| OCR Text |
Show AFRC 2015 INDUSTRIAL COMBUSTION SYMPOSIUM Mesh Resolution Issues for CFD Analysis of Gas-fired Process Furnaces Paula Sun Mike Henneke Abstract Computational Fluid Dynamics (CFD) analysis of process furnaces is an important tool in the assessment of new furnace designs and especially in the assessment of furnace revamps where burner clearance may not meet current standards. CFD analysis is commonly employed to predict flame shapes to ensure that the selected burner layout will produce good flame quality at the operating conditions of interest. CFD is also used to predict the heat flux distribution onto the radiant coil. Managing the heat flux distribution is critical to ensuring long tube life and avoiding problems such as unwanted coking in the process tubes. Quality metrics for these CFD simulations are not provided in typical engineering specifications or in standard documents such as API 560. The engineer performing the CFD modeling must use his or her judgment to select the turbulence modeling approach, combustion modeling approach, and mesh resolution. In this paper, the impact of mesh resolution on the CFD simulation of fired process heaters is evaluated with particular focus on the quantities relevant to burner design. Introduction Computational Fluid Dynamics (CFD) analysis is a discipline involving engineering, physics, and numerical mathematics. The equations governing fluid motion in a viscous fluid were developed by Claude-Louis Navier and George Gabriel Stokes. In vector form, the NavierStokes equation has the form: This type of equation is called a partial differential equation and it cannot be solved analytically except for certain very limited circumstances. However engineers and mathematicians have developed so-called numerical solution procedures for these types of equations. Examples of numerical solution methods are finite difference, finite volume, and finite element. Modern CFD software packages have gravitated toward the finite volume method although a minority use the finite element method. These numerical solution methods introduce errors that are called discretization errors. Discretization errors are determined by the CFD grid, the order of approximation used to discretize the governing equations. These numerical solution methods also introduce convergence errors which are not discussed in this paper. Copyright 2015, John Zink Company, LLC. All rights reserved 1 AFRC 2015 INDUSTRIAL COMBUSTION SYMPOSIUM Roache (1997) discusses the concept of numerical uncertainty and makes the distinction between verification and validation: "I adopt the succinct description of verification as solving the equations right and of validation as solving the right equations." In this paper, the focus is on the verification aspect of numerical uncertainty. Modeling choices such as the treatment of turbulence and combustion processes should only be addressed through validation studies once verification is done. This mesh study is split into two efforts: 1. Free jets - in this effort, simulations of a free jet (gas tip with a single port) are presented to determine how the jet spread and decay varies with the number of cells across the jet opening as well as the mesh resolution in the downstream sections of the jet. These results are nondimensionalized using the jet diameter. 2. Near burner flow and mixing - in this effort, results are presented to show how mesh resolution impacts flow and mixing predictions. The mesh resolution in the flame zone (where reactions occur) is evaluated. This work uses the results from step 1 to establish the near tip mesh resolution. The simulation work here uses isotropic hexahedral cells. For other cell types, such as tetrahedral or polyhedral, one would expect the results and conclusions to be similar but not necessarily identical. Finally, it should be noted that the purpose of these simulations is not to validate the models with experimental data. Rather the purpose is to compare the model results on different meshes to gain an understanding of the impact of mesh resolution on the simulation results. In other words, the purpose is to verify rather than validate following Roache (1997). Mesh resolution requirements for free jet flows Many industrial combustion devices employ circular jets to introduce gaseous fuels. Similar turbulent jets have been studied extensively in the fluid mechanics literature from CushmanRoisin, 2014, which shows a schematic of a typical turbulent fluid jet where the discharge velocity is U and the centerline velocity decays with distance from the jet while the jet entrains ambient fluid and spreads. A series of CFD meshes have been applied to a simple circular jet to evaluate the impact of CFD mesh resolution on the results. A 3.175 mm (1/8 inch) I.D. port is set in a 0.5 m x 0.5 m x 1.2 m (tall) box. The mass flow rate through the jet is set so that the Mach number at the port is 1.0. All box boundaries are set as pressure outlets. To assess the jet entrainment, the flow in the jet is 100% CH4, while the gas in the box is 100% air at 60°F. The mass fraction of CH4 is used to assess mixing predictions. To better control mesh resolutions, a number of refinement zones are used to control the mesh size as shown in Figure 1. These refinement zones cover the near jet outlet field (tip, cylinder 1), mid-jet zone (cylinder 2) and far field (cylinders 3 and 4). CFD meshes have been generated using 4, 6, 8, and 16 cells across the diameter of the jet nozzle. An example of the type of mesh used is shown below in Figure 2. Copyright 2015, John Zink Company, LLC. All rights reserved 2 AFRC 2015 INDUSTRIAL COMBUSTION SYMPOSIUM Figure 1: Refinement zones Mass Flow Inet Figure 2: Example mesh using 8 cells across the jet diameter - the left image is a far view while the right image is a close-up of the near-jet mesh Copyright 2015, John Zink Company, LLC. All rights reserved 3 AFRC 2015 INDUSTRIAL COMBUSTION SYMPOSIUM Figure 3: Velocity magnitude at jet centerline - the legend indicates the number of cells across the diameter of the jet nozzle Figure 4: Jet shape defined by mass fraction of CH4 at 0.025 Copyright 2015, John Zink Company, LLC. All rights reserved 4 AFRC 2015 INDUSTRIAL COMBUSTION SYMPOSIUM CFD simulation results for the different meshes are shown in Figure 3 and Figure 4. Based on this series of CFD simulations, the cell sizes shown in Table 1 are recommended to be used near a fuel jet for a mesh independent solution. In a real-world CFD analysis, accuracy requirements and computational cost should be considered to select an appropriate mesh resolution. Table 1: Recommended CFD cell size in the interior of the jet. Note that the distance and cell size are non-dimensionalized by the jet diameter, D. Distance from jet origin Recommended cell size 0-15D D/8 35D (D/8) x 2 50D (D/8) x 4 80 D (D/8) x 8 Mesh resolution requirements for process burners Building on the results shown previously for the individual jets, a series of CFD meshes have been generated for the burner geometry shown below in Figure 5. The CFD model is based on a single burner installed in Furnace 10 at the John Zink Hamworthy Combustion R&D Test Facility. The burner is firing Tulsa Natural Gas at 3.48 MW (LHV) with 15% excess air. This furnace is water jacket cooled so there are no process tubes in the CFD simulation. Figure 5: Geometry of low NOx burner installed in test furnace. The furnace selected for this work is a single burner furnace that will not have significant furnace currents that could distort or bend the flame. In future work, multi-burner installations with furnace currents will be considered. Copyright 2015, John Zink Company, LLC. All rights reserved 5 AFRC 2015 INDUSTRIAL COMBUSTION SYMPOSIUM These meshes have followed the jet guidelines described above and used cell sizes ranging from 1.25 cm to 10 cm in the flame zone shown in Figure 6. Figure 7 shows zoom in mesh on tips. 10 cm 5 cm below 1.5 m elevation 2.5 cm below 1.5 m elevation 2.5 cm below 4.0 m elevation 5 cm below 4.0 m elevation 1.25 cm below 4.0 m elevation Figure 6: Section view of several of the meshes used - the sublabels on each figure indicate the mesh size Copyright 2015, John Zink Company, LLC. All rights reserved 6 AFRC 2015 INDUSTRIAL COMBUSTION SYMPOSIUM Figure 7: Near jet mesh close-up view 10 cm mesh size 1.25 cm mesh Figure 8: CO isosurfaces (left) and velocity magnitude isosurfaces (right image) for two mesh sizes Copyright 2015, John Zink Company, LLC. All rights reserved 7 AFRC 2015 INDUSTRIAL COMBUSTION SYMPOSIUM Figure 8 shows CO isosurfaces (2000 ppmvd) and velocity magnitude at 50 m/s isosurface colored by elevation from the furnace floor for several of the CFD meshes used in this study. Note that the finest mesh produces the shortest flame height prediction of 2.1 m. For the coarsest mesh, the predicted flame height is as high as 2.7 m. For the finest mesh, the velocity isosurface extends to 0.7 m elevation, while the coarsest mesh isosurface extends to only 0.32 m. From each simulation result, the solution variables are probed along the probe lines shown in Figure 9. These results shown in Figure 10 through Figure 13 are compared with the intent of finding the largest cell size that produces mesh-independent results. 3.5 m from heater floor 2.0 m from heater floor 1.0 m from heater floor 0.4 m from heater floor 0.2 m from heater floor Figure 9: Section view showing probe locations for data extraction Copyright 2015, John Zink Company, LLC. All rights reserved 8 AFRC 2015 INDUSTRIAL COMBUSTION SYMPOSIUM Figure 10: Velocity profile at 0.2 m elevation above the furnace floor Figure 11: Velocity profile at 0.45 m elevation above the furnace floor Copyright 2015, John Zink Company, LLC. All rights reserved 9 AFRC 2015 INDUSTRIAL COMBUSTION SYMPOSIUM Figure 12: Velocity profile at 2.0 m elevation above furnace floor Figure 13: Velocity profile at 3.5 m elevation above furnace floor Copyright 2015, John Zink Company, LLC. All rights reserved 10 AFRC 2015 INDUSTRIAL COMBUSTION SYMPOSIUM Based on the results shown above and other results not shown, the following mesh size guidelines is developed shown below in Table 2. As discussed before, specific project accuracy requirements and computational cost should be considered to select an appropriate mesh resolution. Table 2: Cell size guidelines for process burner CFD simulations Distance above floor Recommended cell size 0.2 m (around tile and gas injectors) 1.25 cm 0.45 m (lower flame above tile) 1.25 cm 1.0 m (intermediate flame) 2.5 cm 2.0 m (near end of flame) 5.0 cm Conclusion Mesh resolution guidelines for CFD simulations of fired process furnaces would benefit the industrial combustion community. The benefits would include accuracy assessment, consistency of results, and optimal use of computational resources. This paper has focused on mesh resolution guidelines in the near-burner region. Further research is needed to both verify the proposed guidelines for different burners and firing conditions and to extend these guidelines to the entire volume of the process furnace where multi-burner interactions can occur. Also note that in any particular simulation, accuracy requirements and computational cost need to be considered together to determine the appropriate mesh resolution. References Roache, P. J., "Quantification of Uncertainty in Computational Fluid Dynamics." Ann. Rev. Fluid Mech. (1997) 29:123-160 Cushman-Roisin, Environmental Fluid Mechanics, John Wiley and Sons, 2014. Copyright 2015, John Zink Company, LLC. All rights reserved 11 |
