Numerical simulation of a radial diffuser turbulent airflow

Applied Mathematics and Computation 189 (2007) 1491–1504 www.elsevier.com/locate/amc Numerical simulation of a radial diffuser turbulent airflow Alysson Kennerly Colaciti a, Luis Miguel Valdés López a, Hélio Aparecido Navarro b, Luben Cabezas-Gómez a,c,* a b Tecumseh do Brasil LTDA, Product Research & Development. Rua Cel. J.A. de Oliveira Salles, 478, Caixa Postal 54 – CEP 13565-900, São Carlos, SP, Brazil Departamento de Estatı́stica, Matemática Aplicada e Computação, Instituto de Geociências e Ciências Exatas, Universidade Estadual Paulista ‘‘Julio de Mesquita Filho’’, Av. 24-A, 1515, Cx. P178, CEP 13506-700, Rio Claro, SP, Brazil c Departamento de Engenharia Mecânica, Escola de Engenharia de São Carlos, Universidade de São Paulo, Av. Trabalhador São Carlense, 400-Centro, CEP 13566-590, São Carlos, SP, Brazil Abstract In the present work are presented results from numerical simulations performed with the ANSYS-CFX code. We have studied a radial diffuser flow case, which is the main academic problem used to study the flow behavior on flat plate valves. The radial flow inside the diffuser has important behavior such as the turbulence decay downstream and recirculation regions inside the valve flow channel due to boundary layer detachment. These flow structures are present in compressor reed valve configurations, influencing to a greater extent the compressor efficiency. The main target of the present paper was finding the simulation set-up (computational domain, boundary conditions and turbulence model) that better fits with experimental data published by Tabatabai and Pollard. The local flow turbulence and velocity profiles were investigated using four different turbulence models, two different boundary conditions set-up, two different computational domains and three different flow conditions (Rein – Reynolds number at the diffuser inlet). We used the Reynolds stress (BSL); the k–e; the RNG k–e; and the shear stress transport (SST) k–x turbulence models. The performed analysis and comparison of the computational results with experimental data show that the choice of the turbulence model, as well as the choice of the other computational conditions, plays an important role in the results physical quality and accuracy.  2007 Elsevier Inc. All rights reserved. Keywords: Radial diffuser flow; Turbulence models; Numerical simulation; ANSYS-CFX software 1. Introduction The Radial outward flow between stationary disks has industrial and scientific applications such as in radial diffusers (present in hermetic compressor reed valves), non-rotating air bearings and disk-type heat exchangers. Such flows are rather complex, having a pressure gradient either that is positive or negative depending on * Corresponding author. Address: Departamento de Engenharia Mecânica, Escola de Engenharia de São Carlos, Universidade de São Paulo, Av. Trabalhador São Carlense, 400-Centro, CEP 13566-590, São Carlos, SP, Brazil. E-mail addresses: [email protected] (A.K. Colaciti), [email protected] (L.M. Valdés López), [email protected] (H.A. Navarro), [email protected] (L. Cabezas-Gómez). 0096-3003/$ - see front matter  2007 Elsevier Inc. All rights reserved. doi:10.1016/j.amc.2006.12.029 1492 A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 the radial location and radius values. A positive pressure gradient, resulting from a decrease in the velocity with increasing radius, may lead to separation and secondary flows. In some cases, a flow that starts as a turbulent flow may revert to a laminar flow at some distance downstream [1,2]. Many investigations have been performed to study the laminar radial flow between parallel disks [3–9]. Livesey [3], Moller [4], Savage [5], Jackson and Symmons [6], among others, developed analytical and experimental studies; while Hayashi et al. [7], Raal [8], and Piechna and Meier [9] among others, developed numerical studies with the same aim. After these works other investigations were performed to study how a turbulent radial flow behaves between parallel disks. Two important experimental works concerning this kind of study are those developed by Tabatabai and Pollard [1] and Ervin et al. [2]. Recently, many other works have been developed to study more deeply the flow inside radial diffusers taking advantage of the flow details that Computational Fluid Dynamics (CFD) techniques allows one to obtain. Cyklis [10] investigated the suitability of CFD techniques for the analysis of compressor valves. Using the simplified geometry of a compressor valve consisting of a radial diffuser with axial feeding was computed the steady planar mass-flow rate as a function of pressure difference, the results being slightly lower than the measured data. Deschamps et al. [11] considered a turbulent flow using the Renormalization Group k–e model and fixed walls. The pressure distribution along the frontal disc showed a good agreement with the experimental data, for different valve openings and Reynolds numbers. In this work these authors obtained some flow details that were not possible to obtain with the previous models used in [12,13], where they used the k–e model for high Reynolds numbers and two versions of the k–e models for low Reynolds numbers. Perez-Segarra et al. [14] considering three different versions of the k–e model showed significant differences in the computed flow force and effective flow area. This agrees with the comparison of Ottitsch and Scarpinato [15] developed for different types of valves. In the next step using CFD techniques for compressor valves Matos et al. [16] simulated the fluid–structure interaction. The authors considered an axis-symmetric laminar flow around a circular plate with a prescribed pressure difference. The structure was modeled as a mass–spring system with a single degree of freedom. The gas force was found to be in phase with the harmonically varying pressure difference, except near valve closure when this force experiences a temporary drop. When both pressure difference and flow force become negative, the mass-flow rate at the exit becomes negative too. Possamai et al. [17] computed the laminar flow between concentric inclined disks and conclude that this flow is significantly affected by the inclination for inclinations as small as 0.1. For some combinations of Reynolds number, valve opening and inclination, the pressure distribution showed regions of negative pressure difference, which produce a restoring moment tending to force the disks to become parallel. In the work of Matos et al. [18] was computed an axi-symmetric turbulent flow around a circular plate, which was modeled as a mass–spring system. The CFD techniques, along with other simulation and experimental techniques, also were applied by Having [19], presenting a very detailed study of the flow through compressor valves. In the present paper four turbulence models are tested, comparing the obtained simulation results for a radial air diffuser flow with the experimental data of [1]. The influence of three computational parameters over the simulation results is also addressed. These parameters include the type of boundary condition at the lateral walls of the computational domain, the type of the employed computational geometry, and the inlet conditions through the inlet Reynolds number. Among the tested models the shear stress transport (SST) model proposed by Menter [20] and implemented into the ANSYS-CFX software, seems to be the best compromise for obtaining a good quality result with a reasonable computational cost. In the next section are presented succinctly the balance equations of each turbulence model. 2. Mathematical models The first three turbulence models belong to the two-equation class of turbulence models, namely the traditional k–e model [21], the RNG k–e model [22] and the SST model. The SST model was proposed in [20] from the k–x turbulence model, initially formulated by Wilcox [23]. The other turbulence model is a version of the Reynolds Stress Turbulence kind of model, using a differential equation to compute the Reynolds stresses. The models are presented in the above-mentioned order, considering only the main equations used in the numerical simulations. Model constants are also introduced. It is important to note that are presented the model definitions and formulation used in the ANSYS-CFX manual [24]. The main interest is to study how different A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 1493 models can lead to very different computational results only considering the default definition of each model, including the default boundary conditions. 2.1. Standard k–e model The standard k–e model [21] introduces two new variables into the equation system. One is for the computation of the turbulent kinetic energy, k, m2/s2; and the other is for the calculation of the turbulence eddy dissipation, e, m2/s3. The following equations are then obtained: Continuity equation: oq ~  ðqU Þ ¼ 0: þr ot ð1Þ Momentum equation:   oðqUÞ ~ ~ 0þr ~  leff ðrU ~ þ ðrUÞ ~ T Þ þ B; þ r  ðqU  UÞ ¼ rp ot ð2Þ where B is the sum of body forces, leff is the effective viscosity accounting for turbulence, and p 0 is the modified pressure. leff and p 0 are given respectively by leff ¼ l þ lt ; 2 p0 ¼ p þ qk: 3 ð3Þ ð4Þ The k–e model uses the eddy viscosity concept, assuming that the turbulence viscosity is computed by lt ¼ C l q k2 ; e ð5Þ where Cl is a model constant. The quantities k and e are computed directly from the resolution of the following differential transport equations:    oðqkÞ lt ~ ~ ~ þ r  ðqUkÞ ¼ r  l þ ð6Þ rk þ Pk  qe; ot rk    oðqeÞ ~ lt ~ e ~ þ r  ðqUeÞ ¼ r  l þ ð7Þ re þ ðC e1 Pk  C e2 qeÞ ot k re where Ce1, Ce2, rk and re are model constants and Pk is the turbulence production tensor due to viscous forces. Buoyancy forces are not considered in the present work. This last term is modeled as      ~  rU ~ þ rU ~ T 2 r ~  U 3lt r ~  U þ qk : Pk ¼ lt rU ð8Þ 3 If the flow is incompressible the mean velocity divergence is zero. In this case the second term of Eq. (8) does not contribute to the turbulence production. In the present simulations the flow is also considered as compressible. In these cases all the above terms are taken into account. The standard k–e model employs values for the constants that were found by a comprehensive data fitting for a wide range of turbulent flows. The values of these constants are C l ¼ 0:09; C e1 ¼ 1:44; C e2 ¼ 1:92; rk ¼ 1:00; and re ¼ 1:30: ð9Þ 2.2. RNG k–e model The RNG k–e model is based on renormalization group analysis of the Navier–Stokes equations [22]. The transport equations for turbulence generation and dissipation are the same as those for the standard k–e model, but the model constants differ. The equations for the momentum and continuity are also the same. 1494 A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 For the RNG k–e model the transport equation for turbulence dissipation becomes oðqeÞ ~  ðqUeÞ ¼ r ~ þr ot  lþ lt reRNG   ~ þ e ðC e1RNG Pk  C e2RNG qeÞ; re k ð10Þ where C e1RNG ¼ 1:42  fg ð11Þ and  g g 1  4:38 ; fg ¼ ð1 þ bRNG g3 Þ sffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffi Pk g¼ : qC lRNG e ð12a; bÞ The values of the constants are C lRNG ¼ 0:085; C e2RNG ¼ 1:68; rkRNG ¼ 0:7179; and reRNG ¼ 0:7179: ð13Þ 2.3. Shear stress transport (SST) model The other two-equation turbulence model refers to the shear stress transport model taken from [24]. This model was proposed by Menter [20], and grew from the denominated baseline k–x model in [24]. The baseline k–x model makes use of the k–e model in regions far away from the walls and the k–x Wilcox model (cf. [23]) near the surface. The SST model is an improvement of the baseline k–x model, taking into account the transport of the turbulent shear stress by a limitation of the eddy viscosity mt by the following equation: mt ¼ a1 k ; maxða1 w; SF 2 Þ ð14Þ where mt ¼ lt =q and S represents an invariant measure of the strain rate. F2 is a blending function, which restricts the limiter to the wall layer computed by F 2 ¼ tanhðarg22 Þ ð15Þ ! pffiffiffi 2 k 500m arg2 ¼ max : b0 xy 0 y 2 x ð16Þ with The turbulent kinetic energy k and turbulent frequency x are computed by the following relations:    oðqkÞ ~ lt ~ ~ þ r  ðqUkÞ ¼ r  l þ rk þ Pk  b0 qkx; ot rk3    oðqxÞ lt ~ 1 ~ ~ x ~ ~ þ r  ðqUxÞ ¼ r  l þ rk rx þ a3 P k  b3 qx2 : rx þ ð1  F 2 Þ2q ot rx2 x k rx3 ð17Þ ð18Þ The constants used in the SST model equations are b0 ¼ 0:09; a2 ¼ 0:44; a1 ¼ 5=9; b1 ¼ 0:075; b2 ¼ 0:0828; rk2 ¼ 1; rk1 ¼ 2; and rx1 ¼ 2; rw2 ¼ 1=0:856: ð19Þ The coefficients of the SST model are a linear combination of the corresponding coefficients of the underlying models: U3 ¼ F 2 U1 þ ð1  F 2 ÞU2 : ð20Þ It should be noted that the stress tensor computed from the eddy viscosity concept is used in Eq. (1) for the conservation of mass. 1495 A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 2.4. Reynolds stress turbulence (BSL) model The Reynolds stress turbulence model is based on the formulation of transport equations for all components of the Reynolds stress tensor and dissipation rate. The eddy viscosity concept is not used, and is solved a transport equation for Reynolds stresses in fluid. The transport equations are solved for the individual stress components. In this model is used a differential equation for the Reynolds stress transport computation, based on the turbulence frequency. Because the turbulence frequency, x is computed using the baseline k–x model, the present Reynolds stress model is denominated as the BSL Reynolds stress model following the denomination from [24]. There are various Reynolds stress turbulence models as those published by Launder et al. [25] and Speziale et al. [26]. The present BSL model has some differences in relations to these models. In this case the modeled equation for the Reynolds stresses is written as   oðqsij Þ oðU k qsij Þ 2 o  l  osij þ ¼ qP ij þ b0 qxkdij  qPij þ l þ t : ð21Þ ot oxk 3 oxk r oxk The turbulent frequency is modeled by Eq. (18) assuming other values for the constants presented in the equation. The values of these constants are presented in pages 85 and 86 of the ANSYS-CFX manual [24]. Two pairs of constants are assumed, one set for each simulated zone. In the first zone is used the x-based model constants. In the second zone is used the e-based model constant transformed to the x formulation (cf. [24]). The constant r* from Eq. (21) also assumes two values as a function of the modeled zone. The constitutive relation for the pressure–strain correlation is given by         _ 2 2 2 1 _ _ 0 Pij ¼ b C 1 x sij þ kdij  a P ij  P dij  b Dij  P dij  c k S ij  S kk dij : ð22Þ 3 3 3 3 The production tensor of Reynolds stresses is given by P ij ¼ sik oU j oU i þ sjk ; oxk oxk and 1 P ¼ P kk : 2 ð23a; bÞ The tensor D term only differs from the above equation in the dot-product indices: Dij ¼ sik oU k oU k þ sjk : oxj oxi ð24Þ The turbulent viscosity in the diffusion terms of the balance equations of the Reynolds stresses equation is computed as in the [23] k–x model: k : x In the above equations the constant coefficients are equal to ð25Þ lt ¼ q b0 ¼ 0:09; _ a ¼ ð8 þ C 2 Þ=11; _ b ¼ ð8C 2  2Þ=11; _ c ¼ ð60C 2  4Þ=55; C 1 ¼ 1:8; C 2 ¼ 0:52: ð26Þ For more detailed information about this model formulation one should be consult the above documentation [24] and the literature cited herein. The books by Tennekes and Lumley [27], Wilcox [23], Versteeg and Malalasekera [28] and Pope [29] present the theory of turbulence modeling more deeply. 3. Set-up of the numerical simulations In this section are described all the computational conditions assumed in the numerical simulations. In Figs. 1 and 2 are shown the two different computational domains used in simulations. The first one (see Fig. 1) it is composed of the inlet section, the two valve plates, the lateral walls and the outlet section. The second domain (see Fig. 2) is composed of all these sections, including an opening section, right after the plate diameter, D. In this case the outlet section is displayed after the opening section. The simulated geometry is 1496 A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 Fig. 1. Computational domain considering the outlet section situated at the disc diameter. Fig. 2. Computational domain considering an extension of the outlet section situated after the disc diameter. composed from two valve plates with diameter D and a central orifice of the diffuser of diameter, d ¼ 75 mm. The valve configuration is characterized by the diameter relation which equals to D=d ¼ 16. Each valve plate has a thickness of 25 mm. This is the height of the inlet region shown in Figs. 1 and 2. The separation between the plates is equal to 10 mm. The computational geometry (Figs. 1 and 2) was made rotating one lateral wall for 10, making a three-dimensional domain in the form of a wedge. In Figs. 1 and 2 are also shown six small lines, denoting the position where were obtained the experimental profiles of the mean time local gas velocity along the plate radius. These sections are those used to compare the numerical results with the experimental data. Before the specification of the different boundary conditions assumed it is specified which type of fluid was used for each simulation. In the case of the first geometry (Fig. 1) the air was simulated as an incompressible fluid using the software database (air at 25 C fluid type from ANSYS-CFX code). For the second geometry the air was considered as a compressible ideal fluid, but without any heat transfer with the walls and outlets, assuming an air temperature equal to 298.15 K in the entire domain. In this case was computed the total energy equation considering the working terms due to the viscous dissipation (cf. [24]). With the exception of the above difference, regarding the kind of fluid used in the numerical simulations for each geometrical configuration, the other parameters were tested for both geometrical configurations. Thus, besides the four different turbulence models, also were considered two different boundary conditions for the lateral walls of each geometry, and three different inlet conditions depending on the inlet Reynolds number. The following boundary conditions (BC) were assumed: • Inlet: The inlet velocity normal to the domain is specified in the negative direction regarding the Y-axes (this velocity changes for each assumed inlet Reynolds number). Medium turbulence intensity, I, and, eddy viscosity ratio (cf. [24]) are assumed. For the compressible fluid the inlet temperature is provided as equal to 298.15 K. A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 1497 Table 1 Computational mesh parameters Geometry type Total number of nodes Total number of elements Total number of faces Fig. 1 Fig. 2 1,244,489 343,008 2,742,344 956,403 203,293 66,946 • Outlet: A subsonic flow with an average static pressure is assumed, over the entire outlet region, and is equal to 0.0 Pa. At the outlet the fluid can flow only out of the domain. • Opening: A relative pressure of 0.0 Pa and a static temperature equal to 298.15 K is assumed (this kind of BC is used only for the compressible fluid). At the openings the fluid can flow in and out of the computational domain. Medium turbulence intensity and eddy viscosity ratio are assumed. • Lateral walls: For these walls are assumed two BC. One is a symmetry boundary condition, and the other is the free slip BC. At the symmetry BC the normal velocity at the wall is zero and the scalar variable gradients normal to the boundary are also zero. For the free slip walls, the velocity component parallel to the walls has a finite value, but the velocity normal to the wall, and the wall shear stress, are both set to zero. For the compressible fluid the walls are assumed as adiabatic. • Other walls: In this case the no slip BC is assumed, meaning that the fluid velocity at the wall has a zero value. For the compressible fluid the walls are assumed as adiabatic. For all the turbulence models used in the work were assumed the ANSYS-CFX software default turbulent wall functions. A detailed explanation about the formulation of these functions is presented in Volfang et al. [30]. The flow is simulated to obtain the steady state solution considering a maximum of 200 false time temporal iterations. These temporal iterations do not represent a truly transient flow behavior, and are used to achieve the steady state solution. In Table 1 are shown the main parameters assumed for the construction of computational meshes. The mesh used for the Fig. 1 geometry is much more refined than that used for the Fig. 2 geometry. Nevertheless, even considering these two different meshes the Fig. 2 geometry leaded to better simulation results, indicating how the computational domain greatly influences the results and flow behavior. This is discussed in more detail in the next section. Due to the great number of performed simulations other computational meshes were not considered for the present work. The computations were run out in parallel using a cluster with eight processors. 4. Numerical results In Figs. 3–6 are shown the profiles of the mean time local gas velocity at different radial positions, considering the four turbulence models, the two different BC at the lateral walls and the two computational geometries considered in the paper (see Figs. 1 and 2). In all figures are displayed the experimental data taken from [1] to be able to compare the numerical results. The displayed velocity profiles are disposed in the red lines shown in Figs. 1 and 2. We now discuss the results obtained. It is very important to note that the results are shown partially, due to the number of parameters analyzed and the space limitation. The first aspect addressed is related to the performance of the turbulence models in relation to the experimental data. Considering all displayed results it is seen clearly that the k–e and RNG k–e models lead to simulation results, which are not in agreement with the experimental data and also with the physics of the flow. The more distorted results obtained with these two turbulence models are those shown in Figs. 3 and 4, overall for the smaller and mean inlet Reynolds number values. For the high value Reynolds number (Figs. 3c and 4c) the velocity profiles are more adequate, but very inaccurate at the discs’ walls, where the expected no slip BC is not represented. This behavior shows well that these two turbulence models are adequate for high Reynolds numbers in regions far away from the domain walls. In fact there are several modifications of the k–e model for low Reynolds number flow simulation. Hrenya et al. [31] present a comparative study of 10 different versions of this k–e model type. Nevertheless, even considering these low Reynolds number k–e models, it is known that these models use complex non-linear damping functions for the wall treatments, leading to erroneous results for the flow at the walls. This conclusion can be extended even for high Reynolds number 1498 A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 Fig. 3. Mean velocity distribution across the discs gap at various radial locations, considering the geometry shown in Fig. 1, the symmetric BC at the lateral walls and the four turbulence models. (a) Rein ¼ 19; 096; (b) Rein ¼ 32; 804; (c) Rein ¼ 164; 441. flows as can be seen from Figs. 3c and 4c, where these two models fail to catch the right behavior at the disc’s walls. The same comments apply for the results displayed in Figs. 5 and 6, obtained for other geometrical configurations and fluid models (compressible fluid). In this case, the velocity profiles are more coherent in relation to the results of Figs. 3 and 4, mainly at the centerline, but have a very poor behavior at the channel walls. In several works Churchill and coworkers (cf. [32] and other related works) discussed and showed that the k–e turbulence type of models have determined failures, because they use the concepts of eddy viscosity and mixing length to compute the turbulent viscosity. The failures are associated with the unbounded character of the eddy viscosity and mixing length at some locations of channels, and also with the assumption of negative values over some adjacent to the walls finite regions, although the turbulent stresses remain well behaved. Considering all these comments and the presented results, it can be concluded that the simulation results of the turbulent diffuser flow obtained with the k–e and RNG k–e should be treated with care, to avoid obtaining erroneous conclusions about the flow structures and main characteristics. Analyzing the results obtained with the SST and BSL models, it is perceived that both models allow obtaining numerical results physically coherent and generally very adequate in relation to the experimental data. However, some differences between these two turbulence models are pointed out. In Figs. 3 and 4 are shown the results for the BSL model only for the smaller inlet Reynolds number ðRein ¼ 19; 096Þ. In the case of the SST model are displayed results only for Rein equals to 19,096 and 32,804. The main reason for not showing the other results is that in these cases the software does not converge inside the number of temporal iterations fixed, equally to 200 iterations. These iterations are related to false time iterations to obtain a steady state solution. In the case of the BSL model, the time step was reduced to obtain a converged solution, considering the quantity of equations that should be solved for this model. When it simulates the Fig. 2 geometry and fluid model, the above two models converge, except the BSL one for Rein ¼ 164; 441. The same conditions were considered in this case. Note that for the Fig. 1 geometry a very refined computational mesh was used A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 1499 Fig. 4. Mean velocity distribution across the discs gap at various radial locations, considering the geometry shown in Fig. 1, the free slip BC at the lateral walls and the four turbulence models. (a) Rein ¼ 19; 096; (b) Rein ¼ 32; 804; (c) Rein ¼ 164; 441. Fig. 5. Mean velocity distribution across the discs gap at various radial locations, considering the geometry shown in Fig. 2, the symmetric BC at the lateral walls and the four turbulence models. (a) Rein ¼ 19; 096; (b) Rein ¼ 32; 804; (c) Rein ¼ 164; 441. 1500 A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 Fig. 6. Mean velocity distribution across the discs gap at various radial locations, considering the geometry shown in Fig. 2, the free slip BC at the lateral walls and the four turbulence models. (a) Rein ¼ 19; 096; (b) Rein ¼ 32; 804; (c) Rein ¼ 164; 441. (see Table 1), approximately three times more refined than that used for the Fig. 2 geometry. However, even using this fine mesh some turbulence models do not converge for the considered number of iterations. For the Fig. 2 geometry only one simulation case does not converge. Considering only the results displayed in Figs. 3 and 4, it is noted that the BSL model leads to more correct results, at least for the low inlet Reynolds number (Rein ¼ 19; 096) for which both models can be compared. The more accentuated differences between the models, are observed at the radial coordinate r=R ¼ 0:98, where the SST model does not present a very symmetric profile. This behavior is not correct, because at this radial distance the flow dissipates the initial asymmetry due to the cross-stream momentum transfer [1]. However, this does not mean that the SST model leads to erroneous results for the other flow cases, as can be observed in Figs. 3b and 4b. For this value of Rein (Rein ¼ 32804) the SST model presents a more coherent behavior in relation to the experimental data, showing the asymmetry at r=R ¼ 0:98, but to a less extent. From the results shown in Figs. 5 and 6, we can note that both the models present a very similar behavior showing small differences between each other and in comparison with the experimental data. For these simulations, the SST model converged for all the tested cases, contrary to the BSL model, which does not converge for the higher value of Rein . Thus, even knowing that the BSL model is more universal, due to the use of transport equations for the Reynolds stress computations, the present results indicate that the SST model can be preferred for simulating different flow conditions, characteristics of a design phase of any engineering project. In fact, the BSL model is more time consuming that the SST model, leading in the case of Figs. 5 and 6, to the results that are very similar and of the same quality. In Table 2 are presented the values of the Table 2 Comparison of the running computational time for the BSL and SST models Turbulence model Rein ¼ 19; 096 (Symm. BC) Rein ¼ 32; 804 (Symm. BC) Rein ¼ 19; 096 (free BC) Rein ¼ 32; 804 (free BC) SST BSL 42m58s 1h2m59s 47m4s 1h4m6s 43m41s 1h3m5s 46m45s 1h3m51s A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 1501 computational times for these two models for some of the performed simulations. As can be seen, the SST has a very small computational time regarding the BSL model. Considering this advantage of the SST model and the good results obtained with this model, it seems that this turbulence model is a good choice for numerically simulating the diffuser turbulent flow. Focusing on the influence of the type of BC applied for the lateral walls over the studied gas turbulent flow inside a diffuser, the results show that this influence is very small in all the analyzed cases. The only slight differences are perceived for the results of Rein ¼ 164441 displayed in Figs. 5c and 6c. As seen in these pictures, the k–e and RNG k–e models depend more on the type of this BC than the SST model. Making a careful observation it can be noted that the symmetric BC is more adequate to the kind of flow simulated in comparison with the free slip BC. It should be commented that the use of these BCs is a necessary step in order to decrease the required computational time. The risk of this type of assumption is the loss of tri-dimensional flow effects or the formation of artificial flow structures. However from the obtained results, it is noted that for the kind of flow studied, both these two types of BCs represent the flow behavior well. A more pronounced influence over the diffuser turbulent flow is noted when compared the type of the computational domain and fluid type employed in the simulations. Comparing the results from Figs. 3 and 4 with those represented in Figs. 5 and 6, it is noted that the extended computational domain (see Fig. 2) allows us to obtain better computational results for all the tested turbulence models, including both the BCs at the domain lateral walls. This was achieved even using a coarser mesh as indicated in Table 1. This points to the fact that Fig. 7. Velocity distribution between the discs gap along the diffuser radius. (a) distribution for Fig. 1 geometry, (b) distribution for Fig. 2 geometry. 1502 A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 the type of computational domain used is an important aspect to be taking into account while performing CFD numerical simulations. Many simulations in the literature, of problems similar to the present one, use only the geometry shown in Fig. 1 when the disc’s radius is higher in relation to the diffuser orifice radius. Nevertheless, when turbulent flows are simulated, as in the present one, this type of computational geometry exerts a considerable influence over the simulation results. In the present case it is perceived that even if the flow has a symmetrical characteristics near the outlet, properly of laminar flows, the assumed outlet geometrical configuration influences to a very high degree the numerical results. Note that the higher differences in the results of simulations for the two types of computational domains are observed at the r=R ¼ 0:98 crosssection. In Fig. 7 are plotted the velocity distribution profiles situated on a central plane with regard to the lateral walls along a diffuser radius. Fig. 7a shows the velocity distribution for the Fig. 1 geometry. Fig. 7b shows the same distribution for the Fig. 2 geometry. Alongside in Fig. 7b are also shown the streamlines in order to note that the Fig. 2 geometry allows simulating in more detail the flow behavior in the outlet zone. From Fig. 7a and b it is seen that the velocity distribution is very similar in both cases, until the flow reaches the outlet region. For the first geometry (Fig. 1) it is assumed that the flow is fully developed in this region setting the outlet BC. In the second geometry case the flow is simulated extending the outlet region domain, situating the outlet BC at some distance away from the plate diameter, D. In this case the opening type of BC is also used at the other two surfaces. This outlet configuration leads to different velocity profiles and also to some low velocity flow recirculations, which are not considered in the first geometry case due to the domain set-up. This observation support is the conclusion that the outlet geometry type and consequently the disposition of BCs at the outlet influence in a high degree the flow behavior near this region. The above commented conclusion is reinforced observing the profiles for the turbulent eddy viscosity shown in Fig. 8. These results were obtained for the higher Reynolds number (Rein ¼ 164; 441) at r=R ¼ 0:98 considering only the SST model for each geometrical configuration. It is noted that the turbulent eddy viscosity assumes different values for both models, being the great differences in a central channel region having a maximum relative error approximately equal to 15 %. Other turbulence parameters such as the turbulence kinetic energy, frequency and eddy dissipation also have significant differences with maximum errors of the same order. These errors can be considered high enough showing how the computational domain geometry configuration influences the simulation results for turbulent flows. Fig. 8. Turbulent eddy viscosity, lt, across the discs gap at r=R ¼ 0:98 and Rein ¼ 164; 441, considering the SST turbulence model for Figs. 1 and 2 geometries. A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 1503 For instance, it should be noted that besides the difference in the computational domain geometry in the present work are used two different fluid models, where one is incompressible and the other considers the compressibility effects on the flow turbulence. Thus, it cannot associate all the reported results’ differences only for the type of computational domain. Nevertheless, the simulations for the compressible fluid were performed assuming an adiabatic flow with the same inlet and outlet flow static temperatures. From Fig. 7 it is noted that the velocity distributions are qualitatively and quantitatively very similar. Considering the highest inlet Reynolds number (Rein ¼ 164; 441) is was found that the maximum Mach number from all simulations including both types of geometries was approximately equal to 0.281 for each fluid model. Thus, it can be concluded that the fluid type influence over the computational results is very small. The computational domain is the parameter which is contributing more for the presented results’ differences. 5. Conclusions In the present work is shown that the use of one or another turbulence model depends on a compromise between the quality of the results, the number of simulations needed and the geometrical and computational characteristics employed in the simulations. Using as a base the present simulation results it can be affirmed that for the turbulent diffuser flow simulation the SST model is a good choice, considering the use of the BSL model for a comparative purpose for some simulation cases. The use of the k–e and RNG k–e models is not recommended, even if these models are more stable from the numerical point of view and consume less computational time. In any case, the obtained results with these last two models are less correct when compared with the experimental data and physically incorrect at the walls. The numerical results confirm the poor influence exerted over the flow by the type of BC applied at the lateral walls. Nevertheless, we recommend the use of the symmetric BC based on the results shown for the SST model at Rein ¼ 16; 441 and the Fig. 2 geometry. Finally, it was found that the type of computational domain can exert a significant influence over the simulation results, even if the domains only differ in the exit zone configuration. It is very important to note that for turbulent flows this region is characterized by complex flow structures and should be modeled with caution. Acknowledgement The authors fully acknowledge the support obtained from the Tecumseh do Brasil LTDA Company for the development of this research work. References [1] M. Tabatabai, A. Pollard, Turbulence in radial flow between parallel disks at medium and low Reynolds numbers, J. Fluid Mech. 185 (1987) 483–502. [2] J.S. Ervin, N.V. Suryanarayana, H.C. Ng, Radial, turbulent flow of a fluid between two coaxial disks, ASME J. Fluids Eng. 111 (1989) 378–383. [3] J.L. Livesey, Inertia effects in viscous flows, Int J. Mech. Sci. 1 (1960) 84–88. [4] P.S. Moller, Radial flow without swirl between parallel discs, Aeronaut. Quart. 14 (1963) 163–186. [5] S.B. Savage, Laminar radial flow between parallel plates, ASME J. Appl. Mech. 31 (1964) 594–596. [6] J.D. Jackson, G.R. Symmons, An investigation of laminar radial flow between two parallel discs, Appl. Sci. Res. Sect. A 15 (1965) 59–75. [7] S. Hayashi, T. Matsui, T. Ito, Study of flow and thrust in nozzle-flapper valves, ASME J. Fluid Eng. 97 (1975) 39–50. [8] J.D. Raal, Radial source flow between parrallel discs, J. Fluid Mech. 85 (1978) 401–416. [9] J.R. Piechna, G.E.A. Meier, Numerical investigation of steady and unsteady flow in valve gap, in: Proceedings of the International Compressor Engineering Conference. Purdue, 1986, pp. 1–14. [10] P. Cyklis, CFD simulation of the flow through reciprocating compressor self-acting valves, in: Proceedings of the International Compressor Engineering Conference, Purdue, 1994, pp. 427–432. [11] C.J. Deschamps, R.T.S. Ferreira, A.T. Prata, Turbulent flow through valves of reciprocating compressors, Proceedings of the International Compressor Engineering Conference, Purdue, 1996, pp. 377–382. [12] C.J. Deschamps, R.T.S. Ferreira, A.T. Prata, Application of the it k–e model to turbulent flow in compressor valves, in: Proceedings of the 2nd Brazilian Thermal Science Meeting. São Paulo, Brasil, 1988, pp. 259–262. 1504 A.K. Colaciti et al. / Applied Mathematics and Computation 189 (2007) 1491–1504 [13] C.J. Deschamps, R.T.S. Ferreira, A.T. Prata, Turbulent flow modeling in presence of stagnation recirculation, acceleration and adverse pressure gradient, in: Proceedings of the X Brazilian Congress of Mechanical Engineering, vol. 1, 1989, pp. 57–60. [14] C.D. Perez-Segarra, J. Cadafalch, J. Rigola, A. Oliva, Numerical study of turbulent fluid-flow through valves, in: Proceedings ImechE conference transaction. C542/021, 1999, pp. 399–408. [15] F. Ottitsch, P. Scarpinato, CFD a viable engineering tool for compressor valve design or just a toy? in: Proceeding International Compressor Engineering Conference, Purdue, 2000, pp. 423–428 (2000). [16] F.F.S. Matos, A.T. Prata, Deschamps, Numerical analysis of the dynamic behaviour of plate valves in reciprocating compressors, in: Proceedings ImechE Conference Transactions, C542/031, 1999, pp. 453–462. [17] F.C. Possamai, R.T.S. Ferreira, A.T. Prata, Pressure distribution in laminar radial flow through inclined disks, Int. J. Heat Fluid Flow. 22 (2001) 440–449. [18] F.F.S. Matos, A.T. Prata, C. Deschamps, Numerical simulation of the dynamics of reed type valves, in: Proceedings of the International Compressor Engineering Conference, Purdue, 2002, p. C15-2. [19] R.A. Having, Flow and Plate Motion in Compressor Valves, Ph.D. Thesis, University of Twente, Enschede, Netherlands, 2005. [20] R.F. Menter, Two-equation eddy-viscosity turbulence models for engineering applications, AIAA J. 32 (8) (1994) 269–289. [21] B.E. Launder, D.B. Spalding, The numerical computation of turbulent flows, Comput. Methods Appl. Mech. Eng. 3 (1974) 269–289. [22] V. Yakhot, S.A. Orszag, S. Thangam, T.B. Gatski, C.G. Speziale, Development of turbulence models for shear flows by a double expansion technique, Phys. Fluids A 4 (7) (1992) 1510–1520. [23] D.C. Wilcox, Turbulence Modeling for CFD, DCW Industries, La Cañada, CA, 1993. [24] ANSYS-CFX Solver Theory manual, Release 10.0, 1996. [25] B.E. Launder, G.J. Reece, W. Rodi, Progress in the developments of a Reynolds-stress turbulence closure, J. Fluid Mech. 68 (1975) 537–566. [26] C.G. Speziale, S. Sarkar, T.B. Gatski, Modelling the pressure–strain correlation of turbulence: an invariant dynamical systems approach, J. Fluid Mech. 277 (1991) 245–272. [27] H. Tennekes, J.L. Lumley, A First Course in Turbulence, MIT Press, Cambridge MA, 1972. [28] H.K. Versteeg, W. Malalasekera, An Introduction to Computational Fluid Dynamics. The Finite Volume Method, Prentice Hall, UK, 1995, 257 p. [29] S.B. Pope, Turbulent Flows, Cambridge University Press, UK, 2000, 771 p. [30] V. Volfang, E. Thomas, M. Florian, Heat transfer predictions using advanced two-equation turbulence models, CFX Technical Memorandum-CFX-VAL10/0602, 2002. [31] C.M. Hrenya, E.J. Bolio, D. Chakrabarti, J.L. Sinclair, Comparison of low Reynolds number k–e turbulence models in predicting fully developed pipe flow, Chem. Eng. Sci. 50 (12) (1995) 1923–1941. [32] S.W. Churchill, Progress in the thermal sciences: AIChE Institute Lecture, AIChE J. 46 (9) (2000) 1704–1722.