Best Practice Advice AC2-08

From QNET
Jump to navigation Jump to search

Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice

Premixed Methane-Air Swirl Burner (TECFLAM)

Application Challenge 2-08 © copyright ERCOFTAC 2011

Key Fluid Physics

Flows with internal recirculation zones generated by vortex breakdown, chemical reactions, high swirl and Reynolds numbers are challenging for numerical simulations due to their high complexity. The key fluid physics are:

  • Size and intensity of the recirculation zone
  • The large coherent structure (Precessing vortex core, PVC)
  • Mean flame position
  • Extent of the turbulent flame brush
  • Mixing of the coflowing air with the premixed reactants as well as with the burnt gas

The measurements outlined in the 'Test Data' section are well suited to assess whether they are reproduced by the simulation.

Application Uncertainties, Computational Domain and Boundary Conditions

Since the main computational uncertainty of this configuration is related to the choice of the computational domain considered and the corresponding inlet boundary conditions these topics should be considerer together. Mainly two uncertainties have to be dealt with:

  • The development of mean and fluctuating quantities. This issue arises in many configurations where the amount of upstream geometry considered is often partly reduced by assuming for example a fully developed pipe flow. This assumption already introduces errors since turbulent quantities like the Reynolds stress tensor or, in case of a two equation model, the turbulent kinetic energy and especially the dissipation are rarely known for the RANS computation. Regarding LES this is even more critical and even the use of sophisticated inflow generators (e.g. Klein et al.[1]) can not completely replace the inclusion of sufficient upstream geometry. But the swirling flow in the annulus around the bluff-body is more complex leading us to the second point
  • To avoid a strong sensitivity related to the inlet boundary conditions the swirl nozzle should — at least to some extent — be included in the computational domain. Therefore the computational domain shown in the 'CFD Simulations' section includes the whole swirl nozzle with the radial and tangential channels where the swirl is generated. At the inlets, the deduction of the mass flow partitioning through these channels from experimental data is not possible because only the overall volume flow in the plenum chamber has been measured. Information about the azimuthal component is only available at the swirler exit and will be below the swirl found further upstream due to viscous forces. Therefore this component of the inlet boundary condition has to be estimated and we refer to the study done by Hahn et al.[2] where interesting findings regarding the interaction of the swirl intensity and the order of the numerical scheme are given.

The remaining boundary conditions are less critical. As observed for other unconfined configurations the extent in radial and axial direction should be large enough such that the region of interest is not influenced. The dimensions given in the CFD Simulation section have been found to be very conservative. If the CFD program allows entrainment from the side (we used slip walls) the extent in radial direction can be reduced.

Physical Modeling

The flow inside the combustor can be well approximated by the low Mach-number assumption. Following the recommendations the time averaged quantities of the isothermal flow field could be reproduced sufficiently accurate with the RANS approach using the standard k-e model of Launder and Spalding[3]. Nevertheless the turbulent kinetic energy showed large deviations from the experiment. Using LES it was possible to capture the turbulent fluctuations represented by the standard deviation of the velocity components much more accurate.

In the reacting case it turned out that the k-e based RANS simulations reveal difficulties to adequately predict the flow field and scalar distribution. Especially the flame position and turbulent flame brush was poorly predicted resulting in large deviations from the experiment. Regarding this, the use of LES yielded significant improvements justifying the higher computational costs. A general suggestion as to which combustion model is best suited for this case cannot be given but — since the flamelet-like behavior has been verified experimentally —any model that is able to reproduce premixed flame propagation should be appropriate.

Recommendations for Swirl Combustors Similar to the Testcase

In order to allow an identification of the numerical uncertainty the following steps should be conducted when simulating this test case. Otherwise the errors of the models employed (e. g. combustion model and turbulence model) cannot be delineated.

  • Start with the isothermal case
    • Follow the procedure given by Hahn et al.[2] to identify the connection between the swirl intensity given by the boundary conditions and the order of the numerical — spatial discretization — scheme
    • Check whether the observations made depend strongly on the resolution of the swirl nozzle. If so, the resolution is insufficient
    • The measurements planes, especially the one directly at the nozzle exit (1 mm) are well suited to quantify the above steps
    • When using LES (the above steps should be done with RANS) the energy spectrum, especially the existence of the PVC can be used in addition to the mean and fluctuating part of the velocity components to assess the simulation
    • Check whether the trend is consistent in all measurement planes when adjusting the boundary conditions
  • Going over to the reacting case
    • If the isothermal flow field is predicted satisfactory (after the steps outlined above this should be the case) deviations in the velocity components are most likely caused by the thermal expansion acting at the wrong location
    • Check the mean flame position and the turbulent flame brush using the measurements of temperature and species mass fraction
    • Especially in RANS simulations a tuning of the model coefficient to adjust the flame position may be necessary
    • In addition the turbulent flux in the scalar transport equation may need adjustments to reproduce the turbulent flame brush (e.g. turbulent Schmidt number when using the gradient diffusion hypothesis)
    • The latter problem can often be found in RANS simulations and one of the major advantages of LES is that it can be overcome because LES resolves these turbulence dominated processes

Recommendations for Future Work

In order to get a more complete picture regarding the numerical treatment of premixed swirl combustors like the one presented here, further simulations should be carried out to add knowledge considering the following points.

  • Further systematic grid studies
  • Application of different RANS closure models, e.g.:
    • K-Epsilon
    • K-Omega
    • Reynolds-Stress-Models ...
  • Study the influence of the wall treatment (e.g.: resolve the visous sublayer or use of wall functions...)
  • Assess the behavior of different subgrid-scale models, e.g.:
    • Smagorinsky
    • Germano
    • Wale
    • Using additional transport equations (e.g.: one-eq. subgrid turbulent kinetic energy)
  • Systematic comparison of the results obtained from different CFD-codes to study the influence of the overall numerical scheme.
  • Application of different combustion models, e.g:
    • Artificially thickened flame
    • G-Equation
    • Flame surface density
    • Filtered tabulated chemistry

References

  1. M. Klein, A. Sadiki, J. Janicka, Journal of Computational Physics 186 (2003) 652–665.
  2. 2.0 2.1 F. Hahn, C. Olbricht, C. Klewer, G. Kuenne, R. Ohnutek, J. Janicka, in: Proc. of the ISTP19 (2008d).
  3. B. E. Launder and D. B. Spalding, The numerical computation of turbulent flows, Computer Methods in Applied Mechanics and Engineering 3 (1974) 269-289




Contributors: Guido Kuenne (EKT), Andreas Dreizler (RSM), Johannes Janicka (EKT)
EKT: Institute of Energy and Power Plant Technology, Darmstadt University of Technology
RSM: Institute Reactive Flows and Diagnostics, Center of Smart Interfaces, Darmstadt University of Technology


Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice


© copyright ERCOFTAC 2011