Experimental Validation of Computer Fluid Dynamics Simulation

0 downloads 0 Views 1MB Size Report
Modeling of air flow over buildings belongs to a challenge that was accepted by ... Computer Fluid Dynamics (CFD) simulation by experimental measurement in ...
Available online at www.sciencedirect.com

ScienceDirect Procedia Engineering 190 (2017) 377 – 384

Structural and Physical Aspects of Construction Engineering

Experimental Validation of Computer Fluid Dynamics Simulation aimed on Pressure Distribution on Gable Roof of Low-rise Building Juraj Králika,*, Lenka Konečnáb, Dagmar Lavrinčíkováa a

Slovak Univesity of Technology in Bratislava, Faculty of Architecture, Institude of Constraction in Architecture and Engineering Structures, Námestie Slobody 19, 812 45 Bratislava, Slovakia b Slovak Univesity of Technology in Bratislava, Faculty of Civil Engineering, Department of Structural Mechanics, Radlinského 11, 810 05 Bratislava, Slovakia

Abstract Modeling of air flow over buildings belongs to a challenge that was accepted by several authors. There are couple reasons for it, from which the most frequent is simulation in order to obtain pressure or external pressure coefficients distributions. These simulations are always a balance between accuracy and computer needs and consumed time. Aim of this contribution is to validate Computer Fluid Dynamics (CFD) simulation by experimental measurement in Boundary Layer Wind Tunnel (BLWT). A low-rise building with gable roof will be examined and results will be compared to wind tunnel test. For the purpose of this simulation were chosen Delayed Detached Eddy Simulation (DDES) and Scale-Adaptive Simulation (SAS) turbulence models. It is observed that the DDES model failed in predicting pressures around the roof ridge. The average deviations on the gable roof from the BLWT measurements are 37.2 % for DDES and 26.7 % for SAS model. ©2017 2017Published The Authors. Published by Elsevier Ltd. © by Elsevier Ltd. This is an open access article under the CC BY-NC-ND license Peer-review under responsibility of the issue editors. (http://creativecommons.org/licenses/by-nc-nd/4.0/). Peer-review under responsibility of the organizing committee of SPACE 2016 Keywords: experiment; Ansys; airflow; presure; presure coeficients; gable roof

1. Introduction As Computer Fluid Dynamic (CFD) software develops, problems of fluid dynamics becoming interesting for more engineers. CFD is a handy tool capable of reasonable predicting of air-flows and in this article will be used to predict pressure distribution on simple rectangular low-rise building with gable roof. Setting up CFD simulation using table

* Corresponding author. Tel.: +421-903-951-403. E-mail address: [email protected]

1877-7058 © 2017 Published by Elsevier Ltd. This is an open access article under the CC BY-NC-ND license

(http://creativecommons.org/licenses/by-nc-nd/4.0/). Peer-review under responsibility of the organizing committee of SPACE 2016

doi:10.1016/j.proeng.2017.05.352

378

Juraj Králik et al. / Procedia Engineering 190 (2017) 377 – 384

PC is always a balance between accuracy, consumed time and computational demands needed for simulation. And at the same time there’s no universal turbulent model, in fact there are several turbulence models which are being offered by several commercial or non-commercial software. There are three turbulent flow simulation methods Reynolds Averaged Navier-Stokes Simulations (RANS), Scale Resolving Simulations (SRS) and Direct Numerical Simulation (DNS). For the purpose of this analysis was used commercial software package ANSYS Fluent R16.2. Some experiments in wind tunnel were carried out by Ho, where he was in his work, [1], was describing the background of the project, the basic models, testing configurations, the wind simulation, the standard archival format for distribution of the data, and a basic analysis of the data. He claims that the data obtained within his study are consistent with the expected aerodynamic behavior and comparisons with full scale data show that the wind tunnel tests match the full-scale reasonably well, but cannot reproduce the largest of the peak point suctions near roof edges. The air flow around isolated gable-roof buildings with different roof pitches was investigated by wind tunnel experiments and Computational Fluid Dynamics (CFD) simulations based on steady Reynolds Averaged Naviere Stokes equations (RANS) model by Tominaga, [2]. He used three different pitches, 3:10 (16.7°), 5:10 (26.5°), and 7.5:10 (36.9°) and furthermore he tested four turbulence models, namely, the standard k-ε, the RNG k-ε, the realizable k-ε, and the k-ω SST model. He observed large difference in the flow patterns is between the pitches, this implies that the flow pattern around a building with a pitched roof changes critically at a roof angle of around 20°. Another research based on wind tunnel experiment was done by Krejsa, [3], where he in his work was studding aeroelastic behavior of bridge deck under influence of the wind. His experiments show that the traffic can have influence on the stability of the bridge. And the traffic situated leeward influenced the heave damping, perhaps due to different reattachment of the flow at the bridge deck, creating the vertical negative net damping force. On the other hand the bridge was mostly sensitive to torsional flutter, while setup without traffic was the most unstable. Thus, such influences cannot be neglected, when analyzing the instability of a bridge loaded by the wind. A low-rise building was constructed near Shanghai Pudong International Airport by East China Sea to study the characteristics of wind field and wind pressure on the roof of the building. The remarkable feature of the test building is that the roof pitch can be adjusted range from 0° to 30°. This analysis was done by Xu, [4], where he in his work was analyzing wind pressures on gable roof with different roof pitches (0°, 10° and 20°) and then comparison was done with a wind tunnel test on a rigid model of 1:30 scale. His field measurement was consistent with that by wind tunnel test. Furthermore he analyzed the probability distributions of fluctuating pressures, which agrees well with Gaussian processes when the skewness is larger than -0.5, while having better agreement with Gamma distribution when the value of skewness is between -1 and -0.5. Aim of this contribution is to compare experiment in Boundary Layer Wind Tunnel (BLWT) with CFD simulation. As experiment object was chosen a low-rise building with gable roof with roof pitch of 20°. Experiment was focused on obtaining pressure values from pressure taps in selected locations on the gable roof. During this experiment were also measured velocity profiles. CFD final volume element model was created with respect to y+ value, with limit to accuracy set by number of polyhedral elements to around 2·106 (a table PC task). Nomenclature z0 zref uref ufric κ k ε ω Cμ

terrain roughness reference high reference velocity friction wind velocity Von Karman constant turbulent kinetic energy turbulence dissipation rate specific turbulence dissipation rate model constant

Juraj Králik et al. / Procedia Engineering 190 (2017) 377 – 384

2. The y+ approach The y+ value is a non-dimensional distance (based on local cell fluid velocity) from the wall to the first mesh node, and is determining whether the influences in the wall adjacent cells are laminar or turbulent. In CFD often used to describe if mesh is fine or coarse. There are three subdivisions of the near wall region in turbulent boundary layer, see Fig. 1 (a) : viscous sub layer region with y+ < 5 (velocity profiles assumed to be laminar and dominate the wall shear); buffer region with 5 < y+ < 30 (dominates both viscous and turbulent shear); fully turbulent portion or log-law region with 30 < y+ < 300 (turbulent shear dominates). Values of y+ close to the lower bound y+ ≈ 30 are most desirable for wall function and y+ ≈ 1 for near wall modelling, [5]. So we can say that y+ is a suitable selection criterion for determining the appropriate mesh configuration and turbulence model.

Fig. 1. (a) subdivisions of near-wall region, [5]; (b) model view in BLWT at 90° rotation.

Desired First Layer Thickness (FLT) for this analysis is y+ = 0.5 so the thickness of first cell should be 1.0·10-5 m according to calculations of first cell thickness. 3. Wind tunnel experiment Experimental measurements were carried out in universal wind tunnel - BLWT SvF STU in Bratislava, more about this BLWT can found in references, [6-8]. The model was placed on the rotating table, which was used for changing of the wind direction (0º, 45º and 90º), see Fig. 1 (b). External pressures were measured by three 16-channel pressure scanners SCANIVALVE DSA 3217. Totally, 173 pressure taps were placed on the model with gable roof. Reference velocities were measured by Almemo probe type MA25902 (AHLBORN). Vertical profiles were measured by Hotwire Anemometer MiniCTA 54742 and by Almemo probe. Two Prandtl tubes were used for control of equability of pressures in wind tunnel during the tests. Self-developed programs created in software LabView (National Instruments) were used for recording and analyzing of data. Example of measured velocity profile 600 mm in front of object can be seen on Fig. 2 (a). 4. CFD simulation There are two fundamental approaches to design and analysis of engineering systems that involve fluid flow: experimentation and calculation. Modern engineers using both, where experimental in many cases are used to validate computational. CFD simulations can offer engineer good inside view all over computational domain and can quickly provide results of velocity magnitudes, pressures and many other turbulent parameters. In this case was CFD used to obtain pressure in selected points on the gable roof. For this study case were chosen two turbulence models, first was DDES (from experience with this model) and as second it was SAS turbulence model.

379

380

Juraj Králik et al. / Procedia Engineering 190 (2017) 377 – 384

4.1. Boundary conditions Each surface in computational domain had its “named section” to which were in solution module set boundary condition. Inlet was set as velocity inlet. Outlet as outflow as this boundary don’t require additional information and data at exit plane are extrapolated from interior. Left, right and top faces of domain were defined as symmetry. Object faces and bottom plane were set as no slip walls without roughness.

Fig. 2. (a) measured velocity profile; (b) location of pressure taps on the right symmetry part of the roof.

4.2. CFD inputs Wind velocity profile, which was used, was defined exactly same as was measured in BLWT. Other turbulent inputs, like friction velocity ufric, turbulent kinetic energy k, turbulence dissipation rate ε and specific turbulence dissipation rate ω were defined as follows: uref ˜ N

u fric

k

§ z  z0 · ¸¸ ln ¨¨ ref © z0 ¹

u fric

H z Z z

2

1.414 2 0.09

CP

u fric

7.11 ˜ 0.4 1.414 m / s § 0.1  0.01545 · ln ¨ ¸ © 0.01545 ¹

(1)

6.67m 2 / s 2

(2)

3

N ˜ z  z0

(3)

H z k

(4)

Juraj Králik et al. / Procedia Engineering 190 (2017) 377 – 384

These conditions following specification by Richards and Hoxey of fully developed inlet profile, [9]. Terrain roughness z0 was calculated from friction velocity, the value 1.414 m/s comes from BLWT inlet profile measurement that was made 600 mm in front of object. 4.3. DDES Detached Eddy Simulation (DES) was introduced by Spalart and co-workers, to eliminate the main limitation of LES models by proposing a hybrid formulation that switches between RANS and LES based on the grid resolution provided. By this formulation, the wall boundary layers are entirely covered by the RANS model and the free shear flows away from walls are typically computed in LES mode. The formulation is mathematically relatively simple and can be built on top of any RANS turbulence model. DES has attained significant attention in the turbulence community as it was the first SRS model that allowed the inclusion of SRS capabilities into common engineering flow simulations. As the grid is refined below the limit the DES-limiter is activated and switches the model from RANS to LES mode. The intention of the model is to run in RANS mode for attached flow regions, and to switch to LES mode in detached regions away from walls. This suggests that the original DES formulation, as well as its later versions, requires a grid and time step resolution to be of LES quality once they switch to the grid spacing as the defining length scale. DES limiter can already be activated by grid refinement inside attached boundary layers. In order to avoid this limitation, the DES concept has been extended to Delayed DES (DDES) by Spalart, [10,11]. 4.4. SAS The Scale-Adaptive Simulation (SAS) concept is based on the introduction of the von Karman length-scale into the turbulence scale equation. The information provided by the von Karman length-scale allows SAS models to dynamically adjust to resolved structures in a URANS simulation, which results in a LES-like behavior in unsteady regions of the flow field. The advantage of SAS model over hybrid RANS-LES models (called Detached Eddy Simulation ̢ DES) is in no explicit dependency on grid spatial resolution, [12]. The scale equation of SAS models is based on an exact transport equation for the turbulence length scale as proposed by Rotta. This method was re-visited by Menter and Egorov and avoids some limitations of the original Rotta model, [10]. 4.5. Final volume model Geometry of project was built in Ansys Fluent Design modeler. Final volume model (FVM) was created under fluent Meshing module. Model itself consisted of three boxes from which one was used as computational domain with size 2x1.5x0.5 m and the other two were used as body of influence. The smaller one (0.4x0.5x0.2 m) was covering object with 0.1 m from all sides and was set to have max elements size to 0.005 m. Longer one (1.0x0.5x0.2 m) was used to dense mesh in leeward zone behind object and was set to have max element size 0.015 m, see Fig. 3 and 4. Mesh was created as follows: fixed advanced sizing function, fine relevance center, high smoothing and slow transition. Maximum element size was set as 0.05 m. Sizing function on object surfaces was set to 0.002 m what represents 50 elements per object high. Inflation was used on object walls with FLT of 1.0·10 -5 m with 30 layers and 20% growth rate. To obtain same velocity profile from BLWT was inlet face divided with face sizing function set to 0.005 m. All together were generated 7 441 578 tetrahedron elements which were next converted into polyhedral mesh with 2 261 492 polyhedral elements. 4.6. Solver setup A double precision solver with parallel processing was used with a Semi-Implicit Method for Pressure Linked Equations algorithm (SIMPLE) for the velocity-pressure coupling. Second-order schemes were used for pressure, momentum and turbulent quantities discretization. The unsteady formulation was based on a second order implicit

381

382

Juraj Králik et al. / Procedia Engineering 190 (2017) 377 – 384

scheme, but when the SAS model was used, the momentum equations were discretized with a bounded central discretization while the transient formulation was based on a bounded second-order implicit scheme. Solution was initialized with hybrid initialization with default settings. A fixed time stepping method was used with time step size of 0.0005 sec in case of DDES and in case of SAS it was 0.0001 sec and sampling of transient data started from 0.5 sec and ended at 1 sec.

Fig. 3. Final volume model: tetrahedron mesh view in middle plane.

Fig. 4. Final volume model: polyhedral mesh view in middle plane.

5. Results and discussion As mentioned before aim of this contribution is to compare performance of two selected SRS turbulence models with experimental measurement in BLWT. An object of 0.2x0.3x0.1 m with gable roof of 20° was examined in wind tunnel and next by CFD. Because of large amount of results is the comparison limited only to pressure distribution on gable roof and velocity contours in middle plane. Example of mean pressure distribution of on the gable roof can be seen in Fig. 5, here we can see how DDES over predicted pressures at roof ridge.

Fig. 5. Pressure distribution on the roof; (a) DDES; (b) SAS.

383

Juraj Králik et al. / Procedia Engineering 190 (2017) 377 – 384

Fig. 6. Contours of mean velocity in middle vertical plane; (a) DDES; (b) SAS.

On Fig. 6 we can see how differently resolved wind flow around building with gable roof was. If we take a look on windward area (from inlet to windward wall on building) there is almost no difference. It start to differ when wind approach windward wall and a small recirculation is created above windward part of roof. After that wind approaches to roof ridge where DDES model clearly couldn’t reproduce the flow around roof ridge and higher velocity speed shows up. Here also pressures reaching higher values compared to experiment, approximately 3x higher for DDES turbulence model compared to BLWT. The leeward part of roof was also resolved differently, while the DDES resolved the flow almost as laminar (leeward part of roof) with a large recirculation region formed behind the building starting from the leeward edge of roof. The SAS model recirculation region started from the roof ridge and the length of it is around the same but it’s higher, this is believed to happen because of different turbulent intensity resolved by models. Compared to BLWT the values of turbulent intensity near surfaces were around 51.7% and for DDES it was around 26% and for SAS around 15%.

0 1 4 7 10 13 16 19 22 25 28 31 34 37 40 43 46 49 52 55 58 61 64 67 70 73 76 79 82 -0.5

Cp

-1 -1.5 -2 -2.5 Pressure taps

BLWT

DDES

Fig. 7. External pressure coefficients on gable roof.

SAS

384

Juraj Králik et al. / Procedia Engineering 190 (2017) 377 – 384

External pressure coefficients calculated in CFD-Post for both BLWT and CFD are shown on Fig. 7. Taps at roof ridge are easily to identify, all have values higher than -2. The average deviations are for DDES within 2 to 160% and for the SAS model 0.6 to 54 %. Best was resolved windward corner of the roof by DDES (points 65 to 82) and worst was resolver roof ridge by DDES. 6. Conclusions This paper has presented a 3D unsteady (SRS) CFD simulation for the prediction of the mean wind pressure distribution on gable roof of a low-rise building and validation with BLWT measurements. The results show that the best match between BLWT experiment and CFD simulation was on the windward corner. The SAS model gave average deviations of 26.7%, the DDES model would be more accrue with average deviations of 37.2% and after removing ridge taps and taps in middle of windward roof part, where were the highest deviations, average deviations drop to 24.8% for the SAS model and 20.1% for the DDES model. This analysis can help researchers better understand behaviour of selected turbulence models and choosing and setting up their own simulations. The future plans are to examine the influence of turbulent intensity on the wind flow as a part of wind tunnel experiment outputs and CFD inputs. Furthermore examine influence of inflation layers on results. Acknowledgements This contribution is the result of the researches supported by Slovak Grant Agency VEGA. Registration numbers of the projects are 1/0256/16 and 1/0951/16. This paper was created with the support of the Ministry of Education, Science, Research and Sport of the Slovak Republic within the Research and Development Operational Programme for the project "University Science Park of STU Bratislava", ITMS 26240220084. The authors acknowledge with thanks the support of the TU1304 COST ACTION “WINERCOST”. This paper was supported also by STU in Bratislava, from the STU Grant scheme for support of excellent team – projects no. 1619 and no. 1651. References [1] T.C.E. Ho, D. Surry, D. Morrish, G.A. Kopp, The UWO contribution to the NIST aerodynamic database for wind loads on low buildings: Part 1. Archiving format and basic aerodynamic data, in: Journal of Wind Engineering and Industrial Aerodynamics, 93, 1–30, 2005. [2] Y. Tominaga, S. Akabayashi, T. Kitahara, Y. Arinami, Air flow around isolated gable-roof buildings with different roof pitches: Wind tunnel experiments and CFD simulations. Building and Environment 84, 2015, pp. 204-213. [3] M. Machacek, S. Pospisil and M. Krejsa, Wind Tunnel Experiments Focused on the Bridge Deck Stability Coefficients, in: Applied Mechanics and Materials, Vols. 752-753, 2015, pp. 662-667. [4] W. Xu, H. Peng, G. Ming, Field measurement of wind loads on low-rise building with adjustable roof pitch, The Seventh International Colloquium on Bluff Body Aerodynamics and Applications (BBAA7), Shanghai, China, 2012. [5] ANSYS Fluent 14.0 Theory Guide [6] T. Skrucany, B. Sarkan, J. Gnap, The influence of aerodynamic trailer devices on drag reduction measured in a wind tunnel. Maintenance and Reliability, Vol. 18(1), 2016, pp.151–154. [7] O. Hubova, L. Konecna, I. Oleksakova, Experimental and numerical determination of wind pressure distribution on an object with atypical form. Applied Mechanics and Materials, Vol. 769, 2015, pp.185–191. [8] O. Hubova, P. Lobotka, L. Konecna, Pressure coeficients on the model of SILSOE cube determined by tests in BLWT tunnels. Roczniki inzynierii budowlanej, Vol. 14, 2014, pp.85-90. [9] P. Richards, R. Hoxey, Appropriate boundary conditions for computational wind engineering models using the k–ε turbulence model. Jornal of Wind Engineering and Industrial Aerodynamics, Vols. 46 (47), 1993, pp.145–153. [10] Spalart, P., S. Deck, M. Shur, K. Squires, M. Strelets, and A. Travin. A New Version of Detached Eddy Simulation, Resistant to Ambiguous Grid Densities, Journal of Theoretical and Computational Fluid Dynamics 20, 2006, pp. 181–195. [11] F.R. Menter, Best Practice: Scale Resolving Simulations in ANSYS CFD. Version 2.0. http://www.ansys.com/staticassets/ANSYS/staticasse ts/resourcelibrary/techbrief/tb-best-practices-scale-resolving-models.pdf, 2015. [12] F. R. Menter, Y. Egorov, The Scale-Adaptive Simulation Method for Unsteady Turbulent Flow Predictions. Part 1: Theory and Model Description, Flow Turbulence Combust, vol. 85, no. 1, Jul. 2010, pp. 113–138.