Two computational fluid dynamic (CFD) benchmarks have been performed to assess the prediction accuracy and sensitivity of CFD codes for heat transfer in different geometries. The first benchmark focused on heat transfer to water in a tube (first benchmark), while the second benchmark covered heat transfer to water in two different channel geometries (second benchmark) at supercritical pressures. In the first round with the experimental data unknown to the participants (i.e., blind calculations), CFD calculations were conducted with initial boundary conditions and simpler CFD models. After assessment against measurements, the calculations were repeated with the refined boundary conditions and material properties in the follow-up calculation phase. Overall, the CFD codes seem to be able to capture the general trend of heat transfer in the tube and the annular channel but further improvements are required in order to enhance the prediction accuracy. Finally, sensitivity analyses on the numerical mesh and the boundary conditions were performed. It was found that the prediction accuracy has not been improved with the introduction of finer meshes and the effect of mass flux on the result is the strongest among various investigated boundary conditions.
Heat transfer to water at supercritical pressures is complex even in the simplest geometries, such as a straight vertically installed smooth bore tube ([1–4]). This is attributed to three different heat transfer regimes that can be encountered: the normal heat transfer (NHT), enhanced heat transfer (EHT), deteriorated heat transfer (DHT) regimes. Among these regimes, the deteriorated heat transfer regime is of the most concern because the heated solid surface could exceed its temperature limit (it is maximum 620 °C for the most advanced nuclear grade materials, for, e.g., Inconel alloy). The most of the heat-transfer correlations have been developed for normal and enhanced heat transfer regimes ([1,4]) while properly estimating the results for heat-transfer deterioration cases remains impossible. The advanced computational fluid dynamics (CFD) models have been applied in support of the understanding of the deteriorated heat transfer phenomena ([3,5]). At this point, the accurate calculation of this phenomenon remains challenging and there is no consensus on the choice of models to be used for modeling ([3,4]).
As the temperature and pressure of the supercritical water (SCW) increases, its thermophysical properties (such as density, dynamic viscosity, isobar specific heat, and thermal conductivity) change nonlinearly and drastically over the pseudocritical point [6,7]. This causes significant changes in the flow pattern, wall temperature, and turbulent fields. Under distinct conditions ([1,8]), the heat transfer deteriorates and undesirably high wall temperatures (hot spots) could occur on the heated wall of structural materials. Therefore, the accurate simulation capability of supercritical water is essential for the detailed design of supercritical-water-cooled reactors (SCWRs) ([1–4]).
The previously mentioned heat-transfer (Nu–Nusselt number) correlations have been applied in predicting cladding temperatures in fuel design and safety analysis of SCWRs. These correlations were developed from experimental results of local wall and bulk temperature measurements ([9–11]). The formulations of these correlations are relatively simple and hence can be easily implemented into analytical tools (such as subchannel and system codes). However, these correlations have been developed for specific channel geometries (mainly circular tubes) over a limited range of conditions and are limited to normal and enhanced heat transfer regimes only. In case of such correlations, the extrapolation is not recommended as these correlations mimic the experimental data but do not cover the complex heat transfer mechanism of supercritical water (). A more fundamental approach is needed to understand the phenomena and extend the prediction capability beyond the current experimental database in support of the SCWR development.
In this study, a more fundamental approach in predicting heat transfer at supercritical pressure is applied using the Reynolds-averaged Navier–Stokes (RANS) approach of the CFD tools. CFD simulations adopt different turbulence models, built in tables of material properties and other models to simulate the thermal hydraulics of supercritical water ([3–5,12,13]). The development process for a turbulence model is time-consuming and requires validation against experimental results. Existing turbulence models are general in nature and not specifically developed for supercritical water. Their applicability for heat transfer to supercritical water must be investigated.
A benchmarking exercise has been initiated in the framework of the coordinated research project (CRP) “Understanding and prediction of thermal-hydraulics phenomena relevant to super-critical water-cooled reactors (SCWRs)” of the international atomic energy agency. It aimed to assess CFD models and methods through comparisons of results of independently performed CFD calculations against experimental heat transfer results obtained in a tube and two different annular channels. The experimental results, which were not released to the participants of the benchmark until at the end of the “blind” stage, consisted of wall temperatures at different axial positions on the heated wall of the tube or the annular channels. After the “blind” stage, a follow-up calculation stage has been performed containing two different parts: repeated CFD calculations with improved boundary conditions and sensitivity analyses of the mesh resolution and global boundary conditions in order to quantify their effect on CFD results.
The objectives of this paper are to provide an overview about the investigated geometries, the used boundary conditions, suggested CFD settings, etc., of the two benchmarks, present the comparisons between the CFD predictions and experimental results, and describe the outcome of the sensitivity analyses. The two benchmark specifications are introduced with some details of the experimental facilities, and boundary conditions of the investigated cases. Models and numerical approaches used by the participants are presented together with their results for the blind benchmarks. Some participants (Budapest University of Technology and Economics (BME) and Karlsruhe Institute of Technology (KIT)) repeated the calculations after the results were released. Their results of the follow-up calculations are also presented. A detailed sensitivity analysis on the mesh and boundary conditions was performed. Its findings are described afterward.
The Specifications of Blind Benchmarks
The first benchmark specification was based on the experiment with an upward flow of water at supercritical pressures in a vertical tube performed at the CIAE (). Two cases were analyzed in the framework of this first benchmark.
The experiments with an upward flow of water at supercritical pressures in two different annular channels performed at University of Wisconsin–Madison (UW), Madison, WI provided the measured results ([15,16]) to the second benchmark. These channels consisted of a central heated tube with inside wall temperature measurements at 14 positions. One of these channels had a circular shroud while the other had a square shroud. Four cases (two for each channel) were analyzed in the framework of this second benchmark.
BME organized the two benchmarks with major help from the originators of the experimental data. The tasks of the organizer covered the following fields: preparation of the two benchmark specifications in order to make the boundary conditions applied at different participants as uniform as possible, compilation and release of the CFD results data sheet, collection of the results from participants, and analyzation-comparison of the collected results with each other and with experimental data.
The Blind Benchmark Specification of CIAE.
Five CRP partners (GIDROPRESS, BME, Bhabha Atomic Research Center (BARC), KIT, University of Pisa (UPisa)) participated in the first CFD benchmark ,which was against the tube heat transfer data provided by CIAE. This benchmark was intended to improve the understanding of the participants on the CFD modeling of SCW flow in simple tube geometries. An experiment was performed with upward SCW flow inside a straight, smooth bore, vertically installed tube (see Fig. 1). The geometrical parameters are as follows: the inner (Di) and outer (Do) diameters are 7.98 and 9.6 mm, respectively, and the heated length (Lh) is 2.85 m. The outer wall temperatures were measured at nine positions: 0.4, 0.7, 1.0, 1.3, 1.6, 1.9, 2.2, 2.5, and 2.75 m from the beginning of the heated length (see Fig. 1). A direct current power supply was connected to the test section, as shown in the Fig. 1. The tube was made from INCONEL alloy 625. The thermal hydraulic parameters of the two experimental cases provided by CIAE are listed in Table 1. The outer surface of the tube was assumed to be adiabatic due to sufficient thermal insulation applied at the experiment.
The Blind Benchmark Specification of UW.
Two similar geometries have been investigated in the second benchmark. Here, four CRP partners (namely BME, BARC, Canadian Nuclear Laboratories (CNL), UPisa) participated. This benchmark was against the heat transfer data of two different shaped annular channels. The UW experiments were performed in a SCW test loop ([15,16]).
the outer diameter of the heater rod is 10.7 mm;
the inner and outer diameters of the outer piping are 42.9 and 60.33 mm, respectively;
the heated length is 1.01 m;
the entrance and discharge lengths upstream and downstream of the test section are 760 mm;
the square annular test section geometry is a 10.7 mm diameter heater rod within a 28.8 mm wide flow channel (see Fig. 2(b)).
Two test cases have been selected for each of the circular and the square test section. Thermal hydraulic parameters of these two experimental cases for the circular and square test sections are listed in Tables 3 and 4, respectively ([15,16]). Only case B can be classified as DHT case, the rest are normal or enhanced heat transfer cases. Cases A and C are forced while cases B and D are mixed convection cases.
This section describes numerical approaches applied by the participants in their RANS CFD analysis for the benchmarks. Each participant independently selected the code (commercial or in-house), the configuration of modeling domains and their dimensions, the turbulence models, the mesh configuration and its density, the inclusion (or not) of conjugated heat transfer (CHT), and the method (database) for the water properties. Table 5 summarizes selected numerical approaches of participants.
Only one participant (BARC) used in-house CFD code, which is called as “NAFA.” The other five institutions applied commercial multipurpose CFD packages (star-ccm+ or ANSYS cfx). All participants performed RANS simulations.
All participants have been implemented two equations turbulence models into their CFD models (one exception: CNL used Reynolds stress model for case C). Most of them used built-in models like: standard k–ε, RSM linear pressure strain two-layer, Lien k–ε Low Re or shear stress transport (SST/SST k-ω) model. One participant, UPisa implemented special turbulence model with some self-tuning: algebraic heat flux model for turbulent heat fluxes calculation for cases 1 and 2.
As it is well known, the boundary layer has to be fully resolved in case of heat transfer in SCW ([3,5,13]). That is the reason for the “near wall modeling” indicated in Table 5 among the most important circumstances of CFD modeling and settings. BARC and KIT used (standard) wall function. It is widely known that using (standard) wall functions is rather a bed choice due to wall functions have been derived assuming constant material properties of the fluid. This assumption is invalid for heat transfer of SCW ([1,4,5]).
The participants applied different sizes of numerical grids and modeled different extent of the experimental geometries (Table 5).
Half of the participants (BME, CNL, and GIDROPRESS) modeled the cases considering CHT while the other half developed CFD models without heat conducting solid domain (Table 5).
The material properties of water were modeled by widely used and compared () international formulations like National Institute of Standards and Technology (NIST), IAPWS-95, IAPWS-IF97, or REFRPROP 7.0.
The Results of the Blind Calculations, Comparisons
The distributions of axial wall temperature and radial velocity were compared between the experimental and CFD results for both benchmarks.
Comparisons for the First Benchmark.
Figure 3 shows the comparison between the measured and calculated results for case 1. As it can be seen, the measured values increase monotonically along the axial height. Two of the submitted CFD results (from BARC and KIT) show good qualitative and quantitative agreement with the experimental distribution. The remaining three (from BME, GIDROPRESS, and UPisa) predicted heat transfer deterioration (it was forecasted by the qw/G ratio) at the end of the heated length after the calculated wall temperature exceeded the pseudocritical temperature. It is worth to note that UPisa reported three deteriorations in its CFD results, which appeared within two wall temperature measurement points while the CFD results of BME and GIDROPRESS show only a single deterioration at the position of the eighth thermocouple. It is theoretically possible that between two thermocouples (note that the distance between two thermocouples is 300 mm) deterioration (wall temperature peak) occurred while the two nearest thermocouples measure normal wall temperature value.
Figure 4 shows the comparison between the measured and calculated results for case 2 of CIAE. The measured distribution of wall temperature increases monotonically along the heated length as well as at case 1. The majority of the CFD analyses show a deviation from the measured wall temperature after the sixth measured wall temperature value (∼1.9 m). It is worth to mention that the calculated wall temperatures exceed here the pseudocritical value just like at case 1. The results of BME, GIDROPRESS, and UPisa overestimate the subsequent three wall temperature vales after the sixth thermocouple while the results from BARC and KIT underestimate them with a monotonically increasing trend (see Fig. 4). There is an important difference between the two groups of CFD results: the CFD model of BARC and KIT consists of the k–ε turbulence model and wall function while the others use low Re SST or special k–ε turbulence model (UPisa) with enhanced wall treatment. It was reported in past analyses ([3–5]) that the standard k–ε turbulence model cannot predict the DHT, but the SST model with enhanced near wall treatment at most of the cases can do that.
Comparisons for the Second Benchmark.
Figure 5 shows the comparison between measured and calculated distributions of wall temperature for case A. Best prediction has been given by the model of CNL in qualitative and quantitative terms. The results of BARC and BME are good in qualitative terms although under- and overestimate the measured distribution. The CFD result of UPisa seriously overpredicted the measured distribution with a DHT like wall temperature trend.
Figure 6 illustrates the results for case B of UW. The measured distribution consists of a small peak around the third measurement position of wall temperature. The CFD result of BARC gives back the measured distribution best. The results of CNL and UPisa show deterioration effect along the first one-third of the heated length, which is in disagreement with the experimental result. The result of BME shows good match in qualitative terms but underestimates the measured wall temperatures.
The wall temperature of case C is not discussed here because case C is an isothermal case and the distribution of wall temperature remains unchanged. The radial velocity field was compared instead (see Fig. 7) at the middle of the heated section (0.5 m downstream to the beginning of heating). As it can be seen that the distributions calculated by BME and UPisa agree well with the experimental data, the peak velocity value (∼0.4 m/s) and its radial position (∼3.6 mm) have been well predicted (see Fig. 7). The CFD results of CNL significantly differ from the measured velocity distribution: its peak value is at 7 mm instead of 3.6 mm, the shape of the whole calculated distribution is different, only the peak value (0.413 m/s) agrees approximately well.
Figure 8 shows the comparison between measured data and CFD results for case D of UW. Based on the shape of the measured wall temperature distribution and the boundary conditions (Table 4), this case can be determined as normal or enhanced heat transfer case. The result of UPisa predicts best qualitatively the measured distribution even if there are some discrepancies in the quantitative terms. The CFD predictions of BME and CNL underestimated the measured wall temperatures.
The measured velocity distribution can be seen in Fig. 9. All the three CFD results show good agreement with the experimental data, especially the prediction of UPisa.
The Follow-Up Calculations
After the blind phase of the benchmarks, some discrepancies turned out regarding the boundary conditions specified in the specification of the benchmarks and some details of the CFD modeling. That is the reason why a follow-up calculation phase has been conducted.
In case of the first benchmark, if any the solid domain was modeled, its material was set as stainless steel instead of INCONEL alloy 625 (as it was in the reality). That was the reason the temperature-dependent material properties of the INCONEL alloy 625 () have been specified to the partners in order to model the tube material in their follow-up CFD calculations.
At the second benchmark, it turned out that besides the issue regarding the modeling of solid domain, the boundary conditions were not specified accurately enough. Tables 6 and 7 show the slightly modified (the differences between boundary conditions of blind and follow-up phases are indicated in brackets) boundary conditions set for the follow-up calculations. The material of the heater rod, outer piping, and the square flow guide (see Fig. 2) is INCONEL alloy 625 as well as at the first benchmark.
Results of the Follow-Up Calculations and Mesh
A MSS has been performed together with the follow-up calculations. Thus, the results of the follow-up calculations and the MSS were presented together in this chapter.
Results for Cases 1 and 2 of CIAE.
Figure 10(a) shows the comparison between the blind and the follow-up CFD results of BME and KIT for case 1 of CIAE. As it can be seen practically, there is no difference between the blind and follow-up CFD results. It means that the modeling the INCONEL alloy 625 instead of Stainless steel makes no difference in the heat transfer of SCW.
Two additional numerical grids (a coarser (F1) and a finer (F4)) have been created for the geometry of the first benchmark. The number of elements has been decreased by 50% at F1 (1.247 M) compared to the original grid, F2 (2.6 M). The F4 mesh has 5.628 M elements, so twice as many as F2 have. The mesh sensitivity study was performed for case 1 (see Fig. 10(b)). As it can be seen in Fig. 10(b), there is no significant difference between the CFD results of the three meshes. A small discrepancy can be seen only at the position of the temperature peak (see Fig. 10(b)).
Figure 11 shows further details about the results of the MSS for case 1. Four of the selected target variables () can be seen in Fig. 11 : the maximum and average wall temperatures over the whole heated wall, the total pressure drop and the average velocity over the total fluid domain. All of these comparisons show that the size of the grid influences only marginally the target variables in the investigated mesh size range. The difference between the values of F4-F2 is generally smaller than the difference between the values of F2-F1. The F2 mesh represents a good compromise between the viewpoint of resolution and numerical cost.
Figure 12 depicts the comparison between the CFD results of the blind and the follow-up calculations performed by BME for case 2. As it can be seen, there is no difference between the results of the two CFD calculations, which led to identical conclusion than in case of case 1: modeling the INCONEL alloy 625 instead of Stainless steel does not change the CFD results for the heat transfer of SCW.
Results for Cases A and B of UW.
Figure 13(a) shows the comparison between the CFD results of the blind and follow-up calculations for case A. As it can be seen, the wall temperature values obtained with the modified boundary conditions are closer to the measured values than the result of blind calculation.
Figure 13(b) depicts the results of the mesh sensitivity study for case B. It can be seen that the wall temperature values of the blind calculation fall closer to the measured values than the predictions of the follow-up calculations. It must be noted that all of the three distributions of MSS (F1–1.66 M, F2–3.522 M and F4–7.454 M elements) overlap each other (see Fig. 13(b)).
Results for Case C and D of UW.
Figures 7 and 9 show the radial velocity distributions for the follow-up and the blind calculations of cases C and D. Based on the comparison between the blind and follow-up CFD results of BME, it can be concluded that the blind SST result falls closer to the experimental data than the follow-up SST result for both cases C and D. The application of baseline Reynolds Stress turbulence model (baseline-RSM) improves the CFD prediction (see Figs. 7 and 9).
Figure 14 depicts the comparison between the blind and the follow-up calculations, and the MSS for case D. As it can be seen, the wall temperature values of the follow-up calculations fall closer to the measured values, but neither the blind calculation nor the follow-up calculations predicted qualitatively acceptable the distribution of the measured values.
The Sensitivity Analysis and Their Results
It is widely accepted that the local thermal hydraulic fields strongly depend on the global boundary conditions in supercritical water ([1,3,13,19]). In order to investigate this phenomenon, a detailed BCSS has been performed after the MSS. The sensitivity of the CFD result has been investigated regarding the MFR, the reference pressure, the heat flux, the inlet bulk fluid temperature, and the inlet turbulence intensity.
Sensitivity Analysis on the Mass Flow Rate.
Figure 15 depicts the sensitivity of CFD results of BME on the MFR. MFR has been found to be the only global boundary condition which influences not only the values but the shape of wall temperature distribution as well (Fig. 15(a)): the CFD results with 80% MFR coincide almost perfectly with the experimental data. The lower the MFR, the higher is the wall temperature (see Fig. 15(a)). If MFR increases the maximum and average wall temperature decreases as the heat transfer strengthening (Figs. 15(b) and 15(c)). That is also obvious that the average velocity over the computational domain increases linearly with increasing MFR (Fig. 15(e)). Furthermore, if the velocity increases over the whole computational domain by the increasing MFR, then the pressure drop due to strengthening friction intensifies and thus the total pressure drop consequently increases proportional to the square of the velocity as well (Fig. 15(d)).
Sensitivity Analysis on the Reference Pressure.
Figure 16 shows the sensitivity of CFD results on the set reference pressure (pref). pref does not influence the distribution of wall temperature (Fig. 16(a)), but slightly increases the maximum and average wall temperatures (Figs. 16(b) and 16(c)) as well as the pressure drop (Fig. 16(d)). The average velocity slightly decreases as the reference pressure increases (Fig. 16(e)).
Sensitivity Analysis on the Heat Flux.
The heat flux is among the three boundary conditions (besides the MFR and inlet temperature of SCW), which are expected to have significant influence on the heat transfer in case of the investigated cases. Figure 17 depicts the sensitivity of CFD results of BME on the specified heat flux. The whole distribution of wall temperature increases as the heat flux becomes higher and higher (+10% each step, see Fig. 17(a)), but its shape did not get closer to the measured one: remains monotonically increasing instead. Obviously, the maximum and average wall temperatures get higher and higher values (Figs. 17(b) and 17(c)) as the heat flux increases. The pressure drop shows opposite trend (see Fig. 17(d)) than the wall temperature. The average velocity of the whole fluid domain increases as well with the increasing heat flux (Fig. 17(e)) due to the flow acceleration effect which is well known ().
Sensitivity Analysis on the Inlet Temperature.
This is the third boundary condition, which is expected to have a significant influence on the heat transfer in the examined cases. Figure 18 shows the result of the performed sensitivity analyses on the value of set inlet temperature of SCW. The overall pattern is identical to that what was presented at the sensitivity analyses of heat flux: the higher the inlet temperature, the higher the whole distribution of wall temperature, maximum and average wall temperature (see Figs. 18(a)–18(c)). The average velocity in the whole computational domain slightly increases (Fig. 18(e)) while the total pressure drop moderately decreases due to the effect of the decreasing (strongly temperature dependent) dynamic viscosity (Fig. 18(d)).
Sensitivity Analysis on the Inlet Turbulence Intensity.
The possible effect of the spacer device upstream to the inlet of the test section ([15,16]) was tested by the sensitivity analysis on the inlet turbulence intensity. Figure 19 depicts the sensitivity of CFD results on the specified inlet turbulence intensity. As it can be seen, the whole distribution of wall temperature (Fig. 19(a)), its maximum and average values (Figs. 19(b) and 19(c), just like the pressure drop (Fig. 19(d)), and average velocity (Fig. 19(e)) are independent (at least in the investigated range) of the turbulence intensity. This observation indicates that the spacer device upstream to the inlet very likely does not have significant effect on the thermal hydraulics occurring in the downstream direction in the test section.
Turbulence Model Sensitivity Analysis.
The effect of the applied turbulence model on the CFD result has been investigated by BME in the framework of a detailed turbulence model sensitivity study (TMSS). Figure 20 shows the results of TMSS for case 1, which was performed in the follow-up calculation phase. As it can be seen, the models of k–ε family (k–ε, k–ε explicit algebraic Reynolds stress model, renormalization group k–ε) give significantly different distributions of wall temperature compared to the k–ω type models (BSL, BSL explicit algebraic Reynolds stress model, k–ω, SST). While the k–ω type models predict deterioration of heat transfer at the end of the heated section (directly after the height where the wall temperature exceeds the pseudocritical value, see Fig. 20), the k–ε type models do not. The k–ε type models seem to be not capable to predict heat transfer deterioration while the low Re k–ω type models can predict DHT. So, obviously, the applied turbulence model strongly influences the CFD results as it was reported by previous studies ([1,3,4,12,13,19]).
Two CFD benchmark exercises have been performed in the framework of a coordinated research project of the International Atomic Energy Agency. Heat transfer characteristics in one straight tube and two different annular channels were investigated. Two deteriorated heat transfer cases were examined in the tube and four different heat transfer cases for the annular channel geometries. The blind phase has ended with varying degrees of agreement between calculated and measured values. The calculated CFD results (axial distribution of wall temperature) fall very close to the measured values for case 1 (first case for tube geometry). Significant discrepancies were found only at the end of the heated section. Modeling the conjugate heat transfer did not improve the results in this case. The same can be stated for case 2 as well (second case for tube geometry). Good agreement has been reached for case A (normal heat transfer in circular annulus channel geometry), which was further improved in the follow-up phase by using improved boundary conditions. Acceptable agreements have been shown for case B (deteriorated heat transfer in the circular annular channel geometry). The comparison of calculated and measured radial velocity profiles of case C (isothermal case in square annular channel geometry) and D (normal heat transfer in square annular channel geometry) has been conducted with relatively good agreement. In the last investigated case, case D, moderate agreement has been reached for the axial distribution of wall temperature, which was improved in the follow-up phase by the application of the improved boundary conditions.
The performed mesh sensitivity studies showed that in the investigated range of numerical grid size, the CFD results do not depend strongly on the grid size. The CFD calculations with finer grid do not give significantly better results but require notably higher computational cost.
The conducted sensitivity analysis covered the effect of mass flow rate, reference pressure, heat flux, inlet temperature, and turbulent intensity (as global boundary conditions) on the CFD result. The mass flow rate was found as the only parameter that influences the shape of wall temperature distribution in the right way (improves the agreement of calculated and measured distributions). The variation in the other four examined global boundary conditions only increases or decreases the values of the whole distribution of wall temperature or shifts it in the axial direction. The inlet turbulent intensity was found to have little influence on the selected target variables (e.g., axial distribution of wall temperature) at least in the investigated range of it (from 0 to 10%).
The effect of the used turbulence model on the CFD result has been investigated by a detailed turbulence model sensitivity study. The three investigated k–ε type models seem to be not capable to predict deterioration of heat transfer while the low Re k–ω type models can predict deterioration. Thus, it is obvious that the applied turbulence model strongly influences the CFD results in case of supercritical water heat transfer.
Based on the sensitivity analyses, it can be concluded that the documentation of a CFD-grade experiment for the thermal hydraulics of supercritical water has to be conducted with great care and very accurate measurement of parameters because a small difference in the values of global boundary conditions (e.g., mass flow rate, reference or system pressure, heat flux, inlet temperature of water) could cause significant discrepancies between calculated and measured values during a code validation exercise. In other words, it has been demonstrated that the wall temperature and heat transfer coefficient distributions are very sensitive for small change of global boundary conditions such as the inlet temperature, heat flux, mass flux, and nominal pressure.
This collaborative work was performed in the framework of the CRP on “Understanding and Prediction of Thermal-Hydraulics Phenomena Relevant to Supercritical Water Cooled Reactors (SCWRs).”
The authors express their gratitude to the International Atomic Energy Agency for providing a platform for the collaboration and to all other participants in the CRP for their valuable discussion.
The authors also acknowledge the OECD Nuclear Energy Agency (NEA) for their cooperation in hosting the database to collect and share experimental and analytical data for the CRP.
The Hungarian contribution of this work has been performed in the framework of the National Nuclear Research Program (Grant No. VKSZ_14-1-2015-0021) supported by the National Research, Development and Innovation Office of Hungary. The program was financed from the NRDI Fund.
- 2D =
- 3D =
- ANSYS CFX =
commercial CFD code developed by ANSYS Inc.
- BARC =
Bhabha Atomic Research Center
- BCSS =
boundary condition sensitivity study
- BME =
Budapest University of Technology and Economics
- BoHL =
beginning of heated length
- Baseline-RSM =
baseline Reynolds stress (turbulence) Model
- CFD =
computational fluid dynamics
- CHT =
conjugate heat transfer
- CIAE =
China Institute of Atomic Energy
- CNL =
Canadian Nuclear Laboratories
- CRP =
coordinated research project
- DHT =
deteriorated heat transfer or deterioration of heat transfer
- EHT =
enhanced heat transfer
- F1/F2/F4 =
factor-1/factor-2/factor-4, the number indicates the size of the numerical grid
- GIDROPRESS =
- IAPWS-95 =
formulation of material properties created in 1995 by the International Association for the Properties of Water and Steam
- IAPWS-IF97 =
industrial formulation of material properties created in 1997 by the International Association for the Properties of Water and Steam
- k–ε =
notation of k–ε turbulence model
- k–ω =
notation of k–ω turbulence model
- KIT =
Karlsruhe Institute of Technology
- M =
- MFR =
mass flow rate
- MSS =
mesh sensitivity study
- NAFA =
numerical analysis of flows in axisymmetric geometries (name of in-house CFD code developed by BARC)
- NEA =
short name of OECD Nuclear Energy Agency
- NHT =
normal heat transfer
- NIST =
National Institute of Standards and Technology
- RANS =
Reynolds averaged Navier–Stokes method
- REFRPROP =
NIST reference fluid thermodynamic and transport properties database
- SCW =
- SCWR =
- SST =
notation of shear stress transport turbulence model
- star-ccm+ =
commercial CFD code developed by SIEMENS Gmbh.
- TC =
- TMSS =
turbulence model sensitivity study
- UPisa =
University of Pisa
- UW =
University of Wisconsin-Madison