Comparison Between Three Different Cfd Software And .

3m ago
7.98 MB
66 Pages
Last View : 1m ago
Last Download : n/a
Upload by : Eli Jorgenson

COMPARISON BETWEEN THREEDIFFERENT CFD SOFTWARE ANDNUMERICAL SIMULATION OF ANAMBULANCE HALLNing LiMaster of Science ThesisKTH School of Industrial Engineering and ManagementEnergy Technology EGI-2015-017MSCDivision of Energy TechnologySE-100 44 STOCKHOLMI

Master of Science Thesis EGI 2015: 017MSCComparison between three different CFDsoftware and numerical simulation of anambulance hallNing LiApprovedExaminerSupervisor2015-03-05Joachim ClaessonJoachim ClaessonCommissionerContact personSWECO Systems ABDavid BurmanLiu TingAbstractAmbulance hall is a significant station during emergency treatment. Patients need to be transferred fromambulance cars to the hospital’s building in the hall. Eligible performance of ventilation system to supplysatisfied thermal comfort and healthy indoor air quality is very important. Computational fluid dynamic(CFD) simulation as a broadly applied technology for predicting fluid flow distribution has beenimplemented in this project.There has two objectives for the project. The first objective is to make comparison between the threeCFD software which consists of ANSYS Fluent, Star-CCM and IESVE Mcroflo according to CFDmodeling of the baseline model. And the second objective is to build CFD modeling for cases withdifference boundary conditions to verify the designed ventilation system performance of the ambulancehall.In terms of simulation results from the three baseline models, ANSYS Fluent is conclusivelyrecommended for CFD modeling of complicated indoor fluid environment compared with Star-CCM and IESVE Microflo. Regarding to the second objective, simulation results of case 2 and case 3 haveshown the designed ventilation system for the ambulance hall satisfied thermal comfort level whichregulated by ASHRAE standard with closed gates. Nevertheless, threshold limit value of the contaminantsconcentration which regulated by ASHRAE IAQ Standard cannot be achieved. From simulation results ofcase 4.1 to 4.3 shown that the designed ventilation system cannot satisfy indoor thermal comfort levelwhen the gates of the ambulance hall opened in winter. In conclusion, measures for decreasingcontaminants concentration and increasing indoor air temperature demanded to be considered in furtherdesign.-II-

Table of ContentsAbstract .IIAcknowledgements . VList of Figures . VIList of Tables. VIIINomenclature. IX12Introduction . 11.1Background . 11.2Objectives . 21.3Method. 3Numerical principle of simulation . laws of fluid flow. . 42.1.2Thermal equations of wall boundary condition. . 42.2Turbulence modeling. 52.2.1Different choice of k-ε Model . 52.2.2Near – Wall functions . 72.3Meshing . 82.3.1Shapes of Cell . 82.3.2Classification of Grids . 82.3.3Mesh Quality. 92.43Governing Equations . 4Solver.102.4.1Finite Volume Method .102.4.2Upwind scheme .112.4.3SIMPLE Scheme .11Baseline model and Comparison between Software .133.1Data of ventilation system for baseline model. .133.1.1Design Concept .133.1.2Parameter of supply air diffuser .133.1.3Parameter of Exhaust Grilles .133.2Geometry.143.3Meshing .153.3.1Meshing Independency .153.3.2Meshing Method .173.4Numerical Setup .193.4.1Selection of simulation models .193.4.2Boundary conditions .19-III- Control.21Simulation results .233.5.1Assessment of thermal comfort in an arbitrary point. .233.5.2Velocity Distribution .243.5.3Temperature Distribution.28Ventilation Performance in Different Situations .334.1Geometry.334.1.1Case 2: Improved ventilation system. .334.1.2Case 3: Polluted emission from tailpipes of the ambulance cars. .344.1.3Case 4.1-4.3: With opened gates and installed air curtains. .344.2Meshing .364.3Boundary Conditions Setup .364.3.1Case 2: Improved ventilation system. .364.3.2Case 3: Polluted emission from tailpipes of the ambulance cars. .364.3.3Case 4.1-4.3: With opened gates and installed air curtains. .374.4Simulation Results and Analysis. .384.4.1Case 2: Improved ventilation system. .384.4.2Case 3: Polluted emission from tailpipes of the ambulance cars. .404.4.3Case 4.1-4.3: With opened gates and installed air curtains. .434.5Optimized approaches for improving thermal comfort. .484.5.1One more supply air diffuser on the specified wall. .484.5.2Exhaust extraction system. .494.5.3Supplement of heat in winter. .495Conclusion and future improvement .516Bibliography .52Appendix A: Data sheet/Dimension of Jet Nozzle Diffuser .54Appendix B: Data and Dimension of Exhaust Grilles .55Appendix C: Data and Type of Air curtain. .56Appendix D: CO Level vs. Condition&Health Effects. .57-IV-

AcknowledgementsForemost I would like to express my fully gratitude to Will Sibia from SWECO systems AB, StockholmSweden for giving me the opportunity to do my master thesis within such interesting and cutting edgefield by a practical project.Specially, I would like to extend my deepest thanks to Liu Ting, who is my thesis supervisor fromSWECO in the field of CFD simulation. Encouragements, professional and theoretical supports from herwere very beneficial and helpful for me to complete the project.Sincerely, I would also very thankful to David Berman, who is my thesis supervisor from SWECO in thefield of energy technology and ventilation systems design. Professional advices and positive feedbacksfrom him supervised me done the project in the right way.Moreover, I would like to express my grate gratitude to my supervisor, Associate Professor JoachimClaesson, at the Royal Institute of Technology (KTH) for your fully helpful supports, responsiblefeedback and all the fantastic knowledge were taught from you during the graduate study.Finally, I am deep appreciate to my parents, my friends for their love and supports.-V-

List of FiguresFigure 1, 3D layout of SÖS ambulance hall. . 1Figure 2, Project Outline . 2Figure 3, Velocity distribution near a wall (Versteeg & Malalasekera, 2007) . 7Figure 4, Typical 2D control volume (Versteeg & Malalasekera, 2007). . 8Figure 5, Block-structured mesh (left) and Unstructured mesh (right) of aerofoil (Versteeg & Malalasekera, 2007) . 8Figure 6, Comparison between coarse, medium and fine hybrid grid. . 9Figure 7, Misalignment of midpoints for skewed grid. . 9Figure 8, Conservation of general flow variable within finite volume method (Versteeg & Malalasekera, 2007).10Figure 9, Evaluation of face value according to Upwind Scheme (Cho, et al., 2010). .11Figure 10, Calculation process of SIMPLE Scheme (Versteeg & Malalasekera, 2007).12Figure 11, Air motion of Group A outlets (ASHRAE, 1997).13Figure 12, Geometry of the ambulance hall .14Figure 13, Face sizing for air inlet (Left: Element size is 0.05m; Right: Element size is 0.03m) .15Figure 14, Face sizing for air outlet (Left: Element size is 0.1m; Right: Element size is 0.05m) .16Figure 15, Velocity distribution for the two different meshing cases. .16Figure 16, Generated mesh of the ambulance hall in IESVE Microflo. .17Figure 17, Generated mesh of the ambulance hall in ANSYS mesh. .17Figure 18, Section plane of (a) Air Inlet; (b) Air Outlet; (c) Exterior Wall; (d) Internal space .18Figure 19, Mesh metrics control of ANSYS mesh (Left: Skewness; Right: Aspect Ratio) .18Figure 20, Cell Monitor of point in Case 1.3. .23Figure 21, PPD as a function of PMV (ISO, 1994). .23Figure 22, Thermal comfort zone display in Psychronmetric chart. .24Figure 23, Vector of velocity distribution (h 3m) of case 1.1. .25Figure 24, Velocity Magnitude (h 3m) of case 1.1. (Left: 0 to 5.02m/s, Right: 0 to 1 m/s).25Figure 25, Vector of Velocity distribution (h 1m) of case 1.1. .25Figure 26, Zoomed-in views of velocity distribution at plant (h 1m).s .26Figure 27, Vector of velocity distribution (h 3m) of case 1.2. .26Figure 28, Vector of velocity distribution (h 1m) of case 1.2. .27Figure 29, Vector and contour of velocity distribution (h 3m and h 1m) of case 1.3.27Figure 30, Local mean age of air (h 1m) of case 1.3. .28Figure 31, Temperature distribution (h 1m, local temperature).29Figure 32, Temperature distribution (h 1m, specified temperature). .29Figure 33, Temperature distribution (h 1m, global temperature) with isosurface.30Figure 34, Temperature distribution (Left: x 3.6m, 11m and 18.3m; Right: y 10.3m, 15.5m and 21m). .30Figure 35, Temperature distribution on envelop of ambulance hall.30Figure 36, Temperature distribution of case 1.2. .31Figure 37, Temperature distribution of case 1.3. .32Figure 38, Geometry of case 2 with 4 exhaust grilles. .33Figure 39, Geometry of case 3 with tailpipe emission (Left: whole room; Right: zoomed-in to the tailpipe) .34Figure 40, Configuration of air curtain which installed in case 4.1-4.3. .34Figure 41, Geometry of case 4.1 - 4.3. .35Figure 42, Zoomed-in views of geometry for case 4.1-4.3. .35Figure 43, Meshing of case 4.1-4.3 (Left: Global: Right: Section cut view). .36Figure 44, Velocity distribution at h 3m over the ground (Local Velocity). .38Figure 45, Velocity distribution at h 1m (Local Velocity). .38Figure 46, Zoomed-in views to figure 45. .39Figure 47, Temperature distribution of case 2 at h 1m (Left: local temperature, Right: Specified temperature). .39Figure 48, Temperature distribution of case 2 (Left: h 0.1m, isosurface 18C; Right: Room Envelope). .40Figure 49, Velocity distribution of case 3 (Left: h 3m; Right: h 0.4m) .40-VI-

Figure 50, Velocity distribution of case 3 (h 1m). .41Figure 51, Temperature distribution of case 3 h 0.4m (Left: Local temperature; Right: specified temperature) .41Figure 52, Temperature distribution of case 3 at h 1m (Specified Temperature). .42Figure 53, CO concentration distribution of case 3 (h 1.5m).42Figure 54, CO2 concentration distribution of case 3 (h 1.5m). .43Figure 55, Velocity distribution of case 4.1 (h 1m).44Figure 56, Specified velocity of case 4.1 at h 1m (Left: Velocity 0m/s - 0.2m/s; Right: Velocity 0m/s - 1m/s). .44Figure 57, Velocity distribution of case 4.1 around the opened gates. .45Figure 58, Temperature distribution of case 4.1 (Left 3m; Right 1m). .45Figure 59, Temperature distribution of case 4.1 (Transection view at gate). .46Figure 60, Pressure distribution at h 1m of case 4.2(Left) and case 4.3 (Right). .46Figure 61, Pressure change along the line of case 4.2(red line) and case 4.3 (blue line). .46Figure 62, Velocity distribution at h 1m of case 4.2(Left) and case 4.3 (Right). .47Figure 63,Zoomed-in Velocity distribution at h 1m of case 4.2(Left) and case 4.3 (Right). .47Figure 64, Temperature distribution at h 1m of case 4.2(Left) and case 4.3 (Right). .48Figure 65, Install position of the additional supply air diffuser. .48Figure 66, Conventional exhaust extraction system (Left) and "in ground" exhaust extraction system (Right).49Figure 67, Working principle of "in ground" exhaust extraction system (Nenerman, 2014). .49-VII-

List of TablesTable 1, Cade name of different cases. 2Table 2, Skewness range and cell quality (Fluent, 2006). .10Table 3, Input dimensions of geometry of the ambulance hall. .14Table 4, Performance of 3D modeling for different tools. .15Table 5, Comparison of Mass flow rate and Total heat transfer rate between the two meshing cases .16Table 6, Statistics of mesh which generated from ANSYS mesh and IES VE – CFD Grid. .18Table 7, Performance of meshing for the three software. .18Table 8, Boundary Conditions set up in ANSYS Fluent and Star - CCM . .20Table 9, Solution control for the three software. .22Table 10, Performance of numerical setup for the three software. .22Table 11, Thermal sensation scale for PMV Method. .23Table 12, Simulation results of the three software. .32Table 13, Different between the two types of exhaust grilles in two cases. .33Table 14, Additional parameters of geometry for case 4.1 to 4.3. .34Table 15, Input parameters for boundary conditions of tailpipes. .37Table 16, Air curtain boundary conditions of case 4.1-4.3. .37-VIII-

NomenclatureSymbolsACpCiCughexthfIkPQSmTtuVy extk T ,l T ,tΦ ρΩij i areaspecific heatcontaminant concentrationk-epsilon model constantgravitational constantexternal heat transfer coefficientheat transfer coefficient of the fluid sidetensor of unitthermal conductivitypressureheat transfer ratesource of massTemperaturetimevelocityvolumetric flow ratedimensionless wall distancedissipation rate of kemissivityturbulence kinetic energyStefan-Boltzmann constantlaminar Prandtl numberturbulent Prandtl numberflow variableunder-relaxation factornear-wall temperature equation constantdensityrate-of-rotation tensorlocal mean age of airstress tensorviscosity of utational Fluid DynamicFinite Volume MethodLocal Mean AgePredicted Mean VotePercentage of DissatisfiedRe-Normalization GroupSemi-Implicit Method for Pressure-Linked Equations-IX-

1 Introduction1.1 BackgroundNumerical visualization is a platform provides a simpler way to analysis of large, complex and mutidimensional information. Computational fluid dynamic, also called CFD, has combined fluid mechanicwith this platform to simulate both compressible and incompressible fluid flow behavior. Distribution oftemperature, velocity, pressure, contaminant concentration and other fluid properties can be calculatedand displayed from results of CFD simulation (Stamou, et al., 2007). Output results help engineers toimprove and consummate their design quickly and effectively.In this project, three different CFD commercial software have been employed by the author to evaluateindoor thermal comfort of an ambulance hall which is belong to SÖS hospital renovation project fromSWECO, in Stockholm, Sweden. As defined by international standard ISO 7730, thermal comfort as“condition of mind which expresses satisfaction of thermal environment” has explained that comfort levelneed to be determined by subject method (ISO, 1994). According to the criteria ISO 7730, metabolic rate(MET) and thermal insulation of clothing index (CLO) will be introduced for obtain thermal comfortindexes which are predicted mean vote (PMV) and predicted percentage of dissatisfied (PPD) (ISO, 1994).The three different CFD commercial software consist of ANSYS - Fluent, IES VE – Microflo and Star –CCM . Internal analyses of the ambulance hall were established by the three tools for baseline case.Thereafter, three additional modeling cases which include improvement of ventilation system, hall withtailpipe emissions and opened gates with natural ventilation were implemented by ANSYS – Fluentindependently.Figure 1, 3D layout of SÖS ambulance hall.Ambulance hall is a significant station during emergency treatment. Patients need to be transferred fromambulance cars to the hospital’s building in the hall. High performance of ventilation system which supplyfresh and comfortable indoor environment is required to achieve.As shown in Figure 1, during peak operation condition there has 8 ambulance cars parking in the hall.Consider walls of the ambulance hall, 2 exterior wall are exposed directly to ambient environment and 2interior walls are connected to internal corridors. For sake of simplifying the model and emphasizeperformance of fluid flow within the main hall, interior rooms and internal corridors will be removed infurther 3D modeling.1

1.2 ObjectivesTwo main objectives of the project had been set up.The first objective is to build CFD modeling in three different numerical simulation software which havebeen specified as ANSYS-Fluent, IES VE - Microflo and Star-CCM . Thereafter, made comparison ofperformance among these three software.The second objective is to optimize ventilation system according to output results from baseline model,simulate the optimized model while involving exhaust emission from the ambulance cars or naturalventilation with opening gates.The outline of the project is illustrated in Figure 2, the two objectives are highlighted as orange at the bottomof the chart.Figure 2, Project OutlineFor simplify the names of each scenarios in further discussion, code name of each scenario list as in Table 1.Table 1, Cade name of different cases.Code NameCase 1.1Case 1.2Case 1.3Case 2Case 3Case 4.1Case 4.2Case 4.3Circumstance Description2 exhaust grilles, without tailpipe emission, without opened gates2 exhaust grilles, without tailpipe emission, without opened gates2 exhaust grilles, without tailpipe emission, without opened gates4 exhaust grilles, without tailpipe emission, without opened gates4 exhaust grilles, with tailpipe emission, without opened gates4 exhaust grilles, without tailpipe emission, with opened gates,Outside wind blow perpendicular into the gates wi

The first objective is to make comparison between the three CFD software which consists of ANSYS Fluent, Star-CCM and IESVE Mcroflo according to CFD . In terms of simulation results from the three baseline models, ANSYS Fluent is conclusively recommended for CFD modeling of complicated indoor fluid environment compared with Star-CCM

Related Documents:

refrigerator & freezer . service manual (cfd units) model: cfd-1rr . cfd-2rr . cfd-3rr . cfd-1ff . cfd-2ff . cfd-3ff . 1 table of contents

The CFD software used i s Fluent 5.5. Comparison between the predicted and simulated airflow rate is suggested as a validation method of the implemented CFD code, while the common practice is to compare CFD outputs to wind tunnel or full-scale . Both implemented CFD and Network models are briefly explained below. This followed by the .

430 allocation to elianto cfd o&m 20,577.32 440 allocation to trillium west cfd o&m 27,267.00 450 allocation to west park cfd o&m 70,008.22 460 allocation to festival ranch cfd o&m 177,790.54 480 allocation to tartesso west cfd o&m 27,809.17 481 allocation to anthem sun valley cfd o&

Emphasis is on comparing CFD results, not comparison to experiment CFD Solvers: BCFD, CFD , GGNS Grids: JAXA (D), ANSA (E), VGRID (C) Turbulence Models: Spalart-Allmaras (SA), SA-QCR, SA-RC-QCR Principal results: Different CFD codes on same/similar meshes with same turbulence model generate similar results

Trindade, B.C. and J. Vasconcelos. 2011. "Comparison of CFD with Reservoir Routing Model Predictions for Stormwater Ponds." Journal of Water Management Modeling R241-05. doi: 10.14796/JWMM.R241-05. . This may help to explain why such CFD models are seldom used for detention pond analysis. Comparative Study of a CFD Model and a Reservoir .

an opportunity to use Computational Fluid Dynamics (CFD) to supplement experimental data with . and flow across the physics of interest. In order for CFD to be used confidently, these models must be validated against expected literature correlations as well as experimental data. . Wall Nusselt Number Comparison for CFD and Experimental .

A.2 Initial Interactive CFD Analysis Figure 2: Initial CFD. Our forward trained network provides a spatial CFD analysis prediction within a few seconds and is visualised in our CAD software. A.3 Thresholded and Modified CFD Analysis Figure 3: Threshold. The CFD is thresholded to localise on

performing CFD for the past 16 years and is familiar with most commercial CFD packages. Sean is the lead author for the tutorial and is responsible for the following sections: General Procedures for CFD Analyses Modeling Turbulence Example 3 - CFD Analysis

CFD Analysis Process 1. Formulate the Flow Problem 2. Model the Geometry 3. Model the Flow (Computational) Domain 4. Generate the Grid 5. Specify the Boundary Conditions 6. Specify the Initial Conditions 7. Set up the CFD Simulation 8. Conduct the CFD Simulation 9. Examine and Process the CFD Results 10. F

drag rise Mach number, obtained from the CFD solutions of 18 different participants using different codes, grid types, and turbulence models, showed a large variation, which revealed the general issue of accuracy and credibility in CFD simulations. The objective of this work is to illustrate different sources of uncertainty in CFD simu-

Figure 1. 3D model and CFD boundary conditions 2.2. Spatial discretization For the purpose of the comparison analyses between the different CFD techniques, the computational domain was significantly reduced by introducing two symmetry planes, at the both sides of the manikin. This measure the manikinwas

CFD (Computational Fluid Dynamic) Model Comparison between Two Independent Models 1.ANSYS CFD was utilized by CCNY (CCNY City College of New York) 2.COMSOL CFD was employed by QRDC (QRDC is an R&D Company in Chaska, MN) 3.A virtual wind tunnel was constructed to examine the performance of an INVELOX system 4.The results are in agreement

Comparison of two CFD tools against measurements on complex terrain 1st Symposium OpenFOAM dedicated to Wind Energy - March 21st 2013 Benoit Bichet, Tristan Fabre, Philippe Alexandre . Site conditions and Wind Resource Grids (WRG) comparison with two CFD models: ZephyTOOLS and Meteodyn Mean wind speed and turbulence intensity .

dynamics (CFD) is a promising design methodology . veloping numerical technique by which complex luid-low . by which many complicated luid low problems can be . problems can be solved on computers.To be able to transfer . solved with numerical codes. CFD embraces a variety . CFD expertise to analyze and design a face-ventilation sys-

Comparison between VLM and CFD Maneuver Loads Calculation at the Example of a Flying Wing Con guration (Received: July 7, 2019. Revised: Dec 18, 2019. Accepted: Dec 27, 2019) Arne Voˇ1 Abstract This work presents the results of computational uid dynamics (CFD) based maneu-ver loads calculations for a ying wing con guration. Euler solutions of .

conclusions to be drawn from the comparison other than that further research into more advanced turbulence models for use in commercial CFD codes is required (Freitas, 1995). In order to complete a fair comparison between di erent CFD codes and to establish concrete conclusion on the state-of-the-art of commercial CFD codes, all of the di erences

These models are however limited to flat and smooth topography, limiting the range of their applicability. On the other end of the computational cost scale, are high-fidelity computational fluid dynamics (CFD) tools. Most advanced CFD solvers can solve for buoyancy effects by accounting for different densities of the gas and atmosphere,

with CSD codes. The purpose of this paper is to perform a detailed comparison of the computed rotor airloads from these two CFD solvers, both coupled to the same CSD code, CAMRAD II.7 The computations will be performed for several cases of interest for the UH-60A rotorcraft. The UH-60A is an excellent configuration for CFD/CSD validation, as an

settings along with the post-flight data reduction process. 5 The best HYTHIRM data for CFD comparison, with the highest spatial resolution and lowest uncertainties, corresponds to Mach 8.4. The present report seeks to assess the accuracy and precision of turbulent CFD models for the prediction of

This study investigated microRNA and mRNA expression and protein function associated with DNA repair in human oocytes and embryos. MicroRNAs have been shown to down-regulate and in some cases to stabilise the expression of several genes including repair genes. The first aim of this study was to analyse the differences in the expression of microRNAs and their target mRNAs involved in repair .