.

24 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6686 Drag the slider so that the time is approximately 1.3 seconds. The scene will update as shown below. Values can also be entered rather than using the slider. Click to the right of the Solution Time property and enter 3 s

25 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6687 The updated scene is shown below. Restore the scene to use the most recent solution from the simulation file (stored on the volume mesh representation). Drag the Solution Views > Current Solution node into the scene as previously described. Save the simulation Creating an Animation from the Solution View We will now create an animation that will show the development of vortex shedding from the start to a regular periodic state. Drag the recorded solution view, Solution Views > vortexsheddingdata_view, back into the scene. Select the Solution Views > vortexsheddingdata_view > Animation node. In the Properties window, set the Animation Mode property to Solution Time.

26 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6688 A new node, Solution Time Animation, will appear below the Animation node. When creating an animation, it is important to set the correct framerate. If the framerate is set too high, the video may reuse identical frames. If the framerate is set too low, the video may appear to play too quickly. One way to determine the correct framerate is to divide the total number of states (frames) by the total physical time of the simulation. In this case we have 400 states and a physical time of 8 seconds. Knowing this, we can calculate that 50 frames make up one second of simulation time. We will now adjust the framerate for the animation. Click on the scene/plot button. Select the Scalar Scene 1 > Attributes > Animation node. In the Properties window, set the Target frame rate (fps) property to 50 We will now record the animation. Click on the (Write Movie) button in the Animation toolbar. The Write animation dialog appears. Set the Animation Length to 8 Set the Size to a resolution of your choice. Set the File Name to vorticityanimation.avi.

27 STAR-CCM+ User Guide Solution Recording and Playback: Vortex Shedding 6689 The completed dialog is shown below. Click Save to write the animation to disk. Play back the animation using a player of your choice. Summary This tutorial covered the following: Creating a Solution History file. Selecting appropriate scalars to save to the Solution History file at suitable intervals. Plotting the lift coefficient and validating the period of shedding against reference data. Creating a Recorded Solution View. Viewing recorded solution data in a scene. Recording an animation from the Solution History file. Bibliography [216] Daily, J.W., and Harleman, D.R.F. Fluid Dynamics, Addison-Wesley, MA, 1966

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

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

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

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

More information

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

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

More information

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

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

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

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

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

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

More information

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

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

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

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

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

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

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

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

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

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

More information

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

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

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

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

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

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

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

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

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

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

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

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

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

More information

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

ANSYS AIM Tutorial Steady Flow Past a Cylinder

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

More information

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

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

More information

Simulation of Turbulent Flow around an Airfoil

Simulation of Turbulent Flow around an Airfoil 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

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

Simulation of Turbulent Flow in an Asymmetric Diffuser

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

More information

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

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

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

More information

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

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

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

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

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

More information

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

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

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

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

Appendix: To be performed during the lab session

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

More information

Simulation 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

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

Shape optimisation using breakthrough technologies

Shape optimisation using breakthrough technologies Shape optimisation using breakthrough technologies Compiled by Mike Slack Ansys Technical Services 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Introduction Shape optimisation technologies

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

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

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

ANALYSIS OF VORTEX INDUCED VIBRATION USING IFS

ANALYSIS OF VORTEX INDUCED VIBRATION USING IFS ANALYSIS OF VORTEX INDUCED VIBRATION USING IFS Prateek Chaturvedi 1, Ruchira Srivastava 1, Sachin Agrawal 3, and Karan Puri 4 1 Department of MAE, Amity University, Greater Noida, India 3 Department of

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

Compressible Flow Modeling in STAR-CCM+

Compressible Flow Modeling in STAR-CCM+ Compressible Flow Modeling in STAR-CCM+ Version 01/11 Content Day 1 Compressible Flow WORKSHOP: High-speed flow around a missile WORKSHOP: Supersonic flow in a nozzle WORKSHOP: Airfoil 3 27 73 97 2 Compressible

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

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

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

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

More information

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

STAR-CCM+: Wind loading on buildings SPRING 2018

STAR-CCM+: Wind loading on buildings SPRING 2018 STAR-CCM+: Wind loading on buildings SPRING 2018 1. Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 3, 11 pm) 1. NOTES ON THE SOFTWARE STAR-CCM+ generates

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

OpenFOAM GUIDE FOR BEGINNERS

OpenFOAM GUIDE FOR BEGINNERS OpenFOAM GUIDE FOR BEGINNERS Authors This guide has been developed by: In association with: Pedro Javier Gamez and Gustavo Raush The Foam House Barcelona ETSEIAT-UPC June 2014 2 OPENFOAM GUIDE FOR BEGINNERS

More information

Flow Sim. Chapter 16. Airplane. A. Add-In. Step 1. If necessary, open your ASSEMBLY file.

Flow Sim. Chapter 16. Airplane. A. Add-In. Step 1. If necessary, open your ASSEMBLY file. Chapter 16 A. Add-In. Step 1. If necessary, open your ASSEMBLY file. Airplane Flow Sim Step 2. Click Tools Menu > Add-Ins. Step 3. In the dialog box, scroll down to Flow Simulation and place a check in

More information

Introduction to ANSYS CFX

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

More information

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

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

More information

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 12. F1 Car. A. Enable Flow Simulation. Step 1. If necessary, open your ASSEMBLY file.

Flow Sim. Chapter 12. F1 Car. A. Enable Flow Simulation. Step 1. If necessary, open your ASSEMBLY file. Chapter 12 F1 Car 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 and

More information

An Introduction to SolidWorks Flow Simulation 2010

An 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 information

Adjoint Solver Workshop

Adjoint Solver Workshop Adjoint Solver Workshop Why is an Adjoint Solver useful? Design and manufacture for better performance: e.g. airfoil, combustor, rotor blade, ducts, body shape, etc. by optimising a certain characteristic

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

Wall thickness= Inlet: Prescribed mass flux. All lengths in meters kg/m, E Pa, 0.3,

Wall 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 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

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

Terminal Falling Velocity of a Sand Grain

Terminal Falling Velocity of a Sand Grain Terminal Falling Velocity of a Sand Grain Introduction The first stop for polluted water entering a water work is normally a large tank, where large particles are left to settle. More generally, gravity

More information

SolidWorks Flow Simulation 2014

SolidWorks 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 information

RhinoCFD Tutorial. Flow Past a Sphere

RhinoCFD Tutorial. Flow Past a Sphere RhinoCFD Tutorial Flow Past a Sphere RhinoCFD Ocial document produced by CHAM September 26, 2017 Introduction Flow Past a Sphere This tutorial will describe a simple calculation of ow around a sphere and

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

In this problem, we will demonstrate the following topics:

In this problem, we will demonstrate the following topics: Z Periodic boundary condition 1 1 0.001 Periodic boundary condition 2 Y v V cos t, V 1 0 0 The second Stokes problem is 2D fluid flow above a plate that moves horizontally in a harmonic manner, schematically

More information

Design Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD)

Design Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD) Design Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD) Fernando Prevedello Regis Ataídes Nícolas Spogis Wagner Ortega Guedes Fabiano Armellini

More information

Advances in Cyclonic Flow Regimes. Dr. Dimitrios Papoulias, Thomas Eppinger

Advances in Cyclonic Flow Regimes. Dr. Dimitrios Papoulias, Thomas Eppinger Advances in Cyclonic Flow Regimes Dr. Dimitrios Papoulias, Thomas Eppinger Agenda Introduction Cyclones & Hydrocyclones Modeling Approaches in STAR-CCM+ Turbulence Modeling Case 1: Air-Air Cyclone Case

More information

Document Information

Document Information TEST CASE DOCUMENTATION AND TESTING RESULTS TEST CASE ID ICFD-VAL-3.1 Flow around a two dimensional cylinder Tested with LS-DYNA R v980 Revision Beta Friday 1 st June, 2012 Document Information Confidentiality

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

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

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

INSTED /CFD Post-Processor. Post-Processor. Chapter 5 INSTED /CFD (2D) Post-Processor

INSTED /CFD Post-Processor. Post-Processor. Chapter 5 INSTED /CFD (2D) Post-Processor INSTED /CFD Chapter 5 INSTED /CFD (2D) The part of INSTED/CFD (2D) plots lines or filled contours of variables such as velocities, temperature, pressure, scalars, and stream function. The program also

More information

Free Convection Cookbook for StarCCM+

Free Convection Cookbook for StarCCM+ ME 448/548 February 28, 2012 Free Convection Cookbook for StarCCM+ Gerald Recktenwald gerry@me.pdx.edu 1 Overview Figure 1 depicts a two-dimensional fluid domain bounded by a cylinder of diameter D. Inside

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

Stream Function-Vorticity CFD Solver MAE 6263

Stream 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 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

First Steps - Ball Valve Design

First Steps - Ball Valve Design COSMOSFloWorks 2004 Tutorial 1 First Steps - Ball Valve Design This First Steps tutorial covers the flow of water through a ball valve assembly before and after some design changes. The objective is to

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

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

Comparison Between Numerical & PIV Experimental Results for Gas-Solid Flow in Ducts

Comparison Between Numerical & PIV Experimental Results for Gas-Solid Flow in Ducts Fabio Kasper Comparison Between Numerical & PIV Experimental Results for Gas-Solid Flow in Ducts Rodrigo Decker, Oscar Sgrott Jr., Henry F. Meier Waldir Martignoni Agenda Introduction The Test Bench Case

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

Solved with COMSOL Multiphysics 4.0a. COPYRIGHT 2010 COMSOL AB.

Solved with COMSOL Multiphysics 4.0a. COPYRIGHT 2010 COMSOL AB. Journal Bearing Introduction Journal bearings are used to carry radial loads, for example, to support a rotating shaft. A simple journal bearing consists of two rigid cylinders. The outer cylinder (bearing)

More information

BioIRC solutions. CFDVasc manual

BioIRC solutions. CFDVasc manual BioIRC solutions CFDVasc manual Main window of application is consisted from two parts: toolbar - which consist set of button for accessing variety of present functionalities image area area in which is

More information