Upcoming SlideShare
×

# Combustion tutorial ( Eddy Break up Model) , CFD

2,668 views

Published on

Published in: Design, Technology
3 Likes
Statistics
Notes
• Full Name
Comment goes here.

Are you sure you want to Yes No
• Be the first to comment

Views
Total views
2,668
On SlideShare
0
From Embeds
0
Number of Embeds
0
Actions
Shares
0
0
0
Likes
3
Embeds 0
No embeds

No notes for slide

### Combustion tutorial ( Eddy Break up Model) , CFD

1. 1. STAR-CCM+ User Guide 4410 Combustion Tutorials Three types of models have been chosen for combustion tutorials: • An idealized CAN type gas turbine combustion chamber • A flame tube • Methane on platinum These models will familiarize you with STAR-CCM+’s combustion modeling capabilities and introduce various recommended practices for simulating combusting flows. CAN Type Gas Turbine Combustion Chamber The problem geometry (shown below) consists of three sets of air inlets placed circumferentially at the combustor head to promote maximum mixing and flame stabilization. Swirling air enters the primary combustion zone through the two sets of inlets nearest to the axis of symmetry. Non-swirling air enters the upper inlet and thence the primary, secondary and dilution zones via five injection holes in the baffle. Air is assumed to be composed of 23.3% oxygen and 76.7% nitrogen, by mass, and its initial pressure and temperature are 1 bar and 293 K, respectively. Version 4.04.011
2. 2. STAR-CCM+ User Guide 4411 The use of periodic interfaces allows the cylindrical combustor to be represented by a single sixty-degree sector, reducing the computational effort required by a factor of roughly 5 ⁄ 6 . The combustion models illustrated using the above geometry are: • Propane combustion using a 3-step Eddy Break-up model. • Propane combustion using an adiabatic PPDF model. • Hydrogen combustion using an adiabatic PPDF Flamelets model. Flame Tube The problem geometry consists of a two-dimensional representation of a flame tube. The flow involves an inviscid, compressible, multi-component gas whose components are reacting chemically. A premixed mixture of hydrogen and air enters the pipe through an inlet at a pressure of 1 bar and a temperature of 1000K. The combustion model illustrated using this geometry is the complex chemistry operator splitting model. Methane on Platinum Methane on platinum deposition is modeled by importing complex chemistry descriptions from external files. In this simulation, a premixed combination of methane and air flows over a platinum plate at a pressure of 1 bar and a temperature of 600K. Version 4.04.011
3. 3. STAR-CCM+ User Guide 4412 3-Step Eddy Break-Up Tutorial This tutorial models propane combustion in air using a 3-step Eddy Break-up model as detailed below: C 3 H 8 + 1.5O 2 → 3CO + 4H 2 (9) CO + 0.5O 2 → CO 2 (10) H 2 + 0.5O 2 → H 2 O (11) The physical properties of the air components (23.3% O2 and 76.7% N2, by mass) and the rest of the reaction components (C3H8 , CO, H2 , CO2 , H2O) are defined as follows: O2 N2 C3H CO H2 8 Molecular weights Density Molecular viscosity Specific heat Thermal conductivity 32.0 28.00 8 CO O 2 44.1 28.0 1 2.01 44.01 H2 18.02 8 Ideal gas 1.716 x 10–5 Pas Determined via thermodynamic polynomial functions Determined via the Lewis number Air enters the combustion chamber through the three air inlets and propane gas enters through the fuel inlet, as indicated in the introductory Combustion Tutorials section. Both air and fuel are at a pressure of 1 bar and a temperature of 293 K at the inlets. Importing the Mesh and Naming the Simulation Start up STAR-CCM+ in a manner that is appropriate to your working environment and select the New Simulation option from the menu bar. Version 4.04.011
4. 4. STAR-CCM+ User Guide 3-Step Eddy Break-Up Tutorial 4414 Visualizing the Imported Geometry To view the geometry more clearly, change the viewing direction. • Open the Scenes > Geometry Scene 1 > Attributes node, then right-click on the View node. • Select Edit.... • In the Edit View dialog, enter the values shown below and then click Apply. • Close the Edit View dialog. To make the interior features of the combustor geometry visible, change the opacity of its surfaces. Version 4.04.011
5. 5. STAR-CCM+ User Guide 3-Step Eddy Break-Up Tutorial 4420 • First select the Segregated Flow node. • In the Properties window, change the Convection property to 1st-order. • Repeat this process for the Segregated Species, Segregated Fluid Enthalpy and Standard K-Epsilon nodes. • Save the simulation by clicking on the (Save) button. Setting Material Properties The components of the mixture and its material properties must now be defined. Version 4.04.011
6. 6. STAR-CCM+ User Guide 3-Step Eddy Break-Up Tutorial 4424 • Select the C3H8 > Component Properties > Specific Heat node. • In the Properties window, change the Method property to Thermodynamic Polynomial Data • Repeat this process for the remaining six components. This completes the specification of material properties. • Save the simulation. Deﬁning Reactions • Within the Models node, select the Eddy Break-up node. Version 4.04.011
7. 7. STAR-CCM+ User Guide 3-Step Eddy Break-Up Tutorial 4427 • Select the C3H8 node and, in the Properties window, enter 1.0 for the Stoich. Coeff. • Repeat this for O2 , CO and H2 , assigning stoichiometric coefficients of 1.5, 3.0 and 4.0, respectively. The specification of Reaction 1 is now complete. • Follow the same procedure to define the remaining two reactions of the chemical reaction scheme: CO + 0.5O 2 → CO 2 (12) H 2 + 0.5O 2 → H 2 O (13) • Save the simulation. Setting Initial Conditions and Reference Values The lower temperature limit for the specific heat polynomials imported from the materials database is 200 K. Although this temperature is much lower than we would expect to find in the converged solution, it is possible that temperatures below this may arise early on in the run. For this reason, it is necessary to increase the minimum allowable temperature to match the lower temperature limit for the polynomials. Version 4.04.011
8. 8. STAR-CCM+ User Guide 3-Step Eddy Break-Up Tutorial 4430 • In the Properties window, set the Value property to 293 K. • Select the Turbulence Specification node. • In the Properties window, select Intensity + Length Scale for the Method property. • Set the turbulence intensity to 0.05 and the turbulent length scale to 0.2. • Save the simulation. Creating Interfaces All regions and boundaries already have suitable names so we can proceed to create the periodic interface linking the two plane, rectangular, cyclic boundaries. • Open the Regions > Default_Fluid > Boundaries node. A node will be displayed for each boundary region. Version 4.04.011
9. 9. STAR-CCM+ User Guide 3-Step Eddy Break-Up Tutorial 4432 Two new periodic boundary nodes will appear under the Boundaries node and a new node named Periodic 1 will appear under the Interfaces node. Setting Boundary Conditions and Values All wall boundaries, including the baffle, are adiabatic, no-slip walls. Since this is the default wall boundary type, no changes are required here. The default settings are also suitable for the outlet, so the only boundary conditions that need to be specified are for the four inlets. • Select the Air_Inlet1 > Physics Conditions > Velocity Specification node. • In the Properties window, change the Method property to Components. • Select the Turbulence Specification node and, in the Properties window, change the Method property to Intensity + Length Scale. The air and fuel will be made to swirl on entry to the combustor by specifying inlet velocity vectors in a new cylindrical coordinate system. To create the latter: • Open the Tools node, right-click the Coordinate Systems node and then Version 4.04.011
10. 10. STAR-CCM+ User Guide 3-Step Eddy Break-Up Tutorial 4440 • Click OK. • Select the Fuel_Inlet > Physics Values > Velocity > Constant node. • In the Properties window enter -28,-60,100 m/s for the Value property. Specification of the boundary conditions is now complete. • Save the simulation. Setting Solver Parameters and Stopping Criteria The default under-relaxation factors for the flow and turbulence equations are suitable for this case but those for the species and energy equations need to be reduced to ensure solution convergence. • Select the Solvers > Segregated Species node. • In the Properties window, change the Under-Relaxation Factor property to 0.8 • Select the Segregated Energy node and change the Fluid Under-Relaxation Factor property to 0.8 also. It is important that the under-relaxation factors for the species and energy equations are the same to ensure that the two solutions remain synchronized. Other species and energy modeling settings, such as the choice of differencing scheme, should also be kept the same. The simulation will be run for 500 iterations, which is sufficient to achieve a steady-state solution. This number can be specified using a stopping criterion. Version 4.04.011
11. 11. STAR-CCM+ User Guide 3-Step Eddy Break-Up Tutorial 4447 • Add the plane section part to the Selected list. • Click Close. • Right-click on the scalar bar in the display. In the pop-up menu that appears, select Temperature. • Rotate the scalar scene until the view is roughly perpendicular to the plane section (which is colored beige in the geometry scene), and the inlet boundaries are on the left. • Save the simulation. Reporting, Monitoring and Plotting STAR-CCM+ can dynamically monitor virtually any quantity while the solution develops. This requires setting up a report defining the quantity of interest and the parts of the region to be monitored. A monitor is then defined based on that report. The former also helps to create an appropriate X-Y graph plot. Version 4.04.011
12. 12. STAR-CCM+ User Guide 3-Step Eddy Break-Up Tutorial 4452 • Rename the Carbon In Plot node as Carbon Balance. • Make sure that the Title property of the Carbon Balance node is Carbon Balance. • Double-click the Carbon Balance node to display the empty plot in the Graphics window. The analysis is now ready to be run. • Save the simulation. Running the Simulation • To run the simulation, click the (Run) button on the toolbar. If this is not displayed, use the Solution > Run menu item. You may also activate the Solution toolbar by selecting Tools > Toolbars > Solution and then clicking the toolbar button. The Residuals display will be created automatically and will show the solver’s progress. If necessary, click on the Residuals tab to bring the Residuals plot into view. An example of a residual plot is shown in a separate part of the User Guide. This example will look different from your residuals, since the plot depends on the models selected. Version 4.04.011
13. 13. STAR-CCM+ User Guide 3-Step Eddy Break-Up Tutorial 4454 solution has indeed converged. • Save the simulation. Visualizing the Results • Select the Scalar Scene 1 display to view the temperature profile for the Version 4.04.011
14. 14. STAR-CCM+ User Guide 3-Step Eddy Break-Up Tutorial 4457 angle so that velocity vectors are clearly visible. Summary This tutorial introduced the following STAR-CCM+ features: • Importing the mesh and saving the simulation. • Visualizing the geometry. • Defining models for eddy break-up combustion. • Defining material properties required for multi-component gases. • Defining chemical reactions. • Setting initial conditions and reference values. • Creating interfaces. • Defining boundary conditions. • Setting solver parameters and stopping criteria. • Creating vector and scalar displays for examining the results. • Setting up monitoring reports and plots. • Running the solver for a set number of iterations. • Analyzing the results using STAR-CCM+’s visualization facilities. Version 4.04.011
15. 15. STAR-CCM+ User Guide Adiabatic PPDF Equilibrium Tutorial 4459 combustor.ccm. • Click Open to start the import. The Import Mesh Options dialog will appear. Select the following options: • Run mesh diagnostics after import • Open geometry scene after import • Ensure that the Don’t show this dialog during import option is not selected and then click OK. STAR-CCM+ will provide feedback on the import process, which will take a few seconds, in the Output window. A geometry scene showing the combustor geometry will be created in the Graphics window. • Finally, save the new simulation to disk under file name adiabaticPPDF.sim. Visualizing the Imported Geometry To view the geometry more clearly, change the viewing direction. • Right-click the Scenes > Geometry Scene 1 > Attributes > View node and Version 4.04.011
16. 16. STAR-CCM+ User Guide Adiabatic PPDF Equilibrium Tutorial 4461 • Open the Displayers node and select the Geometry 1 node. • In the Properties window, change the Opacity property to 0.2. The baffle and the five injection holes in it are now visible through the external surface of the combustor. You can now proceed to Setting up the Models. Setting up the Models Models define the primary variables of the simulation, including pressure, temperature and velocity, and what mathematical formulation will be used to generate the solution. In this example, the flow involves a turbulent, compressible, multi-component gas whose components are reacting chemically. The Segregated Flow model will be used together with the standard K-Epsilon turbulence model and the PPDF reaction model. To select the models: • Open the Continua node, right-click on the Physics 1 node and select Version 4.04.011
17. 17. STAR-CCM+ User Guide Adiabatic PPDF Equilibrium Tutorial 4466 node. • In the Properties window, change the Convection property to 1st-order. • Repeat this process for the Adiabatic PPDF and Standard K-Epsilon nodes. • Save the simulation by clicking the (Save) button. The next step is Defining Mixture Components. Deﬁning Mixture Components The PPDF table used in this tutorial involves only six gaseous species: C3H8, O2, N2, CO, CO2 and H2O which, for demonstration purposes, should provide a solution of reasonable accuracy. A more realistic solution could be obtained by including additional intermediate species in the table. To define the gas components corresponding to the above species: Version 4.04.011
18. 18. STAR-CCM+ User Guide Adiabatic PPDF Equilibrium Tutorial 4468 do not need to be changed so we can now proceed to Generating the PPDF Table. Generating the PPDF Table First, we will change the number of heat loss ratio points defined in the table: • Select the PPDF Equilibrium Table node. • In the Properties window, make sure that the Number of heat loss ratio points equals 1. • Change the Relative Pressure of the mixture property to 0.0 Pa. Now define the fuel and oxidizer streams: • Select the Fluid Stream Manager > Fuel Stream node. Change the Temperature of the stream property to 293 K. • Right-click on the Fuel Stream > Components node and select Version 4.04.011
19. 19. STAR-CCM+ User Guide Adiabatic PPDF Equilibrium Tutorial 4471 Setting Initial Conditions The combustor’s initial condition is a stationary flow field consisting entirely of air. The default values of initial mixture fraction, mixture fraction variance and velocity are all zero so no changes to the initial conditions are required. Creating Interfaces All regions and boundaries already have suitable names so we may now create the periodic interface linking the two plane, rectangular, cyclic boundaries. • Open the Regions > Default_Fluid > Boundaries node. A node is shown for each boundary region. • Ctrl+click to select the Cyclic1 and Cyclic2 nodes. Version 4.04.011
20. 20. STAR-CCM+ User Guide Adiabatic PPDF Equilibrium Tutorial 4479 • In the Properties window, enter a Value of 1.0. • Select the Fuel_Inlet > Physics Values > Velocity > Constant node. • In the Properties window enter -28,-60,100 m/s for the Value property. Specification of the boundary conditions is now complete. • Save the simulation. Setting Stopping Criteria Adjust the maximum number of iterations so that the calculation will run for 600 iterations, which should be sufficient for a steady-state solution. This number can be specified using a stopping criterion. • Open the Stopping Criteria node and then select the Maximum Steps node. • Change the Maximum Steps property to 600. The solution will not run beyond 600 iterations, unless this stopping criterion is changed or disabled. • Save the simulation. Version 4.04.011
21. 21. STAR-CCM+ User Guide Adiabatic PPDF Equilibrium Tutorial 4482 appears, select Temperature. • Select the Scenes > Geometry Scene 1 > Displayers > Section Scalar 1 node. • In the Properties window, change the Contour Style property to Smooth Filled. • Rotate the geometry scene until the view is roughly perpendicular to the beige plane section and the inlet boundaries are on the left. • Save the simulation. Running the Simulation • To run the simulation, click the (Run) button on the toolbar. Version 4.04.011
22. 22. STAR-CCM+ User Guide Adiabatic PPDF Equilibrium Tutorial 4484 Visualizing the Results • Go to the Geometry Scene 1 display to view the temperature profile for the converged solution. • Right-click on the scalar bar in the Geometry Scene 1 display and select Version 4.04.011
23. 23. STAR-CCM+ User Guide Adiabatic PPDF Equilibrium Tutorial 4488 The resulting scene is shown below. It will be seen that the ratio’s value is generally rather high, implying that the predicted maximum temperature is considerably lower than the adiabatic flame temperature. In a realistic modeling exercise, a considerably finer mesh would be needed to increase confidence in the calculated temperatures. Summary This tutorial introduced the following STAR-CCM+ features: • Importing the mesh and saving the simulation. • Visualizing the geometry. • Defining an adiabatic PPDF combustion model. • Generating a PPDF table. • Creating interfaces. • Defining boundary conditions. • Setting stopping criteria. • Creating scalar displays for examining the results. Version 4.04.011
24. 24. STAR-CCM+ User Guide 4490 Adiabatic PPDF Flamelets Tutorial In this tutorial, a hydrogen combustion case is set up using the PPDF Laminar Flamelets reaction model for unpremixed flames. The model assumes adiabatic conditions (no heat loss) and accounts for non-equilibrium and finite-rate chemistry effects. For adiabatic PPDF, the physical properties of the fuel (hydrogen in this case) are not utilized directly by STAR-CCM+ as no additional transport equations requiring these properties are solved. Temperature, density and species mass fractions are evaluated using the β function formulation (see the Adiabatic Equilibrium Model section in the User Guide). Air enters the combustion chamber through the three air inlets and hydrogen gas enters through the fuel inlet, as indicated in the introductory Combustion Tutorials section. Importing the Mesh and Naming the Simulation Start up STAR-CCM+ in a manner that is appropriate to your working environment and select the New Simulation option from the menu bar. Continue by importing the mesh and naming the simulation. A predominantly hexahedral cell mesh has been prepared for this analysis. and saved in the STAR .ccm file format. • Select File > Import... from the menu bar. • In the Open dialog, simply navigate to the doc/tutorials/combustor subdirectory of your STAR-CCM+ installation directory and select file Version 4.04.011
25. 25. STAR-CCM+ User Guide Adiabatic PPDF Flamelets Tutorial 4493 • Open the Displayers node and select the Geometry 1 node. • In the Properties window, change the Opacity expert property to 0.2. The baffle and the five injection holes in it are now visible through the external surface of the combustor. You can now proceed to Setting up the Models Setting up the Models Models define the primary variables of the simulation, including pressure, temperature and velocity, and what mathematical formulation will be used to generate the solution. In this example, the flow involves a turbulent, compressible, multi-component gas whose components are reacting chemically. The Segregated Flow model will be used together with the standard K-Epsilon turbulence model and the PPDF reaction model. To select the models: • Open the Continua node, right-click on the Physics 1 node and select Version 4.04.011