A Comparison of RANS-Based Turbulence Modeling for Flow over a Wall-Mounted Square Cylinder
|
|
- Caren Shields
- 6 years ago
- Views:
Transcription
1 A Comparison of RANS-Based Turbulence Modeling for Flow over a Wall-Mounted Square Cylinder P. L. Davis 1, A. T. Rinehimer 2, and M.Uddin 3 N C Motorsports and Automotive Research Center, Department of Mechanical Engineering and Engineering Science, The University of North Carolina at Charlotte, Charlotte, NC 28223, USA 1 pdavis24@uncc.edu 2 arinehim@uncc.edu 3 muddin@uncc.edu s ABSTRACT Using experimental data from a study of flow over a wall-mounted square cylinder (h=4 as a baseline, three Reynolds-Averaged Navier-Stokes turbulence models are used in a commercial CFD code Star- CCM+ to compare the relative accuracy of the tested models. In virtually every standard of comparison applied in this study, the Realizable k ε with a twolayer treatment proved to be far superior to both the k ε V2F (All y + hybrid wall treatment) and the k ω models. To observe mesh dependence for each of the models, all three were run on three different polyhedral mesh cases. Resulting first prism-layer heights of y + 12, y + 5, and y + 1 allowed comparison of results with the mesh resolved to the buffer layer, the buffer layer/viscous sublayer transformation, and into the viscous sublayer, respectively. In all cases, the Realizable k ε proved superior. The mesh study also suggests that applying the twolayer treatment to Realizable k ε allows it to operate well into the viscous sublayer, an area in which k ε models are traditionally expected to suffer degradation in accuracy. The k ω scheme, however, does not show improvements with increased mesh quality. In contradiction to the expected results, mesh independence is reached by y + 5 for k ω in this study. 1. INTRODUCTION To perform a veracity check of popular RANS turbulence models in predicting separated flows, experimental data reported by Bourgeois et al is used as a basis of comparison. The flow being examined consists of a single wall-mounted square cylinder of dimensions (h/d =4) sitting within a steady, wellprofiled air flow of Reynolds number Re=12, Time and phase-averaged flow data sets as well as velocity profiles for a three-dimensional grid are made available by the organizers of the 2012 CFDSC Challenge COMPUTATIONAL EQUIPMENT All CFD simulations were performed using the commercial CFD code Star-CCM+ version 6.04 by CD-Adapco. All simulations were performed on the UNC-Charlotte cluster with 32 cores. Additional postprocessing was performed using EnSight by CEI. 3. SURFACE & VOLUME MESHING All CAD data were drawn and surface meshed using ANSA by Beta CAE. All volume meshing was performed within Star-CCM+ using a polyhedral meshing scheme. A polyhedral scheme was chosen due to the omni-directional nature of wall-bounded turbulent flows (Timothy Yen, CD-ADAPCO, personal communication, February 23, 2012). For the best computational accuracy, an ideal mesh would have each cell oriented with one face normal to the flow. When compared to a tetrahedral or hexahedral cell, a polyhedral cell has more faces, and therefore it has more optimal flow directions (normal to a face) than a tetrahedral or hexahedral cell. With more potential optimal flow directions, the polyhedral cell has an increased likelihood of a particular flow direction being at or near the optimal flow direction of one of the polyhedral cell faces. Also, polyhedral cells have more neighbors which allows for better gradient approximations, especially near boundaries and corners. 3 As a starting point, a mesh with ~16x10 6 cells was generated with polyhedral cells, to be called the
2 coarse mesh case hereafter. After preliminary simulations and subsequent examinations of the y + values, two additional meshes were created. The medium mesh with ~26x10 6 cells had further refinements in the floor, behind the cylinder, and around the cylinder surfaces in order to attain a maximum y + 5. In the fine mesh case, additional refinements were made to the cells around the cylinder edges and the prism-layer meshes on the tunnel floor. This increased the total cell count to ~29x10 6 and reduced the first prism layer heights down to produce a y + 1. Even though some simulations may have suggested further refinements could yield slight improvements, for comparative purposes all simulations were run on these three meshes. Coarse Medium Fine Total Volume Cells ~16x10 6 ~26x10 6 ~29x10 6 Floor Tot. Prism Hgt. 4mm 9mm 9mm Floor Prism Levels Floor Prism 1 st Hgt mm mm mm Cyl. Total Prism Hgt. 4mm 9mm 9mm Cyl. Prism Levels Cyl. Prism 1 st Hgt mm mm mm Cyl. Corners 0.25mm 0.125mm 0.125mm Table 1-Volume Mesh Control Values 4. TURBULENCE MODELS In order to examine a range of RANS modeling, three versions of k ω and k ε turbulence models are selected from the available Star CCM+ physics models for detailed examination. The three models are used with all default settings given in version The first model, the Standard k ω, is a wellestablished model capable of resolving through the boundary layer. 4 The second model is Realizable k ε, an improvement over the standard k ε model. 5 k ε schemes model turbulence based on turbulent core flows, making them traditionally unsuitable for applications in the viscous sublayer. 6 And finally the third model examined is the V2F variant of k ε. This model is expected to offer the possibilities of capturing near-wall turbulence effects more accurately k ω Setup Since k ω is capable of resolving flow through the boundary layer, accuracy is expected to improve as the mesh size is reduced to move y + into the viscous sublayer (y + 5). Salim and Cheah 6 suggested this approach and, accordingly, the fine mesh was tuned to result in a near-wall prism layer of y K-Epsilon Realizable Setup As mentioned, the traditional k ε model is not well-suited in resolving flows in near-wall regions. At or near the viscous sublayer, the viscous forces are dominant over the turbulent forces, effectively damping any effects of turbulence. Due to this damping, traditional k ε can t resolve flows in this region, and thus the medium mesh is designed with a near-wall prism layer that yields y + 5. It could be expected that resolving k ε at a lower value, such as the fine mesh s value of y + 1, could potentially show no improvement. There is likelihood that this may even be detrimental to the accuracy of the solution, a reason why a two-layer wall treatment is also applied. The two-layer approach 8 applies a modified model in the viscous sublayer region, allowing k ε to be applied in meshes that could otherwise be unsuitable for such a model. Because three common meshes are being used rather than an optimized mesh for each individual model, the two-layer approach is expected to produce better results with a mesh that is otherwise not optimized for a k ε scheme. One drawback of the two-layer approach in this study is the fact that, as mentioned, more traditional k ε schemes could be expected to perform poorly with y + < 5. The twolayer approach will likely mitigate these effects, so a full understanding of the effects of y + may not be possible in this study. 4.3 K-Epsilon V2F Setup The V2F variant of k ε model solves two additional transport equations, and is expected to more accurately predict the effects of turbulence near walls. 9 It is to be expected that this scheme will require more computational time, but with such complex wall-bounded flows as this problem, the additional time could be a solution cost worth paying. After running several simulations with this model, the actual difference in computational time was significant, requiring approximately six-fold more time to perform the same iteration count with k ε V2F. Star-CCM+ has two possible wall treatments for the k ε V2F model: All y + and Low y +. The Low y + treatment is intended for situations where the mesh resolves the viscous sublayer, and would likely be suited for the fine and possibly even the medium mesh. But the resolution of the coarse mesh is insufficient for the Low y +. Since all three meshes were to be run on the identical modeling setup, the All y + was the necessary choice.
3 5. COMPARISON WITH EXPERIMENTAL DATA Viewing the various flow visualizations comparing the three turbulence models shows distinct differences in the accuracy of the simulations. Observations from all the figures show that k ω and k ε V2F produced nearly identical results, in spite of using significantly different modeling techniques. However, despite their close agreement, neither k ω nor k ε V2F produces results as close to the experimental data as the Realizable k ε scheme. Figs. 1 and 2 show that Realizable k ε produces a wake shape in the X-Z plane that most closely resembles the experimental data s profile. While k ω and k ε V2F show significantly more downward motion (Fig. 2b and 2 than the experiment, Realizable k ε shows very similar characteristics at the mid-plane. A look at the mid-plane vector plot sheds some light as to why this difference exists. As can be seen in Fig. 3a, the experimental data shows a recirculation region immediately behind the rear top edge of the cylinder, something which also exists in the Realizable k ε case. Also visible in both the experiment and the Realizable k ε case is a distinct saddle region as described by Perry and Chong 10, although it is located slightly higher and farther back in the Realizable k ε. Looking at Fig. 3b and 3d, neither the recirculation at the top nor the saddle region is visible in the k ω and the k ε V2F cases. A further inspection of Fig. 3b and 3d shows that in the k ω and the k ε V2F cases the streamlines closest to the top of the cylinder are already slightly downturned by the time they reach the rear edge, and continue to turn until they reach an approximately 45 approach angle with the ground. They continue with this direction until they interact with the ground, FIG.1 x-velocity on X-Z Plane for Experimental k-ω k-ε Real. k-ε V2F FIG.2 z-velocity on X-Z Plane for Experimental k-ω k-ε Real. k-ε V2F
4 Saddle Region Saddle Region FIG.3 Vector Profiles on X-Z Plane for Experimental k-ω k-ε Real. k-ε V2F then turn to a horizontal direction by about 1h behind the rear of the cube. This strong 45 -downward flow explains the significant negative flow to the near-floor region in Fig. 2b and 2d. Both the experimental data and the Realizable k ε show that the flow close to the top of the cylinder is still upwards at the rear edge of the cylinder, but then quickly curves downward and becomes the recirculation zone. The next layer above this passes over the recirculation zone, and curves more slowly towards the ground at somewhat less than 45. But, unlike in the k ω and the k ε V2F cases, the downward flow is deflected by the saddle region and thus approaches the ground at a much lower angle of approach. While Fig. 3b and 3d show the downward flow interacting with the floor at ~1h, Fig. 3b and 3d show a flow with such a shallow approach that they have not reached the floor even at the end of the visible region (2.5h). This difference in approach angle is visible in other views as well. FIG.4 x-velocity on X-Y Plane at z=0.5h for Experimental k-ω k-ε Real. k-ε V2F Viewing from above, Fig. 4 again shows the closest simulation to be the Realizable k ε. At 0.5h, the flow-direction wake is nearly horizontal and passing through the 0.5h plane all the way to the 2.5h end of the view in both Fig. 4a and 4c. But the downward angle of approach in the k ω and the k ε V2F may be seen as a significantly shorter region of influence by the wake in the 0.5h plane in Fig. 4b and 4d.
5 Viewed from above, the streamlines in all four views of Fig. 6 show twin counter-rotating regions behind the cylinder. The flow past these regions curves first inward then back outward in a bottleneck fashion in both the experiment and the Realizable k ε case. The k ω and k ε V2F cases do not show this bottlenecking, and instead continue to converge towards the mid-plane. FIG.5 y-velocity on X-Y Plane for Experimental k-ω k-ε Real. k-ε V2F Cross-flow velocities in Fig. 5 are also very telling as to the difference in structures generated by the three turbulence models. Again, both the experiment and Realizable k ε are in close agreement. Both produce three pairs of evenly-spaced counter-rotating regions in the twin wake trails. By comparison, k ω and k ε V2F show a single pair directly behind the cubes (as does the experiment). But instead of the two additional pairs of counter-rotating confined regions, a single long region continuing well past the viewing area are visible. FIG.6 Vector Profiles on X-Y Plane for Experimental k-ω k-ε Real. k-ε V2F
6 One area in which the Realizable k ε case does not produce the best results (and in fact the only observable structure in any manner throughout this entire study where Realizable k ε was not best) is in the size and intensity of the recirculating regions in Fig. 6. All three turbulence models demonstrate a larger and more organized rotation region than the experiment, with Realizable k ε being the largest. The flow visualization in Fig. 6 may, however, be somewhat misleading when it comes to recirculation strength due to the large differences in vector seeding density by EnSight between the experimental and CFD data. Looking at the cylinder from the rear, Fig. 7 shows the experimental data as having a pair of large regions of cross-flow, with two more pairs of counter-flowing areas below this. While all three turbulence models show this structure to some extent, the Realizable k ε most closely matches the experimental structure in size, location, and intensity. Fig. 8 also shows that the vertical velocity profile of Realizable k ε most closely matches the experimental data. The experiment shows a confined core of downward flow at the top half of the cylinder, while k ω and the k ε V2F show a core nearly the full height of the cylinder. FIG.7 y-velocity on Y-Z Plane for Experimental k-ω k-ε Real. k-ε V2F FIG.8 z-velocity on Y-Z Plane for Experimental k-ω k-ε Real. k-ε V2F
7 Velocity (m/s) Velocity (m/s) Position (mm) -10 Position (mm) Coarse Mesh X Velocity Medium Mesh X Velocity Fine Mesh X Velocity Coarse Mesh Z Velocity Medium Mesh Z Velocity Fine Mesh Z Velocity Coarse Mesh X Velocity Medium Mesh X Velocity Fine Mesh X Velocity Coarse Mesh Z Velocity Medium Mesh Z Velocity Fine Mesh Z Velocity FIG.9 Selected Velocity Profile for k-ω with Three Mesh Cases 6. MESH INDEPENDENCE In order to examine mesh independence, all simulations were monitored with a set of velocity profiles in various regions of the flow path, as well as with visual comparisons of flow structure and scalar plots. Two samples of these velocity profiles may be seen in Fig. 9 and 10 for k ω and Realizable k ε. Due to computational time, a mesh-dependence study was not performed on k ε V2F. As previously discussed, it could be expected that k- ω would improve with an increasing resolution in the boundary layer. With the medium mesh (y+ 5) resolving to the edge of the viscous sublayer and the fine mesh (y+ 1) resolving well into the viscous sublayer, it was expected that some improvement in accuracy would be yielded by the fine mesh. Salim and Cheah also predicted such behavior. 6 However, Fig. 9 shows that, at least for velocity profiles, this was not the case. As can be seen, there is no significant difference between the medium and fine mesh cases in velocity profiles at the selected regions, suggesting that the k ε scheme used in this study reached mesh independence by y+ 5. This unexpected result was also seen by Salim and Cheah. In their study, their fine mesh (y+ 2) did improve the accuracy of skin friction predictions, but FIG.10 Selected Velocity Profile for Realizable k-ε with Three Mesh Cases their fine mesh showed no improvements in predicting velocity profiles compared to either their coarse (y+ 32.5) or medium mesh (y+ 12.5). Also as discussed, unlike k ω, k ε was expected to not see improvement with a mesh resolved into the viscous sublayer. But again, this study did not support the initial assumptions for k ε, at least not with the two-layer treatment applied. Instead, the fine mesh case produced the best results for the Realizable k ε, as may be seen in Fig. 10. Salim and Cheah had similar results. In their study at the finest mesh (y+ 2) Realizable k ε, with a Standard Wall Function (SWF), did perform the worst of any model tested. But by adding an Enhanced Wall Function (EWF), a two-layer treatment similar to that used here in Star-CCM+, Salim and Cheah found that Realizable k ε was among the best model tested with the fine mesh. It is likely that, had this current study compared a Realizable k ε without the twolayer treatment, poor results similar to Salim and Cheah would have been seen with the fine mesh. 7. CONCLUSION When comparing the three models used in this study, one model has shown a clear and distinct advantage in predicting the flow of a wall-mounted square
8 cylinder. In virtually every measure of comparison, Realizable k ε demonstrates a superior ability to capture the mean flow of the complex structures measured in the experimental data. Neither k ω nor k ε V2F is able to predict the complex saddle structure behind the cylinder or the trail-edge recirculation zone at the top of the cylinder as seen in Fig.3. Without accurately predicting these structures, k ω and k ε V2F are also unable to predict the complex pattern of counter-rotating and alternately shedding vortices captured by the experiment. Realizable k ε, on the other hand, shows very good ability in predicting these complex patterns. While not an exact representation, the Realizable k ε cases are able to very closely predict the three pairs of counter-rotating regions behind the cylinder seen in Fig. 5. The results of the study of any correlation between mesh quality and turbulence modeling are not nearly as straight-forward. The k ω model, which is capable of modeling flows throughout the boundary layer, was expected to see improvements with a mesh resolved into the boundary layer. But in the case observed in this study, k ω reached mesh independence with the medium mesh despite being resolved only to y+ 5, a distance at the edge of the viscous sublayer. To the contrary, Realizable k-ε did not demonstrate mesh independence at y+ 5, and instead showed further improvements all the way to y+ 1. This contradicts the traditional assumption that k ε models perform poorly when resolved into the viscous sublayer. In the case of this study, just as in the literature, the likely reason for the improving results with a viscous sublayer-refined mesh is the application of the two-layer treatment. This treatment applies a different model to the k ε scheme in the viscous sublayer region, allowing for much finer meshes to be used without sacrificing accuracy. cylinder with a thin boundary layer. Physics of Fluids, 23(9):095101, 2011 [2] R. J. Martinuzzi. CFDSC Challenge Data. Retrieved : March 16, [3] M. Peric and S. Ferguson. The Advantage of Polyhedral Meshes. Technical Report, CD Adapco Group, [4] D. C. Wilcox. Turbulence Modeling for CFD, 2 nd ed. DCW Industries, 2006 [5] T. H. Shih, W. W. Liou, A. Shabbir, Z. Yang, and J. Zhu. A New k-ε Eddy Viscosity Model for High Reynolds Number Turbulent Flows Model Development and Validation. Computers Fluids. 24(3): , 1995 [6] Salim M. Salim and S. C. Cheah. Wall y+ Strategy for Dealing with Wall-Bounded Turbulent Flows. Physics of Fluids, 23(9):095101, 2011 [7] L. Davidson and P. V. Nielsen. Modifications of the v 2 -f Model for Computing the Flow in a 3D Wall Jet. Turbulence, Heat and mass Transfer, 23: , 2003 [8] W. Rodi. Experience with Two-Layer Models Combining the k-e Model with a One-Equasion Model Near the Wall. 29 th Aerospace Sciences Meeting, January 7-10, Reno, NV , 1991 [9] Star CCM+ Help Manual. What is the V2F Low- Reynolds Number K-Epsilon Model. CD- Adapco Group. [10] A.E. Perry and M. S. Chong. A Description of Eddying Motions and Flow Patterns Using Critical-Point Concepts. Ann. Rev. Fluid Mech., 19: , 1987 ACKNOWLEDGEMENTS This material is based upon work supported by the national Science Foundation Graduate Research Fellowship under Grant No Also, the authors would also like to thank Timothy Yen of CD-Adapco and Bill Dunn of CEI for their assistance with this project. REFERENCES [1] J.A. Bourgeois, P. Sattari, and R. J. Martinuzzi. Alternating half-loop shedding in the turbulent wake of a finite surface-mounted square
CFD 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 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 informationWALL Y + APPROACH FOR DEALING WITH TURBULENT FLOW OVER A SURFACE MOUNTED CUBE: PART 2 HIGH REYNOLDS NUMBER
Seventh International Conference on CFD in the Minerals and Process Industries CSIRO, Melbourne, Australia 9- December 9 WALL Y + APPROACH FOR DEALING WITH TURBULENT FLOW OVER A SURFACE MOUNTED CUBE: PART
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 informationOptimization of under-relaxation factors. and Courant numbers for the simulation of. sloshing in the oil pan of an automobile
Optimization of under-relaxation factors and Courant numbers for the simulation of sloshing in the oil pan of an automobile Swathi Satish*, Mani Prithiviraj and Sridhar Hari⁰ *National Institute of Technology,
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 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 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 informationInternational Power, Electronics and Materials Engineering Conference (IPEMEC 2015)
International Power, Electronics and Materials Engineering Conference (IPEMEC 2015) Numerical Simulation of the Influence of Intake Grille Shape on the Aerodynamic Performance of a Passenger Car Longwei
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 informationCFD Study of a Darreous Vertical Axis Wind Turbine
CFD Study of a Darreous Vertical Axis Wind Turbine Md Nahid Pervez a and Wael Mokhtar b a Graduate Assistant b PhD. Assistant Professor Grand Valley State University, Grand Rapids, MI 49504 E-mail:, mokhtarw@gvsu.edu
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 informationEffect of Position of Wall Mounted Surface Protrusion in Drag Characteristics At Low Reynolds Number
ISSN (e): 2250 3005 Volume, 07 Issue, 11 November 2017 International Journal of Computational Engineering Research (IJCER) Effect of Position of Wall Mounted Surface Protrusion in Drag Characteristics
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 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 informationPUBLISHED VERSION. Originally Published at: PERMISSIONS. 23 August 2015
PUBLISHED VERSION Yinli Liu, Hao Tang, Zhaofeng Tian, Haifei Zheng CFD simulations of turbulent flows in a twin swirl combustor by RANS and hybrid RANS/LES methods Energy Procedia, 2015 / Jiang, X., Joyce,
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 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 informationReproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software
Reports of Research Institute for Applied Mechanics, Kyushu University No.150 (71 83) March 2016 Reproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software Report 3: For the Case
More informationHealthy Buildings 2017 Europe July 2-5, 2017, Lublin, Poland
Healthy Buildings 2017 Europe July 2-5, 2017, Lublin, Poland Paper ID 0122 ISBN: 978-83-7947-232-1 Numerical Investigation of Transport and Deposition of Liquid Aerosol Particles in Indoor Environments
More 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 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 informationNUMERICAL STUDY OF CAVITATING FLOW INSIDE A FLUSH VALVE
Conference on Modelling Fluid Flow (CMFF 09) The 14th International Conference on Fluid Flow Technologies Budapest, Hungary, September 9-12, 2009 NUMERICAL STUDY OF CAVITATING FLOW INSIDE A FLUSH VALVE
More informationTHE FLUCTUATING VELOCITY FIELD ABOVE THE FREE END OF A SURFACE- MOUNTED FINITE-HEIGHT SQUARE PRISM
THE FLUCTUATING VELOCITY FIELD ABOVE THE FREE END OF A SURFACE- MOUNTED FINITE-HEIGHT SQUARE PRISM Rajat Chakravarty, Noorallah Rostamy, Donald J. Bergstrom and David Sumner Department of Mechanical Engineering
More informationON THE NUMERICAL MODELING OF IMPINGING JET HEAT TRANSFER
ON THE NUMERICAL MODELING OF IMPINGING JET HEAT TRANSFER Mirko Bovo 1,2, Sassan Etemad 2 and Lars Davidson 1 1 Dept. of Applied Mechanics, Chalmers University of Technology, Gothenburg, Sweden 2 Powertrain
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 informationNUMERICAL SIMULATIONS OF FLOW THROUGH AN S-DUCT
NUMERICAL SIMULATIONS OF FLOW THROUGH AN S-DUCT 1 Pravin Peddiraju, 1 Arthur Papadopoulos, 2 Vangelis Skaperdas, 3 Linda Hedges 1 BETA CAE Systems USA, Inc., USA, 2 BETA CAE Systems SA, Greece, 3 CFD Consultant,
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 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 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 informationComputational Fluid Dynamics as an advanced module of ESP-r Part 1: The numerical grid - defining resources and accuracy. Jordan A.
Computational Fluid Dynamics as an advanced module of ESP-r Part 1: The numerical grid - defining resources and accuracy Jordan A. Denev Abstract: The present paper is a first one from a series of papers
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 informationFAR-Wake Workshop, Marseille, May 2008
Wake Vortices generated by an Aircraft Fuselage : Comparison of Wind Tunnel Measurements on the TAK Model with RANS and RANS-LES Simulations T. Louagie, L. Georges & P. Geuzaine Cenaero CFD-Multiphysics
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 informationTHE EFFECTS OF THE PLANFORM SHAPE ON DRAG POLAR CURVES OF WINGS: FLUID-STRUCTURE INTERACTION ANALYSES RESULTS
March 18-20, 2013 THE EFFECTS OF THE PLANFORM SHAPE ON DRAG POLAR CURVES OF WINGS: FLUID-STRUCTURE INTERACTION ANALYSES RESULTS Authors: M.R. Chiarelli, M. Ciabattari, M. Cagnoni, G. Lombardi Speaker:
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 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 informationAssessment of Turbulence Models for Flow around a Surface-Mounted Cube
Assessment of Turbulence Models for Flow around a Surface-Mounted Cube Sercan Dogan, Sercan Yagmur, Ilker Goktepeli, and Muammer Ozgoren Selcuk University, Konya, Turkey Email: {sercandogan, syagmur, ilkergoktepeli}@selcuk.edu.tr
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 informationNumerical Simulation Study on Aerodynamic Characteristics of the High Speed Train under Crosswind
2017 2nd International Conference on Industrial Aerodynamics (ICIA 2017) ISBN: 978-1-60595-481-3 Numerical Simulation Study on Aerodynamic Characteristics of the High Speed Train under Crosswind Fan Zhao,
More informationMOMENTUM AND HEAT TRANSPORT INSIDE AND AROUND
MOMENTUM AND HEAT TRANSPORT INSIDE AND AROUND A CYLINDRICAL CAVITY IN CROSS FLOW G. LYDON 1 & H. STAPOUNTZIS 2 1 Informatics Research Unit for Sustainable Engrg., Dept. of Civil Engrg., Univ. College Cork,
More informationCoupling STAR-CCM+ with Optimization Software IOSO by the example of axial 8-stages jet engine compressor.
Coupling STAR-CCM+ with Optimization Software IOSO by the example of axial 8-stages jet engine compressor. Folomeev V., (Sarov Engineering Center) Iakunin A., (JSC Klimov) 1 Objectives To create the procedure
More informationEffects on a Wedge Flowmeter Installed Downstream of a Double Elbow Out of Plane
Utah State University DigitalCommons@USU All Graduate Theses and Dissertations Graduate Studies 5-2016 Effects on a Wedge Flowmeter Installed Downstream of a Double Elbow Out of Plane Devan S. Radle Utah
More informationReproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software
Reports of Research Institute for Applied Mechanics, Kyushu University, No.150 (60-70) March 2016 Reproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software Report 2: For the Case
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 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 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 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 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 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 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 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 informationImpact of STAR-CCM+ v7.0 in the Automotive Industry Frederick J. Ross, CD-adapco Director, Ground Transportation
Impact of STAR-CCM+ v7.0 in the Automotive Industry Frederick J. Ross, CD-adapco Director, Ground Transportation Vehicle Simulation Components Vehicle Aerodynamics Design Studies Aeroacoustics Water/Dirt
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 informationDetached-Eddy Simulation of a Linear Compressor Cascade with Tip Gap and Moving Wall *)
FOI, Stockholm, Sweden 14-15 July, 2005 Detached-Eddy Simulation of a Linear Compressor Cascade with Tip Gap and Moving Wall *) A. Garbaruk,, M. Shur, M. Strelets, and A. Travin *) Study is carried out
More informationDispersion Modelling for Explosion Risk Analysis
Dispersion Modelling for Explosion Risk Analysis Tim Jones, Principal Consultant, MMI Engineering, The Brew House, Wilderspool Park, Greenall s Avenue, Warrington, WA4 6HL The understanding of the explosion
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 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 informationANSYS FLUENT. Airfoil Analysis and Tutorial
ANSYS FLUENT Airfoil Analysis and Tutorial ENGR083: Fluid Mechanics II Terry Yu 5/11/2017 Abstract The NACA 0012 airfoil was one of the earliest airfoils created. Its mathematically simple shape and age
More informationUSE OF PROPER ORTHOGONAL DECOMPOSITION TO INVESTIGATE THE TURBULENT WAKE OF A SURFACE-MOUNTED FINITE SQUARE PRISM
June 30 - July 3, 2015 Melbourne, Australia 9 6B-3 USE OF PROPER ORTHOGONAL DECOMPOSITION TO INVESTIGATE THE TURBULENT WAKE OF A SURFACE-MOUNTED FINITE SQUARE PRISM Rajat Chakravarty, Nader Moazamigoodarzi,
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 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 informationMesh optimization for ground vehicle Aerodynamics
Mesh optimization for ground vehicle Aerodynamics Ahmad, NE, Abo-Serie, E & Gaylard, A Published PDF deposited in Coventry University s Repository Original citation: Ahmad, NE, Abo-Serie, E & Gaylard,
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 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 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 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 informationIntroduction to C omputational F luid Dynamics. D. Murrin
Introduction to C omputational F luid Dynamics D. Murrin Computational fluid dynamics (CFD) is the science of predicting fluid flow, heat transfer, mass transfer, chemical reactions, and related phenomena
More informationCFD 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 informationPrediction of Turbo Compressor Maps using CFD
Prediction of Turbo Compressor Maps using CFD Master s thesis in Applied Mechanics STEPHANIE BERGQVIST Department of Applied Mechanics Division of Fluid Dynamics CHALMERS UNIVERSITY OF TECHNOLOGY Gothenburg,
More informationSimulation of a Free Surface Flow over a Container Vessel Using CFD
Simulation of a Free Surface Flow over a Container Vessel Using CFD Krishna Atreyapurapu 1 Bhanuprakash Tallapragada 2 Kiran Voonna 3 M.E Student Professor Manager Dept. of Marine Engineering Dept. of
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 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 informationBest Practices: Volume Meshing Kynan Maley
Best Practices: Volume Meshing Kynan Maley Volume Meshing Volume meshing is the basic tool that allows the creation of the space discretization needed to solve most of the CAE equations for: CFD Stress
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 informationSimulation of Turbulent Flow over the Ahmed Body
Simulation of Turbulent Flow over the Ahmed Body 58:160 Intermediate Mechanics of Fluids CFD LAB 4 By Timur K. Dogan, Michael Conger, Maysam Mousaviraad, and Fred Stern IIHR-Hydroscience & Engineering
More informationViscous Hybrid Mesh Generation
Tutorial 4. Viscous Hybrid Mesh Generation Introduction In cases where you want to resolve the boundary layer, it is often more efficient to use prismatic cells in the boundary layer rather than tetrahedral
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 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 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 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 informationValidation of an Unstructured Overset Mesh Method for CFD Analysis of Store Separation D. Snyder presented by R. Fitzsimmons
Validation of an Unstructured Overset Mesh Method for CFD Analysis of Store Separation D. Snyder presented by R. Fitzsimmons Stores Separation Introduction Flight Test Expensive, high-risk, sometimes catastrophic
More informationCIBSE Application Manual AM11 Building Performance Modelling Chapter 6: Ventilation Modelling
Contents Background Ventilation modelling tool categories Simple tools and estimation techniques Analytical methods Zonal network methods Computational Fluid Dynamics (CFD) Semi-external spaces Summary
More informationNumerical Study of Turbulent Flow over Backward-Facing Step with Different Turbulence Models
Numerical Study of Turbulent Flow over Backward-Facing Step with Different Turbulence Models D. G. Jehad *,a, G. A. Hashim b, A. K. Zarzoor c and C. S. Nor Azwadi d Department of Thermo-Fluids, Faculty
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 information3D Modeling of Urban Areas for Built Environment CFD Applications
3D Modeling of Urban Areas for Built Environment CFD Applications using C A.W.M. (Jos) van Schijndel Eindhoven University of Technology P.O. Box 513; 5600 MB Eindhoven; Netherlands, A.W.M.v.Schijndel@tue.nl
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 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 informationAnalysis of a curvature corrected turbulence model using a 90 degree curved geometry modelled after a centrifugal compressor impeller
Analysis of a curvature corrected turbulence model using a 90 degree curved geometry modelled after a centrifugal compressor impeller K. J. Elliott 1, E. Savory 1, C. Zhang 1, R. J. Martinuzzi 2 and W.
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 informationComputational Fluid Dynamics Analysis of an Idealized Modern Wingsuit
Washington University in St. Louis Washington University Open Scholarship Mechanical Engineering and Materials Science Independent Study Mechanical Engineering & Materials Science 12-21-2016 Computational
More informationNumerical Analysis and Geometry Optimisation of Vertical Vane of Room Air-conditioner
Numerical Analysis and Geometry Optimisation of Vertical Vane of Room Air-conditioner Abdulkareem Sh. Mahdi Al-Obaidi 1,*, Chan Wei Yin 1, Felicia Wong Yen Myan 1 and Yan Yao Chen 1 1 School of Engineering,
More informationComputation of Velocity, Pressure and Temperature Distributions near a Stagnation Point in Planar Laminar Viscous Incompressible Flow
Excerpt from the Proceedings of the COMSOL Conference 8 Boston Computation of Velocity, Pressure and Temperature Distributions near a Stagnation Point in Planar Laminar Viscous Incompressible Flow E. Kaufman
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 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 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 informationMulti-Objective Optimization of a Boomerang Shape using modefrontier and STAR-CCM+
Multi-Objective Optimization of a Boomerang Shape using modefrontier and STAR-CCM+ Alberto Clarich*, Rosario Russo ESTECO, Trieste, (Italy) Enrico Nobile, Carlo Poloni University of Trieste (Italy) Summary
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 informationLES Applications in Aerodynamics
LES Applications in Aerodynamics Kyle D. Squires Arizona State University Tempe, Arizona, USA 2010 Tutorial School on Fluid Dynamics: Topics in Turbulence Center for Scientific Computation and Mathematical
More informationCDA Workshop Physical & Numerical Hydraulic Modelling. STAR-CCM+ Presentation
CDA Workshop Physical & Numerical Hydraulic Modelling STAR-CCM+ Presentation ENGINEERING SIMULATION CFD FEA Mission Increase the competitiveness of companies through optimization of their product development
More information