FLUENT实例教程—berl
Tutorial:2D Simulation of a300KW BERL Combustor Using the Magnussen Model
Introduction
The purpose of this tutorial is to provide guidelines and recommendations for setting up and solving a natural gas combustion problem.
Introduction
This tutorial assumes that you are familiar with the FLUENT interface and that you have
a good understanding of the basic setup and solution procedures.
This tutorial demonstrates how to do the following:
?Use the k-epsilon turbulence model and P-1radiation model.
?Use the Eddy Dissipation Finite-rate Reaction model.
?Set up and solve a natural gas combustion problem.
?Postprocess the resulting data.
If you have not used these models before,it would be helpful to?rst refer to the FLUENT
6.3User’s Guide.
Problem Description
This problem was modeled after the experiments carried out at the Burner Engineering Research Laboratory(BERL)as part of a large project(Scaling400study)for combustors ranging in size from30KW to12MW.The schematic of the problem is shown in Figure2.
The?ow under study is an unstaged natural gas?ame in a300KW swirl-stabilized burner.
The furnace is vertically?red.It has an octagonal cross-section with a conical furnace hood and a cylindrical exhaust duct.The furnace walls can be refractory-lined or water-cooled.The burner features24radial fuel ports and a blu?centerbody.Air is introduced through an annular inlet and movable swirl blocks are used to impart swirl.Figure1shows
a closeup of the burner assuming2D axisymmetry.Appropriate area adjustments were
made to account for the2D representation of a3D problem.It has been ensured that the cross-sectional areas of the model and real furnaces are the same.The input conditions for this case,i.e.wall temperature,inlet boundary conditions,and pro?le have been derived from this experimental data.
2D Simulation of a300KW BERL Combustor
Figure1:Closeup of the Burner
Figure2:Schematic of the Problem
2D Simulation of a300KW BERL Combustor Preparation
1.Copy the mesh?le,berl.msh.gz to the working folder.
2.Copy the pro?le?le,berl.prof to the working folder.
3.Start the2D(2d)version of FLUENT.
Setup and Solution
Step1:Grid
1.Read the mesh?le(berl.msh.gz).
File?→Read?→Case...
2.Check the grid.
Grid?→Check
3.Scale the grid to mm.
Grid?→Scale...
4.Display the grid.
Display?→Grid...
Figure3:Grid
2D Simulation of a300KW BERL Combustor
Step2:Models
1.De?ne Pressure Based solver for Axisymmetric Swirl space and Steady time.
De?ne?→Models?→Solver...
2.Select the standard k-epsilon(2eqn)turbulence model.
De?ne?→Models?→Viscous...
3.Enable the Energy Equation.
De?ne?→Models?→Energy...
4.Select Species Transport as the species model.
De?ne?→Models?→Species?→Transport&Reaction...
(a)Enable Volumetric reactions.
(b)Select Finite-Rate/Eddy-Dissipation from the Turbulence-Chemistry Interaction list.
(c)Disable Di?usion Energy Source.
(d)Click OK to close the Species Model panel.
5.Select P1from the radiation model list.
De?ne?→Models?→Radiation...
The P1radiation model is used since it is quicker to run.However the DO radiation
model can be used for more accurate results.
Step3:Materials
1.Copy the following?uid materials from the database.
De?ne?→Materials...
(a)CH4
(b)CO2
2.Rename methane to fuel and delete its chemical formula.
3.Modify the properties for mixture-template.
(a)Reorder the species as follows:
i.h2o
ii.o2
iii.fuel
iv.co2
v.n2
A transport equation is not solved for the last species in the list,instead its
concentration is determined by di?erence.To reduce the round-o?error,the
species of the greatest quantity should be placed last in the list.In most cases,
this is n2.
2D Simulation of a300KW BERL Combustor (b)De?ne the following reaction.
Reactants Stoich.
Coe?cient Rate Exponent Products Stoich.
Coe?cient
Rate Exponent
fuel11CO2 1.0220
O2 2.0331H2O 2.0220
(c)Select mixing-law from the Cp drop-down list.
(d)Select polynomial from the Thermal Conductivity drop-down list.De?ne a two
coe?cient polynomial with0.0076736and5.8837e-05as the?rst and second
coe?cients.
(e)Select polynomial from the Viscosity drop-down list.De?ne a two coe?cient
polynomial with7.6181e-06and3.2623e-08as the?rst and second coe?cients.
(f)Select wsggm-domain-based from the Absorption Coe?cient drop-down list.
(g)Enter1e-09for Scattering Coe?cient.
4.Enter16.313for Molecular Weight and-1.0629e08Standard State Enthalpy for fuel.
5.Select polynomial from the Cp drop-down list for all the species and set the values for
the coe?cients as shown below:
Species1234567
fuel2005-0.3407 2.362e-03-1.178e-6 1.703e-10--
CO2535.40.6393-1.823e-04-5.956e-08 3.784e-11--
H2O1938-0.5904 1.215e-03-7.158e-07 1.519e-10--
N210270.01081 4.955e-5-1.121e-08---
O2876.30.06141 1.861e-04-3.006e-07 2.295e-108.54e-14 1.224e-17
6.Click Change/Create and close the Materials panel.
Step4:Operating Conditions
Retain the default operating conditions.
Step5:Boundary Conditions
1.Read the pro?le?le(berl.prof).
File?→Read?→Pro?le...
The CFD solution for reacting?ows can be sensitive to the boundary conditions,in particular the incoming velocity?eld and the heat transfer through the walls.Here, you will use pro?les to specify the velocity at velocity-inlet-4,and the wall temperature for wall-9.The latter approach of?xing the wall temperature to measurements is common in furnace simulations,to avoid modeling the wall convective and radiative heat transfer.
2D Simulation of a300KW BERL Combustor
De?ne?→Boundary Conditions...
2.Set the boundary conditions for velocity-inlet-4zone.
(a)Select Components from the Velocity Speci?cation Method drop-down list.Select
vel-prof u and vel-prof w for Axial-Velocity and Swirl-Velocity respectively.
(b)Select Intensity and Length Scale from the Turbulence Speci?cation Method drop-
down list.
(c)Enter17%and0.0076m for Turbulence Intensity and Turbulence Length Scale
respectively.
(d)Click the Thermal tab and enter312K for Temperature.
(e)Click the Species tab and enter0.2315for Species Mass Fractions for o2.
(f)Click OK to close the Velocity Inlet panel.
3.Set the boundary conditions for velocity-inlet-5.
(a)Select Components from the Velocity Speci?cation Method drop-down list.
(b)Enter157.25m/s for Radial Velocity.
(c)Select Intensity and Length Scale from the Turbulence Speci?cation Method.
(d)Enter5%and0.0009m for Turbulence Intensity and Turbulence Length Scale
respectively.
(e)Click the Thermal tab and enter308K for Temperature.
(f)Click the Species tab and enter0.97and0.008for Species Mass Fractions for
fuel and co2respectively.
(g)Click OK to close the Velocity Inlet panel.
4.Change the Type for out?ow-3zone to Pressure outlet.
(a)Select Select Intensity and Hydraulic Diameter from the Turbulence Speci?cation
Method.
(b)Enter5%for Intensity and0.6m for Hydraulic Diameter.
(c)Click the Thermal tab and enter1300K for Temperature.
(d)Click the Species tab and enter0.23for Species O2mass fraction.
(e)Click OK to close the Pressure Outlet panel.
5.Set the boundary conditions for wall zones.
(a)Click the Thermal tab and select Temperature from the Thermal Conditions list.
(b)Set the following conditions:
2D Simulation of a300KW BERL Combustor
Zone Name Temperature Internal Emissiv-
ity
wall-61370K0.5
wall-7312K0.6
wall-81305K0.5
wall-9temp-prof t0.6
wall-101100K0.5
wall-111273K0.6
wall-121173K0.6
wall-131173K0.6
(c)Click OK to close the Wall panel.
6.Close the Boundary Conditions panel.
Step6:Solution
1.Modify the solution parameters.
Solve?→Controls?→Solution...
(a)Deselect P1from the Equations selection list.
(b)Select PRESTO!from the Pressure drop-down list in the Discretization group box.
This is often useful for buoyant?ows where velocity vectors near walls may not
align with the wall due to assumption of uniform pressure in the boundary layer.
Thus,PRESTO!can only be used with quadrilateral or hexahedral meshes.
(c)Click OK to close the Solution Controls panel.
2.Initialize the?ow?eld.
Solve?→Initialize?→Initialize...
(a)Select velocity-inlet-4from the Compute From drop-down list.
(b)Set the Swirl Velocity to0m/s.
(c)Click Init and close the Solution Initialization panel.
3.Enable the plotting of residuals during calculation.
Solve?→Monitors?→Residual...
4.Start the calculation by requesting200iterations.(Figure4)
Solve?→Iterate...
2D Simulation of a300KW BERL Combustor
Figure4:Scaled Residuals
5.Save the case and data?les,berl-mag-1.cas.gz and berl-mag-1.dat.gz.
6.Modify the solution parameters.
Solve?→Controls?→Solution...
(a)Select P1from the Equations selection list.
(b)Click OK to close the Solution Controls panel.
7.Request for an additional100iterations.
8.Save the case and data?les,berl-mag-2.cas.gz and berl-mag-2.dat.gz.
9.Modify the solution parameters.
Solve?→Controls?→Solution...
(a)Enter1for P1in the Under-Relaxation Factors group box.
(b)Click OK to close the Solution Controls panel.
2D Simulation of a300KW BERL Combustor
10.Request for an additional500iterations.(Figure5)
The solution converges in approximately30additional iterations.
11.Save the case and data?les,berl-mag-3.cas.gz and berl-mag-3.dat.gz.
Figure5:Scaled Residuals
https://www.wendangku.net/doc/cc11113255.html,pute the gas phase mass?uxes through all the boundaries.
Report?→Fluxes...
(a)Calculate the Mass Flow Rate with velocity-inlet-4and velocity-inlet-5as Bound-
aries.
(b)Calculate Mass Flow Rate with pressure-outlet-3as Boundary.
The mass balance will not be good at this point.Both these?gures should be equal
and opposite in sign to each other.
https://www.wendangku.net/doc/cc11113255.html,pute the gas phase energy?uxes through all the boundaries.
(a)Select Total Heat Transfer Rate from the Options list.
(b)Select all the zones from the Boundaries selection list and click Compute.
(c)Close the Flux Reports panel.
14.Lower the convergence criteria for Continuity to10-5.
Solve?→Monitors?→Residual...
15.Solve for another1000iterations.(Figure6)
The solution converges in approximately900additional iterations.
16.Save the case and data?les,berl-mag-4.cas.gz and berl-mag-4.dat.gz.
2D Simulation of a300KW BERL Combustor
Figure6:Scaled Residuals
https://www.wendangku.net/doc/cc11113255.html,pute the gas phase mass?uxes through all the boundaries.
Report?→Fluxes...
(a)Calculate the Mass Flow Rate with velocity-inlet-4and velocity-inlet-5as Bound-
aries.
(b)Calculate Mass Flow Rate with pressure-outlet-3as Boundary.
The mass imbalance is smaller as compared to the previous case.Both these
?gures should be equal and opposite in sign to each other.
https://www.wendangku.net/doc/cc11113255.html,pute the gas phase energy?uxes through all the boundaries.
(a)Select Total Heat Transfer Rate from the Options list.
(b)Select all the zones from the Boundaries selection list and click Compute.
(c)Close the Flux Reports panel.
19.Display contours of?ow variables of interest.
In particular,look at temperature,velocities,and species variables.(Figures7—9).
2D Simulation of a300KW BERL Combustor
Figure7:Contours of Static Temperature
Figure8:Contours of Velocity Magnitude
2D Simulation of a300KW BERL Combustor
Figure9:Contours of Mass Fraction of O2
Results
Use of the DO radiation model,which is more CPU intensive,and also a second order solution,can help to increase the accuracy of the predictions.
Summary
Inherent limitations in the available models result in inaccuracies while predicting interme-diate species.Overall,fairly meaningful results within engineering accuracy are obtained.