Simulations of a Single-Phase Flow in a Compound Parabolic Concentrator Reactor

This paper deals with the analysis and interpretation of flow visualization and residence time distribution (RTD) in a compound parabolic concentrator (CPC) reactor using computational fluid dynamics (CFD). CFD was calculated under turbulent flow conditions solving the Reynolds averaged Navier–Stokes (RANS) equation expressed in terms of turbulent viscosity and the standard k−ε turbulent model in 3D. A 3D diffusion-convection model was implemented in the CPC reactor to determine the RTD. The fluid flow visualization and RTD were validated with experimental results. The CFD showed that the magnitude of the velocity field remains almost uniform in most of the bulk reactor, although near and inside the 90° connectors and the union segments, the velocity presented lowand high-speed zones. Comparisons of theoretical and experimental RTD curves showed that the k−ε model is appropriate to simulate the nonideal flow inside the CPC reactor under turbulent flow conditions.

Several works show the efficiency of this technology in terms of pollutant concentration decay, during photo-Fenton or solar photoelectro-Fenton water treatment process [2][3][4][5]11].However, CPC studies that describe its performance from a chemical engineering standpoint are scarce.Among these, the nonideal flow analysis distinguishes, because it allows understanding the bulk reactor behavior and thereby to propose more efficient designs [12].
Most of the homogeneous (photo-Fenton) and heterogeneous (TiO 2 photocatalytic) reactions that take place inside the CPC are performed under turbulent flow conditions to guarantee complete mixing conditions and an efficient mass transfer.The CPC is a coil-type tubular reactor, and one way to experimentally characterize the hydrodynamics inside it is through residence time distribution (RTD) analysis [13][14][15][16] or by flow visualization technique [17][18][19][20].Benhabiles et al. [21] developed an experimental RTD study in a five-tube CPC reactor; these authors estimated Péclet numbers (Pe) and axial dispersion coefficients (D a ) with the analytical solution of the axial dispersion model at different volumetric flows.They found that for small values of Pe, the flow presents back mixing and dispersion in the radial direction.
The mathematical models can consider that the flow mixing occurs in the axial coordinate [22][23][24][25] and that the flow is completely mixed as the plug-flow model [24,25].In practice, flow behavior deviates from these owing to nonuniform velocity profile originated by turbulent diffusivity, by short circuiting, by passing and channeling of fluid, and by the presence of stagnant regions of fluid within the reactor.The above deviations can be determined by the diffusion-convection model, although these are scarcely modelled.A model for the CPC geometry must include the inclination of the reactor (see Figure 1(a)) owing to it may cause noncomplete mixing conditions.This paper deals with the analysis and interpretation of flow visualization and RTD in a CPC reactor using CFD in 3D.CFD was calculated under turbulent flow conditions solving the Reynolds averaged Navier-Stokes (RANS) equations expressed in terms of turbulent viscosity and the standard k−ε turbulent model.Theoretical RTD curves were compared with experimental RTD data in order to validate the proposed model.Moreover, experimental and theoretical nonideal flow visualization was also performed.

Description of the CPC Reactor
Figure 1(a) shows a scheme of the CPC reactor which was used as a basis for the computational geometry in order to establish the simulation domain.It consists of 4 acrylic tubes of 90.5 cm length and 1.9 cm inner diameter connected with PVC tube segments and 90 °PVC connections of 2.54 cm inner diameter.The parabolic reflectors are made of aluminum with a 180 °acceptance angle and a concentration ratio of 1.The system has 1400 cm 3 of capacity and an inclination of 21 °from the ground corresponding to the latitude of Guanajuato state, in central Mexico.

Formulation of the Numerical Simulation
Simulations in 3D of turbulent flow and a tracer inside the reactor were carried out.Figure 2(a) shows the simulation domain, and it was considered as "zigzag" pipes of constant diameter equal to 1.9 cm.The wall roughness was assumed to have a negligible effect.Table 1 shows the parameters for the simulations.
where u is the velocity vector, P is the pressure, μ is the dynamic viscosity, and ρ is the fluid density, and the so-called Reynolds stresses can be expressed in terms of a turbulent viscosity μ T , according to the standard k-ε turbulence model where κ is the turbulent kinetic energy, ε is the turbulent energy dissipation rate, P k is the energy production term P k = μ T ∇u ∇u + ∇u T , and C μ 0 09 , C e1 1 44 , C e2 1 92 , σ k 1 , and σ ε 1 3 are dimensionless constant values that are obtained by data fitting for a wide range of turbulent flows [26][27][28].This model is applicable at high Reynolds numbers; for this reason, the near-wall regions, where the velocity is relative to the wall, decrease quickly and these regions are inaccessible by this model.To solve this problem, wall functions 2 International Journal of Photoenergy based on a universal velocity distribution are usually required.In a turbulent layer, these functions are described by the following equation [26][27][28]: where u + is the normalized velocity component inside the logarithmic boundary layer and y + is the dimensionless distance from the wall, y + = ρu τ y/μ, where u τ is the friction velocity, u τ = C 1/4 μ k, and y is the thickness from the wall [26][27][28].
To solve (1), (2), and (3), the corresponding boundary conditions are as follows [26]: (1) A normal inflow velocity at the inlet, u = −nU 0 ; where n is the unit normal vector; in this work, the approximation for the inlet values of k 0 and ε 0 was obtained from the turbulent intensity I T and the turbulent length scale L T , by means of the following simple assumed forms: where I T and L T were fixed at 0.05 and 0.0665 cm, respectively [27].The turbulent intensity for fully turbulent flows has dimensionless values between 0.05 and 0.1.The turbulent length scale can be determined in pipes as a function of the radius by means of L T = 0 07r, where r in this work is the inlet radius of 0.95 cm.
(2) A normal stress equal to a pressure at the outlet, −P + μ + μ T ∇u + ∇u T n = −nP 0 , with ∇ε ⋅ n = 0 and ∇k ⋅ n = 0.This last equation expresses that the turbulent characteristic of whatever is outside the computational domain is guided by the flow inside the computational domain.Such an assumption is physically reasonable as long as relatively small amounts of fluid enter the system [29].
(3) A velocity u + given by ( 4) at a distance y + from a solid surface, for all other boundaries.
After verifying the solution at different values of y + and step sizes, the value of y + was fixed at 11.1.This value is in the fully turbulent region (5 < y + < 30), where the turbulent stresses and fluxes are more important.The corresponding values of y and u τ are 60 μm and 0.31 cm•s −1 , respectively.Equations ( 1), (2), and (3) were solved numerically in stationary regime in 3D through finite elements by using the commercial software COMSOL Multiphysics® (4.4) at different inflow velocities, U 0 : 17.6 cm•s −1 (Re = 3344), 22.2 cm•s −1 (Re = 4218), and 24.4 cm•s −1 (Re = 4636).A simulation domain of 41,500 mesh elements was considered (Figure 2(b)).The numerical accuracy of the magnitude of the local velocity vectors was tested by enlarging and diminishing the size of the tetrahedral elements by a factor of 2 and by verifying that the solution of the magnitude of the local velocity vectors did not show significant differences as the convergence criterion was changed to below 10 −5 .The simulation run times were typically from 30 to 45 minutes depending on the flow rate.A computer with 2 intel® Xeon 2.3 GHz processors, 96 GB of RAM, and 64 bits of operative system was employed.

Tracer Simulation.
The time-dependent behavior of a tracer inside the reactor could be described by the general form of the diffusion-convection equation [30] where c is the concentration of the tracer, t is the time, D is the diffusion coefficient, and u is the velocity vector obtained by the solution of (1).
It is important to mention that in some cases, mass transport models are involved with turbulent flow conditions, the  3 International Journal of Photoenergy term of turbulent diffusivity that appears in (5).This term is associated to jet flows, eddies, and local flow deviations caused by the inherent turbulent flow inside the system [31,32].Worthy of mentioning, we performed several simulations including the turbulent diffusivity coefficient (not shown herein) in order to develop a more rigorous model.However, when this term was included, the theoretical results did not fit with the experimental RTD studies.The explanation of the above behavior is discussed in the analysis of results and discussion in Section 5.
In order to simulate the tracer injection in an instant of time, a Gaussian pulse function was employed [33] where σ is the standard deviation and t is the time which was fixed in an interval of time from 0 to 6 seconds.After several trials and verifying the solution, the standard deviation was fixed at 2 s.In this paper, the diffusion coefficient was fixed In order to solve (5) and considering complete mixing conditions before the inlet and after the outlet of the reactor (Figure 2(a)), the boundary and the initial conditions established are as follows: (i) Before tracer injection inside the reactor at t = 0, c(x, y, z, t) = 0 (ii) An initial concentration at the inlet, c = c 0 y(t)/ y(t = 0) (iii) Cero flux at the outlet and at the walls, D∇c = 0 Equation ( 5) was solved numerically in 3D through finite elements by using the commercial software COMSOL Multiphysics (4.4) at different inflow velocities: 17.6, 22.2, and 24.4 cm•s −1 .Equation ( 5) is in transient state; therefore, it needs an interval of time to be solved, which was established from t = 0 s to t = 140 s at 0.1 s of step size.A simulation domain of 41,500 mesh elements was considered.The simulation run times were typically from 20 to 30 minutes depending on the flow rate.
After solving (5), theoretical RTD curves and computational animations were performed in order to compare with experimental RTD curves and flow visualizations at different inflow velocities.

Experimental Details
The experimental flow visualization and RTD were performed in order to compare the theoretically obtained CFD and RTD results.Experimental tracer tests were filmed by a high-resolution camera and those were compared with computational tracer animations.

Flow Visualization.
In order to visualize experimental flow patterns inside the CPC reactor, 5 mL of colored tracer (Blue 1 at a concentration of 5 g•L −1 ) was injected few centimeters before the CPC inlet and filmed (Figure 1(b)).It is important to mention that the density of the tracer solution does not affect the flow pattern inside the reactor.Moreover, the tracer volume is significantly smaller than the volume of the reactor (1400 mL).A 29-frames-per-second and 1920 × 1080-pixel-resolution camera was used.The tracer tests were performed at different inflow velocities of 17.6, 22.2, and 24.4 cm•s −1 .

RTD Studies.
To determine the mixing flow pattern in the liquid phase, the stimulus response technique was employed.5 mL of 0.05 M copper sulfate was injected as tracer at the inlet of the CPC and the cupric ions were detected at the exit (Figure 1(b)).The measurement of Cu(II) was carried out employing a typical two-electrode cell arrangement using two copper wires as electrodes; the cupric ions were quantified by typical transient current at a holding cell potential of −1.9 V.The current response was recorded every 0.5seconds by a potentiostat-galvanostat model SP-150 from BioLogic™ with EC-Lab® software.It is important to mention that at such cell potential of −1.9 V, a limiting current of copper deposition governs the cathodic process ensuring that the response only depends on the cupric ion concentration.
For the nonideal flow, elements of fluid can take different routes throughout the CPC reactor, spending different periods of time inside the reactor.The RTD curve, E t , describes the distribution of these periods of time for the stream of fluid leaving the CPC, (7).The E t function is normalized and the area under the curve reaches a value of 1, according to (8) [12] ∞ 0 E t dt = 1, 7 where I t is the time-dependent current response.RTD studies were carried out at different inflow velocities of 17.6, 22.2 and 24.4 cm•s −1 .

Analysis of Results and Discussion
5.1.Turbulent Flow. Figure 3 shows a domain velocity field plot for a characteristic inflow velocity of 22.2 cm•s −1 inside the CPC reactor.Here, it could be observed that the velocity field remains almost uniform in most of the bulk reactor.However, near and inside the 90 °connectors and the union segments, the velocity field presents low-and high-velocity zones due to the inherent CPC geometry, showing that the CPC cannot be considered as an ideal plug flow reactor.
Identical patterns (not shown herein) were obtained for the other inflow velocities, 17.6 and 24.4 cm•s −1 .
Figure 4 shows velocity profiles as a function of the tube diameter for a characteristic inflow velocity of 22.2 cm•s −1 .These curves were constructed in order to describe the hydrodynamic behavior of Figure 3.The velocity profiles inside the inner diameter were constructed at different distances from the CPC inlet as shown in Figure 2(a).The profile constructed at distance of 50 cm develops an ideal turbulent profile with a maximum of around 25 cm•s −1 and a minimum of around 15 cm•s −1 and a plug flow region of around 0.4 ≤ d ≤ 1.6 cm.The velocity profile for the union segment at a distance of 100 cm shows the flow deviations generated by the 90 °connector.In this profile, it could be observed that the union segment presents low velocity values of around 0 ≤ d ≤ 0.13 cm with a minimum value of 2 cm•s −1 ; then, the velocity increases until it reaches a maximum of 34 cm•s −1 at d = 1.6 cm.After, the velocity decreases until 26 cm•s −1 at d = 1.9 cm.The above behavior is very similar for the profile at a distance of 117 cm; here, it could be seen that this behavior is less pronounced that the profile performed at 100 cm, which that the flow deviations attenuate away from the 90 °connection as can be observed at distances of 150 and 170 cm.The behavior described in the profiles repeats in every lap of the CPC confirming the need to analyze the RTD.Similar plots not shown herein were obtained for the other inflow velocities at 17.6 and 24.4 cm•s −1 , obtaining the same pattern.
From the analysis of Figures 3 and 4, it could be confirming the convenience of using a mass transport model without the turbulent diffusion coefficient, described in Section 3.2.The above is because the system does not generate significant turbulent flow deviations such as eddies or jet flows, as it can be observed in Figure 3; this behavior confirms the omission of the turbulent diffusion coefficient of (5).Moreover, the velocity profiles develop a pseudoplug flow behavior in almost all regions inside the reactor (Figure 4); this last showed that the system is appropriate to develop a well homogenous environment to carry out the photoreactions inside the system.The above was proved in the analysis of results and discussion of the flow visualization and RTD described below.Nevertheless, a deeper analysis with different photocatalytic reactions is needed to support this statement.This later was beyond the scope of this paper.

Flow Visualization.
Figure 5 shows comparisons of the experimental flow visualization and the tracer simulation at different times for the characteristic inflow velocity of 22.2 cm•s −1 .Here, it could be observed qualitatively that the tracer simulation agrees with the experimental visualization technique, because the tracer follows the same flow patterns at the same instants of time.For the time of 5 seconds, the tracer is completely mixed before entering the 90 °connec- tion.After the first union segment, at the time of 14 seconds, the tracer presents an elongation generated by the 90 °con- nection.This elongation is more marked passing the third and fourth union segments at the time of 19 and 24 seconds, respectively; therefore, it agrees with those discussed in Figures 3 and 4; the 90 °connections generate slow-velocity zones and flow deviations.Similar experimental flow visualization and the tracer simulation were obtained for 17.6 and 24.4 cm•s −1 (not shown), obtaining the same pattern to that obtained at 22.2 cm•s −1 .
5.3.RTD. Figure 6 presents comparisons of theoretical and experimental RTD curves for the different inflow velocities as a function of the dimensionless residence time t/τ , where τ is the spatial residence time given by the ratio between the length of the CPC and the inflow velocity = L/U 0 .This figure shows close agreement between experiments and simulations (error < 5%).Worthy of mentioning, the most fluid elements leave the system around the expected residence time (t/τ = 1).For such cases, the residence time is about 24 s and the dispersion of the tracer in the pipe is dominated by the convective transport, where the turbulent flow predominates (Re > 3000).
From the analysis carried out here, a CPC reactor develops nonideal flow distribution in the 90 °connections, which could influence the efficiency of this technology to be employed in UVA light processes of water treatment, such as photo-Fenton process.This later should serve as a starting point for future research.

Conclusions
This work presented a way to analyze the hydrodynamic behavior inside a CPC reactor.A 3D diffusion-convection model was implemented considering that the flow is not completely mixed inside the CPC reactor.A single-phase flow analysis was performed solving the RANS equations with the standard k−ε turbulent model, for Re > 3000.
The analysis of the turbulent flow simulations showed that near and inside the 90 °connectors and the union segments, the reactor presents low-and high-velocity zones owing to the inherent CPC geometry, showing that the CPC cannot be considered as an ideal plug flow reactor.An appropriate CPC reactor design must consider the flow behavior deviations caused by the perpendicular union segments of the CPC.Then, other connection angles should be tested to improve the hydrodynamics within the "zigzag tubes" and, consequently, to improve the mixing conditions in the photoreactor.
The comparison of flow visualization studies and the computational animations showed good agreement for the inflow velocities of 17.6, 22.2, and 24.4 cm•s −1 .Excellent agreement between theoretical and experimental RTD curves was obtained.This later shows the robustness of the proposed model, envisaging a future application in photo-Fenton-like processes for water treatment.The mathematical  International Journal of Photoenergy model proposed here can be helpful for scaling up the CPC photoreactor, where photoreactions should be adapted, although a deeper analysis with different photocatalytic reactions is needed to support this assertion.

3. 1 .
Turbulent Flow.Under turbulent flow conditions, the equations of the model for an incompressible fluid (water) can be stated as follows.The Reynolds averaged Navier-Stokes and the continuity equations are ρu

Figure 1 :
Figure 1: (a) Scheme of the CPC reactor.(b) Scheme of the system performed to carry out the experimental RTD studies and the flow visualizations.

Figure 2 :
Figure 2: (a) Simulation domain established to implement the tracer simulation.The marked distances (L = 50 cm, L = 100 cm, L = 117 cm, L = 150 cm, and L = 170 cm) represent the regions where velocity profiles were taken at z = 0 cm in the center of the tube.(b) Inset of the mesh employed in the simulations.

Figure 3 :Figure 4 :
Figure 3: Velocity magnitude field plot inside the CPC reactor for an inflow velocity of 22.2 cm•s −1 .

Figure 5 :
Figure 5: Comparisons of different pictures taken from the flow visualizations and the computational animations at different times of 5, 14, 19, and 24 seconds for an inflow velocity of 22.2 cm•s −1 .

Figure 6 :
Figure 6: Comparisons of experimental (solid line) and theoretical (dot line) RTD curves as a function of the dimensionless residence time at different inflow velocities showed inside the figure.