Proceedings of the 2017 25th International Conference on Nuclear Engineering ICONE25 July 2-6, 2017, Shanghai, China ICONE25-67282 EXPERIMENTAL AND NUMERICAL STUDY OF AIRFLOW DYNAMICS THROUGH AN OPENING IN A DEPRESSURIZED ENCLOSURE: APPLICATION TO NUCLEAR DECOMMISSIONING Salima KAISSOUN Institut de Radioprotection et de Sûreté Nucléaire (IRSN) Gif-sur-Yvette, France [email protected] Eric CLIMENT Institut de Mécanique des Fluides de Toulouse. Université de Toulouse CNRS-INPT-UPS, France Corinne PREVOST Institut de Radioprotection et de Sûreté Nucléaire (IRSN) Gif-sur-Yvette, France ABSTRACT In order to understand airflow dynamics through small openings encountered in containment enclosures used for nuclear decommissioning operations, the results of experimental and numerical investigations are analyzed. The main purposes of this work are to identify the required conditions likely to generate flow inversions at the studied opening which lead to pollutant leakage outside depressurized enclosures, and also to verify the ability of CFD1 simulations to predict these flow inversions by using U-RANS2 and LES3 approaches. All along this work, we tried to reproduce the conditions of leakage occurring at the opening in terms of aerodynamics and openings geometries. Laser flow visualizations and CFD results show that an additional flow, such as a turbulent jet in competition with the directional flow and a disturbed level of pressure inside the enclosure are among the main causes leading to the leakage through the opening. Laurent RICCIARDI Institut de Radioprotection et de Sûreté Nucléaire (IRSN) Gif-sur-Yvette, France NOMENCLATURE ∆P pressure drop (Pa) Φ passive scalar concentration k turbulent kinetic energy (m2/s2) ω specific turbulence dissipation rate (s-1) U0 inlet velocity at the opening (m/s) V velocity of the additional flow (m/s) V0 injection velocity of the additional flow (m/s) DΦ kinematic diffusivity of Φ (m2/s) Sct turbulent Schmidt number ∆t time step for the CFD simulations (s) Q flow rate (m3/s) INTRODUCTION Operations of decommissioning and decontamination in nuclear facilities require setting up ventilated enclosures around contaminated equipments in order to prevent leakage of radioactive materials towards the surrounding environment. These enclosures are operated with a negative pressure relative to the room where they are installed, by using exhaust fans. Air arrives through openings which generates a directional airflow ensuring the dynamic containment of hazardous material. Due to operating activities and fluctuating differential pressure on both sides of the opening, local and unsteady flow inversions may occur leading to the propagation of contamination Keywords: Ventilated enclosures, Dynamic containment, Airflows at openings, Particle image velocimetry, Computational fluid dynamics. 1 CFD : Computational Fluid Dynamics U-RANS : Unsteady Reynolds Averaged Navier-Stokes 3 LES : Large Eddy Simulation 2 1 Copyright © 2017 ASME Downloaded From: http://proceedings.asmedigitalcollection.asme.org/ on 10/25/2017 Terms of Use: http://www.asme.org/about-asme/terms-of-use PRELIMINARY EXPERIMENTAL TESTS First of all, exploratory experimental tests were set up in order to observe flow inversions phenomena at a rectangular slit disposed on the front side of an existing airtight box. The purpose of these preliminary tests was to identify aerodynamic conditions likely to induce air leakage through the orifice. For that aim, two flows are involved: the first one represents the containment inflow generated by an exhaust fan as shown in Fig. 3 (enclosure extraction units are installed on the enclosure roof), the second flow is generated by an axial fan mounted inside the box in order to create additional turbulent fluctuations which can disturb the initial directional containment inflow. outwards. Recommendations of an efficient dynamic containment in nuclear installations are provided by the ISO 17873 standard [1] where three values of inlet velocity at the opening are suggested: 1.5 m/s for the tritium, 1 m/s for the plutonium 238 and 0.5 m/s for any other pollutants. However the ISO standard indicates that each case must be investigated specifically. Unlike most investigations on the aerodynamic containment of laboratory fume cupboards that deal with large openings [2] [3] and openings obstructed by the presence of a worker [4] [5], the current study is focusing on airflow dynamics through small openings, such as rectangular slits whose hydraulic diameter does not exceed ten centimeters and where the initial inflow stream is fully turbulent. The specific purpose of the whole study is to identify the main scenarios likely to disturb the containment inflow and possibly lead to air leakage through the studied orifice. Experimental device Experimental tests were conducted within a rectangular box with dimensions 0.8 × 0.8 × 0.6 m3 (depth × height × width). The slit has a surface of 0.2 × 0.03 m2 and a thickness of 5 mm. Geometric features of both the enclosure and the opening are detailed in Fig. 1. Initialy, we intended to study different opening locations and orientations, but we finally focused on the vertical one located at the top left, given that more flow inversions were noticed for this configuration. Incoming air arrives from the studied opening by an exhaust fan (while the remaining slits are sealed) which maintains a negative pressure in the enclosure. A smoke generator is connected to the box; the smoke is used in visualization as a flow tracer. The whole experimental device is detailed in Fig. 3. Thanks to the current study, it has been shown that the containment flow directed from the outside towards the enclosure might be disturbed by an additional parallel or perpendicular flow created inside or outside the enclosure causing flow instabilities in the near field of the opening due to its sharp edged geometry and the turbulent nature of the flows. Unfortunately, this phenomenon is not described in the literature because of the large number of possible configurations and the difficulties related to its quantification. In fact, the unsteadiness and three-dimensional aspects of flow structures make it very difficult to capture quantitatively and locally the amount of pollutant released. For these reasons, at the beginning of our study, some preliminary visualization tests on an existing enclosure formerly used as a glove box were conducted. Basically, a turbulent flow was created inside the enclosure by the motion of an axial fan and was meant to generate velocity fluctuations near the orifice. After that, Unsteady Reynolds Averaged Navier-Stokes computations of similar configurations, consisting of replacing the axial fan by an impinging turbulent jet, were performed using the commercial software ANSYS-CFX version 16.2. The turbulence model SST k-ω, was chosen for these computations since it is considered as the most appropriate for these cases presenting flow separation and recirculation zones [4]. The purpose of the preliminary experimental and numerical studies was to design a reduced scale model dedicated to reproducing appropriate air flows (in this case, external and internal turbulent jets) capable of generating air leakage through the opening. The last section of the paper represents first experiments and computations conducted on the final reduced scale model. Experiments based on laser sheet visualizations were conducted in the case of an external turbulent jet perpendicular to the containment inflow. U-RANS and Large Eddy Simulations were performed in the case of an internal jet blowing directly towards the opening in order to study the competition between both airflows near the orifice and to compare U-RANS and LES models for these types of flow configurations. Fig. 2 shows the laser flow visualization set up around the enclosure. The illumination system is a doubled-pulsed Nd: YAG laser with a head that delivers a green light sheet of 532 nm wavelength oriented towards the central vertical plane of the slit. A CCD camera is positioned perpendicularly to the lightening sheet to record images with a 10 Hz frequency ; flow tracer is filled of 1 µm diameter oil droplets. Fig. 1. Geometric features of the enclosure and the opening. 2 Copyright © 2017 ASME Downloaded From: http://proceedings.asmedigitalcollection.asme.org/ on 10/25/2017 Terms of Use: http://www.asme.org/about-asme/terms-of-use correspond, respectively to inner negative pressure of 0.5 Pa, 1 Pa and 3 Pa. We can observe strong vortex shedding at the slit which are increasingly significant as the inlet velocity is reduced. The axial fan motion produces turbulent fluctuations inside the enclosure and disturbs the inner pressure level which generates fluctuating velocities nearby the opening. At that time, it was difficult to quantify the velocity fluctuations generated by the inner fan. Fig. 2. Laser flow visualization device. Fig. 4. Laser visualizations of tracer leakage through the opening. (a) ∆P = -0.5 Pa, (b) ∆P = -1 Pa, (c) ∆P =-3Pa. Discussion Exploratory experiments have set the starting point of an approach aiming at understanding the phenomenon of flow inversions at the thin opening. It has been shown that turbulent fluctuations inside the enclosure generated by the axial fan motion is likely to disturb the directional containment flow and lead to unsteady flow inversions at the opening. The results of these flow inversions are shown in Fig. 4 as tracer leakage through the orifice. However flow patterns and directions of the additional flow created by the axial fan were not controlled. For that reason, a more controlled flow was set up for the following CFD simulations related to the same enclosure. The additional perturbating flow corresponds to an upstream flow competing with the initial one which is generated by a recirculation loop consisting of blowing and extraction ducts (Fig. 5). The blowing duct provides a turbulent jet impacting against the facing wall perpendicular to the the investigated opening; it constitutes, with the extraction duct, a closed loop so that the same quantity of air injected is extracted. Fig. 3. Details of the experimental set-up. Experiments and results Experiments presented below highlight the competition between the existing inflow at the opening and a second flow created inside the enclosure, which induces turbulent flow dynamics in the near field of the opening. Experiments of air exhaust were conducted first, in order to obtain inlet velocity values at the opening and the associated enclosure pressure. Then, the perturbating flow was included by putting an axial fan inside the enclosure, perpendicularly to the opening (Fig. 3) processed at a constant output speed equal to 20 m/s. Inlet velocities vary between 0.65 m/s and 2.4 m/s at the opening, driven by a range of negative pressure between 0.5 Pa and 7 Pa. Note that velocity magnitude is measured at the central point of the opening by a hot-wire probe. Fig. 4 illustrates instant laser tomographic visualizations of the flow tracer leakage outside the enclosure in the central vertical plane of the slit when both flows are enabled. Three values of initial inlet velocity at the opening are presented in Fig. 4: 0.65 m/s, 0.92 m/s and 1.57 m/s, which PRELIMINARY NUMERICAL SIMULATIONS This section is dedicated to numerical simulations, performed with the commercial CFD software ANSYS-CFX, of airflows in the enclosure and the slit presented above. Airflows in the following computations are, on the one hand, the containment inflow at the opening, and on the other hand, the impinging jet created at the wall adjacent to the slit. The objective of these simulations is to show the ability of U-RANS computations to predict the temporal and spatial details of this type of unsteady flow. The CFD results will permit to describe the airflow dynamics inside the enclosure and around the opening. 3 Copyright © 2017 ASME Downloaded From: http://proceedings.asmedigitalcollection.asme.org/ on 10/25/2017 Terms of Use: http://www.asme.org/about-asme/terms-of-use Pre-processing A description of the computational domain and mesh will be provided in this part as well as a presentation of the computational assumptions. Fig. 5 shows the three-dimensional view of the geometry performed by ANSYS WORKBENCH which is a global simulation system of ANSYS that integrates all necessary software programs from the CAD to the computation. The mesh was generated by ANSYS-ICEMCFD. A non-uniform, hybrid (structured/non structured) mesh containing 10,810,519 cells (10,484,026 tetra and 326,493 hexahedral cells) was employed. Fig. 6 shows horizontal and vertical planes of the mesh used for these computations centered on the investigated opening. Finer cells were used on the edges and around the opening to enable capture of flow recirculation; refinements were also applied along the adjacent walls to the opening. Considering the significant size of the preliminary computational domain (Fig. 5), a hybrid mesh was performed: hexahedral cells were created at the opening and adjacent walls and tetrahedral cells were positioned in the inner volume of the enclosure and the external domain. Thereafter, the geometry and size of the final reduced scale model will be improved; the enclosure will be chosen smaller and the external domain will be significantly reduced in order to have optimized structured meshes with a reasonable number of cells. Inlet and outlet (Fig. 5) are the boundary conditions related to the blowing and extraction of the additional flow. Outlet flow rate boundary conditions were imposed at the extraction of the enclosure and of the additional flow. Inlet flow rate boundary condition was imposed at the blowing of the secondary flow. The free-stream turbulence intensity is fixed as 5% of the inlet velocity. An ‘opening’ boundary condition was imposed on the surfaces of the external domain, specified with a static relative pressure value of 0 Pa. Blue arrows in Fig. 5 were added to show the boundaries between the physical wall related to the inner domain and the surface related to the external domain where an ‘opening’ boundary condition is imposed. In these U-RANS calculations, Shear Stress Transport (SST) kω model was used. Physical quantities related to Air at 25°C were chosen. To simulate the flow tracer injected inside the enclosure from the blowing duct, an additional turbulent transport equation for the variable (passive scalar) Φ is solved.. The kinematic diffusivity for the passive scalar DΦ is fixed to 10−5 m2 /s (correponding to smoke in air [6]) and the turbulent Schmidt number defined as the ratio of the turbulent viscous diffusion to the turbulent mass diffusion was chosen as Sct = 1 for the following studies. Fig. 5. Computational domain with boundary conditions. Fig. 6. Views of the computational mesh centered at the opening, (a) vertical x-y plane, (b) horizontal x-z plane. Computations and Results This part focuses on the CFD computations carried out to characterize airflow dynamics when the containment flow is disturbed by the secondary flow added inside the box. A description of the secondary flow alone is presented first, and then computations including both airflows are detailed. Dynamics of the additional flow In this part, only the additional flow is considered, the outlet boundary condition in the enclosure exhaust has been replaced by a no-slip wall. Flow rate at the inlet and the outlet of the additional flow loop is set to 0.1 m3 / which is equivalent to a mean velocity of 20 m/s through the 5.10−3 m2 blowing and extraction ducts. A time step ∆t of 10−2 s is chosen for the simulation. Fig. 7 shows three-dimensional velocity vectors when the flow goes out of the opening with a maximum speed of 5 m/s; the 4 Copyright © 2017 ASME Downloaded From: http://proceedings.asmedigitalcollection.asme.org/ on 10/25/2017 Terms of Use: http://www.asme.org/about-asme/terms-of-use can notice that the flow tracer goes outside the enclosure through the opening, visibly further, in the case of V0 = 20 m/s than the case of V0 = 6.5 m/s. In both cases, flow inversions occur at the upper part of the rectangular slit as illustrated by the exploratory experiments in Fig. 4 and for the characterization of the additional flow in Fig. 7; this can be explained by the presence of the enclosure roof very close to the slit and the adjacent perpendicular wall which drive the flow towards the top of the slit in the opposite direction of the containment flow. The additional flow in Fig. 7 impinges at the opening at a speed nearly equal to 5 m/s. turbulent jet (Re=10,000) injected from the inlet duct impinges against the face wall, follows it and arrives in front of the opening; in this case the additional flow is parallel to the initial one. Both vertical and horizontal planes given in Fig. 8 show the flow tracer outside the enclosure. We can notice that the additional flow, when it reaches the opening, is parallel to the axis of the containment flow in the opposite direction (countercurrent flows). This specific result will allow us to focus on the competition between the containment flow and a second one directly blowing towards the opening. Fig. 7. Description of the additional flow - three dimensional velocity vectors of the outflow; vertical plane in the near field of the opening. Fig. 9. Passive scalar fields (tracer flow) centered in the opening, vertical x-y plane; (a) = . / , (b) = /. Fig. 8. Description of the additional flow - passive scalar fields (tracer flow) centered at the opening, (a) vertical x-y plane, (b) horizontal x-z plane. Fig. 10. Velocity profiles at the vertical central x-y plane. Competition between two flows The competition between these flows at the opening is displayed in Fig. 9 which shows tracer spatial distribution. Velocity profiles at the central plane of the opening are given in Fig. 10 for the containment flow (dash red line) as well as in the case of competition between the two flows; V0 = 6.5 m/s (solid blue line) and V0 = 20 m/s (solid black line). We can notice that the initial inflow has changed its direction when adding an additional perturbating flow coming at the upper part of the slit. At the same time, the flow has been recovered inside the enclosure through the slit bottom part. Here both the containment flow and the additional one are considered. The flow rate imposed as a boundary condition in the enclosure exhaust is fixed to 0.004 m3 /s which is equivalent to an inflow velocity at the opening of 0.66 m/s. Two flow rates are chosen for the secondary flow: 0.032 m3 /s and 0.1 m3 /s, respectively, corresponding to 6.5 m/s and 20 m/s as mean input velocities through the 5.10−3 m2 blowing and extraction ducts. A time step ∆t of 5. 10−2 s is chosen for these unsteady simulations. These computations were initialized by the results of a stationary calculation with the containment flow only. A uniform negative pressure equal to −0. 6 Pa is given by the results of the containment flow simulation. Discussion Unsteady computations of airflows encountered in the preliminary experiments have been performed with the CFD commercial software ANSYS-CFX by applying the SST k- ω turbulence model. Thanks to these computations, we were able to describe airflow dynamics inside the enclosure in the case of a counter current competition between two flows. Vortices escaping through the investigated slit illustrated through laser flow visualizations in Fig. 4 could not be captured by the U- Fig. 9 shows the vertical central plane near the opening at a given time corresponding to maximum tracer going through the opening for the two output velocities of the additional flow. The flow is convected by the flow dynamics of the additional turbulent jet injected inside of the enclosure; we 5 Copyright © 2017 ASME Downloaded From: http://proceedings.asmedigitalcollection.asme.org/ on 10/25/2017 Terms of Use: http://www.asme.org/about-asme/terms-of-use RANS calculations. In fact CFD analysis of flow tracer illustrated in Fig. 9 shows smooth passive scalar escapes without any eddy structures. Given the large number of cells used for these computations (more than 10,000,000 cells) and the complexity of the unstructured mesh, a new approach was adopted for next CFD calculations. For that aim, a smaller three dimensional domain was used to simulate the competition between the directional flow and the additional one; this latter is either parallel to the initial one or directed towards the opening, both cases were investigated. opening or perpendicular to it as shown in Fig. 13 and in the computational domain in Fig. 16. Both the front face containing the opening and the rear face containing the extract units are removable for simple access to the enclosure. A flow visualization set-up (Fig. 12) consisting of a dual Nd : YAG laser delivering a 532 nm wavelength green light sheet and a 10 Hz CCD camera with 2048 × 2048 pixel resolution is implemented. A smoke generator delivering 1 µm diameter oil particles as flow tracer is connected to the enclosure. FINAL REDUCED SCALE MODEL In the light of the previous numerical and experimental studies, we were able, at that stage, to design a final reduced scale model on which the future investigations will be conducted. Experimental and numerical investigations on the final reduced scale model have started and first results will be presented in the following section. In this section is presented the final enclosure designed in order to reproduce the flows investigated above. The enclosure size and geometry have been carefully designed to ensure the best description of the investigated phenomenon; the studied enclosure is averagesized and its geometry allows a structured computational grid with a reasonable number of cells. The purpose of designing the reduced scale model is to be able to study several airflows competitions on a simple enclosure geometry. In this regard, we intend to study three flow configurations : the turbulent jet perpendicular to the containment inflow, either internal or external to the enclosure, and the internal turbulent jet in front of the orifice is also studied. The influence of the opening dimension and thickness is also intended to be investigated as prospects for further work. In the following section, we will present first experimental results of an external turbulent jet perpendicular to the containment inflow and the U-RANS – LES comparison in the case of a turbulent jet blowing towards the orifice directly competing with the initial containment inflow. Flow visualizations and PIV results A thin (1-3 mm) vertical light sheet is oriented towards the opening central y-z plane. The doubled pulsed laser-CCD camera facility is set in order to record laser tomography images as flow visualizations on both sides of the opening and also to conduct PIV post-processing on the successive particles images. Particle image velocimetry is a non-intrusive method which consists in capturing two images on two separate frames and performing multistep cross-correlation analysis [7]. Basically two experimental campaigns have been conducted; the containment inflow has been investigated first for a mean input speed U0 = 1m/s equivalent to an exhaust flow rate of 10.8 m3 /h. Then, interaction between the containment flow and the external perpendicular turbulent jet has been studied. Initial injection speed from the nozzle was fixed to V0 = 25.5 m/s; the layout of the secondary flow injection nozzle is illustrated in Fig. 13. Two distances between the slit center and the injection nozzle were chosen: 45 cm and 24 cm. In this way the turbulent jet impacts perpendicularly to the opening at two speeds, V0 = 5 m/s and V0 = 6.8 m/s. These two values were measured at the opening central point by a hot-wire anemometer probe. Design of the experimental device A final reduced scale model has been designed. Investigations are carried out on a rectangular small opening centered in the enclosure front wall in order to investigate the dynamics of flows involved without having wall effects that could change flow structures above. The enclosure is 0.5 × 0.5 × 1.2 m3 (see Fig. 11) and the slit has a surface of 0.1 × 0.03 m2 and a thickness of 5 mm. Two square (a = 0.05 m) extract units, located at the rear face parallel to the front wall containing the opening, are chosen for the enclosure exhaust. The square geometry is specifically chosen to keep computational meshes structured. The extract units are centered at the rear face and symmetrically opposed with respect to the slit axis in order to ensure a homogenous internal pressure field and a directional inflow. Enclosure depth (0.5 m) and width (1.2 m) have been carefully chosen to allow an internal additional flow, basically as a turbulent jet injected from a rectangular small 0.1 × 0.01 m2 nozzle located in front of the Fig. 11. Geometric features and dimensions of the reduced scale model. Fig. 12. Experimental device and PIV set-up. 6 Copyright © 2017 ASME Downloaded From: http://proceedings.asmedigitalcollection.asme.org/ on 10/25/2017 Terms of Use: http://www.asme.org/about-asme/terms-of-use Considering the cases of competition between the initial flow and the external perpendicular turbulent jet, leakage flow visualizations outside the enclosure (Fig. 14) show more significant vortices in the case where the injection nozzle is positioned the nearest to the opening (Fig. 14 (b)). The time averaged velocity vector fields shown in Fig. 15 present more intense inversion speeds for the case when the jet is the nearest to the opening; 0.3 m/s is globally the mean velocity at which airflow goes out of the enclosure when the perturbating velocity is about 6.8 m/s (Fig. 15 (b)) perpendicularly to the opening and 0.2 m/s in the case of an additional flow of 5 m/s (Fig. 15 (a)). Fig. 15. Particles images and time-averaged velocity vector fields; competition between two flows-enclosure inner plane. (a) = / , (b) = . /. Numerical simulations: U-RANS vs LES Here are commented the first CFD results about simulations conducted on the final reduced scale geometry. In this part containment flow simulation is described in addition to the competition between this initial airflow and an internal turbulent jet blowing towards the opening. The U-RANS assumptions (working fluid, turbulence modeling, and transport equation) are kept identical all along the article; however new Large Eddy Simulations are conducted. Structured grids are highly refined and time steps are smaller (especially for the ‘LES’ computations). The sub-grid scale model chosen for the Large Eddy Simulations is the Smagorinsky-Lilly model available in ANSYS CFX software. The U-RANS mesh is about 11 million hexahedral cells and the ‘LES’ one is more than 29 million cells. Meshes are refined in the surrounding volume of the opening including opening sides and adjacent walls; cells are also refined in the depth of the opening. The grid horizontal and vertical planes are illustrated in Fig. 17. Unsteady simulations are initialized by the RANS computations results of the containment flow only. Given that a mean velocity of 1 m/s is required, an outlet speed boundary condition was imposed at the extract units equal to 0.6 m/s. Then for the unsteady simulations, an inlet velocity boundary condition of 10 m/s was imposed at the injection nozzle positioned inside the enclosure as shown in Fig. 16. In order to avoid any internal over pressure due to mass contribution of the airflow additionally injected inside the enclosure, the same air flow rate injected was extracted through the exhaust so that outlet boundary condition at extract units became equal to 2.6 m/s. In the U-RANS computations, time step was c equal to 10−2 s. Concerning ‘LES’ computations, a time step of 10−3 s was adopted in simulating the containment flow only and 10−4 s for both the containment flow and the turbulent jet. The Reynolds number of the jet is equal to 10,000. Fig. 13. Additional flow experimental set-up, (a) layout of the injection nozzle, (b) plane view of the investigated cases. Fig. 14. Laser tomography visualization of leakage flow at the vertical plane outside the enclosure. (a) V = 5 m/s , (b) V = 6.8 m/s . 7 Copyright © 2017 ASME Downloaded From: http://proceedings.asmedigitalcollection.asme.org/ on 10/25/2017 Terms of Use: http://www.asme.org/about-asme/terms-of-use the same time t = 2 s. It is noticeable that flow tracer could reach the opening and leave the enclosure in the form of eddy structures driven by the dynamics of the turbulent jet in the case of LES computation. This phenomenon is not observed in the U-RANS computation where we can see that flow tracer was not able to go beyond the opening. In fact, in the developed region of the turbulent jet, a three dimensional mixing zone is obtained where vortices structures disrupt the inflow at the opening and lead to flow inversions. These eddy structures are not captured by the U-RANS approach due to averaging; URANS results can give us information on mean velocities but not local and instantaneous velocity fluctuations. The analysis of U-RANS results shows that in general U-RANS computations are unable to predict the flow leakage through the orifice which is an important feature for further analysis. Fig. 16. View of the computational domain. Fig. 17. Views of the computational mesh centered at the opening, (a) horizontal x-z plane, (b) vertical y-z plane. Fig. 19. Passive scalar fields at the vertical plane, (a) ‘RANS’ computation, (b) ‘LES’ computation. Fig. 20. Passive scalar fields at the horizontal plane, (a) ‘RANS’ computation, (b) ‘LES’ computation. DISCUSSION Due to the few investigations conducted in the exploration of flow inversions phenomena at rectangular slits in a depressurized enclosure, the approach adopted was to try to reproduce the phenomenon under different controlled configurations and to characterize its dynamics. It has been found that an additional turbulent flow (typically a jet) either inside the enclosure or outside is the main cause leading to the leakage at the opening. Vortex structures highlighted in our experiments by laser visualizations are not captured by CFD URANS computations even though the meshes used are adequately refined. However U-RANS simulations can provide global information on general flow patterns such as mean velocities and pressure fields. LES computations are able to describe turbulent structures and consequently capture flow Fig. 18. Velocity fields of the containment flow- horizontal and vertical planes, (a) ‘RANS’ computation, (b) ‘LES’ computation. Results of containment flow calculations show for both RANS and LES cases a potential core region of a maximum velocity about 1.55 m/s (Fig. 18). The containment inflow impacts against the rear wall of the enclosure and goes along the adjacent walls. LES velocity fields evidence turbulent structures in a region far from the opening. LES computations results are more interesting when the second turbulent flow is competing with the initial one. In this regard, passive scalar fields are illustrated in both the U-RANS and LES computations in Fig. 19 and Fig. 20; the comparison is made at 8 Copyright © 2017 ASME Downloaded From: http://proceedings.asmedigitalcollection.asme.org/ on 10/25/2017 Terms of Use: http://www.asme.org/about-asme/terms-of-use leakages at the opening. Unfortunately, this type of calculations are highly CPU demanding; almost three weeks of calculation were needed to compute a turbulent case with 29 million cells and a time step of 10−4 s on 48 parallel processors. As prospects for further work, a wide range of V0 /U0 , the ratio of the additional flow velocity at injection to the containment flow velocity, will be studied thanks to the final experimental set-up in the cases of both the internal perpendicular jet and the parallel one (the external perpendicular jet will also be investigated). Lastly, the quantity of outflow leakage will be measured by a helium tracer-gas detection technique. ACKNOWLEDGMENTS This work was conducted as part of a PhD equally supported by IRSN and EDF. The contribution of Luc Lafanechere from EDF is gratefully acknowledged by the authors, particularly for fruitful discussions. REFERENCES [1] ISO 17873:2004, Nuclear facilities —Criteria for the design and operation of ventilation systems for nuclear installations other than nuclear reactors. [2] Nicholson G. P., Clark R. P. and Calcina-Goff M. L. D., (2000). Computational Fluid Dynamics as a Method for Assessing Fume Cupboard Performance. Annals of Occupational Hygiene, 44(3), pp. 203-217. [3] Durst F. and Pereira J. C. F., 1991. Experimental and numerical investigations of the performance of fume cupboards. Building and Environment 26.2, pp. 153164. [4] Karaismail E. and Celik I., 2010. On the inconsistencies related to prediction of flow into an enclosing hood obstructed by a worker. Journal of occupational and environmental hygiene, 7.6, pp. 315325. [5] Chern M.-J. and Cheng W.-Y., 2007. Numerical Investigation of Turbulent Diffusion in Push–Pull and Exhaust Fume Cupboards. Annals of Occupational Hygiene 51.6, pp. 517-531. [6] ANSYS INC., 2009. CFX-Solver Theory Guide. [7] Cao X., Liu J., Jiang N. and Chen Q., 2014. Particle image velocimetry measurement of indoor airflow field: A review of the technologies and applications. Energy and Buildings 69, pp. 367-380. 9 Copyright © 2017 ASME Downloaded From: http://proceedings.asmedigitalcollection.asme.org/ on 10/25/2017 Terms of Use: http://www.asme.org/about-asme/terms-of-use

1/--страниц