Best Practice Advice AC2-01

From KBwiki
Revision as of 10:00, 5 September 2008 by Tonyh (talk | contribs)
Jump to navigation Jump to search

Bluff body burner for CH4-HE turbulent combustion

Application Challenge 2-01 © copyright ERCOFTAC 2004

Best Practice Advice for the AC

Key Fluid Physics

The flame mechanism provided by the bluff-body burner is a suitable test case for the study of turbulence-chemistry interactions. This geometry is simple, its boundary conditions are well defined and it has a stable flame for a wide range of coflow and jet conditions. For this reason it constitutes an interesting model problem, having much of the physics associated with industrial combustors while preserving relatively simple and well-defined boundary conditions. The burner is centered in a co-flowing stream of air and generally consists of a circular bluff-body with an orifice at its center for the main fuel. Masri et al have conducted comprehensive experimental investigations on a series of bluff-body flames, including flames from fully burning to those exhibiting local extinction. All the experimental data are available online at

A complex flow pattern forms downstream the bluff-body where one or two circulation zones can develop. These regions should produce enough hot gases to stabilize the flame to the burner. When the fuel jet velocity is high enough, the flow penetrates through the recirculation zone and forms a jet-like flame further downstream. The jet flame can be extinguished in a region downstream of the recirculation zone where turbulence is well developed and the finite rate chemistry effects are significant. The flame may also reignite further downstream where turbulent mixing rates are relaxed. It should be noted that the bluff-body jet flames consist, generally, of three main zones: stabilisation, extinction and reignition zones.

The major challenges of this test cases are represented by the proper implementation of turbulence closures and the turbulence-chemistry coupling models for this kind of flames.

Ø Turbulent Flows: In the turbulent flows, when the Reynolds number become high, eddies can be detected moving randomly back and forth and across and adjacent fluid layers. The diffusivity of turbulence causes rapid mixing and increased rates of momentum, heat, and mass transfer. The definition of a propagation velocity for turbulent flames which is independent on the fuel-air ratio such as for laminar flows is not possible. In fact the transport properties are mostly dependent on flow features and structures and less on the fluid properties. The non reacting turbulent flows are highly challenging but in this case the presence of chemical reactions and kinetic sand phase changes further increases the complexity of the computation and constitutes one of the most challenging fields of engineering science.

Ø Reaction Mechanism The increased interest in recent years has led to a deeper understanding of the turbulent reaction mechanism and the development of physical models with typical application ranges and limitations. The main outcome is that the turbulent fine structure, which is decisive for the molecular mixing and dissipative process, is concentrated in isolated regions whose total volume is a very small fraction of the global volume of the fluid. These regions are characterized by concentrated vorticity levels and all the molecular processes, such as viscous dissipation of turbulent energy, molecular mixing, molecular heat exchange and consequently, chemical reactions occur at this scale in the turbulent fluid. Even if the initial vorticity has a very flat spatial distribution, the vorticity generation mechanism typical of turbulent flows leads to a narrowly peaked spatial distribution after a time which is large compared with large eddy turn over time. Heat release due to chemical reactions can have an effect on the vorticity and destroy the local vortex tubes. If the vorticity generation terms can not compensate for this effect the turbulent energy decays, combustion is not generating turbulence but damping it and laminarizing the flow. These highly dissipative regions are quantitatively represented by randomly distributed tubes with diameters of the order of the Kolmogorov micro scale length. The Kolmogorov micro scale is strongly dependent on the rate of strain or time mean squared vorticity of the turbulence. The spacing of the tubes is of the order of the Taylor scale (larger than the Kolmogorov scale ), which can be obtained using order of magnitude analysis and by setting the production term equal to the dissipation term in turbulence kinetic energy equation. From this chemical reaction model it is evident that it is necessary to resolve numerically the turbulent flow structures to reproduce the chemical reaction mechanism and this task can be accomplished only with a robust and accurate turbulence model. The first step is thus represented by the set up of a reliable turbulence model which is able to resolve the vortex structures down to the Kolmogorov scales. Then a proper modelling of the reaction mechanism is strongly required to account the chemical reactions due to the incoming fuel injection.

For the deeper understanding of the physical phenomena involved in this AC the analysis of some simpler flow regimes could be helpful. The most important is represented by the UFR2-01.


From the experimental data it is evident that the proper capturing of the flow structures behind the injection area of the bluff body burner is fundamental for the accurate description of the reaction mechanism. The calculation of this complex recirculating flow and mixing field, the estimate of the length of the recirculation zone represent a very complex task even if the reaction mechanism is not included. The flow structures downstream the bluff body are very similar to those encountered behind a blunt trailing edge which is characterized by simpler physical phenomena. This test case can be useful for the preliminary set up of the turbulence modeling and the assessment of the capability of the solver to reproduce the basic vortex structures of the flow field.

In UFR2-01 the essential behaviour and the main controlling parameters are investigated and different available test cases are reported.

Application Uncertainties

For this application challenge the main uncertainty to assemble a high fidelity CFD model is represented by the resolution of the flow field for the bluff-body flames which rarely is in satisfactory agreement with measurements. Usually the computations of the velocity and turbulence fields reported in literature are adequate in the upstream regions of the jet covering the recirculation zone and the necking zone. However, further downstream and starting at about two bluff-body diameters, calculations show increasing deviation from the measurements. This is true regardless of the numerical approach used and of the modifications made to the model constants. The using of modified eddy viscosity models did get better results than those using second moment closure approaches without modifications.

From a modeling point of view another open question is represented by the chemistry models selected. Some computation have been performed with simplifying assumptions: flamelet, fast chemistry, full or constrained equilibrium and the results in terms of temperature and mass fractions of OH and NO are available in the recirculation zones. The numerical solutions clearly indicate that detailed chemical kinetics are needed to adequately compute the mass fraction of minor species such as OH and NO even in regions where local extinction is not prevalent such as in the recirculation zone.

From the experimental point of view the accuracy and reliability of the measurements data for the temperature of the ceramic face of the bluff-body and CO fractions are critical. Especially the measurement of this parameter is not simple and strongly dependent on the measuring technique. In fact a first acquisition campaign obtained with using the Raman scattering technique suffered of fluorescence and other Raman interference, contributing to reduced signal to noise ratio. Recently a more accurate technique was used to measure the CO mass fractions at different locations in the flame and the uncertainty on the CO mass fraction should be reduced.

Computational Domain and Boundary Conditions


The inlet boundary conditions to be applied are reported in Table 1, where the composition and/or flow field measurements are reported for some tested flames. In this table,D34 image1.gif is the jet diameter (mm),D34 image2.gif is the bluff-body diameter (mm),D34 image3.gif is the jet velocity (m/s),D34 image4.gif is the co flow air velocity (m/s),D34 image5.gif is the jet Reynolds number, % B.O. is the percentage ratio of jet velocity over the blow off velocity,D34 image6.gif is the temperature of the fuel at the jet exit plane and D34 image7.gifis the stoichiometric mixture fraction.. When applying the inlet boundary conditions, to the flow field, convergence could be problematic if the boundary conditions are applied exactly in the geometrical inlet of the bluff body. It could be important to move the inlet regions for fuel and air upstream (computations reported in TNF3 proceedings suggest 0.1 m), in order to relax the dependence on the experimental boundary conditions for velocity and turbulent quantities. In some computations a serious under prediction of the bulk mass flow rate and momentum flow rate of the fuel stream was experienced if the exact experimental initial conditions were implemented. If the inlet planes is shifted upstream from a numerical point of view the bulk flow data as initial conditions should be applied rather than the experimental radial profiles. The fuel-stream flow field has sufficient time to form a developed pipe flow before exiting into the flow above the bluff body. This ensures better agreement with the experimental flow field data above the bluff body.

D34 image016.jpg

Table 1- Inlet boundary Conditions

With a two equation turbulence model the proper inlet boundary conditions should be implemented through the imposition of the turbulence level (Tu) and the length scale (L) from the experimental data. The kinetic energy and D34 image8.giforD34 image9.gif should be computed according to the following relations:

D34 image12.gifD34 image10.gifD34 image13.gif

For this test case as well as for typical heat transfer application the length scale is not available from experimental data in view of the complexity of the measurements. Usually when two consecutive values of the kinetic energy are known (ie. Tu) for the incoming flow then L could be esteemed assuming steady homogeneous decay:

D34 image11.gif

In all other situations the length scale has to be guessed according to previous experiences. Usually L is selected in the range between 1-0.1% of a representative dimension of the problem at the inlet. For this present application the chosen value is 0.5%.

The inflow conditions are crucial for any LES approach to describe the turbulent inflow. The most simple approach could be represented by the addition of random noise to the mean flow velocities. A more sophisticated approach has been suggested, which consists of copying the instantaneous velocity profile of a fully developed and turbulent pipe flow to the inflow plane. Finally, the flow through the turbulence generators could be simulated as well, removing the need for any experimental data to describe the boundaries. In this way, fluid properties, geometry and bulk velocity could be computed without arbitrarily setting some parameters to describe the inlet turbulence. The acquired results should depend on the flow code only, not on turbulent boundary conditions or model constants.


In the exit plane, usually the experimental static pressure is imposed. A fully developed flow field is further assumed neglecting all axial derivatives of the fluid dynamics variables.

Ø If a constant static pressure is imposed in the outlet section a remarkable displacement of the outlet boundary downstream the bluff body is strongly suggested: the outlet plane should be located at a distance of al least 5xD downstream the inlet section. In this way pressure reflections can be avoided and the assumption of a perfectly uniform distribution of the pressure and velocity profiles seems more realistic. With insufficient distances the constant pitch-wise pressure field imposed in the outlet section can be inconsistent with the tangential pressure field in the body and influence the upstream flow field.

Ø A better method for the implementation of less reflective boundary condition is maybe represented by the imposition of an integral outlet pressure field instead of a local averaged pressure value. A not reflective outlet boundary condition could be accomplished by the imposition of an integral outlet pressure field instead of a local pitch wise averaged pressure value. To clarify consider the red line indicated in Figure 2. The constant experimental pressure is Pext. The pressure profile extracted from the inner field (red line in the graph) is not constant and has a different mean value. The final pressure distribution, that should be used as a new boundary condition for the outlet section, is obtained scaling this profile so that the external mean average is attained.

File:D34 image14.gif

Figure 1 -Outlet average pressure condition © ERCOFTAC 2004 Discretisation and Grid Resolution


The experience gained in the numerical computations of this test case as well as other combustion and heat transfer applications with different solvers allows drawing some general conclusions about the spatial discretization methods:

Ø The FVM, used in combination with unstructured approaches can cope with a wider range of applications and problems, but the numerical cost is usually higher. Structured FVM schemes are also used with little differences from FDM approaches. FVM methods should be preferred since inherently conservative.

Ø The FDMs require a structured computational domain. These schemes are in most cases faster to execute and easier to manage. Their use is particularly suited for problems where the geometry is simply enough to allow a regular structured grid. The relative simplicity of geometry of bluff body burner test case can allow accurate results with structured approaches. Actually this is the most widespread grid topology for this kind of application.

Ø Both for FV and FD methods the accuracy of the results requires at least a second order discretization scheme. Higher order schemes usually can cause instability and a special treatment is needed to provide monotonic solutions. This problem is particularly felt working with unstructured approaches where higher complexity is needed to handle the grid topology. The robustness of a first order scheme may be useful at the beginning when the disturbances of the initial guessed solution are still relevant.

Ø From the computations performed on various test cases it can be concluded that all the most widespread discretization schemes are capable of providing comparable and accurate results: an optimal FV and FD method based on cell vertex, cell centred, vertex centred… scheme did not emerge clearly.

Convection dominated problems (eg. the compressible Navier-Stokes equations) require the use of some kind of artificial dissipation to improve the stability and accuracy of the solver in the presence of sharp discontinuities and strong gradients.

Ø A widely known approach to provide artificial dissipation is to include in the spatial derivatives 2nd and 4th order artificial dissipation terms. These terms are scaled with the pressure gradients of the solution to improve the stability of the method. Artificial dissipation scheme are usually straightforward with structured schemes. The proposed extensions for unstructured approaches are usually complex and not clearly posed.

o The use of artificial dissipation is simple, efficient and stable, but in some cases can introduce excessive diffusion in the computed flow and reduce the accuracy of the solution. Some tuning empirical parameters and special corrections (such as eigenvalues scaling to provide the required anisotropy in wall boundary layers) can constitute useful tools to improve both the solution quality and stability.

Ø The use of flux upwind represents another quite common way to enforce a monotonic computed solution. Upwind schemes try to follow the dominating behaviour of the characteristics of convective terms and may be applied equally to FDM or FVM schemes for structured or unstructured solvers.

o Several proposals for the flux up winding of convective terms are available. From the experience gained by the Florence University the Roe’s method and the AUSM+ first order scheme proved the better performance in terms of accuracy and stability of the solution.

o Higher order upwind schemes can be obtained using a linear reconstruction of the computed solution inside the grid cells. In this case a monotonic solution is ensured using slope or flux limiting in conjunction with flux up winding. TVD schemes can be different depending on the structured or unstructured approach. For structured schemes the Superbee or Van Leer limiters should be preferred (R. LeVeque, 1992). Unstructured solvers should implement the Barths’s limiter in the improved version suggested by Venkatakrishnan (1995).

o The absence of tuning parameters represents a positive feature with respect to the artificial dissipation approaches.

Ø Past experience showed that both artificial dissipation approach and upwind methods showed good capabilities to ensure a monotonic solution if properly applied so there is not an optimal choice between the two approaches

An important aspect related to the CFD simulation is represented by the computation of the flow gradients used for the high order reconstruction in upwind fluxes or the viscous terms in the Navier-Stokes equations.

Ø For the linear reconstruction used for second order up winding, the most adequate schemes for the computation of the solution gradients (more details can be found in Martelli and Adami, 2001) are represented by the Gauss-Green formula and the least squares approach.

o The Gauss-Green method is easy to implement and requires less computational demand. Unfortunately it gives exact gradients for linear functions on tetrahedral elements only and therefore does not ensure the same accuracy level throughout the field when using skewed structured or mixed hybrid grids. This is a serious drawback since prismatic layers are used to represent the viscous boundary layers near solid walls. Here the accurate computation of the solution gradients is relevant especially when the heat transfer prediction is required or a more sophisticate turbulence closure is used.

o The linear least squares reconstruction avoids the above pitfall and allows the same degree of accuracy in the gradient estimate throughout the mesh. More precisely the method is exact for linear functions regardless the cell type. This feature is quite important for stretched structured grids or mixed grids and therefore should be preferred as a default scheme. The least-squares reconstruction is based on a first order Taylor series for the approximation of the solution on each grid cell-centre (more details are available in Martelli and Adami, 2001).

Ø For the computation of viscous stresses the cell centred gradients of the solution, computed in the linear reconstruction can lead to an unstable solution or the decoupling of adjacent nodes.

o The gradients should be computed by a finite difference formula at the midpoint location of every element face. This approach does not involve any reconstruction phase. The fluxes can be obtained by the same quadrature formula (ie. as for the numerical scheme used for convective fluxes) provided that the viscous stresses and conduction heat are computed on the face mid-point. For the viscous terms of Navier-Stokes equations this “staggered” scheme ensures a more stable discretization giving at the same time a simple and accurate representation of the flow.

A grid sensitivity of the solution from the discretization scheme and grid refinement should be always performed. To tackle the additional cost of such test, a fist good indication could be obtained from the comparison of the first and second order solution computed for the same problem. This estimate should be done considering the effect produced by the discretization scheme on some relevant and meaningful parameters such as the temperature distribution, the velocity profile or the vortex structure features.


For the proper discretization of the physical domain of this test case two kinds of advise should be given. The first concerns general grid recommendations in the field turbulent combustion application, the second pertains to the specific requirements of this particular application.

General grid recommendations

In general two basic grid topologies can be used to represent the geometrical domain in the numerical simulation: structured and unstructured grids.

Ø The structured grids are more easily generated especially for simpler geometries. An example is reported in figura 2a. Different structured grid arrangements are usually employed in combustion.

Ø The unstructured grids allow a more flexible assembly of elements and a more efficient local refinement of the mesh. Besides no continuity of grid lines through the whole domain is required. For these reasons unstructured grids are usually indicated in the discretisation of complex domains.

The accuracy of a CFD simulation increases with the increasing number of grid cells. The global element number is an important parameter to assess the accuracy of the CFD simulation. Anyway the spatial accuracy may be lost for complex geometries due to the high distortion and irregularity of the elements. The following requirements should be verified:

Ø The grid lines for structured approaches should not present discontinuities and guarantee as much as possible the mutual perpendicularity in the whole computational domain. The grid lines should be orthogonal to the solid boundaries.

Ø For unstructured approaches highly skewed elements should be avoided. For the tetrahedral elements the internal angles should approximately be equal (Fig 2) while for quadrilaterals the edges should be almost the same.

Ø The grid elements size should vary regularly across the domain. The stretching ratio of adjacent element sides should be in the range between 1.1 to 1.6 for tetrahedral and triangles. In case of quadrilaterals the stretching ratio inside the boundary layers (the growing law) should range from 1.1 to 1.5.

Specific requirements:

For the accurate simulation of this bluff body burner some specific requirements should be fulfilled:

Ø Grid adaptation techniques should be employed to provide efficient localised refinement of the gradient encountered in the complex flows of the chemical reacting zones. These selective clustering techniques are particularly efficient in the reduction of the total number of cells for unstructured grids. A practical example is given in (Fig. 2) for the bluff body burner test case: the elements on the plane section are triangles, which allow an easier clustering close to the bluff-body walls and especially at the sharp leading edges with the fuel and air jets.

Figure 2a: Unstructured grid

Figure 2b: Structured grid

Ø A common error done trying to enforce a very close first cell to the wall may consist in the generation of an excessively stretched grid with badly shaped elements and poor aspect ratios. An evenly refined should be guaranteed when reducing y+ for the first node. The suggested range for the stretching ratio is about 1.15-1.25. This range is a good compromise between the need to lessen the number of elements inside the boundary layers and a regular variation of the grid height between neighboring elements.

Grid sensitivity

To avoid grid sensitivity of the results calculations should be performed using grids with progressively increasing elements number. To reduce this preliminary phase the grid refinement tests of the calculations should be performed with a simpler chemistry model. Once the flow field structure is assessed the complete reaction mechanism should be implemented. © ERCOFTAC 2004 Physical Modelling

Turbulent reactive flow is a complex phenomenon and its computation requires modeling of the various physical and chemical processes. Rigorous mathematical and numerical formulation of these phenomena is prohibitive, and different levels of complexities have to be used in practice, depending on the application. For simple geometries turbulence models such as Reynolds stress model or high-order closures can be used and chemical reactions can be represented by more detailed finite rate kinetic schemes. In practical combustion devices, such as turbine combustors and furnaces, less sophisticated representations have to be used because of computer capability limitations. Turbulence models such as eddy viscosity model, fast or equilibrium chemistry, flamelet models, reduced kinetic scheme, assumed shape pdf, eddy break-up, or eddy-dissipation models are commonly used. The simple geometry of this test case is a very attractive feature because the simulation of the bluff body is affordable even with the more sophisticated models allowing a comparison and tuning of the simpler turbulence closures and kinetic schemes.


In this application the main challenge is represented by the proper modeling of the turbulence structures downstream the bluff body. The main advantages and drawbacks of the different approaches will be briefly underlined here

Two-equation models: represent a widely accepted approach for reactive turbulent flows. The two-equation closures are based on a linear constitutive law, (the Bousinnesq assumption) and

for this reason poor predictions are expected when the non linearity of the flow field is remarkable such as in the presence of chemical reactions. Besides some adjustment of model constants are suggested for an improved matching of the CFD results with experimental data.

Ø Considering that the model is applied to reacting flows, Favre averages should be used instead of Reynolds averages.

Ø The classical, linear Boussinesq hypothesis should replaced by a non-linear relation between the Reynolds stresses and the local mean velocity field (mean rate of strain and mean absolute rotation) the strain rate (Merci, 2000).

Ø The default values of the model constants in the ε equation are and . Most of the turbulent computations reported for the bluff body burner k-ε required a modification of the model to reproduce the observed spreading rate of a round jet. The modification or are the most followed ones. Besides the standard should be replaced by where is a damping function (Merci-2000), and .

B. Merci, D. Roekaerts, T.W.J. Peeters and E. Dick “The impact of the turbulence model and inlet boundary conditions on calculation results for reacting flows”, Proceedings of TNF5 “Fifth international Congress on Turbulent Non-Premixed Flames, July 26-28,2000

Reynolds stresses:

Reynolds stress approaches undeniably introduce more physics in to the model. The major advantages are represented by the provision to account for anisotropy of the free-stream, the exact treatment of the turbulence production and effects of streamline curvature. These features help also in handling other forms of non-equilibrium phenomena, which are frequently encountered in turbulent flames. The higher complexity of this modelling approach implies large computational efforts, also on account of the extremely refined grids required to resolve the regions of strongest gradients.

Large Eddy Simulation

LES has a great potential for the simulation of turbulent flames, because fluctuations of velocity and the chemical composition are resolved down to filter width. An accurate description of mixing, the driving mechanism of combustion in such systems, is therefore possible. Usually when a three dimensional LES is applied; sub-grid fluctuations should be modelled according to Smagorinsky, while the model constant should be determined dynamically by the well known Germano approach. Some recent publications show results of full 3d LES with varying density, combined with equilibrium chemistry (Forkel,1999) for the simulation of turbulent flames.

Although a satisfying overall agreement to experimental results could be achieved with pdf approach, no reasonable information on coexistence, minor species or extinction-related phenomena could be derived. To overcome these shortenings the switching to flamelet chemistry is recommended. The additional numerical effort is justified by the more detailed information about the reaction mechanism.

H.Forkel, J. Janicka, Large-Eddy Simulation of a turbulent Hydrogen Diffusion Flame,1st Symposium on Turbulent Shear Flow Phenomena (1999)

A. Kempf, A. Sadiki, J. Janicka, J.-Y. Chen “Large Eddy Simulation of a Turbulent Diffusion Flame Using Flamelet Modeling”, Proceedings of TNF5 “Fifth international Congress on Turbulent Non-Premixed Flames”,July 26-28,2000


Data obtained from direct numerical simulations are the most accurate methods for the simulation of turbulent reactive flows. This method is particularly suited to investigate the differential diffusion on reacting scalars in isotropic, decaying turbulence. The influence of differential diffusion on ensemble averages of the mass fractions and the reaction rates is important for low Reynolds numbers and diminishes with increasing Reynolds numbers (Re). With increasing Damkhohler numbers, however, differential diffusion effects became more pronounced.


The principal weakness in turbulent combustion calculation is in the modelling the chemical reactions and their interaction with the turbulent flow field. For most hydrocarbon oxidation reactions in diffusion flames, kinetic rates are typically higher than eddy dissipation rates and reactions are controlled by the mixing of fuel and oxidant. For these reactions, assumption of equilibrium chemistry or flamelet combustion, where species concentration and enthalpy can be expressed as function of a single variable (mixture fraction) is adequate. The equations for mixture fraction can be solved to give an assumed shape probability density function (pdf) and reasonably accurate solutions could be obtained been obtained in the present test case. For slow reactions such as and soot formation, or postflame CO oxidation, the above assumption are inaccurate, and finite rate chemical reactions have to be considered simultaneously with turbulent mixing. Due to the highly non linear form of reaction rates, the pdf of the species concentration and temperature is needed to calculate the rates accurately. The assumed pdf method, though successful in some flames with simple chemistry interactions, does not account rigorously for turbulent chemistry interactions and cannot be readily extended to more general cases. Unfortunately, because of the large dimensionality, this method becomes intractable when more than two species are considered. To overcame this difficulty, the Monte Carlo method was formulated, in which the pdf is represented by a large number of notional particles which move and evolve according to the turbulence, diffusion and kinetics model adopted. When turbulence models such as Reynolds stress model or high-order closures are used, chemical reactions can be represented by more detailed finite rate kinetic schemes and some will be suggested here.

PDF_Model: A popular and simple strategy for modelling turbulent non-premixed combustion is to apply a conserved scalar or mixture fraction based approach, typically assuming equilibrium chemistry. By addressing the moments of thermodynamic and chemical quantities via an assumed-shape PDF formulation, turbulence-chemistry interactions may be treated formally. PDF methods have the great advantage that the turbulent transport and the chemical source terms are in closed form and do not have to be modelled. For this test case, generally, the probability density function (pdf) of the mixture fraction is assumed to be a beta function. In combustion systems where non equilibrium effects are not important or when the formation level of pollutant species, such as NOx, should not be predicted the assumption of local chemical equilibrium can be realistic and the PDF model might be particularly appropriate. A stand-alone particle method which solves the joint velocity frequency-composition PDF (JPDF) transport equation has been implemented and discussed in detail by Xu (Xu et al.,1999) and has been successfully applied for various reacting and non-reacting flow configurations of the bluff body burner.

Xu, J. and Pope, S. B. "Assessment of Numerical Accuracy of PDF/Monte Carlo Methods for

Turbulent Reactive Flows; J. of Comp. Phys. 152, 192:230(1999).

FLAMELET Approach:

When the Damköhler numbers are high such as for the methane flames considered here the infinitely fast chemistry assumption is not satisfied, so non equilibrium effects should be accounted for. The flamelet assumption captures the local strain rates in the flow field and provides more accurate predictions of temperature and radical concentrations including the blow off limit as well as indications of local extinction. Look-up tables and assumed-shape PDF formulations analogous to those used in the equilibrium chemistry PDF approach should used in the implementation of this model. In this test case good results have been obtained by the laminar flamelet with strain rate of a = 100/s assumed for the flow field.

FIXED STRAINED-FLAMELET The stretched laminar flameletmodel is based on the assumption that two scalars, a mixture fraction x and scalar dissipation c as a measure for flamelet stretch can determine unambiguously the local instantaneous thermo-chemical state in the turbulent flow. A flamelet library is available for CH4/H2 flames (Bowmann) and stretch rates of 100/s, 200/s and 300/s. Computations with this flamelet library are benchmarked against a CH4/H2 non premixed turbulent bluff body(2) stabilised flame as investigated by Masri et al2. Fluctuations in mixture fraction x and scalar dissipation c can be accounted for, using an assumed beta-function and delta-function shape at mean conditions, respectively. This model provides an efficient mechanism for incorporating finite rate kinetics into computations of non-premixed flames.

1. Bowman, C.T., Hanson, R.K., Davidson, D.F., Gardiner, Jr, W.C., Lissianski, V., Smith, P., Golden, D.M., Frenklach, M. and Goldenberg, M.,

2. Combustion Database, The University of Sydney and The Combustion Research Facility, Sandia National Laboratories:

ILDM Model-The Intrinsic Low-Dimensional Manifolds (ILDM) model, (Maas-1992) has been used to provide a description of the chemical reactions. This approach allows for the generation of reduced chemical mechanisms. The ILDM­approach, as well as all the other approaches, is based on the physical fact that in typical reaction systems a large number of chemical processes are so fast that they are not rate limiting and can be decoupled. For this reason finite-rate chemistry is accounted locally considering only the slowest chemical time scales. The fast chemical time scales as relaxed. The slow reaction represent some manifold which can constrain the species composition. Conservation equations are solved for a small number of reaction progress variables parameterizing the manifold instead of a huge number of species of the detailed mechanism. The evaluation of the ILDMs is computationally demanding, so it should be done only once and the resulting ILDMs should be stored in look-up tables even if some problems could arise in view of the limited disk and memory space for the ILDM tables (Niemann-1997). In fact the dimension of the state needed some industrial applications could exceeds the dimension which can be handled with ILDM tables spanning the whole ILDM space. An efficient approach to overcome that problem should be represented by in-situ tabulation of the ILDMs, where the calculation of the ILDM table is done during the reactive flow calculation (Niemann-1998). The physics of stiff combustion chemistry normally restricts the solution to a very minor subspace of the ILDM parameter space. When the in-situ tabulation approach is used for laminar and turbulent flames thje Monte-Carlo methods are should be used for solving the transport equation of the PDFs.

U. Maas and S.B. Pope. Combustion and Flame, 88, pp.239-264, 1992.

H. Niemann, D. Schmidt, and U. Maas. J. Eng. Math., 31:131{142, 1997

H. Niemann, J. Warnatz. W-I-P Poster 27th Int. Comb. Symp., 1998

CMC (Conditional Moment Closure): Conditional Moment Closure (Klimenko, 1990, Bilger, 1993) is a method for handling turbulence chemistry interactions which is capable of being used with large chemical mechanisms with reduced computational cost. The basic idea of the method is that most of the fluctuation in temperature and composition can be associated with one variable and conditional averaging with respect to that variable allows closure of the conditional average chemical reaction rate terms. For the non premixed combustion systems the conditioning variable of choice should be the mixture fraction. CMC has successfully applied for turbulent non premixed hydrogen jet flames turbulent diffusion flame formed from a partially premixed jet of methane and air. The reacting scalar fields could be calculated by CMC under the initially given flow and mixing field. Details on the numerical simulation procedure may be found in Kim-2000. Due to weak spatial dependence of the conditional averages a coarser spatial grid than that of the flow field is generally suggested for the CMC equations. In general the results for the bluff body application, show a general good agreement with the measured conditional mean concentrations of the major species, including NO, with some minor discrepancies on the fuel-rich side. Predicted conditional mean OH mass fractions tends to be higher than the measurements while for CO lower levels are expected from the computed field. CMC predictions of the conditional mean temperature are in general good agreement with the measurements, although with slight under prediction on the fuel rich side.

Kim, S. H., Huh, K. Y. and Liu, T., Combust. Flame 120:75-90(2000).

Bilger, R.W., Phys. Fluids A 5(2):436-444, 1993.

Klimenko, A.Y., Fluid Dynamics 25:327-334, 1990.

ODT (One Dimensional Turbulence) approach: The model (Kerstein 1999) is based on the distinction between molecular processes (reaction and diffusion) and advective processes. According to this separation a time-resolved simulation of the full range of scales in a single dimension, is used to provide exact treatment of chemical reaction and molecular mixing at Reynolds and Damkohler numbers not accessible to DNS. Molecular processes, including diffusion scalar mixing and reaction, are computed deterministically by solving the unsteady reaction-diffusion equations. All chemically relevant length scales are resolved in one dimension along the ODT domain.

There are two constants within the model that together determine the overall mixing rate and the magnitude of conserved scalar fluctuations.

Advective mixing processes are implemented as a stochastic process using triple-mapping stirring events which emulate the compressive-strain and rotational folding effects of turbulent eddies. In this way, turbulent mixing acts to steeper gradients in locally inhomogeneous regions. The ODT approach incorporates two constants that together determine the overall mixing rate and the magnitude of conserved scalar fluctuations from the local shear rate and the total elapsed time for non stationary flows. More details can be found in Kerstein (1997).

This formulation shows good capability in the description of finite scale processes, including differential diffusion effects, and the detailed account of turbulence-chemistry interactions. Simulations performed for turbulent non premixed hydrogen-air and piloted methane-air flames show that ODT is able to reproduce some of the gross features of turbulent reacting jets except for the effects of dilatation on the mixing rate. Also spatial intermittency of stirring events and cascading from larger to smaller eddies is potentially captured. The main advantage of this method is represented by the relatively small memory and CPU time costs in comparison with Reynolds stress models or DNS

Kerstein, A. R., J. Fluid Mech. 392, 277-334 (1999).

Kerstein, A.R., One-Dimensional Turbulence. Part 1: Homogenous Turbulence and Shear

Flows, in press J. Fluid Mech. (1997).


Various calculations of CH4 and natural gas flames presented at the TNF Workshops have used detailed or reduced versions of several mechanisms and some are available for posting on the web. The following are the most referenced:

1. GRI Mech (versions 1.2, 2.11, and 3.0), available from Web site: Reduced mechanisms have been proposed from J-Y Chen, including 12-step (from GRI 2.11), 13-step (from GRI 3.0), and 15-step (from GRI 3.0). All three reduced mechanisms include NO chemistry.

2. Lindstedt and Warnatz.. Comparisons of several detailed and reduced mechanisms are included in the TNF5 Proceedings and in Barlow-2001 The outcome of their comparison is that the differences in major species from the reduced mechanisms could be considered negligible while the differences among NO predictions can be substantial.

3. The Miller-Bowman mechanism (Miller-1989) The full Miller-Bowman mechanism and 14 step reduced mechanism have been compared for reaction of the given fuels and NO. The results with the two different mechanisms, i.e., full mechanism and 14-step reduced mechanism, show no distinguishable difference for the conditional mean temperature. However the Miller-Bowman mechanism shows better agreement for NO mass fraction in recirculation zones. The 14-step reduced mechanism tends to over predict the conditional mean NO mass fraction on the fuel rich side while in the neck zone and downstream flame locations the conditional mean NO mass fraction tends to be over predicted.

4. ARM2 as used in calculations of methane flames by Steve Pope’s group at Cornell. This is a 16-step reduced mechanism, which is based on GRI Mech 2.11 and includes NO.

Miller, J. A. and Bowman, C. T., Prog. in Energy and Combust. Sci. 15:287-338(1989). © ERCOFTAC 2004 Recommendations for Future Work

For the definitive assessment of the AC2-01 much work should be done to provide further elements of discussion and improve the quality of the test case. The following activities might provide very useful contributions:

Ø The numerical simulation of the present AC and the associated UFRs should be repeated using contemporary and advanced turbulence models. The research activity in the turbulence field is still proceeding and up to date approaches can include more and more physics in the modeling.

Ø For the computation of complex flows with chemical reactions RANS methods are undeniably limited in their possibility to capture real physics in comparison with DNS or large-eddy simulations (LES). DNS and LES numerical simulations have been already performed to reproduce also the temporal development of the flow field. The use of massive computing resources (parallel architectures and clusters) is today commercially available so that the CFD computation of a more complex geometry is possible in reasonable computing times. The DNS or LES simulation of the test case could be profitably used to obtain a reference solution or a data base for the assessment of simpler turbulence models.

Ø The simulation of related UFRs such as UFR2-01 concerning the flow behind a blunt trailing edge is a very interesting test case for the set up and tuning of the turbulence models implemented. This test case is simpler and can be used to tune the turbulence model in absence of other phenomena such as chemical reactions. The comparisons of the performance of the turbulence models on the two different applications could provide interesting information about the accuracy of the model itself. © copyright ERCOFTAC 2004

Contributors: Elisabetta Belardini - Universita di Firenze

Site Design and Implementation: Atkins and UniS

       Top        	      Next