ENERGY-224 Reservoir Simulation Project Report. Ala Alzayer
|
|
- Sheila Wright
- 5 years ago
- Views:
Transcription
1 ENERGY-224 Reservoir Simulation Project Report Ala Alzayer Autumn Quarter December 3, 2014
2 Contents 1 Objective 2 2 Governing Equations 2 3 Methodolgy BlockMesh SnappyHexMesh Boundary Conditions Simulation Results Convergence Study Permeability Tortuosity REV Study Scalability Summary 12 6 References 12 1
3 1 Objective The main objective of this project is to investigate some of the basic parameters computed in a direct numerical simulation for a single phase fluid at the pore scale. My focus will be on the velocity distribution in complex geometry and how it can be used to get an idea of average upscaled quantities such as absolute permeability. I will examine the effects of the choice of simulation model used on these properties. 2 Governing Equations The governing equation for the fluid flow in the pore space will be the mass and momentum balance equations of Navier-Stokes, which for an incompressible fluid (neglecting gravity) are: v = 0 (1) ( ) v ρ + v v = p + µ 2 v t (2) The usual algorithm of choice to solve the pressure-velocity relationship would be the Pressure Implicit Operator-Splitting (PISO) algorithm (Issa, 1985). This is a predictor-corrector method which can handle transient problems. Given that the Reynolds number (ratio of intertial to viscous forces) for the flow in the medium under investigation 1, we can neglect the intertial effects and get a more simplified equation: 0 = p + µ 2 v (3) This is referred to as the Stokes equation which is a steady-state formulation; for that reason the Semi-Implicit Method for Pressure Linked Equations (SIMPLE) algorithm (Patankar, 1980) will be ideal for iteratively guessing/correcting the pressure-velocity fields. This algorithm does not solve transient problems but should be faster than the PISO algorithm in solving Stokes problems which is the case in this study. In addition to the equations of motions, the boundary condition for the fluid/solid interface, where the solid is represented by the grains, is needed. We will impose the condition that the fluid at the surface of the grains will have a zero velocity relative to the boundary, this is referred to as the no-slip condition. 2
4 3 Methodolgy OpenFOAMR software will be the tool used to simulate the fluid flow in the pore space. The main steps to solve these kinds of problems will be to discretize the domain (which is not a trivial task) and set the desired initial and boundary conditions. After that we feed the problem to the simplefoam solver (which utilizes the SIMPLE algorithm) to obtain a converged velocity and pressure field. I will elaborate on the discretization part next since it is more important than one might think. The combination of tools used in OpenFOAMR to mesh complex geometries are blockmesh, which defines the background grid, and snappyhexmesh, which alters the grid to fit the void space being modeled. I will elaborate on the two steps below. 3.1 BlockMesh This step involves simply generating a cartesian grid which is of the same size of the desired object to be meshed. Note that the object files usually either represent the solid grains or the pore space (figure 1). When the objects represent the grains, the cartesian grid generated can be larger or smaller than the domain. When the object file represents the pore space, the cartesian grid should be smaller than the domain as this will make the next step in meshing easier in setting the appropriate boundary conditions. Figure 1: Object file representing the solid grains (left) and pore space (right) with cartesian background grid generated by blockmesh Although this step does not take so much time and could be considered a very simple step, it is quite important in resolving the behavior in tight pore spaces. I will elaborate on this point in the simulation results section. 3
5 3.2 SnappyHexMesh The next step after ensuring that the generated grid covers the desired domain involves cutting out the grains. This will leave us with a mesh that only represents the pore space. The snappyhexmesh tool does this in two steps as shown in figure 2. The first step involves removing the grid blocks adjacent to the grains, the next step smoothens the edges and snaps the grid onto the surfaces of the grains. The cells with faces touching the grains are all identified as an additional boundary in our domain to be specified. Figure 2: The first (left) and second (right) step used in snappyhexmesh This step is the more time consuming (as well as memory consuming) part of the meshing; the snappyhexmesh step can take up to 12 hours on a single processor for a 2D sandstone image (0.6 mm 1.83mm) and a cartesian grid with cells. 3.3 Boundary Conditions With the domain fully discretized, the only step left is to initialize the domain and set the boundary conditions. The only constance we use is the kinematic viscosity of the fluid which in this case is set to 1e-6 m 2 s 1. For the Stokes problem we are only concerned with velocity and pressure fields and therefore initalize the internal domain with zero pressure and velocity, while the boundary conditions are shown in Table 1 below. Table 1: Boundary Conditions Boundary Pressure [m 2 /s 2 ] Velocity [m/s] Inlet 1e-3 zero gradient Outlet 0 zero gradient Walls zero gradient 0 (no slip condition) Grain Surfaces zero gradient 0 (no slip condition) (Note: pressure is normalized by density) 4
6 4 Simulation Results As mentioned before, with the domain discretized and initial/boundary conditions set, the simplefoam solver is used to iteratively guess/correct the pressure-velocity fields until convergence (residual smaller than 1e-6). Since we are dealing with a steady state problem, the results will include only the steady state pressure and velocity distributions which depend solely on the boundary conditions and pore geometry. The two main geometries I am considering here are shown in figure 3, I will refer to the one on the left as simple case whereas the one on the right as SS2 which is a sandstone slice used in the SUPRI-A group (courtesy of Soulaine). Both these models are 2D slices of the pore geometry and therefore all simuations run are in the x-y plane. I am showing the pressure distributions in both geometries which will practically be the same in all the cases considered here. In the next part I will show the results of the convergence study done on both these geometries which should highlight the importance of the grid used in modeling pore scale flow. Figure 3: Pressure distribution for simple (left) and SS2 (right) pore geometry 5
7 4.1 Convergence Study The main parameters I am considering here are the average and maximum velocity of the domain after convergence. I am normalizing the results for each case with that of the highest resolution case (figure 4). Note the dashed black line which shows the number of pixels in the real image for each geometry. We see that the significant difference in results are seen for any grid that has a lower resolution than the actual image. After that we see that the simple geometry converges to the solution faster than the SS2 case. This is expected as SS2 is much more complicated with a wider distribution of pore throat sizes. This supports the current best practices which emphasizes mesh quality even beyond the base image resolution (Soulaine, 2014). Ideally we would like to capture the poiseuille flow regime in all the pore throats, which would require 5-10 cells resolution atleast. Figure 4: Convergence study of the simple (left) and the SS2 (right) geometry One interesting observation here is that the average velocity seems to be more restrictive than the maximum velocity, which is the opposite of what one would expect. However, when looking at the velocity distribution in the different cases we see that the less resolved cases are capable of capturing the high velocities in the small pore throats. On the other hand we see that due to the low resolution the velocities can be overestimated in the large pores between the pore throats where the high resolution model show more variation (figure 5). I included the case just to show the extreme case of when the grid resolution is less than the image size; we see a significant loss of connectivity which should not even be considered a valid simulation model. Figure 6 shows the same trend for the SS2 geometry. The significance of these results show the importance of having a converged model especially when it comes to obtain effective parameters such as permeability. 6
8 Figure 5: Velocity distribution for the simple case with (top-left) (top-right) (bottom-left) (bottom-right) Figure 6: Velocity distribution for the SS2 case with (left) (center) (bottom-left) 7
9 4.2 Permeability Absolute permeability is probably one of the most common effective parameters obtained from direct numerical simulation at the pore scale. This is quite easy to do once an accurate velocity field is obtained; previous section shows that caution needs to be taken when deciding that the model being used is representative. models for the two geometries: k simple = µl x P 1 V k ss2 = µl y P 1 V Below I estimate the absolute permeabilities using the converged v v v x dv = v y dv = (1e 5)(9.2e 4)(1.697e 6) (1e 3) (1e 5)(1.6e 3)(1.28e 6) (1e 3) = d = d If we use a less resolved model we can use an average velocity value that is 1.1 the converged value as seen in figure 4. This would result in permeabilities values of 17.4 and darcies respectively. This might not seem so severe for this case since the geometries being used, despite being complex, are relatively homogeneous. 4.3 Tortuosity Tortuosity is another average parameter which can be deduced from pore scale simulation. There are relatively more sophisticated ways of computing the tortuosity of a medium by computing the dispersion tensor. However, here an attempt was made to compute tortuosity using stream lines. Once the velocity field is obtained we are able to trace particle paths (using the stream tracer tool in ParaViewR). The simplest definition of tortuosity is the length of path traveled (length of streamline) over the distance between the two points (length of domain). For this project, I only traced 5 streamlines on the simple geometry case (figure 7) and took the average length of the 5 streamlines. This gives us an idea about the average tortuosity in this geometry: τ = StreamlineLength LengthofDomain = = Ideally we would have a much larger number of streamlines to obtain a value which is more representative. The next section will investigate the idea of a representative elementary volume (REV) which plays an important role in estimating effective properties such as permeability and tortuosity. 8
10 Figure 7: Variation of average porosity and speed (left) and the corresponding error (right) with increasing sample size 4.4 REV Study The use of effective properties such as porosity and permeability is based on the assumption that the source of these averaged properties is statistically representative of the entire domain. The following study is a simple investigation of the porosity and average velocity which could be considered as an indication of permeability. This was conducted on a square domain obtained from stiching the SS2 geometery (Efros and Freeman, 2001). For this study a simulation was run on the whole domain to obtain the velocity profile. The methodolgy presented was followed to make sure that we are using a converged grid. We then used an averaging tool which can extract the results from a given sample size of the domain and obtain the average porosity and velocity. A total of 24 samples were taken from the domain; the results and relative errors compared to the full domain solution are shown in Figure 8. 9
11 Figure 8: Variation of average porosity and speed (left) and the corresponding error (right) with increasing sample size If we assume that the sample size is considered an REV once the error is bounded by 2% (arbitrary number), we can see that the two averaged properties differ in REV size (figure 8). This confirms the well known idea that different averaged parameters might have different respective REV sizes. Ideally the REV size should be representative of all required averaged parameters (tortuosity, permeability, dispersion tensor...etc). Figure 9: REV size for average porosity (left) and velocity (right) for a bounded error of 2% 10
12 4.5 Scalability Despite the fact we are dealing with the millimeter scale, due to the size of the simulation grids (O(10 7 ) cells) it is obvious how expensive these computations are. This brings us to concern of computational speed where the importance of parallelizing comes into play. This is done in OpenFOAMR by decomposing the full domain into multiple domains. These sub-domains are then linked with one another through boundary conditions. Once the simulation are done the full domain is reconstructed. The following strong scaling study was conducted on the SS2 geometry with 1.92 million cells (figure 10). Figure 10: Strong scaling for 1.92 million cell case showing speed up (left) and clock time (right) From the results we can see that these simulation are scalable up to a point, which is expected. We see that the speed up factor is almost a 1 to 1 relationship with the number of processors up to 64 processors where we see a deviation. That is exactly the point where each processor deals with 30,000 cells; which has been observed with OpenFOAMR to be the point where communication time starts to counter the speed up resulting from decomposing the domain to multiple processors. We also see the point at which we start to loose speed up (20,000 cells per processor). 11
13 5 Summary Direct numerical simulation in complex geometry is a powerful tool for gaining insight of the underlying physics of fluid flow in porous media, however care should be taken when dealing with these models. We have highlighted the importance of the mesh starting from the background cartesian grid, which could seem trivial. Having enough resolution to capture the flow in tight pore throats is necessary for obtaining an accurate and representative overall velocity field, where we saw that the average velocity is more restrictive than the maximum velocity with convergence. The impact of that is seen in estimating effective properties such as absolute permeability. Obtaining a REV is also a very important part of analyzing results from pore scale simulations. In this study we looked at porosity and average velocity in a 2D relatively homogeneous sandstone. This difference in REV size could be the case with other properties estimated which lie beyond the scope of this study. 6 References 1. Issa. Solution of the implicitly discretised fluid flow equations by operator-splitting. Journal of Computational Physics, 62:40-65, Patankar. Numerical Heat Transfer And Fluid Flow. Taylor and Francis, C. Soulaine notes on Direct numerical simulation in fully saturated porous media, A.A. Efros and W.T. Freeman, Image Quilting for Texture Synthesis and Transfer, Computer Graphics (Proc. Siggraph 2001), ACM Press, New York, 2001, pp
Pressure Correction Scheme for Incompressible Fluid Flow
AALTO UNIVERSITY School of Chemical Technology CHEM-E7160 Fluid Flow in Process Units Pressure Correction Scheme for Incompressible Fluid Flow Ong Chin Kai 620503 Lee De Ming Benedict 620448 Page 1 Abstract
More informationIntroduction to fluid mechanics simulation using the OpenFOAM technology
Introduction to fluid mechanics simulation using the OpenFOAM technology «Simulation in porous media from pore to large scale» Part II: Mesh complex geometries, application to the evaluation of permeability,
More informationDriven Cavity Example
BMAppendixI.qxd 11/14/12 6:55 PM Page I-1 I CFD Driven Cavity Example I.1 Problem One of the classic benchmarks in CFD is the driven cavity problem. Consider steady, incompressible, viscous flow in a square
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 information1.2 Numerical Solutions of Flow Problems
1.2 Numerical Solutions of Flow Problems DIFFERENTIAL EQUATIONS OF MOTION FOR A SIMPLIFIED FLOW PROBLEM Continuity equation for incompressible flow: 0 Momentum (Navier-Stokes) equations for a Newtonian
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 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 informationFEMLAB Exercise 1 for ChE366
FEMLAB Exercise 1 for ChE366 Problem statement Consider a spherical particle of radius r s moving with constant velocity U in an infinitely long cylinder of radius R that contains a Newtonian fluid. Let
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 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 informationVelocity and Concentration Properties of Porous Medium in a Microfluidic Device
Velocity and Concentration Properties of Porous Medium in a Microfluidic Device Rachel Freeman Department of Chemical Engineering University of Washington ChemE 499 Undergraduate Research December 14,
More informationStrömningslära Fluid Dynamics. Computer laboratories using COMSOL v4.4
UMEÅ UNIVERSITY Department of Physics Claude Dion Olexii Iukhymenko May 15, 2015 Strömningslära Fluid Dynamics (5FY144) Computer laboratories using COMSOL v4.4!! Report requirements Computer labs must
More informationCalculate a solution using the pressure-based coupled solver.
Tutorial 19. Modeling Cavitation Introduction This tutorial examines the pressure-driven cavitating flow of water through a sharpedged orifice. This is a typical configuration in fuel injectors, and brings
More informationOptimizing Bio-Inspired Flow Channel Design on Bipolar Plates of PEM Fuel Cells
Excerpt from the Proceedings of the COMSOL Conference 2010 Boston Optimizing Bio-Inspired Flow Channel Design on Bipolar Plates of PEM Fuel Cells James A. Peitzmeier *1, Steven Kapturowski 2 and Xia Wang
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 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 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 informationDebojyoti Ghosh. Adviser: Dr. James Baeder Alfred Gessow Rotorcraft Center Department of Aerospace Engineering
Debojyoti Ghosh Adviser: Dr. James Baeder Alfred Gessow Rotorcraft Center Department of Aerospace Engineering To study the Dynamic Stalling of rotor blade cross-sections Unsteady Aerodynamics: Time varying
More informationA Lattice-Boltzmann Based Method Applied to Digital Rock Characterization of Perforation Tunnel Damage
SCA2016-058 1/6 A Lattice-Boltzmann Based Method Applied to Digital Rock Characterization of Perforation Tunnel Damage Bernd Crouse, David M Freed, Nils Koliha, Gana Balasubramanian EXA CORP Rajani Satti,
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 informationFAST ALGORITHMS FOR CALCULATIONS OF VISCOUS INCOMPRESSIBLE FLOWS USING THE ARTIFICIAL COMPRESSIBILITY METHOD
TASK QUARTERLY 12 No 3, 273 287 FAST ALGORITHMS FOR CALCULATIONS OF VISCOUS INCOMPRESSIBLE FLOWS USING THE ARTIFICIAL COMPRESSIBILITY METHOD ZBIGNIEW KOSMA Institute of Applied Mechanics, Technical University
More informationOpen Source Software Course: Assignment 1
Open Source Software Course: Assignment 1 Mengmeng Zhang Aeronautical and Vehicle Engineering, Royal Insistute of Technology (KTH), Stockholm, Sweden 2012-09-09 Mengmeng Zhang Open Source Software Course
More informationCGT 581 G Fluids. Overview. Some terms. Some terms
CGT 581 G Fluids Bedřich Beneš, Ph.D. Purdue University Department of Computer Graphics Technology Overview Some terms Incompressible Navier-Stokes Boundary conditions Lagrange vs. Euler Eulerian approaches
More informationHomogenization and numerical Upscaling. Unsaturated flow and two-phase flow
Homogenization and numerical Upscaling Unsaturated flow and two-phase flow Insa Neuweiler Institute of Hydromechanics, University of Stuttgart Outline Block 1: Introduction and Repetition Homogenization
More informationRealistic Animation of Fluids
Realistic Animation of Fluids p. 1/2 Realistic Animation of Fluids Nick Foster and Dimitri Metaxas Realistic Animation of Fluids p. 2/2 Overview Problem Statement Previous Work Navier-Stokes Equations
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 informationISSN(PRINT): ,(ONLINE): ,VOLUME-1,ISSUE-1,
NUMERICAL ANALYSIS OF THE TUBE BANK PRESSURE DROP OF A SHELL AND TUBE HEAT EXCHANGER Kartik Ajugia, Kunal Bhavsar Lecturer, Mechanical Department, SJCET Mumbai University, Maharashtra Assistant Professor,
More informationFLOWVISION CFD FREQUENTLY ASKED QUESTIONS
FLOWVISION CFD FREQUENTLY ASKED QUESTIONS 1. Installation and Licensing 1.1. Does FlowVision have floating licenses? 1.1.1. Actually all FlowVision licenses have floating capability and no extra fees are
More informationNUMERICAL INVESTIGATION OF THE FLOW BEHAVIOR INTO THE INLET GUIDE VANE SYSTEM (IGV)
University of West Bohemia» Department of Power System Engineering NUMERICAL INVESTIGATION OF THE FLOW BEHAVIOR INTO THE INLET GUIDE VANE SYSTEM (IGV) Publication was supported by project: Budování excelentního
More informationUse of CFD in Design and Development of R404A Reciprocating Compressor
Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 2006 Use of CFD in Design and Development of R404A Reciprocating Compressor Yogesh V. Birari
More informationLisa Michelle Dahl June 04, 2008 CHEM E Finlayson Mixing Properties of an Optimized SAR Mixer (2D and 3D Models)
Mixing Properties of an Optimized SAR Mixer (2D and 3D Models) I. Introduction While mixing is the most common unit-operation in chemical industrial processes, optimizing mixing in microchemical processes
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 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 informationIMPROVED WALL BOUNDARY CONDITIONS WITH IMPLICITLY DEFINED WALLS FOR PARTICLE BASED FLUID SIMULATION
6th European Conference on Computational Mechanics (ECCM 6) 7th European Conference on Computational Fluid Dynamics (ECFD 7) 1115 June 2018, Glasgow, UK IMPROVED WALL BOUNDARY CONDITIONS WITH IMPLICITLY
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 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 informationNumerical Modeling Study for Fish Screen at River Intake Channel ; PH (505) ; FAX (505) ;
Numerical Modeling Study for Fish Screen at River Intake Channel Jungseok Ho 1, Leslie Hanna 2, Brent Mefford 3, and Julie Coonrod 4 1 Department of Civil Engineering, University of New Mexico, Albuquerque,
More informationNavier-Stokes & Flow Simulation
Last Time? Navier-Stokes & Flow Simulation Implicit Surfaces Marching Cubes/Tetras Collision Detection & Response Conservative Bounding Regions backtracking fixing Today Flow Simulations in Graphics Flow
More information2.7 Cloth Animation. Jacobs University Visualization and Computer Graphics Lab : Advanced Graphics - Chapter 2 123
2.7 Cloth Animation 320491: Advanced Graphics - Chapter 2 123 Example: Cloth draping Image Michael Kass 320491: Advanced Graphics - Chapter 2 124 Cloth using mass-spring model Network of masses and springs
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 informationInvestigation 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 informationComputational Simulation of the Wind-force on Metal Meshes
16 th Australasian Fluid Mechanics Conference Crown Plaza, Gold Coast, Australia 2-7 December 2007 Computational Simulation of the Wind-force on Metal Meshes Ahmad Sharifian & David R. Buttsworth Faculty
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 informationINVESTIGATION OF HYDRAULIC PERFORMANCE OF A FLAP TYPE CHECK VALVE USING CFD AND EXPERIMENTAL TECHNIQUE
International Journal of Mechanical Engineering and Technology (IJMET) Volume 10, Issue 1, January 2019, pp. 409 413, Article ID: IJMET_10_01_042 Available online at http://www.ia aeme.com/ijmet/issues.asp?jtype=ijmet&vtype=
More informationLagrangian methods and Smoothed Particle Hydrodynamics (SPH) Computation in Astrophysics Seminar (Spring 2006) L. J. Dursi
Lagrangian methods and Smoothed Particle Hydrodynamics (SPH) Eulerian Grid Methods The methods covered so far in this course use an Eulerian grid: Prescribed coordinates In `lab frame' Fluid elements flow
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 informationAERODYNAMIC OPTIMIZATION OF REAR AND FRONT FLAPS ON A CAR
Student: Giannoni Alberto Professor: Ing. Jan Pralits, Advanced Fluid Dynamics Course Co-Professor: Ing. Matteo Colli AERODYNAMIC OPTIMIZATION OF REAR AND FRONT FLAPS ON A CAR ABSTRACT In this work we
More informationCoupling of STAR-CCM+ to Other Theoretical or Numerical Solutions. Milovan Perić
Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions Milovan Perić Contents The need to couple STAR-CCM+ with other theoretical or numerical solutions Coupling approaches: surface and volume
More informationAxisymmetric 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
More informationAero-Vibro Acoustics For Wind Noise Application. David Roche and Ashok Khondge ANSYS, Inc.
Aero-Vibro Acoustics For Wind Noise Application David Roche and Ashok Khondge ANSYS, Inc. Outline 1. Wind Noise 2. Problem Description 3. Simulation Methodology 4. Results 5. Summary Thursday, October
More informationMicrowell Mixing with Surface Tension
Microwell Mixing with Surface Tension Nick Cox Supervised by Professor Bruce Finlayson University of Washington Department of Chemical Engineering June 6, 2007 Abstract For many applications in the pharmaceutical
More informationTutorial Two Built in Mesh
Built in Mesh 4 th edition, Jan. 2018 This offering is not approved or endorsed by ESI Group, ESI-OpenCFD or the OpenFOAM Foundation, the producer of the OpenFOAM software and owner of the OpenFOAM trademark.
More informationAdarsh Krishnamurthy (cs184-bb) Bela Stepanova (cs184-bs)
OBJECTIVE FLUID SIMULATIONS Adarsh Krishnamurthy (cs184-bb) Bela Stepanova (cs184-bs) The basic objective of the project is the implementation of the paper Stable Fluids (Jos Stam, SIGGRAPH 99). The final
More informationUse of HPC to Predict Porous Media Properties and Flow in Hydrocarbon Reservoirs
Use of HPC to Predict Porous Media Properties and Flow in Hydrocarbon Reservoirs Henry Neeman, 2 Dimitrios V. Papavassiliou 1 1 School of Chemical Engineering and Materials Science 2 School of Computer
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 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 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 informationIntroduction to Computational Fluid Dynamics Mech 122 D. Fabris, K. Lynch, D. Rich
Introduction to Computational Fluid Dynamics Mech 122 D. Fabris, K. Lynch, D. Rich 1 Computational Fluid dynamics Computational fluid dynamics (CFD) is the analysis of systems involving fluid flow, heat
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 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 informationALE Seamless Immersed Boundary Method with Overset Grid System for Multiple Moving Objects
Tenth International Conference on Computational Fluid Dynamics (ICCFD10), Barcelona,Spain, July 9-13, 2018 ICCFD10-047 ALE Seamless Immersed Boundary Method with Overset Grid System for Multiple Moving
More informationMESHLESS SOLUTION OF INCOMPRESSIBLE FLOW OVER BACKWARD-FACING STEP
Vol. 12, Issue 1/2016, 63-68 DOI: 10.1515/cee-2016-0009 MESHLESS SOLUTION OF INCOMPRESSIBLE FLOW OVER BACKWARD-FACING STEP Juraj MUŽÍK 1,* 1 Department of Geotechnics, Faculty of Civil Engineering, University
More informationCFD 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 informationTechnical Report TR
Technical Report TR-2015-09 Boundary condition enforcing methods for smoothed particle hydrodynamics Arman Pazouki 1, Baofang Song 2, Dan Negrut 1 1 University of Wisconsin-Madison, Madison, WI, 53706-1572,
More informationStream Function-Vorticity CFD Solver MAE 6263
Stream Function-Vorticity CFD Solver MAE 66 Charles O Neill April, 00 Abstract A finite difference CFD solver was developed for transient, two-dimensional Cartesian viscous flows. Flow parameters are solved
More informationFluent User Services Center
Solver Settings 5-1 Using the Solver Setting Solver Parameters Convergence Definition Monitoring Stability Accelerating Convergence Accuracy Grid Independence Adaption Appendix: Background Finite Volume
More 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 informationNumerical Wave Tank Modeling of Hydrodynamics of Permeable Barriers
ICHE 2014, Hamburg - Lehfeldt & Kopmann (eds) - 2014 Bundesanstalt für Wasserbau ISBN 978-3-939230-32-8 Numerical Wave Tank Modeling of Hydrodynamics of Permeable Barriers K. Rajendra & R. Balaji Indian
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 informationCFD Analysis of a Fully Developed Turbulent Flow in a Pipe with a Constriction and an Obstacle
CFD Analysis of a Fully Developed Turbulent Flow in a Pipe with a Constriction and an Obstacle C, Diyoke Mechanical Engineering Department Enugu State University of Science & Tech. Enugu, Nigeria U, Ngwaka
More informationUnderstanding and Using MINC
Understanding and Using MINC Background In TOUGH2, the MINC (Multiple Interacting Continua) approach is used to model flow in fractured media. It is a generalization of the classical double-porosity concept
More informationAdjoint 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 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 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 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 informationCUDA. Fluid simulation Lattice Boltzmann Models Cellular Automata
CUDA Fluid simulation Lattice Boltzmann Models Cellular Automata Please excuse my layout of slides for the remaining part of the talk! Fluid Simulation Navier Stokes equations for incompressible fluids
More informationFree 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 informationOpenFOAM and Third Party Structural Solver for Fluid Structure Interaction Simulations
OpenFOAM and Third Party Structural Solver for Fluid Structure Interaction Simulations Robert L. Campbell rlc138@arl.psu.edu Fluids and Structural Mechanics Office Applied Research Laboratory The Pennsylvania
More informationAn added mass partitioned algorithm for rigid bodies and incompressible flows
An added mass partitioned algorithm for rigid bodies and incompressible flows Jeff Banks Rensselaer Polytechnic Institute Overset Grid Symposium Mukilteo, WA October 19, 216 Collaborators Bill Henshaw,
More informationSTCE. An (more) effective Discrete Adjoint Model for OpenFOAM
An (more) effective Discrete Adjoint Model for OpenFOAM Markus Towara, Uwe Naumann Software and Tools for Computational Engineering Science RWTH Aachen University EuroAD 2013, Oxford, 10. December 2013
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 informationBest Practices Workshop: Overset Meshing
Best Practices Workshop: Overset Meshing Overview Introduction to Overset Meshes Range of Application Workflow Demonstrations and Best Practices What are Overset Meshes? Overset meshes are also known as
More informationSIMULATION OF FLOW FIELD AROUND AND INSIDE SCOUR PROTECTION WITH PHYSICAL AND REALISTIC PARTICLE CONFIGURATIONS
XIX International Conference on Water Resources CMWR 2012 University of Illinois at Urbana-Champaign June 17-22, 2012 SIMULATION OF FLOW FIELD AROUND AND INSIDE SCOUR PROTECTION WITH PHYSICAL AND REALISTIC
More informationLATTICE-BOLTZMANN METHOD FOR THE SIMULATION OF LAMINAR MIXERS
14 th European Conference on Mixing Warszawa, 10-13 September 2012 LATTICE-BOLTZMANN METHOD FOR THE SIMULATION OF LAMINAR MIXERS Felix Muggli a, Laurent Chatagny a, Jonas Lätt b a Sulzer Markets & Technology
More informationSERBIATRIB 15 STATIC PERFORMANCE OF SURFACE TEXTURED MAGNETORHEOLOGICAL FLUID JOURNAL BEARINGS. 14 th International Conference on Tribology
Serbian Tribology Society SERBIATRIB 15 14 th International Conference on Tribology Belgrade, Serbia, 13 15 May 015 University of Belgrade, Faculty of Mechanical Engineering STATIC PERFORMANCE OF SURFACE
More informationµ = 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 informationNUMERICAL 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)
More informationcuibm A GPU Accelerated Immersed Boundary Method
cuibm A GPU Accelerated Immersed Boundary Method S. K. Layton, A. Krishnan and L. A. Barba Corresponding author: labarba@bu.edu Department of Mechanical Engineering, Boston University, Boston, MA, 225,
More informationPossibility of Implicit LES for Two-Dimensional Incompressible Lid-Driven Cavity Flow Based on COMSOL Multiphysics
Possibility of Implicit LES for Two-Dimensional Incompressible Lid-Driven Cavity Flow Based on COMSOL Multiphysics Masanori Hashiguchi 1 1 Keisoku Engineering System Co., Ltd. 1-9-5 Uchikanda, Chiyoda-ku,
More informationAbstract. 1 Introduction
On the Use of Pore-Scale Computational Models for Two-Phase Porous-media Flows M.A. Celia, P.C Reeves, H.K. Dahle Environmental Engineering and Water Resources Program, Department of Civil Engineering
More informationLS-DYNA 980 : Recent Developments, Application Areas and Validation Process of the Incompressible fluid solver (ICFD) in LS-DYNA.
12 th International LS-DYNA Users Conference FSI/ALE(1) LS-DYNA 980 : Recent Developments, Application Areas and Validation Process of the Incompressible fluid solver (ICFD) in LS-DYNA Part 1 Facundo Del
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 informationInfluence of mesh quality and density on numerical calculation of heat exchanger with undulation in herringbone pattern
Influence of mesh quality and density on numerical calculation of heat exchanger with undulation in herringbone pattern Václav Dvořák, Jan Novosád Abstract Research of devices for heat recovery is currently
More informationModeling a Nozzle in a Borehole
Modeling a Nozzle in a Borehole E. Holzbecher, F. Sun Georg-August Universität Göttingen *Goldschmidtstr. 3, 37077 Göttingen, GERMANY; E-mail: eholzbe@gwdg.de Abstract: A nozzle, installed in an injecting
More informationMASSACHUSETTS INSTITUTE OF TECHNOLOGY. Analyzing wind flow around the square plate using ADINA Project. Ankur Bajoria
MASSACHUSETTS INSTITUTE OF TECHNOLOGY Analyzing wind flow around the square plate using ADINA 2.094 - Project Ankur Bajoria May 1, 2008 Acknowledgement I would like to thank ADINA R & D, Inc for the full
More informationA NURBS-BASED APPROACH FOR SHAPE AND TOPOLOGY OPTIMIZATION OF FLOW DOMAINS
6th European Conference on Computational Mechanics (ECCM 6) 7th European Conference on Computational Fluid Dynamics (ECFD 7) 11 15 June 2018, Glasgow, UK A NURBS-BASED APPROACH FOR SHAPE AND TOPOLOGY OPTIMIZATION
More informationBackward 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
More informationCFD design tool for industrial applications
Sixth LACCEI International Latin American and Caribbean Conference for Engineering and Technology (LACCEI 2008) Partnering to Success: Engineering, Education, Research and Development June 4 June 6 2008,
More informationDirect Numerical Simulation of a Low Pressure Turbine Cascade. Christoph Müller
Low Pressure NOFUN 2015, Braunschweig, Overview PostProcessing Experimental test facility Grid generation Inflow turbulence Conclusion and slide 2 / 16 Project Scale resolving Simulations give insight
More informationShape 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