Tutorial: Modeling Liquid Reactions in CIJR Using the Eulerian PDF transport (DQMOM-IEM) Model
|
|
- Paula O’Connor’
- 5 years ago
- Views:
Transcription
1 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 reactions using the Eulerian Composition PDF transport model with Discrete Quadrature Method of Moments (DQMOM) in ANSYS FLUENT. For reactions involving liquids, mixing at molecular level- termed as micromixing, plays a significant role in determining the conversion of products. In cases where there are parallel competing reactions, the micromixing can singularly affect the yield of the desired product. Fast chemistry models in ANSYS FLUENT like Non-premixed equilibrium model, steady laminar flamelet and eddy dissipation model cannot capture the physics of micromixing and thus may not predict conversion, selectivity and scale-up accurately. While the Full composition PDF transport is well equipped to solve liquid reactions, the computation cost involved with the lagrangian approach is very high since kinetic calculations are performed using particle based methods (Monte-carlo methods) which are computationally intensive. The DQMOM-IEM model solves for the PDF transport in Eulerian framework, this significantly reduces the computational cost involved while preserving the accuracy of the calculations. This tutorial demonstrates how to do the following: Set up liquid chemical reactions in a confined impinging jet reactor. Set up DQMOM-IEM PDF Transport model with liquid micro-mixing extension. Calculate the solution.. Examine results using graphics. Prerequisites This tutorial is written with the assumption that you have completed Tutorial 1 from the ANSYS FLUENT 14.5 Tutorial Guide, and that you are familiar with the ANSYS FLUENT navigation pane and menu structure. Some steps in the setup and solution procedure will not be shown explicitly. A good understanding of turbulence and species mixing/reaction, as well as their modeling is desirable. c ANSYS, Inc. December 4,
2 Problem Description A confined impinging-jets reactor (CIJR) consists of two high-velocity, coaxial liquid jets that collide and produce mixing times on the order of milliseconds. In this tutorial, the following pair of second- order parallel reactions is employed to evaluate the extent of mixing. H + (A) + CH 3 C(OCH 3 ) 2 (D) H + (A) + (OH) (B) K1 H 2 O(P 1) K2 H + (A) + CH 3 COCH 3 (P 2) = 2CH 3 OH(P 3) The first reaction is very fast (K1 = 1.4E8m 3 /mol.s), and the second is very slow (K2 = 643E 3m 3 /mol.s). When the liquid micro-mixing model is enabled, ANSYS FLUENT interpolates the mixing constant used in IEM model from model turbulence and scalar spectra. A diagram of the CIJR with two reactants impinging at the center of the reactor is shown in Figure 1. The solution will be performed in two stages: Figure 1: Problem Schematic Preparation 1. Copy the mesh file, dqmom.msh.gz to the working folder. 2. Use FLUENT Launcher to start the (3D) version of ANSYS FLUENT. 3. Enable Double-Precision in the Options list. 2 c ANSYS, Inc. December 4, 2012
3 Setup and Solution Step 1: Mesh 1. Read the mesh file, dqmom.msh.gz. File Read Mesh... As the mesh file is read, ANSYS FLUENT reports the progress in the console. Figure 2: Mesh Display Step 2: General Settings 1. Retain the default settings. General 2. Check the mesh. General Check ANSYS FLUENT performs various checks on the mesh and reports the progress in the console. Pay attention to the minimum volume reported and make sure this is a positive number. Scaling is not required for this case. 3. Scale the mesh. General Scale... c ANSYS, Inc. December 4,
4 (a) Select mm from the Mesh Was Created In drop-down list. (b) Select mm from the View Length Unit In drop-down list. (c) Close the Scale Mesh dialog box. All dimensions will now be shown in millimeters Step 3: Models 1. Select the standard k-turbulence model. Models Viscous Edit... (a) Select k-epsilon(2 eqn) from the Model list to open the Viscous Model dialog box. The dialog box will expand after the selection. (b) Select Enhanced Wall Treatment from the Near-Wall Treatment group box. (c) Click OK to close the Viscous Model dialog box. 4 c ANSYS, Inc. December 4, 2012
5 2. Define species model. Models Species Edit... (a) Select Composition PDF Transport from the Model list. The dialog box will expand after the selection. (b) Select Eulerian in the PDF Transport Options group box. (c) Enable Volumetric in the Reactions group box. (d) Enable Liquid Micro-Mixing in the Options group box. (e) Click OK and close the Species Model dialog box. At this stage, ANSYS FLUENTrequires the chemical mechanism which contains the species, their properties, and kinetics. Since these have not been provided an Error dialog box is displayed. (f) Click OK to close the Error dialog box. An information dialog box will open reminding you to confirm the property valuesthat have been extracted from the database. c ANSYS, Inc. December 4,
6 (g) Click OK to close the Information dialog box. Step 4: Materials The DQMOM model requires the mixture materials to be setup. This is done by creating the species participating in the reactions and then by adding them to the mixture species list. Materials Create/Edit Add water to the material list. (a) Click Fluent Database to open the Fluent Database Materials dialog box. (b) Select fluid under Material Type drop-down list. (c) Select water-liquid (h2o<l>) from the Fluent Fluid Materials list and click Copy. (d) Close the Fluent Database Materials dialog box. 2. Create a new material. 6 c ANSYS, Inc. December 4, 2012
7 (a) Enter the name as a in the Name text field. (b) Delete the entry for Chemical Formula. (c) Enter 962 for Density. (d) Enter 1 for Molecular Weight. (e) Click Change/Create. (f) Click Yes to overwrite water-liquid material. 3. Similarly create other species materials b,d,p1,p2,p3 and bulk with the properties given in the following table. Species Molecular Weight b 17 d 104 p1 18 p2 58 p3 32 bulk Add the created species to the mixture list c ANSYS, Inc. December 4,
8 (a) Select Mixture from Material Type drop-down list. (b) Click Edit... next to Mixture Species and add the species in the order a,b,d,p1,p2,p3 and bulk being the last species. (c) Click OK to close the Species dialog box. 5. Add the reactions. (a) Click Edit... next to Reaction. (b) Enter 2 for Total Number of Reactions. i. For the first reaction, (a + b p1), set Number of Reactants to 2. ii. Select a and b from the Species drop-down lists. iii. Enter 1 for Stoich. Coefficient and Rate Exponent for a. iv. Enter 1.4e+11 for Pre-Exponential Factor. v. Enter 0 for Activation Energy. vi. Select p1 from the Species drop-down list for product. vii. Enter 1 for Stoich. Coefficient for p1. 8 c ANSYS, Inc. December 4, 2012
9 (c) Similarly set the second reaction, (a + d + bulk a + p2 + 2p3), by changing ID to 2. i. Enter 3 for Number of Reactants and Number of Products. ii. Enter 2 for Stoich. Coefficient of p3. iii. Enter for Pre-Exponential Factor. iv. Enter 0 for Activation Energy. v. Click OK in the Reactions dialog box. 6. Change the mixture properties. (a) Select volume-weighted-mixing-law from the Density drop down list, as this is more applicable for liquid reactions. (b) Enter for Viscosity. (c) Enter 2e-9 for Mass Diffusivity. Note: This is to account for the high Schmidt number for liquids due to which the diffusivity is low. (d) Click Change/Create and close the Create/Edit Materials dialog box. c ANSYS, Inc. December 4,
10 Step 5: Boundary Conditions 1. Define the species properties in species model. Models Species Edit... (a) Click Boundary tab in the Species Model dialog box. i. Enter for a and for bulk for Fuel. ii. Enter for b, for d, and for bulk corresponding to Oxidizer stream. iii. Click Apply and close the Species Model dialog box 10 c ANSYS, Inc. December 4, 2012
11 2. Set the boundary conditions for the leftinlet zone. Boundary Conditions leftinlet Edit... (a) Enter m/s for Velocity Magnitude. (b) Retain the selection of Intensity and Viscosity Ratio from the Specification Method drop-down list in the Turbulence group box. (c) Retain 5% for Turbulent Intensity and enter 5 for Turbulent Viscosity Ratio. c ANSYS, Inc. December 4,
12 (d) Click the Species tab and enter 1 for Mixture Fraction. This is the fuel reactant inlet, so the Mixture Fraction is 1. (e) Click OK to close the Velocity Inlet dialog box. 3. Set the boundary conditions for the rightinlet zone. Boundary Conditions rightinlet Edit... (a) Enter m/s for Velocity Magnitude. (b) Retain the selection of Intensity and Viscosity Ratio from the Specification Method drop-down list in the Turbulence group box. (c) Retain 5% for Turbulent Intensity and enter 5 for Turbulent Viscosity Ratio. (d) Click the Species tab and retain 0 for Mixture Fraction. (e) Click OK to close the Velocity Inlet dialog box. 4. Set the boundary conditions for the pressure outlet zone. Boundary Conditions outlet Edit... (a) Retain the selection of Intensity and Viscosity Ratio from the Specification Method drop-down list in the Turbulence group box. (b) Retain 5% for Backflow Turbulent Intensity (c) Retain 10 for Backflow Turbulent Viscosity Ratio. (d) Click OK to close the Pressure Outlet dialog box. 12 c ANSYS, Inc. December 4, 2012
13 Step 6: Solution 1. Set the solution parameters. Solution Methods (a) Select Green-Gauss Node Based from the Gradient drop-down list. (b) Select PRESTO! from the Pressure drop-down list. c ANSYS, Inc. December 4,
14 2. Set the solution controls. Solution Controls (a) Enter 0.8 for Eulerian PDF in the Under-Relaxation Factors group box. (b) Click Equations... and de-select Energy from the equations list. (c) Click OK to close the Equations dialog box Note: Energy equation is enabled by default for species model with reactions. However for your case the flow is isothermal. The densities are also constant. Therefore solving for energy is not necessary. 14 c ANSYS, Inc. December 4, 2012
15 3. Set the convergence limits. Monitors Residuals Edit... (a) Enter 1e-4 for fmean, a, b, d, and p3. (b) Enter 5e-4 for p1 and p2. (c) Click OK and close the Residual Monitors dialog box. 4. Initialize the solution. Solution Initialization Initialize Hybrid Initialization is the default Initialization Method in ANSYS FLUENT Refer to the section Hybrid Initialization, in the ANSYS FLUENT 14.5 User s Guide. 5. Save the case file (dqmom.cas.gz). File Write Case... c ANSYS, Inc. December 4,
16 6. Run the calculation for 100 iterations. Run Calculation Calculate 7. Change under relaxation factor for Eulerian PDF to Run the calculation for 50 iterations. Run Calculation Calculate 9. Select Second Order Upwind for all the rest of the parameters in the Spatial Discretization group box. Solution Methods 10. Run the calculation for 700 iterations. Run Calculation Calculate The solution converges in approximately 36 more iterations. See Figure 3. Figure 3: Residual History 11. Save the data file (dqmom.dat.gz). File Write Data c ANSYS, Inc. December 4, 2012
17 Step 7: Postprocessing 1. Display contours of velocity magnitude. Graphics and Animations Contours Set Up... (a) Enable Filled from the Options group box. (b) Select Velocity... and Velocity Magnitude from the Contours of drop-down lists. (c) Select symmetry from the Surfaces selection list. (d) Click Display (Figure 4). Figure 4: Contours of Velocity Magnitude 2. Display contours of mixture fraction. (a) Select Eulerian PDF Transport... and Mixture Fraction from the Contours of dropdown lists. (b) Click Display (Figure 5). c ANSYS, Inc. December 4,
18 Figure 5: Contours of Mixture Fraction 3. Display contours of mass fraction of a. (a) Select Species... and Mass Fraction of a from the Contours of drop-down lists. (b) Click Display (Figure 6). Figure 6: Contours of Mass Fraction of a 18 c ANSYS, Inc. December 4, 2012
19 4. Similarly display the contours of mass fraction of b and d species. Refer to Figures 7 and 8 Figure 7: Contours of Mass Fraction of b Figure 8: Contours of Mass Fraction of d Summary This tutorial has demonstrated that the DQMOM model can simulate reactions in liquids with slow chemistry and low diffusivity. c ANSYS, Inc. December 4,
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 informationUsing the Eulerian Multiphase Model for Granular Flow
Tutorial 21. Using the Eulerian Multiphase Model for Granular Flow Introduction Mixing tanks are used to maintain solid particles or droplets of heavy fluids in suspension. Mixing may be required to enhance
More informationUse 6DOF solver to calculate motion of the moving body. Create TIFF files for graphic visualization of the solution.
Introduction The purpose of this tutorial is to provide guidelines and recommendations for setting up and solving a moving deforming mesh (MDM) case along with the six degree of freedom (6DOF) solver and
More informationTutorial: Hydrodynamics of Bubble Column Reactors
Tutorial: Introduction The purpose of this tutorial is to provide guidelines and recommendations for solving a gas-liquid bubble column problem using the multiphase mixture model, including advice on solver
More informationModeling Evaporating Liquid Spray
Tutorial 17. Modeling Evaporating Liquid Spray Introduction In this tutorial, the air-blast atomizer model in ANSYS FLUENT is used to predict the behavior of an evaporating methanol spray. Initially, the
More informationTutorial 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 informationTutorial: Riser Simulation Using Dense Discrete Phase Model
Introduction The purpose of this tutorial is to demonstrate the setup of a dense discrete phase model (DDPM) with the example of 2D riser. DDPM is used for the secondary phase that has a particle size
More informationFlow in an Intake Manifold
Tutorial 2. Flow in an Intake Manifold Introduction The purpose of this tutorial is to model turbulent flow in a simple intake manifold geometry. An intake manifold is a system of passages which carry
More informationUsing a Single Rotating Reference Frame
Tutorial 9. Using a Single Rotating Reference Frame Introduction This tutorial considers the flow within a 2D, axisymmetric, co-rotating disk cavity system. Understanding the behavior of such flows is
More informationUsing Multiple Rotating Reference Frames
Tutorial 10. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive
More informationSimulation of Flow Development in a Pipe
Tutorial 4. Simulation of Flow Development in a Pipe Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D turbulent fluid flow in a pipe. The pipe networks are common
More informationThis tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following:
Tutorial 22. Modeling Solidification Introduction This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following: Define a
More informationModeling Evaporating Liquid Spray
Tutorial 16. Modeling Evaporating Liquid Spray Introduction In this tutorial, FLUENT s air-blast atomizer model is used to predict the behavior of an evaporating methanol spray. Initially, the air flow
More informationNon-Newtonian Transitional Flow in an Eccentric Annulus
Tutorial 8. Non-Newtonian Transitional Flow in an Eccentric Annulus Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D, turbulent flow of a non-newtonian fluid. Turbulent
More informationUsing the Discrete Ordinates Radiation Model
Tutorial 6. Using the Discrete Ordinates Radiation Model Introduction This tutorial illustrates the set up and solution of flow and thermal modelling of a headlamp. The discrete ordinates (DO) radiation
More informationExpress Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing
Express Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry Oriented HPC Simulations,
More informationTutorial 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 informationTutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing
Tutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing Introduction The purpose of this tutorial is to demonstrate how to simulate a ball check valve with small displacement
More informationModeling Flow Through Porous Media
Tutorial 7. Modeling Flow Through Porous Media Introduction Many industrial applications involve the modeling of flow through porous media, such as filters, catalyst beds, and packing. This tutorial illustrates
More informationUsing Multiple Rotating Reference Frames
Tutorial 9. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive
More informationTutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow
Tutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow Introduction This tutorial illustrates the setup and solution of the two-dimensional turbulent fluid flow and heat
More informationCold Flow Simulation Inside an SI Engine
Tutorial 12. Cold Flow Simulation Inside an SI Engine Introduction The purpose of this tutorial is to illustrate the case setup and solution of the two dimensional, four stroke spark ignition (SI) engine
More informationModeling Unsteady Compressible Flow
Tutorial 4. Modeling Unsteady Compressible Flow Introduction In this tutorial, FLUENT s density-based implicit solver is used to predict the timedependent flow through a two-dimensional nozzle. As an initial
More informationA B C D E. Settings Choose height, H, free stream velocity, U, and fluid (dynamic viscosity and density ) so that: Reynolds number
Individual task Objective To derive the drag coefficient for a 2D object, defined as where D (N/m) is the aerodynamic drag force (per unit length in the third direction) acting on the object. The object
More informationAppendix: 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 informationModeling External Compressible Flow
Tutorial 3. Modeling External Compressible Flow Introduction The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a nonzero angle of attack. You will use the Spalart-Allmaras
More informationTutorial: Heat and Mass Transfer with the Mixture Model
Tutorial: Heat and Mass Transfer with the Mixture Model Purpose The purpose of this tutorial is to demonstrate the use of mixture model in FLUENT 6.0 to solve a mixture multiphase problem involving heat
More informationExpress Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil
Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 -
More informationVerification and Validation of Turbulent Flow around a Clark-Y Airfoil
1 Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 2 (ANSYS 19.1; Last Updated: Aug. 7, 2018) By Timur Dogan, Michael Conger,
More informationSimulation of 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 informationAuto Injector Syringe. A Fluent Dynamic Mesh 1DOF Tutorial
Auto Injector Syringe A Fluent Dynamic Mesh 1DOF Tutorial 1 2015 ANSYS, Inc. June 26, 2015 Prerequisites This tutorial is written with the assumption that You have attended the Introduction to ANSYS Fluent
More informationSimulation of Turbulent Flow around an Airfoil
Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Pre-Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew Opyd, Dong-Hwan
More informationSimulation of Turbulent Flow around an Airfoil
1. Purpose Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew
More informationModeling 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 informationLab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders
Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders Objective: The objective of this laboratory is to introduce how to use FLUENT to solve both transient and natural convection problems.
More informationSimulation and Validation of Turbulent Pipe Flows
Simulation and Validation of Turbulent Pipe Flows ENGR:2510 Mechanics of Fluids and Transport Processes CFD LAB 1 (ANSYS 17.1; Last Updated: Oct. 10, 2016) By Timur Dogan, Michael Conger, Dong-Hwan Kim,
More informationAdvanced 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 informationModule D: Laminar Flow over a Flat Plate
Module D: Laminar Flow over a Flat Plate Summary... Problem Statement Geometry and Mesh Creation Problem Setup Solution. Results Validation......... Mesh Refinement.. Summary This ANSYS FLUENT tutorial
More informationSupersonic Flow Over a Wedge
SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 2 Supersonic Flow Over a Wedge Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification A uniform supersonic stream encounters a wedge
More informationCompressible Flow in a Nozzle
SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 1 Compressible Flow in a Nozzle Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification Consider air flowing at high-speed through a
More informationGrid. Apr 09, 1998 FLUENT 5.0 (2d, segregated, lam) Grid. Jul 31, 1998 FLUENT 5.0 (2d, segregated, lam)
Tutorial 2. Around an Airfoil Transonic Turbulent Flow Introduction: The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a non-zero angle of attack. You will use the
More informationTUTORIAL#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 informationStratified Oil-Water Two-Phases Flow of Subsea Pipeline
Stratified Oil-Water Two-Phases Flow of Subsea Pipeline Adib Zulhilmi Mohd Alias, a, Jaswar Koto, a,b,*, Yasser Mohamed Ahmed, a and Abd Khair Junaidi, b a) Department of Aeronautics, Automotive and Ocean
More informationSolution Recording and Playback: Vortex Shedding
STAR-CCM+ User Guide 6663 Solution Recording and Playback: Vortex Shedding This tutorial demonstrates how to use the solution recording and playback module for capturing the results of transient phenomena.
More informationc Fluent Inc. May 16,
Tutorial 1. Office Ventilation Introduction: This tutorial demonstrates how to model an office shared by two people working at computers, using Airpak. In this tutorial, you will learn how to: Open a new
More informationVerification of Laminar and Validation of Turbulent Pipe Flows
1 Verification of Laminar and Validation of Turbulent Pipe Flows 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 1 (ANSYS 18.1; Last Updated: Aug. 1, 2017) By Timur Dogan, Michael Conger, Dong-Hwan
More informationThe purpose of this tutorial is to illustrate how to set up and solve a problem using the. Moving Deforming Mesh (MDM) using the layering algorithm.
Tutorial: Introduction The purpose of this tutorial is to illustrate how to set up and solve a problem using the following two features in FLUENT. Moving Deforming Mesh (MDM) using the layering algorithm.
More informationExpress Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM)
Express Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM) Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry
More informationExpress Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes
Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School
More informationNovember c Fluent Inc. November 8,
MIXSIM 2.1 Tutorial November 2006 c Fluent Inc. November 8, 2006 1 Copyright c 2006 by Fluent Inc. All Rights Reserved. No part of this document may be reproduced or otherwise used in any form without
More informationIsotropic Porous Media Tutorial
STAR-CCM+ User Guide 3927 Isotropic Porous Media Tutorial This tutorial models flow through the catalyst geometry described in the introductory section. In the porous region, the theoretical pressure drop
More informationA HYBRID FINITE VOLUME/PDF MONTE CARLO METHOD TO CAPTURE SHARP GRADIENTS IN UNSTRUCTURED GRIDS
A HYBRID FINITE VOLUME/PDF MONTE CARLO METHOD TO CAPTURE SHARP GRADIENTS IN UNSTRUCTURED GRIDS Genong Li and Michael F. Modest Mechanical Engineering Department The Pennsylvania State University University
More informationSolver Basics. Introductory FLUENT Training ANSYS, Inc. All rights reserved. ANSYS, Inc. Proprietary
Solver Basics Introductory FLUENT Training 2006 ANSYS, Inc. All rights reserved. 2006 ANSYS, Inc. All rights reserved. 3-2 Solver Execution The menus are arranged such that the order of operation is generally
More informationSimCafe. ANSYS WB - Airfoil - Setup (Physics) Added by Benjamin J Mullen, last edited by Benjamin J Mullen on Apr 29, :18
Page 1 of 5 Search Cornell SimCafe Home Edit Browse/Manage Login Simulation > > ANSYS WB - Airfoil - Setup (Physics) Search ANSYS WB - Airfoil - Setup (Physics) Added by Benjamin J Mullen, last edited
More informationWorkbench Tutorial Minor Losses, Page 1 Tutorial Minor Losses using Pointwise and FLUENT
Workbench Tutorial Minor Losses, Page 1 Tutorial Minor Losses using Pointwise and FLUENT Introduction This tutorial provides instructions for meshing two internal flows. Pointwise software will be used
More informationPreliminary Spray Cooling Simulations Using a Full-Cone Water Spray
39th Dayton-Cincinnati Aerospace Sciences Symposium Preliminary Spray Cooling Simulations Using a Full-Cone Water Spray Murat Dinc Prof. Donald D. Gray (advisor), Prof. John M. Kuhlman, Nicholas L. Hillen,
More informationSimulation of Turbulent Flow over the Ahmed Body
Simulation of Turbulent Flow over the Ahmed Body 58:160 Intermediate Mechanics of Fluids CFD LAB 4 By Timur K. Dogan, Michael Conger, Maysam Mousaviraad, and Fred Stern IIHR-Hydroscience & Engineering
More informationPDF-based simulations of turbulent spray combustion in a constant-volume chamber under diesel-engine-like conditions
International Multidimensional Engine Modeling User s Group Meeting at the SAE Congress Detroit, MI 23 April 2012 PDF-based simulations of turbulent spray combustion in a constant-volume chamber under
More informationCFD MODELING FOR PNEUMATIC CONVEYING
CFD MODELING FOR PNEUMATIC CONVEYING Arvind Kumar 1, D.R. Kaushal 2, Navneet Kumar 3 1 Associate Professor YMCAUST, Faridabad 2 Associate Professor, IIT, Delhi 3 Research Scholar IIT, Delhi e-mail: arvindeem@yahoo.co.in
More informationMiddle East Technical University Mechanical Engineering Department ME 485 CFD with Finite Volume Method Fall 2017 (Dr. Sert)
Middle East Technical University Mechanical Engineering Department ME 485 CFD with Finite Volume Method Fall 2017 (Dr. Sert) ANSYS Fluent Tutorial Developing Laminar Flow in a 2D Channel 1 How to use This
More informationExpress Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding
Express Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry Oriented HPC Simulations,
More informationIntroduction To FLUENT. David H. Porter Minnesota Supercomputer Institute University of Minnesota
Introduction To FLUENT David H. Porter Minnesota Supercomputer Institute University of Minnesota Topics Covered in this Tutorial What you can do with FLUENT FLUENT is feature rich Summary of features and
More informationTUTORIAL#3. Marek Jaszczur. Boundary Layer on a Flat Plate W1-1 AGH 2018/2019
TUTORIAL#3 Boundary Layer on a Flat Plate Marek Jaszczur AGH 2018/2019 W1-1 Problem specification TUTORIAL#3 Boundary Layer - on a flat plate Goal: Solution for boudary layer 1. Creating 2D simple geometry
More informationTurbulencja w mikrokanale i jej wpływ na proces emulsyfikacji
Polish Academy of Sciences Institute of Fundamental Technological Research Turbulencja w mikrokanale i jej wpływ na proces emulsyfikacji S. Błoński, P.Korczyk, T.A. Kowalewski PRESENTATION OUTLINE 0 Introduction
More informationCFD Simulation for Stratified Oil-Water Two-Phase Flow in a Horizontal Pipe
CFD Simulation for Stratified Oil-Water Two-Phase Flow in a Horizontal Pipe Adib Zulhilmi Mohd Alias, a, Jaswar Koto, a,b,* and Yasser Mohamed Ahmed, a a) Department of Aeronautics, Automotive and Ocean
More informationProblem description. The FCBI-C element is used in the fluid part of the model.
Problem description This tutorial illustrates the use of ADINA for analyzing the fluid-structure interaction (FSI) behavior of a flexible splitter behind a 2D cylinder and the surrounding fluid in a channel.
More informationSimulation of Turbulent Flow in an Asymmetric Diffuser
Simulation of Turbulent Flow in an Asymmetric Diffuser 1. Purpose 58:160 Intermediate Mechanics of Fluids CFD LAB 3 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University of Iowa C.
More informationIntroduction to ANSYS CFX
Workshop 03 Fluid flow around the NACA0012 Airfoil 16.0 Release Introduction to ANSYS CFX 2015 ANSYS, Inc. March 13, 2015 1 Release 16.0 Workshop Description: The flow simulated is an external aerodynamics
More informationInvestigation of mixing chamber for experimental FGD reactor
Investigation of mixing chamber for experimental FGD reactor Jan Novosád 1,a, Petra Danová 1 and Tomáš Vít 1 1 Department of Power Engineering Equipment, Faculty of Mechanical Engineering, Technical University
More informationTutorial: Modeling Domains with Embedded Reference Frames: Part 2 Sliding Mesh Modeling
Tutorial: Modeling Domains with Embedded Reference Frames: Part 2 Sliding Mesh Modeling Introduction The motion of rotating components is often complicated by the fact that the rotational axis about which
More informationAPPLIED COMPUTATIONAL FLUID DYNAMICS-PROJECT-3
APPLIED COMPUTATIONAL FLUID DYNAMICS-PROJECT-3 BY SAI CHAITANYA MANGAVELLI Common Setup Data: 1) Mesh Proximity and Curvature with Refinement of 2. 2) Double Precision and second order for methods in Solver.
More informationSimulation of Turbulent Flow over the Ahmed Body
1 Simulation of Turbulent Flow over the Ahmed Body ME:5160 Intermediate Mechanics of Fluids CFD LAB 4 (ANSYS 18.1; Last Updated: Aug. 18, 2016) By Timur Dogan, Michael Conger, Dong-Hwan Kim, Maysam Mousaviraad,
More informationFLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016
FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016 Note: These instructions are based on an older version of FLUENT, and some of the instructions
More informationand 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 informationEulerian transported probability density function sub-filter model for large-eddy simulations of turbulent combustion
Combustion Theory and Modelling Vol. 10, No. 3, June 2006, 439 458 Eulerian transported probability density function sub-filter model for large-eddy simulations of turbulent combustion VENKATRAMANAN RAMAN,
More informationLab 8: FLUENT: Turbulent Boundary Layer Flow with Convection
Lab 8: FLUENT: Turbulent Boundary Layer Flow with Convection Objective: The objective of this laboratory is to use FLUENT to solve for the total drag and heat transfer rate for external, turbulent boundary
More informationVerification and Validation of Turbulent Flow around a Clark-Y Airfoil
Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose 58:160 Intermediate Mechanics of Fluids CFD LAB 2 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University
More informationIntroduction to C omputational F luid Dynamics. D. Murrin
Introduction to C omputational F luid Dynamics D. Murrin Computational fluid dynamics (CFD) is the science of predicting fluid flow, heat transfer, mass transfer, chemical reactions, and related phenomena
More informationCFD Best Practice Guidelines: A process to understand CFD results and establish Simulation versus Reality
CFD Best Practice Guidelines: A process to understand CFD results and establish Simulation versus Reality Judd Kaiser ANSYS Inc. judd.kaiser@ansys.com 2005 ANSYS, Inc. 1 ANSYS, Inc. Proprietary Overview
More information1 Thomas Chengattu MAE 494 November Project # 2: Transient Simulation using VOF Methods
1 Thomas Chengattu Project # 2: Transient Simulation using VOF Methods INITIAL SET UP The initial set-up for all the geometries varied with respect to each tasks. The common similarities between these
More informationFlow 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
More informationSwapnil Nimse Project 1 Challenge #2
Swapnil Nimse Project 1 Challenge #2 Project Overview: Using Ansys-Fluent, analyze dependency of the steady-state temperature at different parts of the system on the flow velocity at the inlet and buoyancy-driven
More informationTOUGHREACT Example: Aqueous Transport with Adsorption and Decay
403 Poyntz Avenue, Suite B Manhattan, KS 66502 USA +1.785.770.8511 www.thunderheadeng.com TOUGHREACT Example: Aqueous Transport with Adsorption and Decay PetraSim 2016.1 Table of Contents Overview...1
More informationSteady 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 informationRevolve 3D geometry to display a 360-degree image.
Tutorial 24. Turbo Postprocessing Introduction This tutorial demonstrates the turbomachinery postprocessing capabilities of FLUENT. In this example, you will read the case and data files (without doing
More informationSimulating Sinkage & Trim for Planing Boat Hulls. A Fluent Dynamic Mesh 6DOF Tutorial
Simulating Sinkage & Trim for Planing Boat Hulls A Fluent Dynamic Mesh 6DOF Tutorial 1 Introduction Workshop Description This workshop describes how to perform a transient 2DOF simulation of a planing
More informationRyian Hunter MAE 598
Setup: The initial geometry was produced using the engineering schematics provided in the project assignment document using the ANSYS DesignModeler application taking advantage of system symmetry. Fig.
More informationANSYS 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 informationANSYS FLUENT. Lecture 3. Basic Overview of Using the FLUENT User Interface L3-1. Customer Training Material
Lecture 3 Basic Overview of Using the FLUENT User Interface Introduction to ANSYS FLUENT L3-1 Parallel Processing FLUENT can readily be run across many processors in parallel. This will greatly speed up
More informationCFD in COMSOL Multiphysics
CFD in COMSOL Multiphysics Christian Wollblad Copyright 2017 COMSOL. Any of the images, text, and equations here may be copied and modified for your own internal use. All trademarks are the property of
More informationIntroduction to CFX. Workshop 2. Transonic Flow Over a NACA 0012 Airfoil. WS2-1. ANSYS, Inc. Proprietary 2009 ANSYS, Inc. All rights reserved.
Workshop 2 Transonic Flow Over a NACA 0012 Airfoil. Introduction to CFX WS2-1 Goals The purpose of this tutorial is to introduce the user to modelling flow in high speed external aerodynamic applications.
More informationExperimental and Numerical Study of Fire Suppression Performance of Ultral-Fine Water Mist in a Confined Space
Available online at www.sciencedirect.com Procedia Engineering 52 ( 2013 ) 208 213 Experimental and Numerical Study of Fire Suppression Performance of Ultral-Fine Water Mist in a Confined Space LIANG Tian-shui
More informationComputational 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 informationThe viscous forces on the cylinder are proportional to the gradient of the velocity field at the
Fluid Dynamics Models : Flow Past a Cylinder Flow Past a Cylinder Introduction The flow of fluid behind a blunt body such as an automobile is difficult to compute due to the unsteady flows. The wake behind
More informationThree Dimensional Numerical Simulation of Turbulent Flow Over Spillways
Three Dimensional Numerical Simulation of Turbulent Flow Over Spillways Latif Bouhadji ASL-AQFlow Inc., Sidney, British Columbia, Canada Email: lbouhadji@aslenv.com ABSTRACT Turbulent flows over a spillway
More informationNumerical analysis of fluid flow inside air intake system
Numerical analysis of fluid flow inside air intake system Numerical analysis of fluid flow inside air intake system Regis Ataides Martin Kessler Marcelo Kruger Geraldo Severi Jr. Cesareo de La Rosa Siqueira
More informationAdvanced Applications of STAR- CCM+ in Chemical Process Industry Ravindra Aglave Director, Chemical Process Industry
Advanced Applications of STAR- CCM+ in Chemical Process Industry Ravindra Aglave Director, Chemical Process Industry Outline Notable features released in 2013 Gas Liquid Flows with STAR-CCM+ Packed Bed
More informationFlat-Plate As stated earlier, the purpose of the flat-plate study was to create an opportunity for side-by-side comparison of ÒfastÓ RNG and
Chapter Six: Comparison of Turbulence Models Performance Comparisons There are a number of criteria by which to judge turbulence models. One criterion sometimes important to mathematicallyminded model
More informationHealthy Buildings 2017 Europe July 2-5, 2017, Lublin, Poland
Healthy Buildings 2017 Europe July 2-5, 2017, Lublin, Poland Paper ID 0122 ISBN: 978-83-7947-232-1 Numerical Investigation of Transport and Deposition of Liquid Aerosol Particles in Indoor Environments
More informationNumerical Simulation of Fuel Filling with Volume of Fluid
Numerical Simulation of Fuel Filling with Volume of Fluid Master of Science Thesis [Innovative and Sustainable Chemical Engineering] Kristoffer Johansson Department of Chemistry and Bioscience Division
More information