Simulation of air flow in the typical boiler windbox segments

Transcription

1 Advances in Engineering Software 33 (2002) Simulation of air flow in the typical boiler windbox segments C. Bhasker* BHEL R&D Division, Vikasnagar, Hyderabad , India Received 6 June 2002; accepted 31 July 2002 Abstract Simulation of turbulent air flow distribution in CFBC furnace, wherein primary air is entrained through inlet duct system called windbox, is attempted through state of art CAD/CFD softwares. Establishment of flow in windbox channel, distributed plate nozzle and combustor is complicated, due to sharp turns and presence of several solid boundaries makes the fluid flow highly turbulent. Hence, the simulation process is aimed in different parts to understand the flow behavior in each of the component associated with windbox. Towards this, the present paper develops the basic understanding for airflow distribution in windbox channel, wherein air exit is considered only through 6 3 array of distributed plate nozzle bottom faces. This analysis also highlights that recirculation flow, at several locations of windbox channel/distributed plate nozzle, which aids to generate high pressures zones and severe turbulent fluctuations. These effects in turn leads to unequal air-flow at exit, which are unable to carry the incoming crashed coal particles and lime stones to furnace for efficient combustion. q 2002 Elsevier Science Ltd. All rights reserved. Keywords: CFBC boiler; Air flow; Windbox channel; Distributed plate nozzles; Combustor geometry; Multi-block grids; Simulation of flow; Recirculation flow; Unequal air flow 1. Introduction Over the last decade, circulating fluidized bed combustion (CFBC) technology has demonstrated its ability [1] to reliably burn a wide range of fuels in the large industrial and utility steam generators, while meeting stringent emission requirements. Recognizing this, Indian industries have already opted for CFBC boilers for their new plants [2,3]. However, Indian coals are characterized by high ash content, i.e..30%, high volatile matter.15% and high abrasive ash as reported in Ref. [4]. Due to these coal characteristics, the components of CFBC suffers surface erosion by particle impacts, resulting to performance degradations. Therefore, there is a need to improve overall cycle efficiency and minimize environmental impacts, while controlling the emission rates. One of the component of CFBC is primary air-inlet system to boiler furnace, wherein experience of plant manufacturers concern is mal-distribution of air [5 7], due to momentum and pressure losses and hence, inefficient combustion, high burner resistance and high emission rates. * Tel.: þ ; fax: þ address: bskr2k@yahoo.com (C. Bhasker). Equal distribution of air to burners is required for optimum performance. Simple modification can be made to redistribute the air and correct existing air unbalances. These modifications require the knowledge of the existing flow pattern in primary air-inlet system. Conventional engineering analysis rely heavily on empirical correlations and experience to develop boiler and auxiliary equipment designs. Today s design processes must be more accurate, while minimizing development costs to compete in a world economy. This forces engineering companies to take advantage of design tools, which augment existing experience and empirical data, while minimizing cost. One tool, which excels under these conditions are numerical modeling through computational fluid dynamics techniques. The goal of numerical simulations are to improve the design of new or existing boiler components by optimizing the flow distribution. Examples of boiler related numerical applications include furnaces, air supply ducts, windboxes, coal piping, precipitators, pulverizers, burners and scrubbers. The simulation is aimed with the use of computational fluid dynamic softwares, executing on high speed, large memory workstations. Numerical modeling has significant cost advantages, when compared to physical modeling and /02/$ - see front matter q 2002 Elsevier Science Ltd. All rights reserved. PII: S (02)

2 794 field testing. Also numerical modeling provides additional insight into the physical phenomena being analyzed and flexibility, with which, geometric changes can be studied. The commercially procured software from AEA s CFX- TASCflow is employed in the present paper to understand the air flow firstly in windbox channel and subsequently in distributed plate nozzle and also through array of nozzles. TASCflow solver is an advanced general purpose software, which works on PC NT and Unix workstations with advance features in terms of multi-block grid connections, boundary conditions, choice of discretization schemes and solution methods. The solver has been extensively applied to several complex industrial systems and obtained good success, whose details are outlined in Refs. [8 11]. 2. Description of problem The CFB process utilizes a fluidized bed combustor in which crushed coal and lime stones are suspended in a stream of upward flowing air. Due to high velocities of gas, the fine particles from coal fed pipes are carried out to combustor. Combustion air is introduced into furnace at multiple ports. About 40% combustion air is passed through windbox as primary air, as shown in Fig. 1 and the balance air is admitted as secondary air, through multiple ports in the walls of combustor. Modeling of burners and overfire air ports requires the proper air distribution in the windbox channel so that the losses in primary air-inlet system are minimum. Windbox is used to transport the balanced air flow, which mixes with coal and lime stones for efficient combustion in boiler. Windbox typically involves inlet duct, channel, distributed plate nozzles of the order several hundreds as shown in Fig. 2, is proposed to use in flow solver, which comprises 975 grid blocks, 495 grid interfaces and runs into 500,000 grid points. Three-dimensional flow analysis helps to reduce turning losses and burner resistance (i.e. windbox to furnace differential pressure). This is one of the source for air-imbalance and means that higher burner resistance will offset some of the influence from turning losses and estimation of these parameters for the above grid needs heavy computational resources in terms of high virtual memory. Numerical simulation models are tends to large due to complex flow structure in primary air-inlet system even with scale down models due to presence of typical configured nozzles. Domain discretization process comprises several thousands of structured multi-block grids for coarse grid flow analysis, which runs into millions of grid points. Problem setup takes considerable time for elimination of several walls in the computational domain. To avoid the solver failure for computation of flow in such a large size geometrical problem, it is aimed to Fig. 1. CFBC sketch showing primary inlet housing for CFD modeling.

3 795 Fig. 2. Computational grid primary inlet air housing with several hundred nozzles. study the flow pattern in different steps. Towards this, the present paper simulates the turbulent flow firstly in lower portion of windbox channel, whose top surface is provided nozzles bottom faces are placed in staggered array of rows and columns. Using appropriate flow conditions flow simulation has been carried out in single nozzle and array of nozzles. 3. Geometry creation The dimensions of windbox of CFBC power plant is typical primary air housing of windbox is about m height and 7.21 m width. At 6.8 m height of windbox, about 400 annular nozzles with different radii of cylinders embedded in a single nozzle and several such nozzles are placed in staggered rows on the distributed plate. The flow, which is entering from the side duct to windbox channel and takes different turns in the annular nozzles and leaves from the outer annular region towards outlet. Though the geometry has been created for lower portion of windbox using the SDRC-IDEAS software initially, further geometric modeling and grid generation has developed using ICEM CAD software. 4. Grid generation A state-of-art CAD/Grid generation software package IDEAS from SDRC/USA is used to generate

4 796 three-dimensional structured multi-block grid for windbox channel and side duct. The volume of multi-block grid points are generated with the help of simulation software module features, as universal file type, has been imported in the flow solver. The resultant grid contains about 100,000 grid points, as universal file, after importing in TASCflow solver, is shown in Fig. 3, which is free from negative volume and are in allowable limits of required skew angles. Using ICEM-CFD Powermesh software, computational grid for nozzle portion has been generated separately, is shown in Fig. 4. The grid comprises about 19 grid blocks comprises about 10,000 grid points are however, contains walls in flow domain, has been eliminated by physical connection of corresponding faces in respective grid blocks. Using the grid transformation features in solver, computational grid for array of 6 3 nozzles on the distributed plate has been generated and shown in Fig. 5. This grid is shown at the wall boundary, after removal of walls in rows and columns of nozzles and bottom and top portions in the computational domain are indicating inlet and outlet regions. To avoid flow blockage between different segments in the nozzles, required physical connections have been made between corresponding grid planes. 5. Flow solver The TASCflow commercial software package was used to compute the flow in windbox channel, and distributed plate nozzle. This software solves the threedimensional Navier Stokes equations in strong conservative form. A collocated variable arrangement is used to solve primitive variables (pressure, Cartesian velocity components) in stationary and rotating coordinate system. Multi-block boundary fitted grids with local grid refinements and physical connections of different types between grids helps to solve the problem with more ease. The transport equations are descretized using a conservative finite volume method. Turbulence effects are modeled using standard two equation k 1 model. A second order accurate skew upwind difference scheme with physical advection correction scheme is employed. A coupled algebraic multi-grid methods solves the system Fig. 3. Computational grid for lower portion of air housing.

5 Author's Personal Copy Fig. 4. Velocity vectors at different locations of lower portion of air housing. Fig. 5. Flow lines at different locations of lower portions of air housing. 797

6 798 of equations. Detailed descriptions for the mathematical formulation and approximation are available in Ref. [12]. 6. Boundary conditions and solution To establish the flow simulation process, it has been considered that turbulent incompressible air mass flow of order 64 kg/s is entered at inlet duct of wind box. Different cases have been obtained by applying the pressure (below/above atmospheric and atmospheric conditions) at the windbox exit. It is also considered that entrained fluid is turbulent, whose intensity and length scales are of order 3 and 2%, respectively. With the help of more guidelines [13] concerned to initial estimates, time step, etc., solution is marched on the grid points in the computational domain, till the maximum residuals for each scalar, i.e. mass, momentum, turbulence intensity and length scalars are reached to the target value After obtaining the successful converged solution, analysis has been repeated for the flow in distributed plate nozzle. 7. Discussion of results After obtaining the converged results, the result files, i.e..rso, are loaded into post processing and flow parameters in terms of velocity vectors, streak lines, pressure and turbulence effects are visualized in different planes of lower portion of windbox. The velocity distribution at different locations of windbox are shown in Fig. 6. From the graph, it is seen that velocity distribution shows lot of recirculation flows, which, in fact, increases over height of windbox channel. As a result, the uniform velocity which is supposed to enter with equal magnitudes in distributed plate nozzles are unequal. This behavior also clearly observed in the streakline plots shown in Fig. 7, wherein flow lines on speed scale, in computational domain, travel towards exit after creating the low velocity regions at bottom, right, left corners on top side of lower portion of windbox. The behavior of velocity components creates low pressure regions at recirculation flow zones where turbulence effects are prevailing in those regions are observed in Figs. 8 and 9. To visualize the flow from the windbox channel to distributor plate nozzles, turbulent incompressible air flow through single nozzle is simulated and several parametric results in different planes of nozzle are obtained. The velocity vectors at different locations of annular nozzle are shown in Fig. 10. As expected, flow of velocity after reaching top of inner cylinder turns to annulus region and leaves from the opening of bottom side of outer nozzle towards outlet with unequal velocities. It can be observed from the figure that velocity distribution is highly non-uniform and its intensity is less in the outlet regions except corner locations. The corresponding streaklines plotted in same plane is shown in Fig. 11, indicates the imbalance of Fig. 6. Static pressure distributions at different locations of lower portion of air housing.

7 799 Fig. 7. Turbulence intensity pattern at different locations of lower portion of air housing. Fig. 8. Computational grid for nozzle on the distributed plate of air housing.

8 800 Fig. 9. Velocity vectors in the nozzle on the distributed plate of air housing. Fig. 10. Flow lines in the nozzle on the distributed plate of air housing.

9 801 Fig. 11. Turbulence intensity pattern in the nozzle on the distributed plate of air housing. airflow towards combustor region. At low velocity regions, turbulent fluctuations prevailing at different locations in computational domain are quite high as shown in Fig. 12. Simulation has been extended to array of inline nozzles and the results obtained are interpreted in terms of velocity vectors and flow lines, shaded pressure contours and turbulences loss pattern in the computational domain. The velocity vectors are shown in Fig. 13 indicates low velocities at some locations in the nozzles and travels towards exit. Due to these low velocities, possible recirculations causes unequal airflow at the different locations of nozzles, as observed in Fig. 14. As a result of typical flow distribution in the array of distributed plate nozzles, locations of high pressure and intensive turbulence effects are visualized in Figs. 15 and Conclusions Importance for understanding of air distribution pattern in a typical CFBC boiler primary air-inlet system-windbox segments with distributed plate nozzles, through CFD techniques, are addressed. Due to complex nature of flow, the analysis is presented in steps, firstly in windbox channel and later in single nozzle of distributed plate nozzle to understand flow distribution. This analysis also highlights that recirculation flow in flow domain at several locations of windbox channel/distributed plate nozzle aids to generate high pressures/turbulent fluctuations. This results to unequal air flow, which provides indications to carry the incoming crashed coal particles and lime stones to furnace inefficient combustion. The basic understanding developed through CFD techniques in the present paper has successfully identified low velocity regions, where high pressures and intensive turbulence effects are concentrated. The variations of these parameters will have considerable impact on air flow distribution to burner. More pronounced effects can be brought out after completion of simulation in all components of primary inlet system together. However, computational grid generation is difficult process, analysis of grid and elimination of walls prior to flow simulation involves considerable time. The non-uniform air-flow distribution to burner is very important to the production of combustible products like carbon monoxides and nitrogen oxides. The analysis tool can then be utilized to recommend geometric changes so that the flow can be redistributed and losses can be minimized. This process continues until optimum solutions are obtained and requires few weeks or a month, as one analysis may require three or four alternates before finding acceptable arrangement, while a similar analysis may require twenty. Nevertheless, due to cost effectiveness and success of increased software capabilities, numerical modeling will continue to grow in simulation of power plant boiler auxiliaries.

10 802 Fig. 12. Computational grid for the array of nozzles on the distributed plate of air housing. Fig. 13. Velocity vectors in the array of nozzles on the distributed plate of air housing.

11 803 Fig. 14. Flow lines in the array of nozzles on the distributed plate of air housing. Fig. 15. Static pressure in the array of nozzles on the distributed plate of air housing.

12 804 Fig. 16. Turbulence pattern in the array of nozzles on the distributed plate of air housing. References [1] R&D in clean coal technologies. Report CB011. DTI publication, UK; [2] Fluidised bed combustion system for power generation and other industrial application. Technology Status Report 011. DTI Publication, UK; [3] Balagurunathan S. Technical presentation on circulating fluidized bed combustion boilers on power plant systems and equipments. HRDC Training Course Material. BHEL, Hyd; [4] Rajaram S. Design features and operating experience of circulating fluidised bed boilers firing high ash coals in India. Paper No. FBC Proceedings of 15th Fluidised Bed Combustion; [5] Voyles R, Gagliardi C, Wolfson D. Design considerations for a 250 MW CFB. ASME 13th Conference on FBC, vol. 2; p [6] Abdualally IF, Reed K. Experience of firing waste fuels in faster wheelers circulating fluidized bed boilers. ASME 13th Conference on FBC, vol. 2; p [7] Basu P. Boiler and burners, vol. 11. New York: Springer; p [8] Mull Jr TV, Hopkins MW, White DG. Numerical simulation models for a modern boiler design. Paper No. BR Power-Gen, International, Florida; [9] Rose La, Hopkins MW. Numerical flow modeling of power plant windboxes. Paper No. BR Power-Gen International Conference, California, USA; [10] Bhasker C. Flow predictions in power station equipment components through state of art CFD software tools. Paper No. JPGC/PWR ASME-IJPGC Conference, New Orleans, USA; [11] Bhasker C. Numerical simulation of turbulent flow in complex geometries used in power plants. International Journal-Advances in Engineering Software, vol. 33. Amsterdam: Elsevier; p [12] Eaton AM, Smoot LD, Hill SC, Eatough CN. Components, formulations and applications of comprehensive combustion models. Prog Energy Combust Sci 1989;25: [13] TASCflow User Documentation (Theory and User Manual), AEA Technologies, Waterloo, Ont., Canada.