Grid independence study.
Abstract
The growing energy demand is expected to be met with increased oil and gas production. Hence, there is a need to design high-performance industrial centrifugal pumps. Recent improvements in CFD are considered as a valuable research tool to investigate the flow inside the pump and its influence on the performance of the centrifugal pump. The scope of the chapter is to emphasize the use of CFD and theoretical analysis for design and to show the prospect of improving the efficiency of a centrifugal pump. The chapter discusses the computational approaches to the CAD modeling and CFD simulation of the industrial centrifugal pumps, and the strategies and methodologies adopted. The chapter would be relevant and useful to both the pump designers, manufacturers, and industrial users.
Keywords
- centrifugal pump
- CFD
- geometric modeling
- computational modeling
- NPSH
- cavitation
1. Introduction
Centrifugal pump has wide application areas as it is being used in the sectors like agriculture, oil and natural gas, public water supply, sanitation, domestic, household utilities, petroleum refining, petrochemicals, mining, etc. That is why the centrifugal pump has a significant effect on the nation’s economy. The present chapter describes the steps in detail that include the design of industrial centrifugal pumps, construction of geometrical models of various components of centrifugal pumps, grid generation, governing equations, boundary conditions, discretization, CFD solver settings, and the importance of CFD in improving pump design and performance.
Despite wide applications, the design of the pump and its performance prediction using a conventional approach involves trial and error which is a time-consuming task. CFD is a robust tool for prediction of performance of the centrifugal pumps that can be used to analyze and design the pump for performance and cavitation prediction [1], and condition monitoring [2] with a better understanding of flow physics. CFD analysis of any problem of engineering interest consists of three major steps, namely, pre-processing, simulation, and post-processing.
2. Pre-processing for centrifugal pump
Pre-processing consists to define the domain of interest (i.e., creation of geometry), then dividing it into a finite number of elements known as computational grid or mesh generation of the flow domain, and formulation of the problem.
2.1 Geometrical modeling of a centrifugal pump
Modeling is a process to create the complex engineering model of an industrial machine or device that can be shaped into the desired model by assembling the different parts (called solid volumes) and thus the final solid model is a virtual replica of the actual product that can be functioned (for example, rotated) like a real product. Therefore, such a complex geometrical machine or device can be modeled (constructed) by any computer-aided design (CAD) software, such as CATIA, Solid works, ProE, AutoCAD, and also with the help of non-CAD software, like BladeGen, Ansys Design Modeler (DM), etc. Modeling of an industrial centrifugal pump is always a tedious task for engineers as it deals with complex and intricate shapes associated with the impeller and volute geometries [3, 4].
A two-dimensional geometry of a single-suction, single-stage industrial centrifugal pump having a double-volute casing and impeller with three blades is generated as per the drawings made available with the help of CAD software- CATIA. The two-dimensional geometry of the impeller and double volute of an industrial pump is then converted into three-dimensional geometry for further processing. The major dimensions of the centrifugal pump are furnished in Figure 1 shows the impeller and volute casing as separate entities, assembled and cut section of the centrifugal pump.
The three-dimensional pump geometry constructed in CATIA is imported to Ansys Design Modeler (DM) through Solid works using appropriate format to avoid loss of surface in the process and to ensure the accurate geometry. Next, the flow domain is extracted from the imported geometry after using capping option available in Ansys DM. The extracted flow domain requires cleanup before the meshing. A flow chart explaining the steps involved in the complete process is shown in Figure 2.
Wireframe of the flow domain after cleanup is shown in Figure 3 while parts of the final flow domain are shown in Figure 4 which is used for further processing.
A pump impeller consists of an array of blades (or vanes) arranged in a certain fashion and covered with the shrouds on either side. In order to study the effect of blade geometry on the performance of the centrifugal pump, pump impellers are constructed with six different blade outlet angles. The baseline impeller consists of three backward curved-twisted blades with a 16° outlet angle. The blade thickness is varied from 6 mm at the leading edge to 3 mm at the trailing edge with a wrap angle of 278°. The construction of the impeller blade with different blade outlet angle in CATIA software is a daunting and time-consuming task. Hence, many researchers [5, 6, 7, 8] relied on BladeGen tool available in the Ansys Blade Modular software in modeling the blade geometry of turbomachines. A two-dimensional meridional view of the impeller blade is shown in Figure 5, which is referred to as baseline profile. The top layer of the profile is termed as the shroud layer, while the bottom layer is known as the hub layer. The liquid flows around the blade profile radially and discharges at the outlet. Three-dimensional profile of a single blade of impeller is shown in Figure 6a, while the geometry of three blades of the impeller is shown in Figure 6b. The geometry of the blades thus created is imported from BladeGen to Ansys-Workbench. The extracted flow domain of a three bladed impeller is shown in Figure 7a.
2.2 Generation of computational grid
Grid generation (or meshing) is the next step required to perform after extraction of flow domain. It is the process of dividing the given flow domain into a number of small domains or parts called control volumes. It is seen from the literature survey that most of the researchers [8, 9, 10, 11, 12, 13, 14, 15, 16, 17, 18, 19] used unstructured tetrahedral elements for grid generation of the centrifugal pumps. Some of the researchers [20, 21] used both structured and unstructured element, while others [22] used combined unstructured hexahedral and tetrahedral elements for centrifugal pump. Zhang et al. [23] used tetrahedral grids for meshing double-volute casing while impeller was meshed with hexahedral grids.
Due to complex profile of the impeller and the volute casing, unstructured tetrahedral grid is used in the present study for all flow domains of the centrifugal pump using grid generation software available in Ansys-Workbench. Patch independent method has been used, which performs meshing from surface to volume, to maintain the quality of the grid to a great extent. The accuracy of the computational results depends upon the grid density and quality. Therefore, a high-density and high-quality grid is desirable to capture the complex flow phenomena, like flow separation and recirculation in the diffusing passages accurately [24]. However, high grid density increases computational time and memory. Therefore, a tradeoff between the computational cost and the grid density is required.
Grid independence test is performed to ensure the independency of solution with the grid size. This test is performed by refining the grid using patch independent algorithm. The number of elements are gradually increased from 1.6 million to 5.2 million in the present study to carry out the grid independence test. The results of the grid independence test are presented in Table 1. The results show that no significant change in the computed value of the head is observed from 4.2 to 5.2 million grid size. Therefore, in order to save computational time, the grid with around 4.16 million elements is chosen for further simulation. The corresponding average element size is 3.86 mm and the convergence time is 181 minutes.
Grid size | Average element size (mm) | CPU time (min.) | No of iteration | Head (m) |
---|---|---|---|---|
1,628,749 | 5.28 | 52 | 245 | 215.72 |
2,162,341 | 4.9 | 67 | 347 | 214.91 |
2,833,632 | 4.39 | 84 | 458 | 213.62 |
3,682,491 | 4.02 | 135 | 667 | 213.08 |
4,725,137 | 3.7 | 224 | 976 | 210.46 |
5,152,315 | 3.56 | 258 | 1014 | 210.56 |
Apart from size of element, the quality of a computational grid is also determined by the shape of the individual cells in the computational flow domain. The skewness of the element describes the shape of the element. CFD results are greatly affected by skewness and are therefore considered as one of the main measures for grid quality. Ansys-CFX provides a general guideline to determine the grid quality based on the value of skewness as reproduced in Table 2 for ready reference.
Value of Skewness | 0.0–0.25 | 0.25–0.50 | 0.50–0.75 | 0.75–0.90 | 0.90–0.99 | 1.00 |
Grid quality | Excellent | Good | Acceptable | Poor | Bad | Degenerate |
It is not always easy to reduce the skewness of all the elements in the acceptable limit as indicated by Table 1 in the complex flow domain as in the case of centrifugal pump. The literature [17, 23, 25, 26] also reports maximum skewness of centrifugal pumps’ grid between 0.82 to 0.95, indicating poor to bad quality of the grid as per Table 1. However, it is not only the high skewness of the elements but their number and location are also important. It is found that if the highly skewed elements are few and are away from the region of interest, they do not bring a significant effect on the computational results. Histogram in Figure 8 shows the frequency distribution of the skewness of the elements corresponding to 4.2 million elements in the present study. The histogram shows that insignificant number of elements are present above 0.5 skewness and almost negligible above 0.75 skewness.
The maximum skewness reported in the present study is 0.852 (affecting only 29 elements) and their locations are shown in Figure 9. It is observed in the present study that their presence does not influence the computational results. The final grid corresponding to 4.2 million elements is thus selected for further simulation as shown in Figures 10 and 11.
2.3 Governing equations
Various governing equations used in the present study to simulate the performance of the centrifugal pump are discussed in this section.
2.3.1 Continuity equation
2.3.2 Momentum equations
where
where
where,
where
For the simulation of steady case, time derivative term will be zero in Eqs. (1) and (2).
2.3.3 Turbulence model
Various turbulence models are available to capture the turbulence behavior of the flow. Thus, the selection of appropriate turbulence model for CFD analysis of the centrifugal pump is a difficult task. The literature review reveals that most researchers used two-equation turbulence models in turbo machinery application as they offer a good compromise between computational accuracy and computational effort. A number of researchers [2, 5, 6, 9, 12, 20, 21, 22, 23, 24, 27, 28] used the standard
Thus, four well-known two-equation turbulence models, namely standard
Inlet boundary condition | Outlet boundary condition | Turbulence model | Head (m) | Output power (kW) | Input power (kW) | Efficiency (%) |
---|---|---|---|---|---|---|
Total pressure (Pa) | Mass flow rate (kg/s) | Standard | 210.55 | 138.84 | 176.27 | 78.76 |
RNG | 210.49 | 138.80 | 176.15 | 78.79 | ||
203.53 | 137.19 | 174.00 | 78.84 | |||
SST | 204.62 | 134.93 | 172.57 | 78.18 | ||
Experimental results | 206.54 | 136.65 | 185.11 | 73.82 |
It is found that predicted result by
where
where model constants are
P
Scalable wall function is used to capture near wall flow physics in
This approach also incorporates the effect of wall surface roughness as dimensionless sand-grain roughness,
2.3.4 Turbulence intensity
The turbulence intensity is defined as the ratio of root mean square of fluctuating velocity (
Nominal turbulence intensity ranges from 1–5% depending up on the specific application. In absence of experimental data, the default turbulence intensity value of 3.7% is considered good estimate for nominal turbulence through a circular inlet.
It is found that many researchers [25, 37, 38, 39, 40, 41] used 5% turbulence intensity at the inlet boundary conditions for turbomachines, while Shahin et al. [27] used 2% turbulence intensity, Jafarzadeh et al. [20] used 1% turbulence intensity, Murmu et al. [42] and Alam et al. [43] investigated varied turbulence intensity at the inlet boundary condition.
Three standard turbulence intensity, 1%, 5%, and 10%, are tested in the present study for CFD simulation of flow through the centrifugal pump. The results are presented in Table 4 for comparison. The results show almost negligible variation in the value of head, output power, input power, and efficiency of centrifugal pump. Hence turbulence intensity equal to 5% is finally chosen for further study.
Turbulence intensity (%) | Head (m) | Output power (kW) | Input power (kW) | Efficiency (%) |
---|---|---|---|---|
1.0 | 210.5 | 138.83 | 176.26 | 78.76 |
5.0 | 210.5 | 138.83 | 176.26 | 78.76 |
10.0 | 210.5 | 138.84 | 176.27 | 78.77 |
2.3.5 Boundary conditions
While solving the Navier–Stokes equations and continuity equation, an appropriate boundary conditions need to be applied. Boundary conditions are a very important set of the properties and conditions applied on the surfaces of computational domains. These are required to define the flow field completely. The solid and fluid regions are generally represented by domains or cell zones while internal surfaces and boundaries are represented by the face zones. The data corresponding to boundary conditions are then assigned to these face zones. Each variable equation requires the meaningful values at the boundaries at the domain in order to generate the values in entire domain. Boundary conditions used by various researchers working in computational study of centrifugal pump are summarized in Table 5.
Authors | Year | Inlet | Outlet |
---|---|---|---|
Blanco-Marigorta et al. [26] | 2000 | Flow rate | Static pressure. |
Stickland et al. [9] | 2000 | Flow rate | Static pressure. |
Gonzalez et al. [10] | 2002 | Total pressure | A variable static pressure proportional to the kinetic energy at the outlet for their unsteady pump. |
Majidi [37] | 2005 | Mass flow rate | For all variables (with exception of pressure) a zero-gradient condition. |
Gonzalez and Santolaria [13] | 2006 | Total pressure | A pressure drop proportional to the kinetic energy at the outlet. |
Cheah et al. [14] | 2007 | Mass flow rate | Mass flow is being specified. |
Cheah et al. [38] | 2008 | Total pressure | Mass flow rate. |
Spence and Teixeira [44] | 2009 | Mass flow rate | Static pressure. |
Feng et al. [45] | 2010 | Total pressure | Mass flow rate. |
Perez et al. [16] | 2010 | Relative Pressure of 0 Pa | Mass flow rate. |
Houlin et al. [17] | 2010 | Velocity | Outflow. |
Li [46] | 2011 | Velocity | Mass flow rate |
Jafarzadeh et al.[20] | 2011 | Volume flow rate | Pressure. |
Hedi et al. [47] | 2012 | Total pressure of 1 atm | Mass flow rate. |
Kumar et al. [22] | 2013 | Maas flow rate | Static pressure. |
Bellary and Samad [5] | 2013 | Pressure | Mass flow rate. |
Lei et al. [48] | 2014 | Velocity | Pressure. |
Kim et al. [40] | 2014 | Pressure of 0 atm | Mass flow rate. |
Li [41] | 2014 | Absolute velocity | Zero Static pressure. |
Bellary and Samad [49] | 2015 | Pressure | Mass flow rate. |
Alemi et al. [25] | 2015 | Mass flow rate | Pressure. |
Siddique et al. [19] | 2017 | Static pressure | Mass flow rate. |
Deshmukh et al. [8] | 2017 | Static pressure of 1.01 kPa | Mass flow rate. |
After analyzing all the boundary conditions, it is found that the computational results of centrifugal pump corresponding to the boundary condition of total pressure at inlet and mass flow rate matches most closely with the experimental measurement. The inlet total pressure is known from the measured data corresponding to different discharge. The turbulence kinetic energy and turbulence dissipation rate at the inlet totally depends on the upstream history of the flow.
The inlet pipe and casing are considered as stationary reference frames while impeller is considered as rotating reference frame. These frames are coupled through frozen-rotor interface model. There are two interfaces, one connecting pipe and impeller and other connecting impeller and casing. Walls associated with impeller are considered as rotating walls while those associated with pipe and casing are considered as stationary walls. No-slip boundary conditions are applied over the impeller blades and casing walls. A list of boundary conditions used for the CFD simulation of the pump in the study is given in Table 6.
Parameters | Description |
---|---|
Inlet | Total Pressure |
Outlet | Mass flow rate |
Blades | Rotating wall |
Pipe | Stationary reference frame |
Impeller | Rotating reference frame |
Casing | Stationary reference frame |
Interface-1 (Between pipe outlet and impeller inlet) | Fluid–Fluid |
Interface-2 (Between impeller outlet and casing inlet) | Fluid–Fluid |
2.4 CFD solver settings
The governing equations along with boundary conditions are discretized using second order upwinding scheme. The discretized equations result in a set of algebraic equations. Ansys-CFX, an element based finite volume method (EbFVM) solver with a cell vertex formulation is used for the present study to solve the algebraic equations. Table 7 shows various solver settings used during the CFD simulation.
2.4.1 Convergence criteria
Ansys-CFX uses a multigrid (MG) accelerated incomplete lower upper (ILU) factorization technique for solving the discretized system of equations. This technique is iterative in nature. The measure of convergence of iterative solution is the residual which quantifies the error in the computational solution. In a CFD analysis, the residual quantifies the local imbalance of each conservative control volume equation. Thus, after specifying all the boundary conditions, numerical schemes, convergence criteria are specified to solve the problem.
Researchers used various convergence criteria for numerical simulation of centrifugal pumps. Feng et al. [45] taken convergence criteria 10−3. Majidi [37], Cheah et al. [14], Perez et al. [16], Hedi et al. [47], Li [46], Alemi et al. [25], Siddique et al. [19] used 10−4 residual, while Gonzalez et al. [10] used a residual of 10−5 for mass and momentum and 10−4 for
The computational effort and computational accuracy are always competing parameters. Thus, the accuracy of the computation in terms of root mean square (RMS) of residual up to10−6 is calculated with the corresponding computational effort for two different turbulence models,
2.4.2 Steady state flow simulation
Moving reference frame (MRF) allows the computational analysis of cases involving domains that are rotating relative to one another. Since MRF is based on the general grid interface (GGI) technology, this feature allows rotor/stator interaction in the investigation of turbomachines in Ansys-CFX. In GGI, a control surface approach is used to connect across the interface or periodic condition. This intersection algorithm allows the complete freedom to change the physical distribution and the grid topology across the interface. This permits the use of most appropriate meshing style for each component involved in the analysis. Many researchers [14, 15, 18, 20, 27, 39, 41, 45, 50] carried out computational investigation of centrifugal pump to assess its performance using MRF approach in Ansys-Fluent and Ansys-CFX.
The steady state CFD simulation is carried out using MRF approach considering the volute and pipe sections as stationary frame while impeller flow field as rotating frame. In this case, the relative position between volute casing and impeller flow field is considered fixed in time and space. The grids of pipe section, impeller, and volute that are generated separately with the help of tetrahedral elements are connected by means of a “frozen-rotor” interface. The interface treatment is fully implicit that preserves the flow field variation across the interface and does not adversely affect convergence of the overall solution.
2.4.3 Unsteady flow simulation
Transient/unsteady behavior can be caused by changing the boundary conditions of the flow or can be related to the flow where steady state condition is never reached, even when all other aspects of the flow conditions are not changing. For the unsteady simulation of the present problem, the surface fluxes at each side of the interface are first computed at the start of each time step at the current relative position. The dissimilar meshes at the pipe, impeller, and volute interfaces are connected by GGI connections to permit transient flow interaction between a stator and rotor passages across the sliding (transient rotor-stator/frame change) interface. This approach allows the accounting of all interaction effects between the components that are in the transient relative motion to each other across the interface. The interface position is updated at each time step as the relative position of the grid’s changes on each side of the interface. To determine the real time information, the transient simulations require appropriate time interval at which the Ansys-CFX solver calculates the flow field.
A few researchers [10, 22, 26, 27, 37, 42] also studied the transient CFD simulation. Three different time step sizes (3°, 6°, 9°) are compared for
Solver | Coupled |
---|---|
Analysis method | Multiple reference frame (MRF) or Frozen rotor method |
Steady/Unsteady state analysis | |
Reference Pressure | 1 atm |
Impeller rotation/step | Total no of time steps/6 revolutions | Time taken/revolution (ms) | Time per step size (ms) | Total time taken for 6 revolution (ms) |
---|---|---|---|---|
9° | 240 | 20.46 | 0.51 | 122.74 |
6° | 360 | 20.46 | 0.34 | 122.74 |
3° | 720 | 20.46 | 0.17 | 122.74 |
2.4.4 Cavitation simulation using Rayleigh–Plesset equation
In the present study, the steady state numerical simulation with cavitation is carried out with a multiple frames of reference (MRF) approach using the Rayleigh Plesset equation to investigate the cavitation in the centrifugal pump. The Rayleigh–Plesset equation provides the basis for the rate equation controlling vapor generation and condensation. The Rayleigh–Plesset equation that describes the growth of a gas bubble in a liquid is derived from a mechanical balance, assuming no thermal barriers to bubble growth. The equation is given as:
where
The rate of change of bubble volume is:
thus, the rate of change of bubble mass is:
The volume fraction
where
and the total inter-phase mass transfer rate per unit volume is:
This expression has been derived assuming bubble growth due to vaporization. The expression can be generalized to include condensation as follows:
where
where
To obtain an inter-phase mass transfer rate, the values of bubble concentration and radius are required. The Rayleigh–Plesset cavitation model uses the following default values for the model parameters as implemented in Ansys-CFX:
2.4.5 Acoustics simulation
Noise in the pump is produced primarily by the unsteady pressure field. To predict mid- to far-field noise, the methods based on Lighthill’s acoustic analogy offer sustainable alternative to the direct method. The acoustic analogy decouples the generation of sound from its propagation. Thus, enabling the separation of the flow solution process from the acoustics analysis. Therefore, in this approach, the near-field flow is obtained from the appropriate flow governing equations such as unsteady RANS equations. Then the sound is predicted with the help of analytically derived integral solutions of wave equations using determined flow.
2.4.6 The Ffowcs-Williams and Hawkings Equation for Acoustic Study
Ansys-Fluent offers an acoustic study method based on the Ffowcs-Williams and Hawkings (FW-H) formulation. The Ffowcs-Williams and Hawkings (FW-H) equation is essentially an inhomogeneous wave equation that is derived by manipulating the Navier–Stokes equations and the continuity equation. The FW-H formulation uses the most general form of Light hill’s acoustic analogy neglecting the interaction between fluid and solid. This formulation predicts sound generated by equivalent acoustic sources. ANSYS-Fluent uses a time domain integral formulation to compute time histories of sound pressure, or acoustic signals, at prescribed receiver locations. The FW-H equation can be written as:
where
In order to facilitate the use of generalized function theory and the free space Green function to obtain the solution, a mathematical surface represented by
For a Stokesi an fluid, the compressive stress tensor, P
The subscript 0 denotes the free-stream properties.
2.4.7 Proudman’s formula
Proudman [51] derived a formula for acoustic power generation by isotropic turbulence without mean flow using Light hill’s acoustic analogy. For a given turbulence field, the Proudman’s formula yields an approximate measure of the local contribution to total acoustic power per unit volume. Proudman’s original derivation neglected the retarded time difference. Later, the formula was re-derived by accounting for the retarded time difference. Both derivations provide acoustic power due to the unit volume of isotropic turbulence in (W/m3) as
where
Eq. (25) can be rewritten in terms of
where
In the present study, the FW-H model is used to measure acoustics in terms of the level of noise radiation induced by the inner flow field in the centrifugal pump encompassing the impellers and volute. In FW-H acoustic model, it is essentially required that all the receivers are located far away (at least at a distance of 1 m) from the primary sources of sound. Thus, for monitoring, 24 receivers, indicated by P1-P24, are arranged in circular surface at an angular gap of 15° is shown in Figure 12.
Receiver P7 is placed in line with the volute tongue and receiver P19 is placed in line with the volute splitter. To extract the relevant acoustic spectra, a Fourier transformation is applied connecting the acoustic signals found at these receivers. The sound pressure level (SPL) in decibel (dB) is calculated by:
where
It is necessary to derive a temporal intensity profile to obtain the intensity of noise radiation, involving a superposition of acoustic pressures at each Fourier frequency. In this regard, the total sound pressure level(TSPL) is introduced and expressed as:
Detailed analysis of cavitation detection in a centrifugal pump impeller using acoustic generation can be found in Jaiswal et al. [52].
3. Conclusions
Intensive computation coupled with geometric modeling helps the engineers and industrial users of the centrifugal pumps to investigate its performance characteristics [53] and cavitation prediction while dealing with multiple working fluids [54] and geometric modification of blades and its number [55, 56]. The present chapter discussed the computational strategies that encompasses the CAD modeling, computational grid generation, steps involved in the CFD solvers, and the various issues associated with it.
Further studies in this field may include computational analysis on a double-suction, double-volute centrifugal pump impeller [57] to investigate the effects of double-suction on its hydraulic performance and cavitation characteristics. Besides, optimization of impeller blades using surrogate modeling [58] can also lead to design of an improved centrifugal pump impeller.
References
- 1.
Rehman AU, Vinoth Kumar K, Jain A, Paul AR. Performance and cavitation prediction in an industrial centrifugal pump for different working fluids. In: Proceedings of First International Conference on Thermal and Fluid Engineering (ICTF-2017), 3-5 July 2017, Phuket (Thailand). 2017. pp. 36-42 - 2.
Rehman AU, Shinde S, Singh VK, Paul AR, Jain A, Mishra R. CFD based condition monitoring of centrifugal pumps. In: Proceedings of COMADEM 2013, 11–13 June 2013, Helsinki, Finland. 2013 - 3.
Rehman AU, Shinde S, Paul AR, Jain A. Effects of discharge on the performance of an industrial centrifugal pump. In: Proceedings of International Conference on Computing Techniques and Mechanical Engineering (ICCTME-2015), Oct. 1–3, 2015, Phuket (Thailand). 2015 - 4.
Rehman AU, Paul AR, Jain A. Effect of impeller volute interaction on performance of the centrifugal pump: A CFD approach. In: Proc. of Indian Conference on Applied Mechanics (INCAM-2017) at MNNIT Allahabad, July 5-7, 2017. 2017 - 5.
Bellary SAI, Samad A. Exit blade angle and roughness effect on centrifugal pump performance. In: ASME 2013 Gas Turbine India Conference. 2013 - 6.
Bellary, S.A.I. and Samad, A., 2015-a. Pumping crude oil by centrifugal impeller having different blade angles and surface roughness. Journal of Petroleum Exploration and Production Technology, 6l, pp.117-127. - 7.
Yun JE, Kim JH. Effect of surface roughness on performance analysis of centrifugal pump for wastewater transport. Transactions of the Korean Society of Mechanical Engineers B. 2014; 38 (2):147-153 - 8.
Deshmukh D, Siddique MH, Samad A. Surface roughness effect on performance of an electric submersible pump. In: ASME 2017 Gas Turbine India Conference. 2017 - 9.
Stickland MT, Scanlon TJ, Blanco-Marigorta E, Fernández-Francos J, González-Pérez J, Santolaria-Morros C. Numerical flow simulation in a centrifugal pump with impeller-volute interaction. In: Proceedings of the ASME, Fluids Engineering Division Summer Meeting. 2000 - 10.
Gonzalez J, Fernández J, Blanco E, Santolaria C. Numerical simulation of the dynamic effects due to impeller-volute interaction in a centrifugal pump. Journal of Fluids Engineering. 2002; 124 (2):348-355 - 11.
Zhou W, Zhao Z, Lee TS, Winoto SH. Investigation of flow through centrifugal pump impellers using computational fluid dynamics. International Journal of Rotating Machinery. 2003; 9 (1):49-61 - 12.
Gonzalez, J., Parrondo, J., Santolaria, C. and Blanco, E., 2006-a. Steady and unsteady radial forces for a centrifugal pump with impeller to tongue gap variation. Journal of Fluids Engineering, 128(3), pp.454-462. - 13.
Gonzalez, J. and Santolaria, C., 2006-b. Unsteady flow structure and global variables in a centrifugal pump. Journal of Fluids Engineering, 128(5), pp.937-946. - 14.
Cheah KW, Lee TS, Winoto SH, Zhao ZM. Numerical flow simulation in a centrifugal pump at design and off-design conditions. International Journal of Rotating Machinery. 2007; 83641 :1-8 - 15.
Bacharoudis EC, Filios AE, Mentzos MD, Margaris DP. Parametric study of a centrifugal pump impeller by varying the outlet blade angle. Open Mechanical Engineering Journal. 2008; 2 (5):75-83 - 16.
Perez J, Chiva S, Segala W, Morales R, Negrao C, Julia E, et al. Performance analysis of flow in a impeller-diffuser centrifugal pumps using CFD: Simulation and experimental data comparisons. In: V European Conference on Computational Fluid Dynamics EECMV, ECCOMAS CFD. 2010 - 17.
Houlin L, Yong W, Shouqi Y, Minggao T, Kai W. Effects of blade Numberon characteristics of centrifugal pumps. Chinese Journal of Mechanical Engineering-English Edition. 2010; 23 (6):742-747 - 18.
Cui B, Wang C, Zhu Z, Jin Y. Influence of blade outlet angle on performance of low-specific-speed centrifugal pump. Journal of Thermal Science. 2013; 22 (2):117-122 - 19.
Siddique MH, Bellary SAI, Samad A, Kim JH, Choi YS. Experimental and numerical investigation of the performance of a centrifugal pump when pumping water and light crude oil. Arabian Journal for Science and Engineering. 2017; 42 (11):4605-4615 - 20.
Jafarzadeh B, Hajari A, Alishahi MM, Akbari MH. The flow simulation of a low-specific-speed high-speed centrifugal pump. Applied Mathematical Modelling. 2011; 35 (1):242-249 - 21.
Hedi ML, Hatema K, Ridha Z. Numerical flow simulation in a centrifugal pump. International Renewable Energy Congress. 2010; 2010 :300-304 - 22.
Kumar S, Mohapatra SK, Gandhi BK. Investigation on centrifugal slurry pump performance with variation of operating speed. International Journal of Mechanical and Materials Engineering. 2013; 8 (1):40-47 - 23.
Zhang, Y.L., Zhu, Z.C., Dou, H.S., Cui, B.L., Li, Y. and Zhou, Z.Z., 2017-a. Numerical investigation of transient flow in a prototype centrifugal pump during Startup period. International Journal of Turbo & Jet-Engines, 34(2), pp.167-176. - 24.
Sagar D. Akshoy Ranjan Paul, Anuj Jain, “computational fluid dynamics investigation of turbulent separated flows in axisymmetric diffusers”, international journal of engineering. Science and Technology (IJEST). 2011; 3 (2):104-109 - 25.
Alemi H, Nourbakhsh SA, Raisee M, Najafi AF. Effects of volute curvature on performance of a low specific-speed centrifugal pump at design and off-design conditions. Journal of Turbomachinery. 2015; 137 (4):041009-041010 - 26.
Blanco-Marigorta E, Fernandez-Francos J, Parrondo-Gayo J, Santolaria-Morros C. Numerical simulation of centrifugal pumps. In: ASME Paper. 2000 - 27.
Shahin I, Abdelganny M, Abdellatif OE, Abdrabbo MF. Performance and unsteady flow field prediction of a centrifugal pump with CFD tools. In: Proceedings of ICFD 10: Tenth International Congress of Fluid Dynamics. 2010 - 28.
Paul AR, Jain A, Alam F. Drag reduction of a passenger car using flow control techniques. International Journal of Automotive Technology. 2019; 20 (2):397-410. DOI: 10.1007/s12239-019-0039-2 - 29.
Bhattacharyya S, Chattopadhyay H, Benim AC. Simulation of heat transfer enhancement in tube flow with twisted tape insert. Progress in Computational Fluid Dynamics. 2017; 17 (3) - 30.
Bhattacharyya S, Dey K, Hore R, Banerjee A, Paul AR. Computational study on thermal energy around diamond shaped cylinder at varying inlet turbulent intensity. Energy Procedia. 2019; 160 (2018):285-292 - 31.
Bhattacharyya S, Khan AI, Maity DK, Pradhan S, Bera A. Hydrodynamics and heat transfer of turbulent flow around a rhombus cylinder. Chemical Engineering Transactions. 2017; 62 (1987):373-378 - 32.
Bhattacharyya S, Benim AC, Chattopadhyay H, Banerjee A. Experimental and numerical analysis of forced convection in a twisted tube. Thermal Science. 2019; 23 - 33.
Bhattacharyya S, Das S, Sarkar A, Guin A, Mullick A. Numerical simulation of flow and heat transfer around hexagonal cylinder. International Journal of Heat and Technology. 2017; 35 (2):360-363 - 34.
Bhattacharyya S, Chattopadhyay H, Biswas R, Ewim DRE, Huan Z. Influence of inlet turbulence intensity on transport phenomenon of modified diamond cylinder: A numerical study. Arabian Journal for Science and Engineering. 2020; 45 (2):1051-1058 - 35.
Bhattacharyya S, Chattopadhyay H, Bandyopadhyay S. Numerical study on heat transfer enhancement through a circular duct fitted with Centre-trimmed twisted tape. International Journal of Heat and Technology. 2016; 34 (3):401-406 - 36.
Srivastav VK, Paul AR, Jain A. Capturing the wall turbulence in CFD simulation of human respiratory tract. Mathematics and Computers in Simulation. s; 160 :23-38 - 37.
Majidi K. Numerical study of unsteady flow in a centrifugal pump. Journal of Turbomachinery, Transactions of the ASME. 2005; 127 :363-371 - 38.
Cheah KW, Lee TS, Winoto SH. Unsteady fluid flow study in a centrifugal pump by CFD method. In: 7th ASEAN ANSYS Conference Biopolis, Singapore 30th and 31st October. 2008 - 39.
Mentzos MD, Vouros AP, Margaris DP, Filios AE, Kaldellis JK. The effect of the blade geometry in the velocity profile in a radial pump impeller. In: 5th International Conference on Experiments/ Process/ System Modeling/ Simulation/ Optimization. 2013. pp. 1-7 - 40.
Kim S, Lee KY, Kim JH, Choi YS. Numerical study on the improvement of suction performance and hydraulic efficiency for a mixed-flow pump impeller. In: Mathematical Problems in Engineering. 2014.A - 41.
Li WG. Mechanism for onset of sudden-rising head effect in centrifugal pump when handling viscous oils. Journal of Fluids Engineering. 2014; 136 (7):074501-074510 - 42.
Murmu SC, Bhattacharyya S, Chattopadhyay H, Biswas R. Analysis of heat transfer around bluff bodies with variable inlet turbulent intensity: A numerical simulation. International Communications in Heat and Mass Transfer. 2020; 117 :104779 - 43.
Alam MW, Bhattacharyya S, Souayeh B, Dey K, Hammami F, Rahimi-Gorji M, et al. CPU heat sink cooling by triangular shape micro-pin-fin: Numerical study. International Communications in Heat and Mass Transfer. 2020; 112 (February):104455. DOI: 10.1016/j.icheatmasstransfer.2019.104455 - 44.
Spence, R. and Amaral-Teixeira, J., 2009.A CFD parametric study of geometrical variations on the pressure pulsations and performance characteristics of a centrifugal pump. Computers and Fluids, 38(6), pp.1243-1257. - 45.
Feng J, Benra FK, Dohmen HJ. Application of different turbulence models in unsteady flow simulations of a radial diffuser pump. For schIngenieurwes. 2010; 74 (3):123-133 - 46.
Li WG. Effect of exit blade angle, viscosity and roughness in centrifugal pumps investigated by CFD computation. Task Quarterly. 2011; 5 :21-41 - 47.
Hedi ML, Hatema K, Ridha Z. Numerical analysis of the flow through in centrifugal pumps. International Journal of Thermal Technologies. 2012; 2 (4):216-221 - 48.
Lei T, Baoshan Z, Shuliang C, Hao B, Yuming W. Influence of blade wrap angle on centrifugal pump performance by numerical and experimental study. Chinese Journal of Mechanical Engineering. 2014; 27 (1):171-177 - 49.
Bellary, S.A.I. and Samad, A., 2015-b. Numerical analysis of centrifugal impeller for different viscous liquids. International Journal of Fluid Machinery and Systems, 8(1), pp.36-45. - 50.
Yong, W., Lin, L.H., Qi, Y.S., Gao, T.M. and Kai, W., 2009. Prediction research on cavitation performance for centrifugal pumps. International Conference on Intelligent Computing and Intelligent Systems, IEEE, 1(1), pp. 137-140. - 51.
Proudman I. The generation of noise by isotropic turbulence. Proceedings of the Royal Society A: Mathematical, Physical and Engineering Sciences. 1952; 214 - 52.
Jaiswal AK, Rehman AU, Paul AR, Jain A. Detection of cavitation through acoustic generation in centrifugal pump impeller. Journal of Applied Fluid Mechanics. 2019; 12 (4) - 53.
Mishra AK, Rehman AU, Paul AR, Jain A. Performance analysis of an impeller of a centrifugal pump using OpenFOAM. In: Proceedings of 6th International and 43rd National Conference on Fluid Mechanics and Fluid Power (FMFP-2016) 15-17 Dec. 2016. 2016 - 54.
Rehman AU, Paul AR, Jain A. Performance analysis and cavitation prediction of centrifugal pump using various working fluids. Recent Patents on Mechanical Engineering. 2019; 12 (3):227-239. DOI: 10.2174/2212797612666190619161711 - 55.
Rehman AU, Srivastava S, Jain A, Paul AR, Mishra R. Effect of blade trailing edge angle on the performance of a centrifugal pump impeller. In: Proceedings of COMADEM-2015. 2015 - 56.
Rehman AU, Yadav P, Paul AR, Jain A. Effect of number of blades on performance of a centrifugal pump. In: Proceedings of 6th International and 43rd National Conference on Fluid Mechanics and Fluid Power (FMFP-2016) 15-17 Dec. 2016, MNNIT Allahabad (India). 2016 - 57.
Kalyan DK, Rehman AU, Paul AR, Jain A. Computational flow analysis through a double-suction impeller of a centrifugal pump. In: Proceedings of 40th National Conference on Fluid Mechanics & Fluid Power (FMFP-2013), 12-14 December 2013, NIT Hamirpur, Himachal Pradesh. 2013 - 58.
Jaiswal AK, Siddique H, Paul AR, Samad A. Surrogate based design optimization of a centrifugal pump impeller. In: Engineering Optimization. 2021