Analysis of the Multiphase Flow With Condensation in the Two-Phase Ejector Condenser Using Computational Fluid Dynamics Modeling

Ejectors are devices where the high-pressure stream of the motive medium is used for withdrawing the secondary fluid. Ejectors are also known as injectors, jet pumps, or educators [1]. They are usually used as environmentally and economically friendly devices because they increase system efficiency, e.g., utilizing the waste heat [2,3]. A typical design consists of a motive nozzle, suction and mixing chambers, and a diffuser. The construction of ejectors has been developed at least from the beginning of the twentieth century [4], but dynamic development can be observed in the last decade. This is due to strengths of the ejectors: simplicity of construction (no moving parts), operational reliability, low capital, and operational costs. Ejectors can also operate with aggressive environmental conditions and not require intensive maintenance [5].

Ejectors are applied in many industrial and laboratory facilities. They are taking the role of pumps in the plumbing installation [6,7], where they also allow to protect pumps against cavitation. In ventilation systems, ejectors suck in toxic gases [8,9]. They are taking the role of mixers, condensers, and compressors in heating and power systems [10,11]. Dynamic growth of ejector development can be observed in the refrigeration system, where they compress the working medium, replacing standard compressors [12–14]. The ejectors can also be used as an expansion device in the refrigeration cycle to decrease compressing work and increase the evaporation performance [15]. To increase energy efficiency, combined power and ejector-based cooling systems are developed [16,17]. Some of these cycles are based on solar energy as a heat input, decreasing fossil fuel consumption [18].

There are many ways of ejector division. Considering the phenomenon’s phase conditions and complexity, we can distinguish between one-phase ejectors and two-phase ejectors without or with phase change [19,20]. Two-phase ejectors can be divided into gas-liquid, liquid-gas, liquid-solid, and gas-solid. Classification of ejectors can be connected with the cycle role, e.g., jet pumps, jet compressors, or jet ventilators. Ejectors can be distinguished due to the velocity of the flow: supersonic ejectors and subsonic ejectors. In the first one, a velocity higher than the speed of sound occurs (Mach Number greater than 1). Supersonic and subsonic ejectors differ mainly in the construction of the motive nozzle. The motive nozzle of the subsonic ejector is converging, whereas the motive nozzle of the supersonic ejector is converging-diverging (de Laval Nozzle). This paper presents the results of computational fluid dynamics (CFD) calculations of water-driven, subsonic, liquid-gas ejector.

Two-phase ejector or two-phase ejector condensers operation analysis is challenging because of the high complexity of the phenomenon [21,22]. Multiphase, turbulent flow often combined with phase change process is difficult for theoretical describing. Generally, in the two-phase ejector operation analysis, the modeling approaches possible for application can be divided into thermodynamic 0D models, 1D models, and multidimensional models [23]. 0D calculations are based on the thermodynamic and mechanical equilibrium assumptions at chosen parts of the ejector. Thermodynamic models are used successfully for the evaluation of the ejector operation [12,24,25] because of their robustness and sufficient accuracy. They are mainly based on one of the two mixing assumptions: constant area or constant pressure passage. However, these simplified models don’t fully reflect the complexity of the physics of the process, especially non-equilibrium effects. 1D and 2D/3D CFD models overcome the limitations of the 0D models. They allow for the investigation of local features of the flows, a wide range of geometry variants, and boundary conditions; therefore, the CFD approach is an efficient tool for geometry optimization [26].

Recently, the vast majority of ejector computational analysis concerns the numerical investigation of gas-driven, two-phase supersonic ejectors for use in refrigeration and air condition systems [11,13,19,23,27,28]. In such devices, spontaneous condensation often occurs due to the rapid expansion of steam. In the case of a liquid-driven, two-phase ejector, water-air is most often an object of numerical investigations [29–32]. There are several papers on the numerical analysis of water-steam ejectors [33] but there is still space for a deeper understanding of the complex phenomenon that occurs during two-phase ejector condenser operation.

The object of the numerical research is a water-driven, two-phase ejector which is one of the critical components in a developed gas power plant with negative CO₂ emission [34]. The main task of the presented ejector is to suck in and condense steam contained in the exhaust gas, which is the main product of the oxy-combustion process [35]. Preparation of accurate operating conditions to ensure high performance of the power plant cycle requires many experimental and numerical activities. One of the novelty is the values of flowrates, pressure, and temperature of fluids inside the spray-ejector condenser (high CO₂ content in gas mass flowrate which reduces the condensation rate, high mass flowrate of motive water, high-temperature differences between cooling water and hot gases (steam + CO₂)). Simulation of the spray-ejector operation required the development of a novel and original CFD model to capture turbulence and multiphase flow of water, steam, and CO₂, heat transfer between hot gases and cooling water, steam condensation and water heating in the presence of CO₂. The experimental validation of CFD modeling results is a very important issue, but test-rig needs to be specially designed and built allowing to obtain accurate and good experimental results. Madejski et al. [36] proposed the design together with all detailed assumptions needed for building and for conducting experimental investigations with the use of developed spray-ejector condenser.

The study uses CFD methods to numerically investigate the operation of a two-phase, subsonic water-steam ejector for different operational modes and two condensation models. A brief review concerning the main features of the modeling approaches of multiphase, turbulent flow with phase change is presented. The most suitable models for CFD modeling of the water-steam ejector were chosen and applied. The numerical 2D, axisymmetric model was developed using simcenter star ccm+ software based on the finite volume method. The multiphase flow was calculated using the one-fluid mixture approach, where the mass, momentum, and energy equation is solved for a whole mixture. Two-equation eddy viscosity k–ω SST model was applied to take into account turbulence. The direct contact condensation was computed using two various models: Spalding evaporation/condensation and boiling/condensation. Based on the scalar contours and changes in average velocity, temperature, and steam mass flowrate along the flow path, the ejector performance was analyzed for various operating conditions. Different exhaust gas inlet velocities were considered. The influence of the condensation models and the presence of CO₂ on the two-phase ejector operation have been assessed.

Two-phase ejectors are devices where the primary and secondary fluids exist in various physical states. Fluid momentum with high energy potential is used for entraining the secondary fluid. The motive fluid can be a gas or liquid. In case of secondary fluid, there are more possibilities: liquid, gas, and a mixture of fluid and solid. The most popular are liquid-gas or gas-liquid ejectors, but gas-solid or liquid-solid ejectors can also be applied [37]. Compared to one-phase ejectors, the theoretical description of phenomena in two-phase ejectors is more complicated because the differences in fluid properties between phases exist in various physical states.

The scheme of the water-driven, two-phase ejector condenser is presented in Fig. 1. The water is delivered to the nozzle. The nozzle is converging; therefore, the velocity of the motive fluid is rising while static pressure is falling rapidly. Significantly reduced pressure at the nozzle exit causes the entrainment of the secondary fluid. After exiting the nozzle, the shape of the motive fluid is still conical-cylindrical, and there are clear boundaries between the two fluids until it comes to the mixing section. The pressure of both fluids in the area between the nozzle and the mixing chamber is relatively constant, equal to the suction pressure. Suddenly, a strongly turbulent mixing process occurs in the mixing section. Condensation takes place under non-equilibrium conditions: the water droplets don’t form as soon as the vapor reaches the saturation pressure [38]. Due to all processes in the mixing section, fluid mixture pressure rises while the velocity decreases. The kinetic energy of the fluid is scattered. The pressure increase is most significant in the mixing chamber and is responsible mainly for the pressure lift effect in the ejector [39]. The pressure rises in the diffuser much less. The mixing section outlet expects a fully homogeneous mixture with a stable velocity field.

Phenomena that take place in the water-driven, two-phase ejector are complex and occur simultaneously. CFD modeling is a tool that allows for taking into account all these effects in complex geometrical models. Three flow features should be considered: multiphase, turbulent, and phase change. Considering multiphase flow modeling: two approaches can be distinguished: Euler–Euler and Euler–Lagrange [40].

The Euler–Lagrange approach is connected with simulating and tracking individual particles. The various interaction types between particles can be modeled realistically, e.g., particle-particle and particle-wall collisions. The Euler–Lagrange approach allows modeling of differences in local particle velocity as well as a distribution of particle sizes [41]. This approach is more accurate but also more computationally costly. The Euler–Lagrange approach is appropriate for the calculation of a single particle or a dilute suspension [42].

The Euler–Euler approach is based on the assumption, that all phases are treated like interpenetrating continua. The discrete (solid, bubble, etc.) phase is treated as a continuous medium with the physical properties of the fluid. The volume fraction idea is applied to take into account the share of different phases in the same space. The sum of the volume fraction must be one. The governing equations are solved separately for each phase but some simplification can be applied (e.g., mixture model). In case of CFD modeling of the ejectors, the Euler–Euler approach is commonly used [19,43,44]. The most popular models are the mixture model, volume of fluid, and the two-fluid Eulerian multiphase model.

In the mixture model, which is based on a single-fluid approach, the mass, momentum, and energy equations are solved for the mixture of phases. Typical application includes dispersed multiphase flow: bubbly flow and droplet flow. The mixture model is the homogeneous model where the phases are moving in the same velocity, which is solved from a single momentum equation. The presence of additional submodels gives a chance to consider additional effects, e.g., boiling, condensation, slip velocity, or surface tension force. The mixture model was successfully used for modeling the ejectors [45,46]. Compared to the standard two-fluid Eulerian model, computing power is significantly reduced. Moreover, the mixture model for numerical modeling of the water-air ejector is more accurate and efficient than the two-phase model [29]. Considering features of the mixture model presented in this section and the analysis concerning multiphase modeling prepared by Ref. [47], the mixture model was chosen to model the multiphase flow in the two-phase ejector condenser.

Considering the turbulence modeling, the Reynolds-averaged Navier–Stokes (RANS) approach is used most often in the case of ejector phenomena modeling. The RANS approach replaces each solution variable as the sum of the mean values and their fluctuating component. It leads to the presence of an additional term in Navier–Stokes equations, which should be solved. RANS equations can be closed using eddy viscosity models, where the most versatile are two-equation models: k–ω SST and k–ε. The k–ε model is a two-equation model that contains turbulent kinetic energy transport and dissipation rate of turbulent kinetic energy equations [48]. The model is successfully used in case of ejectors modeling [39]. The k–ω SST is a hybrid model that allows switching between k–ω and k–ε. The blending function provides smooth transitions between models. The model is accurate in non-equilibrium boundary layers modeling (separation). According to the “NASA Technical Memorandum,” it is the most accurate model for aerodynamic calculations [49]. Similar to the k–ε model, it is one of the most popular models for ejector phenomena modeling [13,27]. Taking into account all the advantages mentioned above, the k–ω SST model was chosen to simulate two-phase turbulent flow through the ejector condenser.

Numerical modeling of direct contact condensation is still challenging due to the complexity of the phenomenon. Because of the very high values of the heat transfer coefficient, numerical calculations are connected with large instabilities. Moreover, direct contact condensation is less explored compared to wall condensation. Four types of direct contact condensation can be distinguished: drop type, bubble type, jet type, and film type. Choosing the appropriate model should consider what type of condensation should be calculated. In this study, two condensation models are considered Spalding evaporation/condensation and boiling/condensation. The main idea of the first one is to express the steady convective mass transfer phenomena using Ohm's law relation [50]. The Spalding/evaporation condensation model is used to modeling droplet evaporation/condensation dispersed in the gas phase. The second model is the condensation model. It is a two-resistant, thermally-driven model where the mass transfer is computed from the heat-balance calculations on the interphase surface. This approach is often used to model direct contact condensation of steam [51].

The 2D geometrical model of the two-phase ejector condenser was developed according to the ejector drawing presented in Fig. 2. The model is assumed to be axisymmetric. The most important dimensions are presented in Table 1.

Two types of meshes are considered: polyhedral and trimmed (Fig. 3). For polyhedral-type mesh, a mesh independence study was done (for case with 8.9 m/s gas inlet velocity). Cross-sectional average temperature and velocity along the flow path were developed for four meshes with different numbers of elements: 77,598, 161,253, 325,479, and 602,272. Considering cross-sectional average velocity along the flow path presented in Fig. 4, considerably higher velocity can be observed for meshes with 77,598 and 325,479 elements. The most significant difference is between meshes with 161,253 and 325,479. Further increasing the number of elements, the difference is small. Figure 5 shows the cross-sectional average temperature along the flow path for four meshes with different numbers of elements: 77,598, 161,253, 325,479, and 602,272. Differences occur mainly at the beginning of the mixing chamber. Temperature change between meshes with 325,479 and 161,253 is not significant. Taking into account the conclusions from the mesh independence study as well as computational cost and the stability of the solution, it was decided that mesh with 325,479 elements be used for further investigation.

The properties of meshes (best polyhedral and trimmed) are presented in Table 2. Polyhedral mesh consists of 325,479 polyhedral elements, and the base size is 0.7 mm. The inflation layer with four prism layers is applied near all ejector walls.

Two types of outlet boundary conditions were considered: outlet and pressure outlet. In the case of an outlet boundary condition, the pressure is the result from the calculations. All the rest of the lines are the wall boundary conditions (no-slip and adiabatic). For analysis concerning gas velocity, velocity boundary condition (pure steam) at the gas inlet is assumed. For the investigation of various condensation models and the presence of CO₂, mass flow boundary conditions are applied. In this case, gas is a pure steam or a mixture of steam and CO₂ (20% CO₂ mass content).

The constant physical properties of water and steam (density, dynamic viscosity, thermal conductivity, and isobaric heat capacity) were calculated using available fluid properties data IAPWS-IF97 [53]. The assumed saturation temperature was 100 °C. The constant properties of CO₂ were obtained based on the NIST tables [54]. Table 4 shows the exact values of assumed fluid properties (water, steam, CO₂).

The finite volume method was used for solving partial differential equations. Calculations were performed in steady-state conditions. The reference density was taken of the density of the gas phase and the reference pressure as atmospheric pressure. A segregated solver with a second-order convection scheme was used. Second-order convection was also used in the mixture multiphase model and the k–ω SST turbulence model. Face density reconstruction in case of mixture multiphase model was calculated using the first-order scheme. Relaxation factors used in the CFD study are presented in Table 5.

Verification of the CFD model of the two-phase ejector was carried out in several ways. The mesh independence study was performed. Various types of boundary conditions and different models were applied. Moreover, convergence criteria and mass balance were controlled (mass error below 10⁻⁵). The model was validated based on the comparison between simulation results and the theoretical waveform along the flow path from the literature. Figure 7 shows the comparison of the theoretical pressure chart from Goliński and Troskolański [5] (top) with the CFD results (bottom). Considering the theoretical pressure chart, the highest increase in pressure occurs in the mixing zone. Growth in the diffuser is considerably smaller. Similar trends can be observed in the results from CFD. Pressure rise is the most significant in the mixing chamber (which is much longer than in the scheme from the literature). The pressure is relatively constant downstream of the motive nozzle (before mixing). This comparison shows that the CFD model reflects the main features of the phenomena that take place in the two-phase ejector condenser.

This section presents the influence of the gas inlet velocity (steam mass flow) on the ejector operation. The following model properties are used: polyhedral mesh, gas–pure steam, and Spalding/evaporation condensation model. The following inlet gas velocities are analyzed: 8.90 m/s; 7.60 m/s; 6.50 m/s; 3.47 m/s; 2.50 m/s. Corresponding to them steam mass flowrates are 39.8 g/s; 33.7 g/s, 28.82 g/s, 15.15 g/s, and 11.08 g/s, respectively.

Figure 8 shows the contours of water volume fraction for various steam inlet velocities. For 8.9 m/s and 7.6 m/s steam velocity, steam is not fully condensed. For steam velocity 6.50 m/s and lower, the volume fraction of water equal to one can be observed in almost the entire domain which indicates that all the steam has been condensed. Moreover, for velocities 6.50 m/s to 2.50 m/s, steam is condensed very fast—at the beginning of the mixing chamber.

Static pressure distribution for various steam velocities was presented in Fig. 9. The compression effect of gas can be observed in all cases. The motive water pressure is about 13 bar, therefore outlet pressure is located between the suction and motive pressure. The subpressure region is created in the suction chamber which allows sucked-in the exhaust gas. The less gas is entrained, the more compressed it is. The greatest increase in pressure can be observed in the mixing chamber.

In Fig. 10, the velocity contours for different steam velocities are presented. Gas inlet velocity is growing, mixture velocity is increasing significantly. Moreover, the area of the highest mixture velocity can be observed at the beginning of the mixing chamber. Velocity is gradually decreasing along the length of the ejector. Mixture-specific volume is falling due to steam condensation and forces velocity changes. Velocities, which occur inside the ejector, are far from the supersonic conditions.

Figure 11 presents the temperature distribution for various steam inlet velocities. Lower steam mass flow, lower mixture temperature. It is due to the fact, that less steam is condensed. At the beginning of the ejector, the temperature of gas and motive water can be differentiated. After a short distance, the temperature rapidly changes, and both phases achieve a mixture temperature. The distance is shorter, when the gas inlet velocity is lower. Lower steam mass flow, lower mixture temperature.

Turbulent kinetic energy contours for considering steam velocity are presented in Fig. 12. The most intensive turbulence occurs in the first part of the mixing chamber due to the rapid mixing of the two streams of primary and secondary medium. The highest values of the turbulence kinetic energy are observed for the velocity 8.90 m/s, indicating that the turbulence intensity is falling when the gas mass flowrate is decreasing. Significant turbulence structure can be observed in the diffuser for 8.90 m/s gas velocity which is connected with separation zone created due to cross-sectional area increase.

Figure 13 shows condensation mass transfer rate distribution for various steam inlet velocities. The most efficient condensation occurs in the suction chamber and the first part of the mixing zone. Further, the condensation mass transfer is gradually decreasing. It can be seen that condensation occurs mainly at the interface between phases. This interface has a jet-like shape. This jet is the longest for the medium gas velocity (6.50 m/s).

Figure 14 describes the average velocity change along the flow inside the ejector for various gas inlet velocities. The mixture's average velocity rapidly increases at the distance from the motive nozzle outlet to the beginning of the mixing chamber. Next, rapid fall can be observed until the one-sixth length of the mixing chamber. In the rest of the mixing chamber, velocity is relatively constant. A significant fall of the average velocity can be observed in the diffuser. The lower the gas inlet velocity, the lower the average mixture temperature in each ejector part.

The change of average temperature along the flow inside the ejector for various gas inlet velocities is presented in Fig. 15. In all cases, the temperature is rising and distribution quickly becomes relatively constant. The growth of the temperature is mainly due to the latent heat of condensation. For cases with higher steam mass flow, the mixture temperature is close to the saturation temperature. Outlet mixture temperature of about 91 °C indicates that steam is fully condensed after flowing through the ejector.

Figure 16 shows the cross-sectional average steam mass flow and its derivative charts as a function of the ejector length for various gas velocities. Condensation efficiency is also presented (in percent). Lower steam inlet velocity (steam mass flow)—higher condensation efficiency. Partial steam condensation can be observed for velocities 8.90 m/s and 7.60 m/s (81.6% and 92.2% steam is condensed, respectively). In other cases, steam is fully condensed. The rapid condensation occurs directly after mixing primary and secondary streams in the suction chamber and at the beginning of the mixing chamber.

The results of the simulation using two approaches concerning direct contact condensation modeling for the same operating condition are presented here. Additionally, the influence of CO₂ on the ejector operation is investigated using the boiling/condensation model, where the trimmed-type mesh is applied. Three cases were analyzed: the Spalding evaporation/condensation model for pure steam, boiling/condensation for pure steam, and a mixture of steam (80%) and CO₂ (20%). The constant mass flowrate of gas is assumed at the gas inlet (39.3 g/s).

In Fig. 17, water volume fraction distribution for the Spalding evaporation/condensation model and the boiling/condensation model using pure steam and steam + CO₂ is presented. In considering conditions, the two streams are very poorly mixed. The water is forming the jet. This jet is the most dispersed in case of the boiling/condensation model of pure steam which can indicate that the condensation, it is more intense there than in other cases.

Figure 18 shows static pressure distribution for the Spalding evaporation/condensation model and boiling/condensation model of pure steam as well as boiling/condensation with CO₂ presence. Contours differ significantly for various condensation models. The pressure lift effect is not observed in considering conditions. The lowest value of the pressure at the suction chamber can be observed for the boiling/condensation model. CO₂ presence causes the inlet gas pressure to be higher than pure steam.

Velocitiy distribution for various condensation models with/without CO₂ is presented in Fig. 19. Despite the fact, that the mixture model was used to simulate two-phase flow in the ejector, the region occupied by the gas is characterized considerably higher value of velocity. These differences are most visible in the boiling/condensation model. The highest velocity values can be observed in the mixing chamber, especially at the beginning of this part where two streams met. The velocity gradually decreases in the diffuser part, where the kinetic energy is converted into pressure energy. The presence of the CO₂ doesn't significantly affect the velocities contours.

Figure 20 shows the temperature contours for the Spalding evaporation/condensation model and the boiling/condensation model of pure steam as well as boiling/condensation with CO₂ presence. The temperature is low in the region where the water jet exists. In the rest of the domain, high temperature (significantly over 100 °C) occurs. It means that the gas (steam) is not cooled effectively. The heat transfer phenomenon is weak for considering conditions.

Figure 21 illustrates the turbulent kinetic energy in considering cases. Turbulent kinetic energy achieves the highest value at the beginning of the mixing chamber (constant area section) due to the intensive exchange of momentum between two streams. Diffuser is also a place where the turbulences are strong due to increasing the cross section area of the flow. Significant greater values are obtained for the boiling/condensation model of pure steam. It seems that the presence of the CO₂ dampens turbulence.

The contours of mass transfer condensation rate for two condensation models and one with CO₂ were presented in Fig. 22. The contours contain the suction chamber and the beginning of the mixing chamber. The condensation mass transfer rate achieves the highest value near the border layer between phases which indicates that the direct contact condensation occurs mainly at the interface between the water jet and the hot exhaust gas. Considering the boiling/condensation model, the thin layer of the strongest condensation disappears after a certain length and the contour is blurry. It can show that the flow regime is changing and the condensation occurs at the water droplets. The presence of CO₂ causes the condensation transfer rate to be lower and more concentrated around the phase boundary. The reason for this can be the high concentration of CO₂ at the phase interface, which blocks the heat transfer.

Figure 23 presents the change of average velocity along the flow inside ejector distribution for the Spalding evaporation/condensation model (pure steam), boiling/condensation model (pure steam), and boiling/condensation with CO₂ presence. From the outlet of the suction chamber, the cross-sectional average mixture velocity is decreasing. The decrease is gradual in the mixing chamber and rapid in the diffuser. The differences between the two condensation models can be noticed. The presence of CO₂ doesn’t affect the average mixture velocity charts.

Figure 24 shows the change of average temperature along the flow inside ejector distribution for the Spalding evaporation/condensation model (pure steam), boiling/condensation model (pure steam), and boiling/condensation with CO₂ presence. The outlet temperature is similar and close to the saturation temperature for all cases. The rapid temperature growth in the suction chamber area can be observed for pure steam condensations. The presence of CO₂ causes, that the growth of the temperature is gradual. It can suggest that CO₂ may stabilize the operation of the ejector.

The change of average steam mass flow along the flow inside the ejector for the Spalding evaporation/condensation model (pure steam), boiling/condensation model (pure steam), and boiling/condensation with CO₂ presence is presented in Fig. 25. For all considering cases, the decrease of the steam mass flowrate is gradual and the full condensation doesn't occur. The highest condensation efficiency and condensation speed occur for boiling/condensation model (36%) with pure steam. The presence of CO₂ reduces the amount of condensed steam (36.0% versus 31.7%). The speed of condensation is significantly lower in the case of CO₂ presence until one-fourth length of the mixing chamber.

The numerical 2D, axisymmetric model of a water-driven, two-phase ejector condenser was developed using siemens star ccm+ software. The study aimed to investigate the performance of the ejector considering the turbulent, multiphase flow with direct contact condensation. The multiphase flow was calculated using the one-fluid mixture approach. The turbulence phenomenon was taken into account using the two-equation, eddy viscosity k–ω SST model. Direct contact condensation between water and steam was computed using two different approaches: the Spalding/evaporation model and thermally-driven boiling/condensation. The influence of the gas inlet velocity (gas mass flow) and the presence of CO₂ on the ejector performance was analyzed. The following conclusions can be made:

• – Lower sucked-in mass flowrate of gas, the higher the compression effect and the lower the average outlet temperature. The sub-pressure region at the gas inlet and suction chamber can be noticed. Turbulence is considerably stronger for higher gas mass flowrate values.

• – A very efficient condensation process was obtained (condensation efficiency between 81.6% and 100%) for considering gas inlet velocities. The most intensive condensation can be noticed in the suction chamber and at the beginning of the mixing chamber. Moreover, direct contact condensation occurs mainly near the interface between phases.

• – Two condensation models, which are based on different mass transfer mechanisms, were analyzed. For considering conditions, the thermally-driven boiling/condensation model predicts more intensive condensation (36% versus 23.1% condensed steam) and lower suction pressure. Moreover, the boiling/condensation model seems to give more reliable results for considering conditions (better convergence and robustness of the model).

• – The CO₂ presence in the sucked-in gas mixture reduces the condensation intensity and condensation efficiency (36.0% versus 31.7%). The CO₂ presence decreases turbulence intensity and causes the ejector operation to be more stable (more gradual growth of temperature).

The limitation of this study concerns the applied multiphase approach: mixture which is simplified multiphase model. It does not allow the phases to be considered separately. Moreover, experimental validation is needed to confirm the conclusions and further develop the model. Despite the limitations, the model reflects the main features of the multiphase, turbulent flow with condensation. Results allow for a deeper understanding of the phenomenon and indicate the most profitable operating conditions for the considered geometrical model. Further work will focus on the CFD results validation with the available experimental results to evaluate the accuracy of calculated distributions and computed condensation efficiency of steam with the presence of CO₂.

The research leading to these results has received funding from the Norway Grants 2014–2021 via the National Centre for Research and Development. Work has been prepared within the frame of the project: “Negative CO₂ emission gas power plant”—NOR/POLNORCCS/NEGATIVE-CO₂-PP/0009/2019-00 which is co-financed by programme “Applied research” under the Norwegian Financial Mechanisms 2014–2021 POLNOR CCS 2019—Development of CO₂ capture solutions integrated in power and industry processes.

There are no conflicts of interest.

The authors attest that all data for this study are included in the paper.

g =

surface conductance, kg/s

h =

heat transfer coefficient, W/m²K

k =

turbulent kinetic energy, J/kg

p =

pressure, Pa

$a$ =

surface area vector, m²

B =

Spalding transfer number, J/kg · K

D =

dimensionless driving force, J/kg · s

L =

phase change heat, J

Q =

heat transfer rate, W/m³

T =

temperature, K

V =

volume, m³

$I$ =

unity tensor, –

$m˙$ =

rate of the transfer of material, kg/s

$q˙$ =

unity tensor, –

$v¯$ =

mean velocity, m/s

$fβ$ =

vortex-stretching modification factor, –

f_β* =

free-shear modification factor, –

k₀ =

ambient value of turbulent kinetic energy that counteract turbulence decay [40], J/kg · s

v_m =

mass averaged velocity, m/s

$fb$ =

body force vector, N/m³

A_s =

droplet surface area, m²

C_p =

specific heat capacity, –

D_p =

particle diameter, m

H_m =

total enthalpy of the mixture, m²/s²

P_k =

turbulent kinetic energy production term, W/m³

$Pω$ =

specific dissipation rate production term, W/m³

S_e =

energy source term, W/m³

S_k =

turbulent kinetic energy source term, W/m³

S_u,i =

phase i source term, 1/s

$Sω$ =

specific dissipation rate source term, W/m³

T_mix =

mixture temperature, K

T_s =

saturation temperature, K

T_t =

turbulent time scale, s

Y_p =

liquid mass fraction of component in the particle, –

$Tm$ =

viscous stress tensor, Pa

$g*$ =

mass transfer conductance, when B → 0, kg/s

$m˙b$ =

massflow at boundary surface, kg/s

$m˙p$ =

evaporation/condensation rate, kg/s

$m˙V$ =

rate of the transfer of material per unit volume, kg/s · m³

Nu_p =

particle Nusselt number, –

Δh =

latent heat of phase change, J/kg

α_i =

volume fraction of phase i, –

β =

model coefficient, –

$β*$ =

model coefficient, –

$ε$ =

fractional mass transfer rate, 1/m⁵

θ =

interfacial area per unit volume, 1/m

$θspec$ =

inflow direction, 1/m

λ =

thermal conductivity, W/m K

μ =

dynamic viscosity, Pa s

μ_t =

turbulent dynamic viscosity, Pa s

ρ_m =

density of the mixture, kg/m³

σ_k =

model coefficient, –

σ_t =

turbulent Schmidt number, –

$σω$ =

model coefficient, –

ω =

specific dissipation rate, J/kg s

ω₀ =

ambient value of specific dissipation rate that counteracts turbulence decay [40], J/kg s