Multiphase flow metrology in oil and gas production: Case study of multiphase flow in horizontal tube
|
|
- Daisy Nichols
- 5 years ago
- Views:
Transcription
1 Multiphase flow metrology in oil and gas production: Case study of multiphase flow in horizontal tube Deliverable of Work Package WP5 (Creating Impact) Authors: Stanislav Knotek Czech Metrology Institute (CMI), CZ André Fiebach, Sonja Schmelter, Ellen Schmeyer Physikalisch-Technische Bundesanstalt (PTB), DE A report of the EMRP joint research project ENG58 Multiphase flow metrology in oil and gas production
2 1. Work package WP 5 2. Deliverable number D Reporting date June Title Case study of multiphase flow in horizontal tube 5. Author(s) Knotek, Fiebach, Schmelter, Schmeyer 6. Lead author ( ) sknotek@cmi.cz 7. Contributing researches (institutes) PTB (DE), CMI (CZ) 8. Supplementary notes None 9. Abstract The paper deals with case study of CFD models created for research of liquid flow patterns established for different flow rates and fluid properties in large diameter long horizontal tube which is part of the multiphase flow rate measurement system described in project deliverables. The paper deals with mesh dependency study, influence of boundary conditions and impact of fluid properties on resulting flow patterns. 10. Key words CFD model, flow patterns, mesh study, parametric influence I
3 Contents 1 Introduction 1 2 Geometry 1 3 Mesh 1 4 Boundary conditions 3 5 Solvers and numerical settings 3 6 Test cases Physical and Material properties Results and discussions Mesh dependency study Influence of the inlet boundary conditions Influence of artificial perturbation Influence of phase distribution at inlet section Influence of the fluid properties Conclusion 8 Acknowledgements 9 References 9 II
4 1 Introduction The paper deals with case study of CFD models created for research of liquid flow patterns established for different flow rates and fluid properties in large diameter long horizontal tube which is part of the multiphase flow rate measurement system described in project deliverables. Note that the results described in this paper have been received using OpenFOAM, open source CFD software. 2 Geometry The considered geometry is defined by the transfer package, which is used within the experimental intercomparison in WP 1. It consists of a m long horizontal pipe required for pattern formation and for damping of the influence of different injection points. Therefore a 12 m long horizontal pipe has been constructed. The diameter of the tube is 104 mm, thus the ratio of diameter to the length of the tube is nearly 115 which should be enough for the flow pattern development. 3 Mesh The meshes have been developed using the internal OpenFOAM mesher. For use with interfoam solver the static mesh has been constructed using blockmesh. An adaptive mesh refinement has been used during the solution with interdymfoam solver. Using the blockmesh, four different meshes has been created using increasing refinement in axial and radial direction. The mesh parameters are summarized in Table 1 and the cross sections are shown in Figure 1. Note that in case of extra fine mesh, the symmetry boundary condition has been prescribed in longitudinal section, so that only mesh of half geometry has been used in simulation. However, the number of cells in Table 1 for extra fine mesh is recalculated for hypothetical mesh of whole geometry. Mesh no. of cells per diameter per 1 m in total Coarse Normal Fine Extra fine Table 1: Cell statistics of meshes used for mesh dependency study in OpenFoam. For use with interdymfoam the mesh similar to coarse mesh in Table 1 has been used as basis for adaptive mesh refinement. In every time step, the cells on interface between phases are refined up to the enabled amount of cells. The comparison between coarse static mesh used for interfoam and dynamicaly refined mesh created by interdymfoam is show in Figure 2. 1
5 Figure 1: Cross section of the meshes used for mesh dependency study. Figure 2: Comparison of static and dynamic mesh and corresponding fluid interface. 2
6 4 Boundary conditions The inlet section is divided in two subdomains which have been constructed in several topological schemes as can be seen in Figure 3. The red colour represents the inlet area of liquid phase whereas the blue colour stands for the inlet of gaseous phase. The forms a) - c) have been used in dependence on the supposed level of liquid, i.e. for the cases with low liquid level, the inlet a) has been used, whereas the inlet c) has been used for cases with expected high liquid level. The inlet d) has been constructed for imposing bigger fluctuations in order to accelerate the perturbations on the surface. However, the results have shown, that for cases with enough big flow rate the same flow pattern have been established independently on the used inlet scheme. On the other side for low flow rates, the expected flow pattern was not established in whole length of the computed domain. For these reasons the artificial velocity fluctuations in y- and z- direction have been prescribed in the inlet velocity boundary condition according to formula u i = A i sin( 1 πfφ), (1) 9 where i stands for y and z, f=100 Hz, φ is random number with zero mean value and variance equals 0.5. Using this perturbation, the symmetric inlet c) seems to be appropriate as universal scheme. The impact of different inlet subdomains and influence of inlet perturbation is discussed further in section 7.2. The uniform velocity profile has been prescribed for each liquid phase on inlet whereas the pressure outlet boundary condition has been used at the end of the pipe. No-slip boundary condition has been prescribed on the walls. Figure 3: Phase distribution at inlet section. 5 Solvers and numerical settings Since the fluids are supposed to be separated (evident interface between phases), the volume of fluid method (VOF) has been suggested for numerical solution. Corresponding solvers for incompressible flows in Open- FOAM are interfoam and interdymfoam (solver for dynamic mesh). As was mentioned in [4], second order schemes have been used for spatial discretization, while the time discretization is done by classical first order Euler scheme. 3
7 6 Test cases For this study, eight test cases from the project test envelope have been selected. All these cases are two-phase cases, one half is for oil-gas, the other one for water-gas. The superficial velocities can be read from the Table 2, where the numbering in column signed with No. corresponds to the old internal numbering in the project. The numbering in column signed with Matrix Ref. No. corresponds to the actual numbering, see deliverable It can be seen that each oil-gas case has a corresponding water-gas case with same superficial velocities. Thus, the influence of the fluid can be considered, see Section 7.3. No. Matrix Ref. No. Q W Q O Q G u sw u so u sg l/s l/s l/s m/s m/s m/s Table 2: Volume flow rates Q W, Q O, Q G and superficial velocities u sw, u so, u sg of the water phase, oil phase and gaseous phase, respectively, used for the numerical simulations. 6.1 Physical and Material properties Physical and material properties used for simulations discussed in this paper are set according to published deliverable D [1], D [3] and D and are listed in Table 3. Note that cases No. 5a) - 5d) correspond to case No. 5 in Table 2. 7 Results and discussions 7.1 Mesh dependency study Mesh dependence study based on case No. 1 has been done in [4]. It was shown, that observed flow patterns remain nearly the same for coarse, normal and fine mesh as defined in Table 1. Only the wave origin and pressure loss were slightly dependent on the mesh refinement. For finer mesh, the velocity gradient is bigger on the interface between the phases as can be seen in Figure 4 from the comparison of velocity profiles corresponding to results of case No. 5 using coarse, fine and dynamic mesh. From alpha profiles (liquid volume 4
8 No. M. Ref. No. Temp. Gas density G. viscosity Liquid density L. viscosity Surface tension C kg/m 3 m 2 /s 10 6 kg/m 3 m 2 /s 10 6 kg/s (0.07) (0.07) 5a b c d a b Table 3: Physical and material properties used for the numerical simulations. fraction) in the same figure, it can be seen that the interface resolution is better for the dynamic mesh, since the mesh refinement on the interface is the finest from these three assessed meshes. On the other hand, there are no differences between the liquid velocity profile on the wall as can be seen from the same near wall velocity profiles depicted in logarithmic coordinates in Figure 6. Thus, the near wall region seems to be well resolved for all meshes. Figure 4: Profiles of alpha and velocity in dependence on mesh refinement. Figure 5: Velocity profiles in dependence on mesh refinement. 5
9 Figure 6: Phase interface using dynamic mesh in comparison with coarse and fine static mesh. The bigger velocity gradient on the interface implicates the bigger shear stress between phases, thus the surface instabilities are influenced by the mesh refinement on the interface more than by the mesh refinement in general. Figure 7 shows the comparison of alpha field computed using fine, extra fine and dynamic mesh. In case of extra fine and dynamic mesh, the instabilities are developed earlier and moreover the flow patterns seems to be quite different than in case of fine mesh. The arrows in Figure 7 point on the broad locations where the liquid touches the top wall of the tube and the flow pattern can be named as slug or plug/elongated bubble in dependence on the definitions. In contrast, only classical sharp solitary waves touching the wall in one point are observed using the static coarse, normal and fine mesh. Figure 7: Comparison of alpha field computed using fine, extra fine and dynamic mesh. 6
10 As is shown below, see Figure 9, similar flow patterns are obtained also using coarse mesh with suitable phase inlet distribution. Thus, it can be concluded that appropriate mesh refinement and phase inlet distribution are essential for right flow pattern resolution. Because even fine mesh defined in Table 1 does not reproduce the same flow pattern as extra fine mesh, the mesh study just presented is not completed and some other meshes should be used for mesh dependency study. In Figures 10-13, the comparison of time evolution of alpha computed using dynamic and static meshesh for different fluid properties is depicted. The values of alpha are received as mean values of alpha field in cross-section located in z=11 m. The time intervals are selected so as the mean values over the interval are not affected by the signal representing disturbance which has not been evolved yet. The results in all cases No. 5a) - 5d) show, that the flow patterns are nearly the same for coarse, normal and fine meshes, while different flow pattern is established for dynamic mesh, as was discussed above. Next, the main frequencies decrease with increasing mesh density. Thus, the flow pattern frequency seems to be the appropriate parameter for assessment of the mesh convergence. The summary of these results is shown in Figure 8. The squares correspond to the mean values of alpha in chosen time interval, while the upper and lower points of lines correspond to maximum and minimum alpha values, respectively. As can be seen, the alpha mean values and alpha ranges are nearly the same for all static meshes. The adaptive meshing leads to bigger alpha ranges, which is explained by different flow pattern as can be seen from corresponding plots. Figure 8: Comparison of mean alpha over time in section z=11m for cases No. 5a) - No. 5d). 7
11 7.2 Influence of the inlet boundary conditions Influence of artificial perturbation As was mentioned in section 4, the velocity perturbation is important for right flow pattern development. It was found, see [2], that using uniform velocity profile without artificial perturbation described by formula (1) only stratified flow has been developed even in cases where slug flow should be found according to experimental observations. For these reasons the artificial perturbation has been used in all cases. The velocity fluctuations defined by formula (1) can be driven by amplitude A i. However, no influence has been found for any reasonable values Influence of phase distribution at inlet section The Figure 9 shows the comparison of results computed for case No. 5b) using phase inlet distribution a) - c), see Figure 3, with coarse meshes and using inlet distribution b) with extra fine mesh. As can be seen, the impact of phase inlet distribution is quite important. From the comparison of the alpha evolution for coarse mesh with inlet c) with extra fine mesh results follows, that the inlet distribution should be imposed in similar manner as is the natural established distribution downstream. The impact of this boundary condition in case of enough fine mesh should be the object of next study. 7.3 Influence of the fluid properties Influence of the fluid properties has been studied using case No. 5 for fluid properties 5a) - 5d), see Table 3. The corresponding results are depicted in Figures and in Figure 8. The fluid properties does not influence the mean alpha value, what is the essential need, since it represents the average volume flow rate, which should be similar in all cases. The alpha ranges seem to be wider for oils with higher viscosities, although we should have in mind, that all fluid properties change according to defined temperature. Thus, more detailed study of each fluid property should by done. 8 Conclusion This study gives an overview of the main conclusions from number of simulations computed using OpenFOAM. The aim has been focused on study of mesh dependency, impact of boundary conditions and influence of fluid properties. As was shown in section 7.1, the results using the finest mesh differ from results computed using other meshes. Hence, the presented mesh study can not be assessed as completed and more finer meshes should be used for examination of mesh convergence. Although it was shown, that suitable combination of mesh density and boundary condition can be succesful in flow pattern resolution, the quantitative parameters as slug frequency are still mesh dependent, which also supports the need of better refinement. 8
12 Since the time requirements for numerical solution bounded the number of cells of using meshes, the presented influence of fluid properties can be used rather in qualitative sense. The study suggests, that higher oil viscosity (reached for lower temperature) supports establishing of bigger waves and the resulting flow pattern could be more inclinable to slug creation. Acknowledgements The EMRP is jointly funded by the EMRP participating countries within EURAMET and the European Union. References [1] G. Kok, P. Lucas, D. van Putten, T. Leonard, E. Graham, R. Harvey, A. Lupeau, M. T. Smith, L. Zakharov and R. de Leeuw. Test protocols for single and multiphase intercomparisons. Deliverable of WP1 Multiphase Laboratory Intercomparison in EMRP project ENG58 Multiphase flow metrology in oil and gas production, [2] A. Fiebach, S. Knotek, and S. Schmelter. 5 validated and verified CFD models to determine the influences of selected process / fluid property parameters on flow patterns. Deliverable of WP2 Determination of Multiphase Flow Pattern in EMRP project ENG58 Multiphase flow metrology in oil and gas production, [3] A. Fiebach, S. Knotek, and S. Schmelter. Specification of parametric values, geometry and boundary conditions for multiphase flow simulations covering the conditions of the intercomparison tests. Deliverable of WP3 Advanced Numerical Modelling in EMRP project ENG58 Multiphase flow metrology in oil and gas production, [4] S. Knotek, A. Fiebach and S. Schmelter. Numerical simulation of multiphase flows in large horizontal pipes Flomeko 2016 Sydney, Australia, September 26-29,
13 Figure 9: Mean alpha over time in section z=11m computed using coarse mesh for case No. 5b) with inlet subdomains a) - c) in comparison with mean alpha computed using extra fine mesh with inlet subdomain b). 10
14 Figure 10: Comparison of alpha field computed using static and dynamic mesh for case No. 5a (15 C) defined in Table 2 and 3. 11
15 Figure 11: Comparison of alpha field computed using static and dynamic mesh for case No. 5b defined in Table 2 and 3. 12
16 Figure 12: Comparison of alpha field computed using static and dynamic mesh for case No. 5c defined in Table 2 and 3. 13
17 Figure 13: Comparison of alpha field computed using static and dynamic mesh for case No. 5d defined in Table 2 and 3. 14
Tutorial 17. Using the Mixture and Eulerian Multiphase Models
Tutorial 17. Using the Mixture and Eulerian Multiphase Models Introduction: This tutorial examines the flow of water and air in a tee junction. First you will solve the problem using the less computationally-intensive
More 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 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 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 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 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 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 informationCOMPUTATIONAL FLUID DYNAMICS USED IN THE DESIGN OF WATERBLAST TOOLING
2015 WJTA-IMCA Conference and Expo November 2-4 New Orleans, Louisiana Paper COMPUTATIONAL FLUID DYNAMICS USED IN THE DESIGN OF WATERBLAST TOOLING J. Schneider StoneAge, Inc. Durango, Colorado, U.S.A.
More informationComputational Fluid Dynamics (CFD) Simulation in Air Duct Channels Using STAR CCM+
Available onlinewww.ejaet.com European Journal of Advances in Engineering and Technology, 2017,4 (3): 216-220 Research Article ISSN: 2394-658X Computational Fluid Dynamics (CFD) Simulation in Air Duct
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 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 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 informationCFD modelling of thickened tailings Final project report
26.11.2018 RESEM Remote sensing supporting surveillance and operation of mines CFD modelling of thickened tailings Final project report Lic.Sc.(Tech.) Reeta Tolonen and Docent Esa Muurinen University of
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 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 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 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 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 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 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 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 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 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 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 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 informationNumerical simulation of primary atomization of a sheared liquid sheet. Part 2: Comparison with experimental results
Numerical simulation of primary atomization of a sheared liquid sheet. Part 2: Comparison with experimental results P. Villedieu, G. Blanchard, D. Zuzio To cite this version: P. Villedieu, G. Blanchard,
More informationMcNair Scholars Research Journal
McNair Scholars Research Journal Volume 2 Article 1 2015 Benchmarking of Computational Models against Experimental Data for Velocity Profile Effects on CFD Analysis of Adiabatic Film-Cooling Effectiveness
More informationSimulations of the vortex in the Dellenback abrupt expansion, resembling a hydro turbine draft tube operating at part-load
Simulations of the vortex in the Dellenback abrupt expansion, resembling a hydro turbine draft tube operating at part-load H Nilsson Chalmers University of Technology, SE-412 96 Gothenburg, Sweden E-mail:
More informationCOMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS
COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS Dr W. Malalasekera Version 3.0 August 2013 1 COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE
More informationTurbulent Premixed Combustion with Flamelet Generated Manifolds in COMSOL Multiphysics
Turbulent Premixed Combustion with Flamelet Generated Manifolds in COMSOL Multiphysics Rob J.M Bastiaans* Eindhoven University of Technology *Corresponding author: PO box 512, 5600 MB, Eindhoven, r.j.m.bastiaans@tue.nl
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 informationA study of Jumper FIV due to multiphase internal flow: understanding life-cycle fatigue. Alan Mueller & Oleg Voronkov
A study of Jumper FIV due to multiphase internal flow: understanding life-cycle fatigue Alan Mueller & Oleg Voronkov Case description Main structural dimensions [1]: deformable jumper [2] in Mixture on
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 informationAerodynamic Study of a Realistic Car W. TOUGERON
Aerodynamic Study of a Realistic Car W. TOUGERON Tougeron CFD Engineer 2016 Abstract This document presents an aerodynamic CFD study of a realistic car geometry. The aim is to demonstrate the efficiency
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 informationCoupled Analysis of FSI
Coupled Analysis of FSI Qin Yin Fan Oct. 11, 2008 Important Key Words Fluid Structure Interface = FSI Computational Fluid Dynamics = CFD Pressure Displacement Analysis = PDA Thermal Stress Analysis = TSA
More informationProject 2 Solution. General Procedure for Model Setup
Project 2 Solution MAE598 Applied Computational Fluid Dynamics Shashank Kunjibettu General Procedure for Model Setup Step 1: Model the given component using design modeler Step 2: Meshing is done for the
More informationPotsdam Propeller Test Case (PPTC)
Second International Symposium on Marine Propulsors smp 11, Hamburg, Germany, June 2011 Workshop: Propeller performance Potsdam Propeller Test Case (PPTC) Olof Klerebrant Klasson 1, Tobias Huuva 2 1 Core
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 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 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 informationProject #3 MAE 598 Applied CFD
Project #3 MAE 598 Applied CFD 16 November 2017 H.P. Huang 1 Task 1 (a) Task 1a was to perform a transient analysis of a 2-D chamber that is initially filled with air, and has water flowing through the
More informationmidas NFX 2017R1 Release Note
Total Solution for True Analysis-driven Design midas NFX 2017R1 Release Note 1 midas NFX R E L E A S E N O T E 2 0 1 7 R 1 Major Improvements Midas NFX is an integrated finite element analysis program
More informationFigure 2: Water Into Kerosene, Volume Fraction (Left) And Total Density Of Mixture (Right)
Jared Bottlinger MAE598 Project 3 11/16/17 Task 1 a) Figure 1: Volume Fraction Of Water At 0.4s Task 1 b) Figure 2: Water Into Kerosene, Volume Fraction (Left) And Total Density Of Mixture (Right) Task
More informationANSYS AIM Tutorial Steady Flow Past a Cylinder
ANSYS AIM Tutorial Steady Flow Past a Cylinder Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Solution Domain Boundary Conditions Start-Up
More 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 informationPressure Drop Evaluation in a Pilot Plant Hydrocyclone
Pressure Drop Evaluation in a Pilot Plant Hydrocyclone Fabio Kasper, M.Sc. Emilio Paladino, D.Sc. Marcus Reis, M.Sc. ESSS Carlos A. Capela Moraes, D.Sc. Dárley C. Melo, M.Sc. Petrobras Research Center
More informationAir Assisted Atomization in Spiral Type Nozzles
ILASS Americas, 25 th Annual Conference on Liquid Atomization and Spray Systems, Pittsburgh, PA, May 2013 Air Assisted Atomization in Spiral Type Nozzles W. Kalata *, K. J. Brown, and R. J. Schick Spray
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 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 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 informationSIMULATION OF FLOW AROUND KCS-HULL
SIMULATION OF FLOW AROUND KCS-HULL Sven Enger (CD-adapco, Germany) Milovan Perić (CD-adapco, Germany) Robinson Perić (University of Erlangen-Nürnberg, Germany) 1.SUMMARY The paper describes results of
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 informationHydrocyclones and CFD
Design of Hydrocyclone Separation Equipment Using CFD Coupled with Optimization Tools David Schowalter 1, Rafiqul Khan 1, Therese Polito 2, and Tim Olson 3. (1) Fluent Inc., 10 Cavendish Court, Lebanon,
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 informationPressure Losses Analysis in Air Duct Flow Using Computational Fluid Dynamics (CFD)
International Academic Institute for Science and Technology International Academic Journal of Science and Engineering Vol. 3, No. 9, 2016, pp. 55-70. ISSN 2454-3896 International Academic Journal of Science
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 informationTHE APPLICATION OF AN ATMOSPHERIC BOUNDARY LAYER TO EVALUATE TRUCK AERODYNAMICS IN CFD
THE APPLICATION OF AN ATMOSPHERIC BOUNDARY LAYER TO EVALUATE TRUCK AERODYNAMICS IN CFD A SOLUTION FOR A REAL-WORLD ENGINEERING PROBLEM Ir. Niek van Dijk DAF Trucks N.V. CONTENTS Scope & Background Theory:
More informationOpenFOAM GUIDE FOR BEGINNERS
OpenFOAM GUIDE FOR BEGINNERS Authors This guide has been developed by: In association with: Pedro Javier Gamez and Gustavo Raush The Foam House Barcelona ETSEIAT-UPC June 2014 2 OPENFOAM GUIDE FOR BEGINNERS
More 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 informationErosion modeling to improve asset life prediction
Erosion modeling to improve asset life prediction Erosion caused by solid particles in process flows impacting on the surfaces of downhole equipment or pipe walls is a common cause of damage and wear in
More informationHeat 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
More informationOffshore Platform Fluid Structure Interaction (FSI) Simulation
Offshore Platform Fluid Structure Interaction (FSI) Simulation Ali Marzaban, CD-adapco Murthy Lakshmiraju, CD-adapco Nigel Richardson, CD-adapco Mike Henneke, CD-adapco Guangyu Wu, Chevron Pedro M. Vargas,
More informationNumerical Simulation of Regular Wave in a Tank
Numerical Simulation of Regular Wave in a Tank Authors: Monica Campos Silva, Dr. student PENO/UFRJ email: mcsilva@peno.coppe.ufrj.br Waldir Terra Pinto, Dr. FURG email: w_pinto@dmc.furg.br Marcelo de A.
More informationDYNAMIC ANALYSIS OF A GENERATOR ON AN ELASTIC FOUNDATION
DYNAMIC ANALYSIS OF A GENERATOR ON AN ELASTIC FOUNDATION 7 DYNAMIC ANALYSIS OF A GENERATOR ON AN ELASTIC FOUNDATION In this tutorial the influence of a vibrating source on its surrounding soil is studied.
More informationWAVE PATTERNS, WAVE INDUCED FORCES AND MOMENTS FOR A GRAVITY BASED STRUCTURE PREDICTED USING CFD
Proceedings of the ASME 2011 30th International Conference on Ocean, Offshore and Arctic Engineering OMAE2011 June 19-24, 2011, Rotterdam, The Netherlands OMAE2011-49593 WAVE PATTERNS, WAVE INDUCED FORCES
More informationCFD VALIDATION FOR SURFACE COMBATANT 5415 STRAIGHT AHEAD AND STATIC DRIFT 20 DEGREE CONDITIONS USING STAR CCM+
CFD VALIDATION FOR SURFACE COMBATANT 5415 STRAIGHT AHEAD AND STATIC DRIFT 20 DEGREE CONDITIONS USING STAR CCM+ by G. J. Grigoropoulos and I..S. Kefallinou 1. Introduction and setup 1. 1 Introduction The
More 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 informationCFD Simulation of Cavitation in an Internal Gear Pump
CFD Simulation of Cavitation in an Internal Gear Pump Dr. Andreas Spille-Kohoff Jan Hesse CFX Berlin Software GmbH Berlin andreas.spille@cfx-berlin.de Contents Introduction Geometry and mesh Simulation
More informationMoving Interface Problems: Methods & Applications Tutorial Lecture II
Moving Interface Problems: Methods & Applications Tutorial Lecture II Grétar Tryggvason Worcester Polytechnic Institute Moving Interface Problems and Applications in Fluid Dynamics Singapore National University,
More informationEXPERIMENTAL VALIDATION OF STAR-CCM+ FOR LIQUID CONTAINER SLOSH DYNAMICS
EXPERIMENTAL VALIDATION OF STAR-CCM+ FOR LIQUID CONTAINER SLOSH DYNAMICS Brandon Marsell a.i. solutions, Launch Services Program, Kennedy Space Center, FL 1 Agenda Introduction Problem Background Experiment
More informationEffect of initial turbulence intensity and velocity profile on liquid jets for IFE beamline protection
Effect of initial turbulence intensity and velocity profile on liquid jets for IFE beamline protection A. Konkachbaev, N.B. Morley and M. A. Abdou Mechanical and Aerospace Engineering Department, UCLA
More informationEFFECTS OF COMPUTATIONAL MESHES ON HYDRODYNAMICS OF AN OPEN CHANNEL JUNCTIONS FLOW USING CFD TECHNIQUE
9th International Conference on Urban Drainage Modelling Belgrade 2012 EFFECTS OF COMPUTATIONAL MESHES ON HYDRODYNAMICS OF AN OPEN CHANNEL JUNCTIONS FLOW USING CFD TECHNIQUE Adrien Momplot, Hossein Bonakdari,
More informationParallelization study of a VOF/Navier-Stokes model for 3D unstructured staggered meshes
Parallelization study of a VOF/Navier-Stokes model for 3D unstructured staggered meshes L. Jofre, O. Lehmkuhl, R. Borrell, J. Castro and A. Oliva Corresponding author: cttc@cttc.upc.edu Centre Tecnològic
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 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 informationThe Level Set Method THE LEVEL SET METHOD THE LEVEL SET METHOD 203
The Level Set Method Fluid flow with moving interfaces or boundaries occur in a number of different applications, such as fluid-structure interaction, multiphase flows, and flexible membranes moving in
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 informationANSYS 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
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 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 informationComparison of Two-Phase Pipe Flow in OpenFOAM with a Mechanistic Model
Comparison of Two-Phase Pipe Flow in OpenFOAM with a Mechanistic Model Adrian M Shuard 1, Hisham B Mahmud 2, Andrew J King 3 1 Mechanical Engineering Department, 2 Petroleum Engineering Department, Curtin
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 informationTerminal Falling Velocity of a Sand Grain
Terminal Falling Velocity of a Sand Grain Introduction The first stop for polluted water entering a water work is normally a large tank, where large particles are left to settle. More generally, gravity
More 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 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 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 informationCoupled Simulation of the Fluid Flow and Conjugate Heat Transfer in Press Hardening Processes
13 th International LS-DYNA Users Conference Session: Metal Forming Coupled Simulation of the Fluid Flow and Conjugate Heat Transfer in Press Hardening Processes Uli Göhner 1), Bruno Boll 1), Inaki Caldichouri
More informationMesh Morphing and the Adjoint Solver in ANSYS R14.0. Simon Pereira Laz Foley
Mesh Morphing and the Adjoint Solver in ANSYS R14.0 Simon Pereira Laz Foley 1 Agenda Fluent Morphing-Optimization Feature RBF Morph with ANSYS DesignXplorer Adjoint Solver What does an adjoint solver do,
More informationTeam 194: Aerodynamic Study of Airflow around an Airfoil in the EGI Cloud
Team 194: Aerodynamic Study of Airflow around an Airfoil in the EGI Cloud CFD Support s OpenFOAM and UberCloud Containers enable efficient, effective, and easy access and use of MEET THE TEAM End-User/CFD
More informationDesign Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD)
Design Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD) Fernando Prevedello Regis Ataídes Nícolas Spogis Wagner Ortega Guedes Fabiano Armellini
More informationHIGH PERFORMANCE COMPUTATION (HPC) FOR THE
HIGH PERFORMANCE COMPUTATION (HPC) FOR THE DEVELOPMENT OF FLUIDIZED BED TECHNOLOGIES FOR BIOMASS GASIFICATION AND CO2 CAPTURE P. Fede, H. Neau, O. Simonin Université de Toulouse; INPT, UPS ; IMFT ; 31400
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 informationApplication of A Priori Error Estimates for Navier-Stokes Equations to Accurate Finite Element Solution
Application of A Priori Error Estimates for Navier-Stokes Equations to Accurate Finite Element Solution P. BURDA a,, J. NOVOTNÝ b,, J. ŠÍSTE a, a Department of Mathematics Czech University of Technology
More informationFirst Steps - Ball Valve Design
COSMOSFloWorks 2004 Tutorial 1 First Steps - Ball Valve Design This First Steps tutorial covers the flow of water through a ball valve assembly before and after some design changes. The objective is to
More 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 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 informationALE and AMR Mesh Refinement Techniques for Multi-material Hydrodynamics Problems
ALE and AMR Mesh Refinement Techniques for Multi-material Hydrodynamics Problems A. J. Barlow, AWE. ICFD Workshop on Mesh Refinement Techniques 7th December 2005 Acknowledgements Thanks to Chris Powell,
More informationITTC Recommended Procedures and Guidelines
Page 1 of 9 Table of Contents 1. OVERVIEW... 2 2. CHOICE OF MODEL OR FULL SCALE... 2 3. NOMINAL WAKE IN MODEL SCALE... 3 3.1 Pre-processing... 3 3.1.1 Geometry... 3 3.1.2 Computational Domain and Boundary
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 information