Available online at www.sciencedirect.com Nuclear Engineering and Design 238 (2008) 492–501 CFD analysis for thermal mixing in a subcooled water tank under a high steam mass flux discharge condition Hyung Seok Kang ∗ , Chul Hwa Song Korea Atomic Energy Research Institute, Yusung, Daejeon 305-600, Republic of Korea Received 26 October 2006; received in revised form 18 January 2007; accepted 2 February 2007 Abstract A Computational Fluid Dynamics (CFD) analysis for a thermal mixing test was performed for 30 s to develop the methodology for a numerical analysis of the thermal mixing between steam and subcooled water and to apply it to Advanced Power Reactor 1400 MWe (APR1400). In the CFD analysis, the steam condensation phenomenon by a direct contact was simulated by the so-called condensation region model. Thermal mixing phenomenon in the subcooled water tank was treated as an incompressible flow, a free surface flow between the air and the water, and a turbulent flow, which are implemented in the CFX4.4. The comparison of the CFD results with the test data showed a good agreement as a whole, but a small local temperature difference was found at some locations. A sensitivity analysis was performed to find the reason of the temperature difference. The commercial CFD code of CFX4.4 together with the condensation region model can simulate the thermal mixing behavior reasonably well when a sufficient number of mesh distributions and a proper numerical method are selected. © 2007 Elsevier B.V. All rights reserved. 1. Introduction The experimental and CFD research for an unstable steam condensation in a Direct Contact Condensation (DCC) which may occur in the In-containment Refueling Water Storage Tank (IRWST) of the APR1400 were performed (Song et al., 2003; Kim et al., 1997; Kim et al., 2005; Park et al., 2005; Kang et al., 2002, 2004, 2005). An unstable steam condensation may damage the IRWST wall (KEPCO, 2002; Su, 1981; Ra, 1999). This unstable steam condensation may happen due to the fluctuation of the interfaces between the steam jet and the condensed water when the temperature of entrained water flowing into the steam jet region is increased (Kang et al., 2005; Su, 1981). Therefore, the prediction of the entrained water temperature and thermal mixing pattern is important for characterizing the instability of steam jet condensation. A set of thermal mixing experiments has been performed to understand the thermal mixing phenomena induced by a steam discharge into the subcooled water in the APR1400 IRWST in order to avoid an unstable steam condensation due to the locally increased water temperature (Song et al., 2003; Kim et al., 2005; Park et al., 2005). ∗ Corresponding author. Tel.: +81 42 868 8948; fax: +81 42 861 6438. E-mail address: [email protected] (H.S. Kang). 0029-5493/$ – see front matter © 2007 Elsevier B.V. All rights reserved. doi:10.1016/j.nucengdes.2007.02.044 In the CFD analysis, the numerical methodology which can predict the local and global thermal mixing in the tank was developed based on a comparison of the CFD results with test data. The currently available commercial CFD codes do not have the model to treat the DCC (AEA Tech., 2001), and the development of a numerical model for the DCC has been recently tried only to an ideal flow case (Davis and Yadigaroglu, 2004). Thus, in this study a steam condensation region model has been developed based on the water temperature data around a steam jet to simulate the DCC (Kang et al., 2002, 2004, 2005; Cook, 1994). In this model, the calculated temperature and velocity of the condensed water and the entrained water in or around the condensation region are used as the boundary conditions for a thermal mixing CFD analysis (Kang et al., 2002, 2004, 2005). The comparison of the CFD results with the test data of a transient steam discharge under the high steam mass flux conditions shows a good agreement in general, but some small temperature differences between the CFD results and the test data are shown at some locations near the region just above the sparger inside the tank (Kang et al., 2002, 2004, 2005). These differences may arise due to an insufficient mesh distribution generated in the grid model to resolve the flow field around the steam jet flow, specially near the region above the sparger discharge head, or an improper selection of the numerical model. The only difference between the CFD results and the test data is observed to H.S. Kang, C.H. Song / Nuclear Engineering and Design 238 (2008) 492–501 493 Nomenclature B D G h H k P ro V xc body force (N) diameter of the condensation region model (cm) mass flux (kg/m2 s) enthalpy (J) height of the condensation region model (cm) specific heat ratio (Cp /Cv ) pressure (Pa) radius of the discharge hole (cm) velocity (m/s) steam penetration length (cm) Greek symbols ␥ volume fraction thermal conductivity [W/m ◦ C] μ viscosity [kg s/m2 ] ρ density [kg/m3 ] Subscripts con condensed ent entrained ex at the condition of the completion of external expansion f fluid i initial o at the condition of discharging hole exit s steam ␣ phase ∞ ambient state in the subcooled water be the increased value of the stagnant water temperature at the upper-most region of the water pool (Kang et al., 2002, 2004, 2005). Therefore, we investigated the sensitivity effect of grid models and the numerical models in the CFD calculations. The objectives of this study are to verify the condensation region model developed and also to develop the optimal CFD analysis methodology for the thermal mixing by comparing the CFD results with test data. 2. Thermal mixing experiment 2.1. Experimental facility The thermal mixing test was performed in the Blowdown and Condensation (B&C) facility, shown in Fig. 1, by changing the steam mass flux and the tank water temperature (Table 1) according to the quasi steady and transient states. In this study, only Table 1 Thermal mixing test conditions (Kim et al., 2005; Park et al., 2005; Kang et al., 2005) PZR pressure (bar) Steam mass flux (kg/m2 s) Water temperature in tank (◦ C) 150 250–1600 20–90 Fig. 1. Schematic diagram of the B&C test facility. a transient state test was considered. The B&C facility consists of a pressurizer, a steam discharge line, a subcooled water tank, a steam sparger, and a steam generator (Fig. 1). The pressurizer supplies a saturated steam at 150 bars into the subcooled water tank through the steam discharge line and the sparger. A modified prototypic steam sparger is installed at the center of the quenching water tank to simulate the IRWST of the APR1400. The sparger, made of a 6 in. schedule 40S pipe, has 64 side discharge holes with 1 cm in diameter (4 rows, 16 holes/row) and one bottom hole of a 2.5 cm diameter. The distance between the bottom of the sparger and the tank floor is set to be 0.9 m. The tank has the dimensions of 3 m in diameter and 4 m of the height. The measurement locations of the temperature and the pressure along the steam line are shown in Fig. 2. Eight thermocouples (Fig. 2(a) and (b)) are located around the sparger in the tank to measure the temperature of the steam and the entrained water flowing into the steam jet region, and two measurement rigs of 27 thermocouples (Fig. 2(a) and (c)) are installed to obtain the overall thermal mixing pattern. The second rig is installed to observe the extent of a thermal mixing along the circumferential direction in the tank. The uncertainties of each measurement are shown in Table 2, and the overall uncertainty of the test was 13.1% (Kang et al., 2006). 2.2. Experimental results The test result selected for the CFD benchmark calculation is a case of transient steam discharge for 60 s with the initial pressurizer pressure of 150 bar and the initial tank water temperature of about 26 ◦ C (Kim et al., 2005; Park et al., 2005; Kang et al., 2006). The variation of the pressure and temperature from the pressurizer to the sparger are shown in Fig. 3(a) and (b). The steam pressure (PT205) at the downstream of the control valve Table 2 Information on the measurement devices (Kim et al., 2005; Park et al., 2005; Kang et al., 2005) Measurement variable Number Uncertainty (%) Temperature Static pressure Differential pressure 67 7 1 ± 0.7 ± 1.6 ± 2.6 494 H.S. Kang, C.H. Song / Nuclear Engineering and Design 238 (2008) 492–501 Fig. 2. Locations of temperature measurement in the subcooled water tank. is abruptly decreased because the flow path in the control valve was narrow and complicated. The steam mass flux is also shown in Fig. 3(c). The discharged steam may condense at about 5–8 cm in the radial direction near the sparger discharge holes (Weimer et al., 1973; Kim, 2001). The temperature of the condensed water could be deduced from the temperature of TC717 and TC718 (Fig. 3(d)) even though the steam jet, based on the boundary layer theory, did not directly flow into those locations (White, 1991). The temperatures of TC716 and TC720 around the sparger (Fig. 3(e)) start to increase at about 17 s because the condensed water returns to the region near the sparger discharge holes after a collision with the quench tank wall. These temperature distributions could give useful information of the entrained water which could directly affect the condensation of steam jets (KEPCO, 2002; Ra, 1999; Su, 1981). From the temperature variation of TC705 and TC635 (Fig. 3(f)) which represents typically a comparison of the measured results between the TC-Rig 1 and the TC-Rig 2, we found that the thermal mixing in the tank shows an almost axi-symmetric pattern. 3. CFD analysis 3.1. Critical ﬂow and condensation region model In the thermal mixing test, the saturated steam at about 10 bar inside the sparger is initially discharged into the pool water at 26 ◦ C at 1 bar in the tank. A choking is likely to happen at the location of the sparger holes during this situation. The dis- charged steam flows into the pool water as a jet flow, and then it is quickly condensed to water in a short time and length by the DCC (Gamble et al., 2001; Kim, 2001; Weimer et al., 1973). The modeling of this condensation process for numerical analysis is so difficult that we use the concept of so-called the steam condensation region model in which the steam is perfectly condensed to water within the steam penetration length (Kang et al., 2002, 2004, 2005, 2006; Cook, 1994; Gamble et al., 2001). 20.57(Go /Gex )0.713 xc = (1) ro (ρ∞ /ρs )0.384 (hf − h∞ )0.801 /(hs − h∞ )0.801 Jet width = tan 13◦ x (2) The penetration length, Eq. (1), is defined as a function of the steam mass flow, a discharge hole diameter, and the temperature and pressure of the subcooled pool water (Kim, 2001; Weimer et al., 1973). The calculated penetration length of the steam jet discharged from the surface holes of 1 cm in diameter at the initial discharge condition is about 5.3 cm. The width of the jet at the end of the penetration length can be calculated as 1.2 cm from the Eq. (2) (White, 1991), but this is only an approximated value based on the boundary layer theory, especially for the region far from the source of the jet. This penetration length and width are used as the constant values in the transient CFD calculation even though those values may be changed because the effect of them may be negligible (Kang et al., 2002, 2004, 2005). Based on the above correlations and assumptions, the condensation region H.S. Kang, C.H. Song / Nuclear Engineering and Design 238 (2008) 492–501 495 Fig. 3. Experimental results of the high steam mass flux discharge condition. model without considering the complicated velocity profiles is established as in Fig. 4. It is assumed that the entrained water located at above and below this condensation region must flow into the condensation region along the direction normal to the surface of this region, and only the condensed water leaves the outlet of the condensation region uniformly with the same velocity and temperature even though the estimated velocity profile shows a variation along the sparger discharge holes. According to the CFD calculation by considering the various velocity profiles, there is no big difference in the analysis results of thermal mixing behaviors for the high steam mass flux discharge conditions (Kang et al., 2002, 2004, 2005). ṁs + ṁent = ṁcon (3) 2 Acon Ps As +P∞ (πDH − As ) + ρs Vs2 As = P∞ Acon + ρcon Vcon (4) ṁs hs + ṁent hent = ṁcon hcon Ps = Po 2 k+1 (5) k/(k−1) (6) The mass flow rate of the condensed water (mcon ) and the entrained water (ment ) at the boundary of the condensation region (Fig. 4) is calculated from the conservation laws of mass, momentum, and energy, Eqs. (3)–(5), over the condensation region (Kang et al., 2002, 2004, 2005). The mass flow rate of the 496 H.S. Kang, C.H. Song / Nuclear Engineering and Design 238 (2008) 492–501 Fig. 4. Steam condensation region model for the direct contact condensation (uniform velocity and temperature are assumed at the outlet of condensation region). steam measured in the experiments is used as the steam velocity (Vs ) through the discharge holes with an assumption of a steam quality of one for solving the equations. The velocity and the enthalpy of the condensed water are obtained by using an assumed density value at 1.22 bar (P∞ ), the hydro-static pressure at the submerged depth of the sparger and the water temperature in the tank. As for the first step, to solve Eq. (4), we must know the pressure (Ps ) of the steam leaving the discharging holes, which can be calculated by the isentropic relation of an ideal gas (Todreas and Kazimi, 1990; Wylen and Sonntag, 1985), expressed by the Eq. (6), with assuming that the choking occurs at the discharging holes. In these relations, the test data of PT207 is used for the static pressure (Po ). And the momentum flow of the entrained water in the vertical direction is cancelled out because we assumed that the entrained water flows only in the direction normal to the upper and lower boundaries of the condensation region. The static pressure on the sparger surface between the adjacent holes is also assumed to be 1.22 bar (P∞ ). The veloc- Fig. 6. Grid model for the CFD calculation (case-1). ity of the condensed water is obtained by substituting the above data into Eq. (4). And then, the mass flow rate of the entrained water is calculated by use of Eq. (3). The obtained mass flow rate (ment ) and the assumed enthalpy (hent ) based on the test results are substituted into Eq. (5) to get the enthalpy of the condensed water. The calculated value of the enthalpy of the condensed water is compared with the initial assumed value. If its difference is lower than 5%, the assumed enthalpy value of the condensed water and the entrained water are decided for boundary conditions of the CFD analysis as shown Fig. 5. With these values, CFX4.4 calculates the thermal mixing between the condensed water and the subcooled pool water in the tank by using an appropriate turbulent model and some other physical models. 3.2. Grid model and boundary conditions A multi-grid is generated with an axi-symmetric condition for simulating the sparger and the subcooled water tank for the CFD calculation (Fig. 6) since the flow pattern in the tank was observed to vary a little in the circumferential direction (Fig. 3) Fig. 5. Boundary conditions for the CFD analysis using the steam condensation region model. H.S. Kang, C.H. Song / Nuclear Engineering and Design 238 (2008) 492–501 Table 3 Grid and numerical model sensitivity calculation Case Cell no. (horizontal × vertical) Convection term discretization Case-1 Case-2 Case-3 Case-4 9,588 (63 × 160) 23,835 (103 × 263) 31,020 (113 × 273) 9,588 (63 × 160) Upwind 1st Upwind 1st Upwind 1st QUICK and additionally it could reduce the computational time. The grid model is generated by considering 27 thermocouple locations in the experiments to evaluate the calculation results easily. The meshes are more densely distributed near both the condensation region and the initial air/water interface region than the other regions to accommodate the high velocity and temperature gradients. The air region above the free surface of the pool water in the tank is modeled to extend to 0.5 m upwardly to move the fully developed condition imposed by applying the pressure outlet condition into the downstream of the flow field. The sensitivity calculations of the grid models and the numerical methods were performed (Table 3). Three different cases of the mesh distributions are used in the grid model by commonly applying the Upwind 1st method (AEA Tech., 2001; Versteeg and Malalasekera, 1995) for discretizing the convection term. For the case-1, a total of 9588 cells were generated, and the first grid from the right wall was located at the position of 100–300 of y+. For the case-2 for the sensitivity study, the mesh distribution is rearranged according to the results of comparison between the CFD data of the case-1 and the test data. A total of 23,835 cells and 12–50 of y+ were generated to predict the temperature close to the test data even though the computation time takes longer than that of the case-1. Additionally, more meshes are distributed around the jet flow and at the region near the wall. The case-3 of grid models has 31,020 cells and 12–50 of y+. The meshes in this case are more densely located at the transition region in the upper region of the free surface of the tank than those of the case-2. In the case-4, the same mesh distribution as in the case1 is used whereas the numerical model of the convection term discretization is changed to the QUICK scheme (AEA Tech., 2001; Versteeg and Malalasekera, 1995). The total cell number shown in Table 3 is not the same as the product of the horizontal cell numbers and vertical ones because the meshes in the region inside the sparger are not generated. The inlet boundary condition, the Dirichlet condition (AEA Tech., 2001), is set at the surface of the steam condensation region with time-dependent velocity and temperature profiles as shown in Fig. 5. The values of the turbulent properties at the inlet boundary are set as a high intensity (AEA Tech., 2001) because the eddy motions are actively generated around the condensation region due to a high speed of steam near the discharge holes. The pressure outlet boundary conditions, the Neumann condition (AEA Tech., 2001), are set for the free surface of the tank, which only allows for the outflow of air. The boundary regions for the entrained water are applied to the upper and lower sides of the steam condensation regions by a negative value of the velocity with the inlet condition in the CFX4.4. The symmetry 497 condition is applied to the center of the pipe line connected to the sparger. 3.3. Flow ﬁeld models and governing equations Thermal mixing phenomenon in the subcooled water tank is treated as an incompressible flow, a free surface flow of air at the upper region of the pool, a turbulent flow, and a buoyancy flow. Therefore, the governing equations used in this study are the Navier–Stokes and energy equations with a homogenous multi-fluid model (Eqs. (7)–(9)) (AEA Tech., 2001). The turbulent flow is modeled by a standard k– turbulent model (AEA Tech., 2001), and the buoyancy is modeled by the Boussinesq approximation (AEA Tech., 2001). In the homogenous model, the inter-phase mass and heat transfer are neglected. Each transport quantity in the governing equations except for the volume fraction is summed over all the phases to give a single transport quantity. The surface sharpening algorithm (AEA Tech., 2001) is also used to treat the numerical diffusion at the interface region effectively. The finite difference scheme for each transport equation is a Hybrid method except for the pressure and the volume fraction equation. The central and the Upwind difference scheme are used for the pressure and the volume fraction equations, respectively. The fully implicit Backward Euler differencing scheme are used for the transient calculation (AEA Tech., 2001). With these calculation methods, 60–100 iterations were performed with the time step of 0.001–0.05 s until the mass, enthalpy, and velocity residual for the water reach below the value of 1.0E−04 (Kang et al., 2002, 2004, 2005). ∂ (γα ρα ) + ∇ · (γα ρα Vα ) = 0 ∂t (7) ∂ (γα ρα Vα ) + ∇ · γa ρα Vα ⊗ Vα − μα ∇Vα + (∇Vα )T ∂t = γα (B − ∇Pα ) (8) ∂ (γα ρα hα ) + ∇ · γα (ρα Vα hα − λα ∇Tα ) = 0 ∂t ρ= Np α=1 (9) Np γα ρα , 1 V = γ α ρ α Vα ρ (10) α=1 3.4. Discussion on the CFD analysis results The velocity vector, temperature distribution, and the comparison of the test data with the CFX results at some locations are shown in Figs. 7–9. As for the sensitivity analysis, all the velocity profiles and thermal mixing patterns were similar to each other regardless of the analysis cases. Fig. 7(a) shows the whole velocity profile in the tank at 6 s and Fig. 7(b) shows the velocity profile, especially the circulation developed above and below the condensed water jet region, at 35 s. It is shown that the condensed water discharged from the condensation region model easily collides with the tank wall in a very short time because the velocity of the condensed water jet is so high to be about 6 m/s and the distance between the sparger 498 H.S. Kang, C.H. Song / Nuclear Engineering and Design 238 (2008) 492–501 Fig. 7. Velocity profiles of the CFD results (case-1). Experiment started at 5 s. and the tank side wall is small to be 1.5 m. After the collision, some of the condensed water moves upward to the free interface of the pool along the wall, and then changes its flow direction due to a gravity force. The rest of the downwardly flowing water after collision also moves along the wall and collides once again with the bottom wall, and then it returns to the region near the sparger. The secondary flow around the condensation region is developed due to the strong momentum flow of the condensed water and the entrained water. Fig. 8 shows the temperature distribution, which is being varied according to the flow pattern with time. The temperature around the main circulation flow path, which forms along the stream of the condensed water, is increased by 2–3 ◦ C from the initial water temperature because of a thermal mixing between Fig. 8. Temperature distribution of the CFD results (cases 1–4). Experiment started at 5 s. H.S. Kang, C.H. Song / Nuclear Engineering and Design 238 (2008) 492–501 499 Fig. 9. Comparison of experimental data with CFD results at thermo-couple locations (cases 1–4). All temperature normalized by the initial water temperature (Ti ). the condensed water and the pool water. From the figures, we can see that the temperature around the sparger increases gradually and it may have an adverse effect on a stable steam condensation. Especially, the temperature in the lower region, below the sparger head, is increased more quickly than that of the upper region. The variation of temperature distribution from 6.0 to 15.0 s shows a typical pattern of flow circulation in the tank, which reveals the fact that the condensed water discharged from the sparger flows upward mostly and downward in part, and then it turns towards the side region of the sparger head and then changes its direction into the sparger. Fig. 8 also shows that one of the flow streams in the upper region moves upward again with a 45◦ angle and reaches the top of the tank. In fact, this upward flow reveals only a virtual display in the CFD results, and this region is actually an air region above the free surface in the tank. This confusingly artificial region comes from a characteristic of the surface sharpening algorithm (AEA Tech., 2001) where all the governing equations except for each phase of the volume fraction are solved by using the average value of both phases. The results of comparing the cases 1–2 for the temperature contours shows that the thermal mixing process of the case-1 is developed faster than that of the case-2, and there are some differences in the temperature distributions around the jet flow at 6 s. The comparison of the cases 2–3 shows almost the same trends for the whole temperature distribution, but they shows locally a very small difference in temperature profile. This difference in temperature distribution, which depends on the number of mesh cells, is due to the use of the Upwind 1st scheme for the convection term. If the cell is not aligned to the flow field when using the Upwind scheme, the results of the flow field are dependent on the mesh distribution (Versteeg and Malalasekera, 1995). The case-4 uses the same grid model but the solving scheme of the QUICK scheme. The results of the case-4 show a thermal mixing pattern and the temperature distribution at 6 and 8 s, which are different from the case of the Upwind 1st scheme. These temperature results are regarded as unreasonable because the accuracy of the QUICK scheme may be deteriorated for a complicated flow field (Versteeg and Malalasekera, 1995). 500 H.S. Kang, C.H. Song / Nuclear Engineering and Design 238 (2008) 492–501 A comparison of the temperature measurements with the CFX analysis results for 30 s at 6 thermocouple locations is shown in Fig. 9. These locations were expected to represent the characteristic thermal mixing pattern in the tank. It is shown that the trend of the temperature variation were very similar between the test and the CFD results as a whole, but the CFD results are higher than those of the testing by 1–3 ◦ C. This can be explained by the fact that the condensation region model in the CFD analysis uses the concept of an area average, but the thermocouple measured the really local phenomena. The temperature distribution at the front of the jet flow (TC705), only in the upper region of the jet flow (TC706), the upper and lower region near the right wall (TC736, TC733), and the high upper region of the middle part (TC728, TC729) are shown as a function of the time. The comparison of temperature between the CFD results and the testing at TC705 shows that the trend of temperature variation for the four cases are almost similar, and all the CFD predictions are higher than those of the testing by 2–3 ◦ C. From the comparison for TC706, it is shown that the CFD results for the four cases predicts the test data reasonably well, but the results for the case-3 are closer to the test data than those of the other cases. In the case-3, the peak value at about 5 s and the trend of the temperature increase are very similar to the test data. From the comparison for TC736, also the CFD results for all the cases predicts the observed trend of temperature variation well, but the CFD results overestimates the peak value at about 6 s and also it could not simulate the temperature fluctuation phenomena. This may be due to the area and time averaged concept of the condensation region model or because the axi-symmetric condition was used so that the temperature of the condensed water in the circumferential direction is constant. Therefore, the CFD results could not simulate the complicated local thermal mixing inside the upward flow along the tank wall. The CFD results at TC733 for all the cases, however, predict the test data, including the peak value, well. From these results, we can see that the temperature distribution at the upper region may have locally three-dimensional effects. The comparison of the temperatures at TC728 and TC729 shows that the starting time of the temperature increase in the CFD results is faster than those of the test data. This means that the condensed water in the CFD analysis arrives at this region quicker than that of the test. And also, it depends on the numerical discretization method of the convection term. The results of the case-4 by using the QUICK scheme are closer to the test data. For all the cases, however, the CFD results had a tendency of a slight over-prediction when compared to the test data. This may be because CFX4.4 uses the Reynolds Analogy concept (Todreas and Kazimi, 1990) where this analogy may fail for an impinging jet flow with a large pressure drop (Bae and Sung, 2001). 4. Conclusion When the steam jet of a high pressure and temperature is condensed and mixed with a subcooled pool water in the tank, thermal mixing phenomenon is simulated with so-called the steam condensation region model for a transient case of 30 s with CFX4.4. The sensitivity analysis of grid and numerical models is also performed to find the optimized methodology for the thermal mixing analysis. The comparison of CFD results with the test data shows a good agreement within 7–8% value. This difference may arise from that the temperature and the velocity of the calculated condensed water by adopting the condensation region model are higher than the real value. Another reason may be due to an applicable limitation of condensation region model to adopt the area average concept. This concept also neglects a three-dimensional flow features in the tank, while the CFX calculation is performed by assuming the axi-symmetry to save a computation time. The sensitivity analysis of CFD calculation for the temperatures at the region between the sparger and the tank wall is very similar to each other regardless of the cases. The CFD results, however, shows a small difference in temperature distribution at the upper and lower region where the condensed water jet comes back after colliding with the tank wall. Especially for the high upper region, the case-4 using the QUICK scheme predicts the test data better than the cases using the Upwind scheme. Finally, the commercial CFD code like CFX4.4 together with the condensation region model proposed in this study can simulate the thermal mixing behavior reasonably well when a sufficient number of mesh distribution and a proper numerical method are adopted. Acknowledgements This work was financially supported for the Nuclear R&D Program from the Ministry of Science and Technology of Korea. The authors are sincerely grateful for the financial support. References AEA Technology, 2001. CFX-4.4 Manual. Bae, S.W., Sung, H.J., October 2001. Breakdown of the Reynolds Analogy in a stagnation region under inflow disturbances. Theo. Comp. Fluid Dyn. 14, 377–398. Cook, D.H., 1994. Pressure Suppression Pool Thermal Mixing. Oak Ridge National Laboratory, ORNL/TM-8906. Davis, J., Yadigaroglu, G., 2004. Direct contact condensation in Himenz flow boundary layers. Int. J. Heat Mass Transfer 47, 1863–1875. Gamble, R.E., Nguyen, T.T., Shiralkar, B.S., Peterson, P.F., Greif, R., Tabata, H., 2001. Pressure suppression pool mixing in passive advanced BWR plants. Nucl. Eng. Des. 204, 321–336. Kang, H.S., Bae, Y.Y., Park, J.K., 2002. Numerical study on the local temperature in IRWST pool. In: Proceedings of the International Conference on Nuclear Engineering (ICONE-10), Arlington, USA, April 14–18. Kang, H.S., Kim, Y.S., Chun, H.G., Yoon, Y.J., Song, C.H., 2004. CFD analysis for thermal mixing phenomena in the subcooled water tank. In: Proceedings of the 5th Korea–Japan Symposium on Nuclear Thermal Hydraulics and Safety (NTHAS-4), Sapporo, Japan, November 29–December 1. Kang, H.S., Kim, Y.S., Chun, H.G., Yoon, Y.J. Song, C.H., June 2005. A CFD Analysis of the Thermal Mixing under the Transient of the Steam Discharging in a Subcooled Water Tank. Technical Report, Korea Atomic Energy Research Institute, KAERI/TR-3008/2005 (in Korean). Kang, H.S., Kim, Y.S., Song, C.H., May 2006. Thermal Mixing Test Data Base Document. Korea Atomic Energy Research Institute, KAERI/THETA-TM1, Rev.0 (in Korean). KEPCO, 2002. APR1400 Standard Safety Analysis Report. Korea Electric Power Corporation. H.S. Kang, C.H. Song / Nuclear Engineering and Design 238 (2008) 492–501 Kim, H.Y., 2001. A study on the characteristics of direct contact condensation of a steam jet discharging into a quenching tank through a single horizontal pipe. Ph.D Thesis. Korea Advanced Institute of Science and Technology. Kim, Y.S., Chung, M.K., Park, J.W., Chun, M.H., 1997. An experimental investigation of direct condensation of steam jet in subcooled water. J. Korea Nucl. Soc. 29 (1), 45–57. Kim, Y.S., Song, C.H., Chun, H.G., Yoon, Y.J., Park, C.K. Kang, H.S., March 2005. Steam Condensation Induced Thermal Mixing Experimental Using B&C facility. Technical Report, Korea Atomic Energy Research Institute, KAERI/TR-2933/2005. Park, C.K., Song, C.H., Chun, H.G., Yoon, Y.J. Kim, Y.S., March 2005. Steam Condensation Test Program and Analysis of Hydraulic Loads. Technical Report, Korea Atomic Energy Research Institute, KAERI/TR2946/2005. Ra, I.S., February 1999. IRWST Thermal Hydraulic Load Analysis Report. Korea Power Engineering Company, N-001-END461-201. 501 Song, C.H., Baek, W.P., Chung, M.K., Park, J.K., 2003. Multi-dimensional thermal-hydraulic phenomena in advanced nuclear reactor systems: current status and perspectives of the R&D program at KAERI. In: Proceedings of the International Conference on Nuclear Reactor Thermal Hydraulics (NURETH-10), Seoul, Korea, October 5–9 (Paper I00121). Su, T.M., November 1981. Suppression Pool Temperature Limits for BWR Containments. United States Nuclear Regulatory Commission, NUREG-0783. Todreas, N.E., Kazimi, M.S., 1990. Nuclear System I. Hemisphere Publishing Corporation, New York. Versteeg, H.K., Malalasekera, W., 1995. An Inriduction to Computational Fluid Dynamics: The Finite Volume Method. Longman. Weimer, J.C., Faeth, G.M., Olson, D.R., 1973. Penetration of vapor jets submerged in subcooled liquids. AIChE J. 19 (3), 552–558. White, F.M., 1991. Viscous Fluid Flow, 2nd ed. Mcgraw-Hill, New York. Wylen, G.J.V., Sonntag, R.E., 1985. Fundamentals of Classical Thermodynamics, 3rd ed. John Wiley & Sons, New York.