Answers to Webinar "Wind farm flow modelling using CFD update" Q&A session
|
|
- Allison Caldwell
- 5 years ago
- Views:
Transcription
1 Answers to Webinar "Wind farm flow modelling using CFD update" Q&A session Christiane Montavon, Ian Jones Physics related Q: Should the roughness map be scaled from the normal WAsP map to the CFD analysis? A: WindModeller expects that the roughness provided in a WAsP.map file will be an aerodynamic roughness z 0. For the simulation, the solver needs a roughness specified as an equivalent sand roughness. The transformation from z 0 to equivalent sand roughness is taken care of within WindModeller, using a relationship between the two which is consistent with the law of the wall applied internally in the solver. Q: Why is it necessary to run transiently when the stability model is on? A: When free stream stability is included, the solution tends to produce gravity waves which travel through the domain. Our experience is that trying to solve this in a steady state mode is not physical and can lead to a complete destabilisation of the flow even for cases where a stationary solution develops over time. When surface stability is included (representing ground heating/cooling), the process is by nature transient (giving rise in particular to the diurnal cycle) and a steady state solution rarely exists. Q: Where in the GUI do you define your stability input? A: Stability is still a beta feature (still evolving) so for now is not available from within the GUI. It can be specified in the parameter file, when WindModeller is run from the command line. The details of how to do this are available from us. Q: How is real mast data used (besides annual energy calculation)? Is it used to adjust the simulation process? A: It is only used for the annual energy calculation, and the simulations are only done at specified reference wind speeds. For cases where the solution is expected to be strongly dependent on the reference wind speed (e.g. when wakes are included, where strong separation is expected), it is worth saying that the user can prescribe more than one reference wind speed for the simulations to be carried out.
2 Q: Is it recommended to run a simulation with different initial conditions (wind speed inlet at 5m/s and then 10m/s?) and evaluate the behaviour? A: This is very dependent on the physics included in the model. Our experience when running with neutral simulations shows that when you model wakes or forestry, the resulting normalised wind speed and normalised turbulence intensity are sensitive to the reference wind speed used. If a user wants to perform simulations at varying reference wind speeds he can do so within a single WindModeller set up (see above). Q: Does your turbine wake effect also include swirl? A: The actuator disk model in WindModeller does not take swirl into account. We have done some tests on variations of the model, to include turbulence generation, swirl, radial variation of the thrust, and also comparisons between Blade Element Theory, using supplied sectional lift and drag coefficients. Some of these variations may make their way into WindModeller in the future, once we have a better idea of which one brings consistent and significant improvement on the results, but our tests so far indicate that these effects are secondary effects, compared to the main blockage effects. Q: Can we nest a mesoscale model with ANSYS? A: We haven t done this at the moment, but one of our customers has implemented this. Q: k- and SST (Menter) turbulence model. Have you tested both turbulence models? What were the discrepancies found? A: Because of its better reputation for capturing flow separation, and better robustness when working with high roughness values, we tend to use the SST turbulence model for complex terrain cases. The SST turbulence model is the default model used in WindModeller. For wake modelling in offshore cases however, we tend to recommend k-. The reasons for the latter are two-fold: separation is not an issue offshore, and in terms of accuracy of the multiple wakes in large arrays we find that k- tends to be more accurate than SST for downstream distances between 6 and 10 turbine diameters which are quite typical of the turbine spacing seen in large arrays. HPC, CPU time related Q: What is the approximate computational time for a typical simulation? A: This is to a large extent dependent on the physics which is used (wakes/no wakes, neutral vs stability) as well as obviously the mesh size.
3 To provide a few examples, we shall give some required times for some of the cases shown in the presentation: 1. Harestanes, neutral simulations (steady state), without wakes, horizontal mesh resolution in central square of 50m, first cell height of 0.5m, domain radius: 15km, domain height: 4km. Mesh size: 2.16 million nodes. Elapsed time per individual simulation: ~37 minutes, running 12 parallel on CPU Type: Intel Xeon X GHz (RAM Memory per Machine: 48 Gigabytes). Simulations are required to converge down to strict RMS residuals of 1e-5, which in this case takes between 50 and 60 iterations. For such a case, a whole WindModeller run for 12 sectors (including pre-processing, solution and post-processing) takes approximately 9 hours. 2. Harestanes, transient simulations with stability, stationary solution reached after ~ 200 time steps. Same domain as case 1 above. Each individual simulation takes ~ min (i.e. approximately 3 times the required time for neutral simulations). 3. Horns Rev, neutral, wake model enabled, 80 turbines. Horizontal mesh resolution in central square of 50m (before mesh adaption), first cell height of 2m, domain radius: 10km, domain height: 1km. Mesh size: 690k nodes before adaption, 2.16 million nodes after adaption. Elapsed time per individual simulation: ~ 26 min, running 12 parallel on CPU Type: Intel Xeon X GHz (RAM Memory per Machine: 48 Gigabytes). Q: Is there any limit to the maximum number of turbines the model can include. A: There is no hardcoded limit. The limit is the size of the machine you are running on. The largest case we ran so far had more than 1800 turbines and was run on 16 processors distributed across two machines on our cluster (each machine with 48 Gigabytes of RAM). Q: How does your simulation time scale up with mesh size? A: This to some extent depends on the selected physics. But for a basic setup (neutral, no wakes) the scaling is more or less linear. Larger mesh sizes can be accommodated by distributing the simulation across a larger number of processors. HPC packs for licenses are available for HPC clusters allowing each simulation to be run on e.g. 32 or 128 processors. Please get in touch for more specific details. Mesh, domain size related. Q: Ho do we change the size of the centre square used in the meshing section? A: The relative size of the central square to the domain radius is controlled by the parameter Centre Block Radius Fraction which is set on the Mesh tab in the GUI.
4 Q: Is there any restriction to the number of cells used for higher resolution? What typical horizontal/vertical resolution do you work with? A: The only limit is the memory available on your computer and the number of CPU you have access to. The horizontal resolution of 100m used in the demo is only for demo purpose. When doing a site assessment we typically work with a horizontal resolution of 20 to 50m in the central part, using horizontal expansion factors around 1.1 in the outer domain. In the vertical, we typically set a first cell height to 1m, and ensure that the vertical expansion factor recalculated for smooth transition of the cell size is also around 1.1. In terms of the set up however, there is no lower limit to the specified resolution. For the Bolund test case, for example, we did some simulations with a horizontal resolution of 1m and first cell height of 0.1m. Q: Why ANSYS is using a "round" domain rather than a "cube" we have seen? What is the advantage?" A: Using a round domain makes it easier to specify inlet/outlet boundary conditions as a function of the wind direction when using a single mesh. With this approach, when smoothing the terrain in the outer part of the domain, we ensure that the same smoothed terrain is applied for every wind direction. This way, small changes in the upstream wind directions are treated consistently without inducing inconsistent behaviours associated with artificial changes in the treatment of the terrain. In addition, in the outer regions where the mesh is coarser, the flow is aligned with the mesh, reducing the associated numerical errors. Q: Is WindModeller able to pre-process and merge large coarse resolution SRTM map (10m resolution, 20kmX20km) and smaller higher resolution (2m resolution, 5kmX5km) map? A: Not automatically. The utility in WindModeller that reads SRTM files is able to read standard SRTM and the SRTM DTED format, and produce ASCII terrain files from both, but is not able to automatically do a merging of both types of files. In such cases, a user has however the option to manually merge the resulting ASCII files, filter the data by regions, and use this merged file as an input to the simulation. Q: It would be nice to automatically calculate the centre of the wind farm. A: While it may be a desired feature to automatically centre the simulation domain on to the centre location given by the wind farm layout, it is not always what the users want to do. In particular, the user may want some control over the centre and extent, to be able to make sure that the appropriate terrain features are included, or excluded, from the domain. Also sometimes when the masts are some distance away from the wind farm, the user may want to centre the domain halfway between some mast and the wind farm. All in all we feel that providing the user with the flexibility of setting the centre has more benefit than drawbacks. But if it is felt that automatically centring the simulation domain onto the centre of the wind farm is a must have, it could be implemented easily.
5 Postprocessing related Q: After a WindModeller set of simulations has finished, can you go back and perform additional post-processing on the simulation? A: Yes you can. The results (.res) files from a WindModeller set up are kept and available for the user to open in our standard CFD Postprocessor. If a user wants to include additional post-processing to the standard output given by WindModeller, he can interactively create a session file in our standard post-processor which can later be called within WindModeller in order to customise the output provided by WindModeller. Examples of this are given in the WindModeller Tutorials. Q: Can we export the images/graphs of our results in eps or png or tiff files? A: Yes you can. The pictures and graphs produced by WindModeller shown in the Report html file are also saved in the Report directory. The default format is.png. Additional format options for the images from the Postprocessor would be (bmp, jpg, pbm, ps, eps). x-y graphs have a more limited range of formats (png, bmp, pbm, xpm). There is also an option to save them as 3D pictures that you can then view with the (free) viewer that comes with our post-processing tool. This allows you to zoom in/out, rotate, translate your picture in order to get a better idea of what you see in some part of the flow. It is also worth pointing out that the profile data at the masts and wind turbines corresponding to the graphs produced by WindModeller is also exported for all the individual simulations. So if users want to post-process these in another package, where they may want to compare them with measured profiles, they can do so. Others Q: What differences are there between using the CFX and Fluent solvers in WindModeller and what are the implications of each? A: New developments in WindModeller tend to make their way into the CFX version first, as the models can be implemented in the CFX Expression Language, rather than by writing User Defined Functions. This is the version that we tend to recommend by default to new users. At existing FLUENT customers request we have included FLUENT in the WindModeller workflow, however at this point, the forestry model and the stability implementation are not yet available in the FLUENT version.
6 Q: Taking into account that many people use Mac are you planning to develop a version for Mac OS X? A: Unlikely in the short term, as standard ANSYS products are not available on OS X. Q: What are the differences between WindModeller and WindSim or MeteoDyn? A: Many! We don t want to get into details of what these software packages do, as they are also evolving. We therefore prefer to focus on our features, such as the use of unstructured and adaptive gridding, the fast convergence of the Coupled Solver algorithms, when associated with the Algebraic Multi-grid method, and our state of the art turbulence models, which have been extensively validated across a wide range of problems. Please get in touch if you want to find out more about the details of our software. Q: Do you have any plans to provide an option for automatic layout optimisation? A: Various products are available to provide site optimisation starting typically from a wind resource grid (.wrg) and using empirical wake models, and various constraints for the site. We have plans to ensure that you can use the output from WindModeller in this context (e.g. through a.wrg file from a WindModeller set up that ignored wake effects). At the moment, we feel that a site optimisation while resolving the wakes via actuator disks as we do in our simulations would be too slow to be economically attractive. Q: How is real mast data compared to CFD result? By turbulence intensity or speed-up factors? Are the two comparable? A: So far, we have mostly done mast to mast cross predictions for the average wind speed not so much for the turbulence intensity. The option to transpose turbulence intensity is very new and we haven t got a lot of experience with the level of accuracy that can be achieved from it. From the limited experience we have so far we find that average wind speed is usually better predicted that the average TI.
Introduction to ANSYS CFX
Workshop 03 Fluid flow around the NACA0012 Airfoil 16.0 Release Introduction to ANSYS CFX 2015 ANSYS, Inc. March 13, 2015 1 Release 16.0 Workshop Description: The flow simulated is an external aerodynamics
More informationRecent Advances in Modelling Wind Parks in STAR CCM+ Steve Evans
Recent Advances in Modelling Wind Parks in STAR CCM+ Steve Evans Introduction Company STAR-CCM+ Agenda Wind engineering at CD-adapco STAR-CCM+ & EnviroWizard Developments for Offshore Simulation CD-adapco:
More informationCFD wake modeling using a porous disc
CFD wake modeling using a porous disc Giorgio Crasto, Arne Reidar Gravdahl giorgio@windsim.com, arne@windsim.com WindSim AS Fjordgaten 5 N-325 Tønsberg Norway Tel. +47 33 38 8 Fax +47 33 38 8 8 http://www.windsim.com
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 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 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 informationTHE INFLUENCE OF MESH CHARACTERISTICS ON OPENFOAM SIMULATIONS OF THE DRIVAER MODEL
6 th BETA CAE International Conference THE INFLUENCE OF MESH CHARACTERISTICS ON OPENFOAM SIMULATIONS OF THE DRIVAER MODEL Grigoris Fotiadis *, Vangelis Skaperdas, Aristotelis Iordanidis BETA CAE Systems
More informationGetting benefits from CFD. in the wind energy industry
Getting benefits from CFD in the wind energy industry Didier DELAUNAY - METEODYN www.meteodyn.com (In Turkey: www.ucyel.com.tr) Meteodyn software suite Meteodyn WT Meteodyn Forecast TopoWind UrbaWind SimulaWind
More informationHigh-Lift Aerodynamics: STAR-CCM+ Applied to AIAA HiLiftWS1 D. Snyder
High-Lift Aerodynamics: STAR-CCM+ Applied to AIAA HiLiftWS1 D. Snyder Aerospace Application Areas Aerodynamics Subsonic through Hypersonic Aeroacoustics Store release & weapons bay analysis High lift devices
More informationMissile External Aerodynamics Using Star-CCM+ Star European Conference 03/22-23/2011
Missile External Aerodynamics Using Star-CCM+ Star European Conference 03/22-23/2011 StarCCM_StarEurope_2011 4/6/11 1 Overview 2 Role of CFD in Aerodynamic Analyses Classical aerodynamics / Semi-Empirical
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 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 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 informationCFD Methods for Aerodynamic Design
CFD Methods for Aerodynamic Design Afandi Darlington Optimal Aerodynamics Ltd Why CFD? Datasheet methods are still very relevant today (ESDU, USAF DATCOM) Validated estimates of lift, drag, moments, stability
More informationPreliminary investigation into two-way fluid structure interaction of heliostat wind loads Josh Wolmarans
Preliminary investigation into two-way fluid structure interaction of heliostat wind loads Josh Wolmarans Supervisor: Prof Ken Craig Clean Energy Research Group (CERG), Department of Mechanical and Aeronautical
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 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 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 informationRBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent
RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent Gilles Eggenspieler Senior Product Manager 1 Morphing & Smoothing A mesh morpher is a tool capable of performing mesh modifications in order
More informationPost conversion of Lidar data on complex terrains
Post conversion of Lidar data on complex terrains Stéphane SANQUER (1), Alex WOODWARD (2) (1) Meteodyn (2) ZephIR Lidar 1. Introduction Data from remote sensing devices (RSD) are now widely accepted for
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 informationDetached Eddy Simulation Analysis of a Transonic Rocket Booster for Steady & Unsteady Buffet Loads
Detached Eddy Simulation Analysis of a Transonic Rocket Booster for Steady & Unsteady Buffet Loads Matt Knapp Chief Aerodynamicist TLG Aerospace, LLC Presentation Overview Introduction to TLG Aerospace
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 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 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 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 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 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 informationCFD Modelling of Erosion in Slurry Tee-Junction
CFD Modelling of Erosion in Slurry Tee-Junction Edward Yap Jeremy Leggoe Department of Chemical Engineering The University of Western Australia David Whyte CEED Client: Alumina Centre of Excellence, Alcoa
More informationUsing WindSim by means of WindPRO-interface gives the user many advantages:
1 Content: Content:...1 1. Introduction...1 Using WindSim by means of WindPRO-interface gives the user many advantages:...1 Important Limitations...2 Important Information about Nested Calculation...2
More informationSimulation and Optimization in the wind energy industry
Simulation and Optimization in the wind energy industry Numerical Simulation & Optimization www.ozeninc.com/optimization optimization@ozeninc.com Summary Why to use numerical simulations and optimization?
More informationSimulation of In-Cylinder Flow Phenomena with ANSYS Piston Grid An Improved Meshing and Simulation Approach
Simulation of In-Cylinder Flow Phenomena with ANSYS Piston Grid An Improved Meshing and Simulation Approach Dipl.-Ing. (FH) Günther Lang, CFDnetwork Engineering Dipl.-Ing. Burkhard Lewerich, CFDnetwork
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 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 informationNASA Rotor 67 Validation Studies
NASA Rotor 67 Validation Studies ADS CFD is used to predict and analyze the performance of the first stage rotor (NASA Rotor 67) of a two stage transonic fan designed and tested at the NASA Glenn center
More informationRANS COMPUTATION OF RIBBED DUCT FLOW USING FLUENT AND COMPARING TO LES
RANS COMPUTATION OF RIBBED DUCT FLOW USING FLUENT AND COMPARING TO LES Máté M., Lohász +*& / Ákos Csécs + + Department of Fluid Mechanics, Budapest University of Technology and Economics, Budapest * Von
More informationSTAR-CCM+: Wind loading on buildings SPRING 2018
STAR-CCM+: Wind loading on buildings SPRING 2018 1. Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 3, 11 pm) 1. NOTES ON THE SOFTWARE STAR-CCM+ generates
More 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 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 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 informationCFD-RANS APPLICATIONS IN COMPLEX TERRAIN ANALYSIS. NUMERICAL VS EXPERIMENTAL RESULTS A CASE STUDY: COZZOVALLEFONDI WIND FARM IN SICILY
CFD-RANS APPLICATIONS IN COMPLEX TERRAIN ANALYSIS. NUMERICAL VS EXPERIMENTAL RESULTS A CASE STUDY: COZZOVALLEFONDI WIND FARM IN SICILY J.Maza (*),G.Nicoletti(**), (*) Pisa University, Aerospace Engineering
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 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 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 informationDrivAer-Aerodynamic Investigations for a New Realistic Generic Car Model using ANSYS CFD
DrivAer-Aerodynamic Investigations for a New Realistic Generic Car Model using ANSYS CFD Thomas Frank (*), BenediktGerlicher (*), Juan Abanto (**) (*) ANSYS Germany, Otterfing, Germany (**) ANSYS Inc.,
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 informationSmall Height Duct Design for 17 Multicopter Fan Considering Its Interference on Quad-copter
Small Height Duct Design for 17 Multicopter Fan Considering Its Interference on Quad-copter Stremousov K.*, Arkhipov M.* **, Serokhvostov S.* ** * Moscow Institute of Physics and Technology, Department
More informationUsage of CFX for Aeronautical Simulations
Usage of CFX for Aeronautical Simulations Florian Menter Development Manager Scientific Coordination ANSYS Germany GmbH Overview Elements of CFD Technology for aeronautical simulations: Grid generation
More informationNumerische Untersuchungen von Windkraftanlagen: Leistung, Wake und Steuerungsstrategien
Fachtagung Lasermethoden in der Strömungsmesstechnik 8. 10. September 2015, Dresden Numerische Untersuchungen von Windkraftanlagen: Leistung, Wake und Steuerungsstrategien Numerical Investigations of Wind
More informationComparison of CFD Simulation of a Hyundai I20 Model with Four Different Turbulence Models
RESEARCH ARTICLE OPEN ACCESS Comparison of CFD Simulation of a Hyundai I20 with Four Different Turbulence s M. Vivekanandan*, R. Sivakumar**, Aashis. S. Roy*** *(Uttam Industrial Engg. Pvt. Ltd., Tiruchirapalli,
More informationThe Spalart Allmaras turbulence model
The Spalart Allmaras turbulence model The main equation The Spallart Allmaras turbulence model is a one equation model designed especially for aerospace applications; it solves a modelled transport equation
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 informationReproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software
Reports of Research Institute for Applied Mechanics, Kyushu University No.150 (47 59) March 2016 Reproducibility of Complex Turbulent Using Commercially-Available CFD Software Report 1: For the Case of
More informationPARAMETERIZATION OF DRAG FORCES IN URBAN CANOPY MODELS USING MICROSCALE-CFD MODELS FOR DIFFERENT WIND DIRECTIONS
PARAMETERIZATION OF DRAG FORCES IN URBAN CANOPY MODELS USING MICROSCALE-CFD MODELS FOR DIFFERENT WIND DIRECTIONS J. L. Santiago 1, O. Coceal 2 and A. Martilli 1 1 Atmospheric Pollution Division, Environmental
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 informationSpeed and Accuracy of CFD: Achieving Both Successfully ANSYS UK S.A.Silvester
Speed and Accuracy of CFD: Achieving Both Successfully ANSYS UK S.A.Silvester 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Content ANSYS CFD Introduction ANSYS, the company Simulation
More informationEstimating Vertical Drag on Helicopter Fuselage during Hovering
Estimating Vertical Drag on Helicopter Fuselage during Hovering A. A. Wahab * and M.Hafiz Ismail ** Aeronautical & Automotive Dept., Faculty of Mechanical Engineering, Universiti Teknologi Malaysia, 81310
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 informationCFD Project Workflow Guide
CFD Project Workflow Guide Contents Select a problem with known results for proof-of-concept testing... 1 Set up and run a coarse test case... 2 Select and calibrate numerical methods... 3 Minimize & quantify
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 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 informationCFD Application in Offshore Structures Design at PETROBRAS
CFD Application in Offshore Structures Design at PETROBRAS Marcus Reis ESSS CFD Director Mooring System Design of Floating Production Systems; Current and Wind Loads; Wave Induced Drag Coefficients. Case
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 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 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 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 informationRecent Developments WIND KNOWLEDGE. WindSim 12 th User Meeting, Tønsberg June PRESENTED BY: Dr. Catherine Meissner IS WIND POWER
IS WIND POWER WIND KNOWLEDGE Recent Developments WindSim 12 th User Meeting, Tønsberg 22-23 June 2017 PRESENTED BY: Dr. Catherine Meissner WindSim 12th User Meeting, Tønsberg 22-23 June 2017 1 Content
More informationComputational Fluid Dynamics Simulation of a Rim Driven Thruster
Computational Fluid Dynamics Simulation of a Rim Driven Thruster Aleksander J Dubas, N. W. Bressloff, H. Fangohr, S. M. Sharkh (University of Southampton) Abstract An electric rim driven thruster is a
More informationCo-Simulation von Flownex und ANSYS CFX am Beispiel einer Verdrängermaschine
Co-Simulation von Flownex und ANSYS CFX am Beispiel einer Verdrängermaschine Benoit Bosc-Bierne, Dr. Andreas Spille-Kohoff, Farai Hetze CFX Berlin Software GmbH, Berlin Contents Positive displacement compressors
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 informationModelling of Bridge Pier Afflux in 2D. Bill Syme / Phillip Ryan
Modelling of Bridge Pier Afflux in 2D Bill Syme / Phillip Ryan Presentation Overview Modelling of Bridge Afflux Why is it important Common Methods used Test Model Numerical Engines Used Model Configuration
More informationSTAR-CCM+: Ventilation SPRING Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 9, 11 pm)
STAR-CCM+: Ventilation SPRING 208. Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 9, pm). Features of the Exercise Natural ventilation driven by localised
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 informationLarge Data Set Computations with CFX: To 100 Million Nodes & Beyond!
Large Data Set Computations with CFX: To 100 Million Nodes & Beyond! Dr. Mark E. Braaten Mechanical Engineer GE Global Research, Niskayuna, NY Acknowledgements Thanks to many people, in particular: GEGR
More informationInduction zone measurements and simulations at Perdigão. Alexander Meyer Forsting, Niels Troldborg, Andreas Bechmann, Nikolas Angelou
Induction zone measurements and simulations at Perdigão Alexander Meyer Forsting, Niels Troldborg, Andreas Bechmann, Nikolas Angelou Overview The induction zone Power curve measurements The UniTTe project
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 informationDEVELOPMENT OF A TOOL FOR OFFSHORE WIND RESOURCE ASSESSMENT FOR WIND INDUSTRY
DEVELOPMENT OF A TOOL FOR OFFSHORE WIND RESOURCE ASSESSMENT FOR WIND INDUSTRY Alberto Rabaneda Dr. Matthew Stickland University of Strathclyde Mechanical and Aerospace Engineering Department Wind resource
More informationEvaluation of hydrodynamic coefficients on riser floaters using CFD
Evaluation of hydrodynamic coefficients on riser floaters using CFD Erico Santos, Pedro Mendes, Bruno Luna PETROBRAS (CENPES/PDEP/TDUT) Ricardo Damian ESSS AGENDA MOTIVATION PROCEADURE OVERVIEW RISER GLOBAL
More informationANSYS Fluid Structure Interaction for Thermal Management and Aeroelasticity
ANSYS Fluid Structure Interaction for Thermal Management and Aeroelasticity Phil Stopford Duxford Air Museum 11th May 2011 2011 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Fluid Structure
More informationCFD Analysis of a Novel Hull Design for an Offshore Wind Farm Service Vessel
CFD Analysis of a Novel Hull Design for an Offshore Wind Farm Service Vessel M. Shanley 1, J. Murphy 1, and P. Molloy 2 1 Hydraulics and Maritime, Civil and Environmental Engineering University College
More informationFeature list. New in windpro 3.2
Feature list New in windpro 3.2 1 Contents 1.1 NEW: Multiple windpro instances... 2 1.2 BASIS: Dynamic background maps... 2 1.3 NEW: MCP tool... 2 1.4 NEW: METEO flagging/screening/validating... 2 1.5
More informationResearch and Design working characteristics of orthogonal turbine Nguyen Quoc Tuan (1), Chu Dinh Do (2), Quach Thi Son (2)
GSJ: VOLUME 6, ISSUE 6, JUNE 018 116 Research and Design working characteristics of orthogonal turbine Nguyen Quoc Tuan (1), Chu Dinh Do (), Quach Thi Son () (1) Institute for hydro power and renewable
More informationTurbulence Modeling. Gilles Eggenspieler, Ph.D. Senior Product Manager
Turbulence Modeling Gilles Eggenspieler, Ph.D. Senior Product Manager 1 Overview The Role of Steady State (RANS) Turbulence Modeling Overview of Reynolds-Averaged Navier Stokes (RANS) Modeling Capabilities
More informationKeywords: CFD, aerofoil, URANS modeling, flapping, reciprocating movement
L.I. Garipova *, A.N. Kusyumov *, G. Barakos ** * Kazan National Research Technical University n.a. A.N.Tupolev, ** School of Engineering - The University of Liverpool Keywords: CFD, aerofoil, URANS modeling,
More informationUse of STAR-CCM+ in Marine and Off-Shore Engineering - Key Features and Future Developments - M. Perić, F. Schäfer, E. Schreck & J.
Use of STAR-CCM+ in Marine and Off-Shore Engineering - Key Features and Future Developments - M. Perić, F. Schäfer, E. Schreck & J. Singh Contents Main features of STAR-CCM+ relevant for marine and offshore
More informationHydro-elastic analysis of a propeller using CFD and FEM co-simulation
Fifth International Symposium on Marine Propulsors smp 17, Espoo, Finland, June 2017 Hydro-elastic analysis of a propeller using CFD and FEM co-simulation Vesa Nieminen 1 1 VTT Technical Research Centre
More informationS-ducts and Nozzles: STAR-CCM+ at the Propulsion Aerodynamics Workshop. Peter Burns, CD-adapco
S-ducts and Nozzles: STAR-CCM+ at the Propulsion Aerodynamics Workshop Peter Burns, CD-adapco Background The Propulsion Aerodynamics Workshop (PAW) has been held twice PAW01: 2012 at the 48 th AIAA JPC
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 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 informationApplication of STAR-CCM+ to Helicopter Rotors in Hover
Application of STAR-CCM+ to Helicopter Rotors in Hover Lakshmi N. Sankar and Chong Zhou School of Aerospace Engineering, Georgia Institute of Technology, Atlanta, GA Ritu Marpu Eschol CD-Adapco, Inc.,
More informationValidation of a Multi-physics Simulation Approach for Insertion Electromagnetic Flowmeter Design Application
Validation of a Multi-physics Simulation Approach for Insertion Electromagnetic Flowmeter Design Application Setup Numerical Turbulence ing by March 15, 2015 Markets Insertion electromagnetic flowmeters
More informationHigh Performance Unsteady Workflows with STAR-CCM+
High Performance Unsteady Workflows with STAR-CCM+ Steve M. Legensky Founder & Gen. Mgr. Intelligent Light Agenda Intelligent Light Background of Bike Wheel Aerodynamic Study Scope & Methodology of Current
More informationUsing ANSYS and CFX to Model Aluminum Reduction Cell since1984 and Beyond. Dr. Marc Dupuis
Using ANSYS and CFX to Model Aluminum Reduction Cell since1984 and Beyond Dr. Marc Dupuis 1980-84, 2D potroom ventilation model Physical model 1980-84, 2D potroom ventilation model Experimental results
More informationSingle Wake Meandering, Advection and Expansion - An analysis using an adapted Pulsed Lidar and CFD LES-ACL simulations
Downloaded from orbit.dtu.dk on: Jan 10, 2019 Single Wake Meandering, Advection and Expansion - An analysis using an adapted Pulsed Lidar and CFD LES-ACL simulations Machefaux, Ewan; Larsen, Gunner Chr.;
More informationGetting started. When the terrain gets rough
4.8.1 Getting started 28.05.2008 WindSim AS Fjordgaten 15 N-3125 Tønsberg Norway Phone: +47 33 38 18 00 Fax: +47 33 38 18 08 http://www.windsim.com When the terrain gets rough WindSim 4.8.1, evaluation
More informationCFD projects at CERN Detector cooling and beyond
CFD projects at CERN Detector cooling and beyond CFD.HU ANSYS User Group Meeting, Budapest 27th November 2015 Aniko Rakai CERN EN-CV, CFD team 11/20/2015 A. Rakai 2 Overview CFD team at CERN SHIP experiment
More informationAxial Fan Optimization Workflow
Axial Fan Optimization Workflow Turbomachinery design optimization using TCFD and CAESES Radek Máca, PhD Head CFD Engineer CFD Support radek.maca@cfdsupport.com Ceyhan Erdem Project and Support Engineer
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 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 informationAshwin Shridhar et al. Int. Journal of Engineering Research and Applications ISSN : , Vol. 5, Issue 6, ( Part - 5) June 2015, pp.
RESEARCH ARTICLE OPEN ACCESS Conjugate Heat transfer Analysis of helical fins with airfoil crosssection and its comparison with existing circular fin design for air cooled engines employing constant rectangular
More information