Revolve 3D geometry to display a 360-degree image.
|
|
|
- Helen Hunt
- 6 years ago
- Views:
Transcription
1 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 the calculation) and perform a number of turbomachinery-specific postprocessing operations. This tutorial demonstrates how to do the following: Define the topology of a turbomachinery model. Create surfaces for the display of 3D data. Revolve 3D geometry to display a 360-degree image. Report turbomachinery quantities. Display averaged contours for turbomachinery. Display 2D contours for turbomachinery. Display averaged XY plots for turbomachinery. Prerequisites This tutorial assumes that you are familiar with the menu structure in FLUENT and that you have completed Tutorial 1. Some steps in the setup and solution procedure will not be shown explicitly. c Fluent Inc. September 21,
2 Problem Description The problem considered in this tutorial is a centrifugal compressor shown schematically in Figure The model comprises a single 3D sector of the compressor to take advantage of the circumferential periodicity in the problem. The flow of air through the compressor is simulated and the postprocessing capabilities of FLUENT are used to display realistic, full 360-degree images of the solution obtained. inlet shroud side hub side outlet Figure 24.1: Problem Schematic 24-2 c Fluent Inc. September 21, 2006
3 Setup and Solution Preparation 1. Download turbo_postprocess.zip from the Fluent Inc. User Services Center or copy it from the FLUENT documentation CD to your working folder (as described in Tutorial 1). 2. Unzip turbo_postprocess.zip. turbo.cas and turbo.dat can be found in the turbo postprocess folder created after unzipping the file. 3. Start the 3D (3d) version of FLUENT. Step 1: Reading the Case and Data Files 1. Read the case and data files (turbo.cas and turbo.dat). File Read Case & Data... When you select turbo.cas, turbo.dat will be read automatically. Step 2: Grid Display 1. Display the grid (Figure 24.2). Display Grid... (a) Retain the default Edges option in the Options group box. c Fluent Inc. September 21,
4 (b) Select Outline in the Edge Type list. (c) Deselect all the surfaces from the Surfaces selection list and click the Outline button (below the Surface Types list). (d) Click Display. (e) Rotate the view using the left mouse button and zoom in using the middle mouse button, to obtain an isometric display of the compressor duct. Y X Z Grid FLUENT 6.3 (3d, dbns imp, rke) Figure 24.2: Graphics Display of the Edges of the Compressor Mesh (f) Close the Grid Display panel. Extra: You can use the right mouse button to check which zone number corresponds to each boundary. If you click the right mouse button on one of the boundaries displayed in the graphics window, its zone number, name, and type will be printed in the console. This feature is especially useful when you have several zones of the same type and you want to distinguish between them quickly c Fluent Inc. September 21, 2006
5 Step 3: Defining the Turbomachinery Topology You will define the topology of the flow domain in order to establish a turbomachineryspecific coordinate system. This coordinate system is used in subsequent postprocessing functions. Specifically, you will select the boundary zones that comprise the hub, shroud, inlet, outlet, and periodics. The boundaries may consist of more than one zone. The topology setup that you define will be saved to the case file when you save the current model. Thus, if you read the saved case back into FLUENT, you do not need to set up the topology again. See Section of the User s Guide for more information on defining turbomachinery topologies. Define Turbo Topology Specify the surfaces representing the hub. (a) Retain the default selection of Hub in the Boundaries list. (b) Select the surfaces that represent the hub (wall-diffuser-hub, wall-hub, and wall-inlet-hub) in the Surfaces selection list. Hint: Scroll down the Surfaces list to locate the surfaces representing the hub. 2. Specify the surfaces representing the casing. (a) Select Casing in the Boundaries list. c Fluent Inc. September 21,
6 (b) Select wall-diffuser-shroud, wall-inlet-shroud, and wall-shroud in the Surfaces selection list. 3. Specify the surfaces representing the periodic boundaries. (a) Select Theta Periodic in the Boundaries list. (b) Select periodic.33, periodic.34, and periodic.35 in the Surfaces selection list. Note: While Theta Periodic represents periodic boundary zones on the circumferential boundaries of the flow passage, Theta Min and Theta Max are wall surfaces at the minimum and maximum θ position on a circumferential boundary. There are no such wall surfaces in this problem. 4. Specify the surface representing the Inlet (inlet). 5. Specify the surface representing the Outlet (outlet). 6. Specify the surface representing the Blade (wall-blade). 7. Retain the default name of new-topology-1 for the Turbo Topology Name. 8. Click Define to set all the turbomachinery boundaries. 9. Close the Turbo Topology panel. FLUENT will inform you that the turbomachinery postprocessing functions have been enabled, and the Turbo menu will appear in FLUENT menu bar at the top of the console. You can define any number of turbo topologies in the Turbo Topology panel. This is especially useful when you have a model comprising multiple blade rows and you need to define more than one blade row simultaneously. Each topology can be assigned a specific name and accessed using the drop-down list in the Turbo Topology panel. See Section of the User s Guide for more information on defining turbomachinery topologies. Note: You can display the selected surfaces by clicking the Display button in the Turbo Topology panel. This is useful as a graphical check to ensure that all relevant surfaces have been selected c Fluent Inc. September 21, 2006
7 Step 4: Isosurface Creation To display results in a 3D model, you will need surfaces on which the data can be displayed. FLUENT creates surfaces for all boundary zones automatically. In a general application, you may want to define additional surfaces for viewing results. FLUENT s turbo postprocessing capabilities allow you to define more complex surfaces, specific to the application and the particular topology that you defined. In this step, you will create surfaces of iso-meridional (marching along the streamwise direction) and spanwise (distance between the hub and the shroud) coordinates in the compressor. 1. Create surfaces of constant meridional coordinate. Surface Iso-Surface... (a) Select Grid... and Meridional Coordinate from the Surface of Constant dropdown lists. (b) Enter 0.2 in the Iso-Values text field. (c) Enter meridional-0.2 for New Surface Name. (d) Click Create. Note: The isovalues you enter for these turbo-specific surfaces are expressed as a percentage of the entire domain (i.e., you just defined a surface of meridional coordinate equal to 20% of the path along the duct). (e) Similarly, define surfaces of meridional coordinates equal to 0.4, 0.6, and 0.8. c Fluent Inc. September 21,
8 2. Create surfaces of constant spanwise coordinate. (a) Select Grid... and Spanwise Coordinate from the Surface of Constant drop-down lists. (b) Enter 0.25 in the Iso-Values text field. (c) Enter spanwise-0.25 for New Surface Name. (d) Click Create. (e) Similarly, define surfaces of spanwise coordinates equal to 0.5 and Close the Iso-Surface panel c Fluent Inc. September 21, 2006
9 Step 5: Contours 1. Display filled contours of pressure on the meridional isosurfaces (Figure 24.3). Display Contours... (a) Enable Filled in the Options group box. (b) Select Pressure... and Static Pressure from the Contours of drop-down lists. (c) Select inlet, meridional-0.2, meridional-0.4, meridional-0.6, meridional-0.8, and outlet from the Surfaces selection list. (d) Enable Draw Grid in the Options group box. The Grid Display panel will open. i. Retain the current settings and close the Grid Display panel. (e) Click Display. (f) Rotate and zoom the display using the left and middle mouse buttons, respectively, to obtain the view shown in Figure In Figure 24.3, you can observe the buildup of static pressure along the duct. 2. Display filled contours of Mach number (Figure 24.4). (a) Select Velocity... and Mach Number from the Contours of drop-down lists. (b) Click Display. In Figure 24.4, you can observe locations at which the flow becomes slightly supersonic, about halfway through the duct. c Fluent Inc. September 21,
10 1.84e e e e e e e e e e e e e e e e e e e e e-01 X Y Z Contours of Static Pressure (atm) FLUENT 6.3 (3d, dbns imp, rke) Figure 24.3: Filled Contours of Pressure on the Meridional Isosurfaces 1.04e e e e e e e e e e e e e e e e e e e e e-02 X Y Z Contours of Mach Number FLUENT 6.3 (3d, dbns imp, rke) Figure 24.4: Filled Contours of Mach Number on the Meridional Isosurfaces c Fluent Inc. September 21, 2006
11 3. Display filled contours of Mach number on the spanwise isosurfaces (Figure 24.5). (a) Deselect all surfaces in the Surfaces selection list. (b) Select spanwise-0.25, spanwise-0.5, and spanwise-0.75 from the Surfaces selection list. (c) Click Display. 1.04e e e e e e e e e e e e e e e e e e e e-02 X 3.05e-02 Y Z Contours of Mach Number FLUENT 6.3 (3d, dbns imp, rke) Figure 24.5: Filled Contours of Mach Number on the Spanwise Isosurfaces The display in Figure 24.5 allows you to further study the variation of the Mach number inside the duct. You may want to explore using different combinations of surfaces to display the same or additional variables. 4. Display a 360-degree image of the Mach number contours on the 0.5 spanwise isosurface (Figure 24.6). (a) Deselect spanwise-0.25 and spanwise-0.75 from the Surfaces selection list. (b) Click Display. c Fluent Inc. September 21,
12 (c) Display the full 360-degree geometry. Display Views... i. Click the Define... button to open the Graphics Periodicity panel. A. Select fluid in the Cell Zones list. This will select all the surfaces in the Associated Surfaces list. The default value for Number of Repeats is set to 20. The display is updated to give a full, 360 degree view. B. Click Set and close the Graphics Periodicity panel. The display will be updated to show the entire geometry (see Figure c Fluent Inc. September 21, 2006
13 Turbo Postprocessing 1.04e e e e e e e e e e e e e e e e e e e e-02 Y 3.05e-02 X Z Contours of Mach Number FLUENT 6.3 (3d, dbns imp, rke) Figure 24.6: Filled Contours of Mach Number on the 0.5 Spanwise Isosurface ii. Close the Views panel. 5. Close the Contours panel. Note: This step demonstrated a typical view-manipulation task. See Tutorial 23 for further examples of postprocessing features. c Fluent Inc. September 21,
14 Step 6: Reporting Turbo Quantities The turbomachinery report provides some tabulated information specific to the application and the defined topology. See Section of the User s Guide for details. Turbo Report Retain the default selection of Mass-Weighted in the Averages list. 2. Click Compute. 3. Close the Turbo Report panel c Fluent Inc. September 21, 2006
15 Step 7: Averaged Contours Turbo averaged contours are generated as projections of the values of a variable averaged in the circumferential direction and visualized on an r- z plane. 1. Disable the periodic repeats. Display Views... (a) Click the Define... button to open the Graphics Periodicity panel. i. Click Reset. ii. Close the Graphics Periodicity panel. (b) Close the Views panel. 2. Display filled contours of averaged static pressure (Figure 24.7). Turbo Averaged Contours... (a) Select Pressure... and Static Pressure from the Contours of drop-down lists. (b) Click Display. (c) Close the Turbo Averaged Contours panel. c Fluent Inc. September 21,
16 1.80e e e e e e e e e e e e e e e e e e e e e-01 Y Z X Averaged Turbo Contour - pressure (atm) (atm) FLUENT 6.3 (3d, dbns imp, rke) Figure 24.7: Filled Contours of Averaged Static Pressure Step 8: 2D Contours In postprocessing a turbomachinery solution, it is often preferable to display contours on constant spanwise coordinates and then, project these contours onto a plane. This permits easier evaluation of the contours, especially for surfaces that are highly threedimensional. FLUENT allows you to display contours in this manner using the Turbo 2D Contours panel. 1. Display 2D contours of Mach number (Figure 24.8). Turbo 2D Contours c Fluent Inc. September 21, 2006
17 (a) Select Velocity... and Mach Number from the Contours of drop-down lists. (b) Enter 0.5 for Normalised Spanwise Coordinates. Note: For highly curved edges, if a surface is created very close to the curved edge the resulting surface may have some void spaces in it. (c) Click Display. (d) Use the mouse to obtain the view shown in Figure e e e e e e e e e e e e e e e e e e e e e-02 Z Y X 2D Turbo Contour - mach-number FLUENT 6.3 (3d, dbns imp, rke) Figure 24.8: 2D Contours of Mach Number on Surface of Spanwise Value 0.5 (e) Close the Turbo 2D Contours panel. c Fluent Inc. September 21,
18 Step 9: Averaged XY Plots In addition to displaying data on different combinations of complex 3D and flattened surfaces, FLUENT s turbo postprocessing capabilities allow you to display XY plots of averaged variables, relevant to the specific topology of a turbomachinery problem. In particular, you will be able to plot circumferentially-averaged values of variables as a function of either the spanwise coordinate or the meridional coordinate. 1. Plot temperature as a function of the meridional coordinate (Figure 24.9). Turbo Averaged XY Plot... (a) Select Temperature... and Static Temperature from the Y Axis Function dropdown lists. (b) Select Meridional Distance from the X Axis Function drop-down list. (c) Enter 0.9 for the Fractional Distance. (d) Click Plot. (e) Close the Turbo Averaged XY Plot panel c Fluent Inc. September 21, 2006
19 3.50e e e+02 Static Temperature (k) 3.20e e e e e X Meridional Distance Z Y Averaged XY - temperature FLUENT 6.3 (3d, dbns imp, rke) Figure 24.9: Averaged XY Plot of Static Temperature on Spanwise Surface of 0.9 Isovalue Summary This tutorial demonstrated the use of some of the turbomachinery-specific postprocessing features of FLUENT. These features can be accessed once you define the topology of the problem. More extensive general-purpose postprocessing features are demonstrated in Tutorial 23. Also, see Chapter 28 and Chapter 29 of the User s Guide for additional information. c Fluent Inc. September 21,
20 24-20 c Fluent Inc. September 21, 2006
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
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
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
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
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
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
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
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
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
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
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
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
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
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
8. BASIC TURBO MODEL WITH UNSTRUCTURED MESH
8. BASIC TURBO MODEL WITH UNSTRUCTURED MESH This tutorial employs a simple turbine blade configuration to illustrate the basic turbo modeling functionality available in GAMBIT. It illustrates the steps
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
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
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
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
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
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
Chapter 24. Creating Surfaces for Displaying and Reporting Data
Chapter 24. Creating Surfaces for Displaying and Reporting Data FLUENT allows you to select portions of the domain to be used for visualizing the flow field. The domain portions are called surfaces, and
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
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
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
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
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
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.
ANSYS AIM Tutorial Compressible Flow in a Nozzle
ANSYS AIM Tutorial Compressible Flow in a Nozzle Author(s): Sebastian Vecchi Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Pre-Analysis Start-Up Geometry Import Geometry Mesh
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
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
Using the Boundary Wrapper
Tutorial 7. Using the Boundary Wrapper Introduction Geometries imported from various CAD packages often contain gaps and/or overlaps between surfaces. Repairing such geometries manually is a tedious and
2. MODELING A MIXING ELBOW (2-D)
MODELING A MIXING ELBOW (2-D) 2. MODELING A MIXING ELBOW (2-D) In this tutorial, you will use GAMBIT to create the geometry for a mixing elbow and then generate a mesh. The mixing elbow configuration is
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
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
Viscous Hybrid Mesh Generation
Tutorial 4. Viscous Hybrid Mesh Generation Introduction In cases where you want to resolve the boundary layer, it is often more efficient to use prismatic cells in the boundary layer rather than tetrahedral
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.
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
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
ANSYS AIM Tutorial Fluid Flow Through a Transition Duct
ANSYS AIM Tutorial Fluid Flow Through a Transition Duct Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Start Up Geometry Import Geometry Extracting Volume Suppress
Turbocharger Design & Analysis Solutions. Bill Holmes Brad Hutchinson Detroit, October 2012
Turbocharger Design & Analysis Solutions Bill Holmes Brad Hutchinson Detroit, October 2012 Agenda ANSYS overview ANSYS TurboSystem Blade row solutions The ANSYS Transformation methods An example: turbocharger
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
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
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,
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
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
Advances in Turbomachinery Simulation Fred Mendonça and material prepared by Chad Custer, Turbomachinery Technology Specialist
Advances in Turbomachinery Simulation Fred Mendonça and material prepared by Chad Custer, Turbomachinery Technology Specialist Usage From Across the Industry Outline Key Application Objectives Conjugate
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
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
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
Flow and Heat Transfer in a Mixing Elbow
Flow and Heat Transfer in a Mixing Elbow Objectives The main objectives of the project are to learn (i) how to set up and perform flow simulations with heat transfer and mixing, (ii) post-processing and
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
Backward facing step Homework. Department of Fluid Mechanics. For Personal Use. Budapest University of Technology and Economics. Budapest, 2010 autumn
Backward facing step Homework Department of Fluid Mechanics Budapest University of Technology and Economics Budapest, 2010 autumn Updated: October 26, 2010 CONTENTS i Contents 1 Introduction 1 2 The problem
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
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
HYDRAULIC DEVELOPMENT OF A CENTRIFUGAL PUMP IMPELLER USING THE AGILE TURBOMACHINERY DESIGN SYSTEM
HYDRAULIC DEVELOPMENT OF A CENTRIFUGAL PUMP IMPELLER USING THE AGILE TURBOMACHINERY DESIGN SYSTEM Krzysztof Denus CTD Technology ñ Ing. Buro Denus Colin Osborne Concepts NREC 1. INTRODUCTION The impeller
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
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
CFD ANALYSIS Of COMBINED 8-12 STAGES Of INTERMIDIATE PRESSURE STEAM TURBINE
CFD ANALYSIS Of COMBINED 8-12 STAGES Of INTERMIDIATE PRESSURE STEAM TURBINE 1st Author name : SHIVAKUMAR VASMATE, 2nd Author name : KAMALADEVI ANANDE. 1 Department of Mechanical Engineering, India 2 Department
Air Movement. Air Movement
2018 Air Movement In this tutorial you will create an air flow using a supply vent on one side of a room and an open vent on the opposite side. This is a very simple PyroSim/FDS simulation, but illustrates
CFD Post-Processing of Rampressor Rotor Compressor
Gas Turbine Industrial Fellowship Program 2006 CFD Post-Processing of Rampressor Rotor Compressor Curtis Memory, Brigham Young niversity Ramgen Power Systems Mentor: Rob Steele I. Introduction Recent movements
Axisymmetric Viscous Flow Modeling for Meridional Flow Calculation in Aerodynamic Design of Half-Ducted Blade Rows
Memoirs of the Faculty of Engineering, Kyushu University, Vol.67, No.4, December 2007 Axisymmetric Viscous Flow Modeling for Meridional Flow alculation in Aerodynamic Design of Half-Ducted Blade Rows by
RAPID DESIGN AND FLOW SIMULATIONS FOR TUBOCHARGER COMPONENTS
EASC ANSYS Conference 2009 RAPID DESIGN AND FLOW SIMULATIONS FOR TUBOCHARGER COMPONENTS Authors Dipl.-Ing. Jonas Belz Dipl.-Ing. Ralph-Peter Müller CFDnetwork Engineering CFturbo Software & Engineering
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
equivalent stress to the yield stess.
Example 10.2-1 [Ansys Workbench/Thermal Stress and User Defined Result] A 50m long deck sitting on superstructures that sit on top of substructures is modeled by a box shape of size 20 x 5 x 50 m 3. It
SOLIDWORKS Flow Simulation Options
SOLIDWORKS Flow Simulation Options SOLIDWORKS Flow Simulation includes an options dialogue window that allows for defining default options to use for a new project. Some of the options included are unit
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
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
PyroSim Example Guide
PyroSim Example Guide 2012 PyroSim Example Guide Table of Contents Table of Contents PyroSim Example Guide... ii Table of Contents... iv Table of Figures... vii Chapter 1. Before Starting...1 Install
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
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
Atrium Smoke Movement
2014 Smoke Movement in Atrium Buildings In this example you will create a simulation of smoke movement in an atrium with and without extraction fans. This tutorial demonstrates how to: Create the atrium
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;
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
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
5. Create two planes and split the outer cylinder volume into four quadrants using the menus
Generating a 3D GAMBIT grid for concentric rotating cylinders Prepared by: Jagannath R Nanduri (jaggu.nanduri@mail.wvu.edu) 304-293-3111x2348 1. In order to overcome the problem of generating small size
Workshop 1: Basic Skills
Workshop 1: Basic Skills 14.5 Release Introduction to ANSYS Fluent Meshing 2011 ANSYS, Inc. December 21, 2012 1 I Introduction Workshop Description: This workshop shows some of the clean up tools in Tgrid
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
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
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
VIEWZ 1.3 USER MANUAL
VIEWZ 1.3 USER MANUAL 2007-08 Zeus Numerix ViewZ 1.3.0 User Manual Revision: 200806061429 The latest copy of this PDF may be downloaded from the website. An online (HTML) version is also available. Zeus
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
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
Import a CAD Model 2018
Import a CAD Model 2018 Import CAD Model In this tutorial you will import a CAD file, then add a 500 kw burner fire. Figure 1. Burner fire in this example This tutorial demonstrates how to: Import a CAD
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,
Proceedings of the ASME 2011 International Mechanical Engineering Congress & Exposition IMECE2011 November 11-17, 2011, Denver, Colorado, USA
Proceedings of the ASME 2011 International Mechanical Engineering Congress & Exposition IMECE2011 November 11-17, 2011, Denver, Colorado, USA IMECE2011-65058 THE EFFECT OF BLADE LEAN, TWIST AND BOW ON
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,
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
Heat Exchanger Efficiency
6 Heat Exchanger Efficiency Flow Simulation can be used to study the fluid flow and heat transfer for a wide variety of engineering equipment. In this example we use Flow Simulation to determine the efficiency
NUMERICAL ANALYSIS OF CENTRIFUGAL PUMP IMPELLER FOR PERFORMANCE IMPROVEMENT
Int. J. Chem. Sci.: 14(2), 2016, 1148-1156 ISSN 0972-768X www.sadgurupublications.com NUMERICAL ANALYSIS OF CENTRIFUGAL PUMP IMPELLER FOR PERFORMANCE IMPROVEMENT S. KALIAPPAN, M. D. RAJKAMAL and D. BALAMURALI
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
Advanced Turbomachinery Methods. Brad Hutchinson ANSYS, Inc. Industry Marketing
Advanced Turbomachinery Methods 1 Brad Hutchinson ANSYS, Inc. Industry Marketing Presentation Overview 1. Turbomachinery challenges 2. ANSYS TurboSystem 3. 2 Blade row fluid dynamics solution methods Available
First Steps - Conjugate Heat Transfer
COSMOSFloWorks 2004 Tutorial 2 First Steps - Conjugate Heat Transfer This First Steps - Conjugate Heat Transfer tutorial covers the basic steps to set up a flow analysis problem including conduction heat
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.
Enhancement of a large injection system for steam turbines
GE Oil & Gas Leonardo Nettis, GE Oil & Gas Enzo Imparato, GE Oil & Gas Lorenzo Cosi, GE Oil & Gas DOWNSTREAM TECHNOLOGY SOLUTIONS PRODUCTS & SERVICES Enhancement of a large injection system for steam turbines
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
NUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING
Review of the Air Force Academy No.3 (35)/2017 NUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING Cvetelina VELKOVA Department of Technical Mechanics, Naval Academy Nikola Vaptsarov,Varna, Bulgaria (cvetelina.velkova1985@gmail.com)
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
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
Turbomachinery Applications with STAR-CCM+ Turbomachinery Sector Manager
Turbomachinery Applications with STAR-CCM+ Fred Mendonça Fred Mendonça Turbomachinery Sector Manager An Integrated Solution The applications of the software seem to be infinite. The user-friendly A single