Steady state CFD analysis of C-D nozzle
2 likes1,108 views
The document outlines a methodology for solving fluid dynamics problems using ANSYS Fluent, including steps for defining the solution domain, material properties, mesh generation, and boundary conditions. It details the CFD analysis of a nozzle design, showcasing results and comparisons between theoretical and CFD outcomes for varying divergence angles. Conclusions indicate that while CFD results may diverge from theoretical calculations, they remain sufficiently close to validate the effectiveness of one-dimensional analyses in predicting nozzle performance.
Steady state CFD analysis of C-D nozzle
- 1. 1 CHAPTER -4 METHODOLOGY 4.1 GENERIC STEPS TO SOLVING PROBLEM IN FLUENT Like solving any problem analytically, you need to define (1) your solution domain, (2) the physical model, (3) boundary conditions and (4) the physical properties. You then solve the problem and present the results. In numerical methods, the main difference is an extra step called mesh generation. This is the step that divides the complex model into small elements that become solvable in an otherwise too complex situation. Below describes the processes in terminology slightly more attune to the software. Build Geometry Construct a two or three dimensional representation of the object to be modeled and tested using the work plane coordinates system within ANSYS. Define Material Properties Now that the part exists, define a library of the necessary materials that compose the object (or project) being modeled. This includes thermal and mechanical properties. Generate Mesh At this point ANSYS understands the makeup of the part. Now define how the Modeled system should be broken down into finite pieces. Define Boundary Conditions Once the system is fully designed, the last task is to burden the system with constraints, such as physical loadings or boundary conditions. Obtain Solution This is actually a step, because ANSYS needs to understand within what state (steady state, transient… etc.) the problem must be solved. Present the Results After the solution is obtained, there are many ways to present ANSYS‟ results, choose from many options such as tables, graphs, and contour plots. The solver used in this model is FLUENT, a commercial popular CFD solver from ANSYS Inc. Solidworks of DS is also used to model the geometry as per the study and its conversion into a neutral format.
- 2. 2 4.1.1 Domain Every CFD simulation requires a domain where it is discretized and apply the governing equations. The domain thus encompass the CAD geometry, boundary conditions, control volumes and governing equations. In this project we have designed a nozzle based on the data garnered from the journal we mostly have referred. The CAD drawing of the model from Solidworks is shown below The dimensions of the model is as follows Table 4.1Nozzle dimensions The model is drawn axisymmetric ally so only half of the dimensions shown is taken to model the nozzle Figure 4.1Cad drawing of a nozzle with a divergence angle of 11.3deg
- 3. 3 This CAD model, in order to do the analysis, has to be converted into a geometrically neutral format called step (*.stp) before importing the model into the simulation environment. Below is how the CAD part looks after it is imported into Ansys. Figure 4.2 Axisymmetric model of the nozzle in Ansys design modeler. In the later phase of the project the divergence angle of the nozzle is changed to 13 and 15 degrees. Figure 4.3 Model with 13 degrees divergence angle
- 4. 4 Figure 4.4 Model with 15 degrees divergence angle The 11.3 degree divergence angle model is initially taken into the meshing environment where mesh will controlled both locally and globally. In any CFD analysis the mesh quality is so important and a critical factor that affects the overall accuracy of the model. In this study we have taken utmost care to make sure all the elements used in the model is of high quality nature. These are achieved by the careful manipulation of the mesh settings available in the Ansys Meshing tool; ICEM CFD. The meshed model is shown underneath. Figure 4.5 11.3 degree nozzle after meshing
- 5. 5 The mesh chosen is high quality HEX mesh with very little or no skew. This mesh has a global as well as local settings. The global settings affect the size and nature of the mesh in a global sense where as local settings help us affect or influence the mesh in a local sense. Figure 4.6 Mesh settings with local and global controls As explained above the shape the mesh is assigned to be very important when considering the solution accuracy and the solver stability. Hence there are two metrics to quantify or asses the condition of the mesh. They are (a) Orthogonal quality and (b) Skewness. Both metrics vary between 0 and 1. Orthogonal quality has to be maximum and Skewness has to be minimum. The pick of mesh elements is so crucial that any distorted from ideal shapes if selected may lead to difficult in solving and less accurate results. The mesh element used in this model is of high quality one i.e. hex mesh in 2D.
- 6. 6 Figure 4.7Mesh Skewness From the above figure it’s obvious that there are 5880 elements and the cell centers of these elements are taken into account for finding out the pressure and velocity fields. The average orthogonal quality is 0.982 and the average skewness value is 0.083. These values when seen as ideal have a values of 1 and 0 respectively. In order to complete the definition of domain we still need the boundary conditions. Boundary conditions are applied over the edges or boundaries in this case as shown below. Ansys needs proper identification of the boundaries or edges in the way of Named Selections. Figure 4.8 Mesh Orthogonal quality
- 7. 7 Figure 4.9. Naming or Identification of boundary zones The boundary conditions taken for this analysis are tabulated as follows Figure 4.10 Boundary condition illustration Table 4.2Boundary conditions Boundary Type Value Inlet Pressure 100atm Inlet Temperature 3300K Outlet Pressure 1.68atm Material chosen for this analysis is Air (ideal gas), Properties are shown below Table 4.3 Material properties Cp=1880J/kgK Thermal conductivity=.0142W/mK Viscosity=8.983e-5 PaS
- 8. 8 CHAPTER -5 SOLVER SETTINGS The solver selected to solve this problem is a density based solver. The dependence of time is turned off in the solver settings. Hence we do a steady state analysis. Compressible flows with Mach number greater than 3 are usually dealt with the density based solver. Mach number is presumed to be higher since the inlet and outlet pressure ranges are so enormous. The application of these nozzle pressures find place in rocket propulsion activities. 5.1 SOLVER AND SOLUTION SETTINGS Table 5.1 Solver and Solution settings `General Solver type- Density based 2D space : Axisymmetric Models Energy equation: On Viscous model: Standard k-epsilon, realizable , enhanced wall treatment Solution controls Courant number=5(Changes with 10 intervals) Solution initialization Full Multi Grid(FMG) Run Calculation Solution steering method is adopted Iterations 5000 Since the axisymmetric model is checked, all the conservation equations will be solved in a cylindrical coordinate system. To include the effects of temperature in the governing equations, energy equation is turned on The turbulent eddy viscosity model used is standard k epsilon model, where k stands for turbulence kinetic energy and epsilon for the turbulent KE dissipation rate. Local mesh settings have been invoked to additionally smear high aspect ratio mesh cells on the geometry to capture the boundary layer turbulence
- 9. 9 phenomenon. That will only be calculated if the enhanced wall treatment is turned on. The only condition that exists for calculation of the wall effects is the height of the first cell adjacent to the wall should be very small. But too much small mesh cells near the boundary layer leads to convergence difficulties. Figure 5.1 High quality mesh cells with inflation layers 5.2 RESIDUALS Since the mathematical model (Governing equations+Boundary conditions) is discretely solved over the domain, two kinds of errors constitute, they are (1) Discretization error and (2) linearization error. The discretization error occurs when the domain is divided into a finite number of control volumes whereby only the cell center values are calculated. The continuous values are then computed after getting the pressure and velocity field values at the cell centers. This is done through advanced interpolation methods on the cells and their immediate neighbors. The distant the neighbors are the inaccurate the interpolated values become. Thus discretization errors are brought down by refining the mesh. But the value never becomes zero. Second error that is inevitable in the CFD simulation or other numerical method is the linearization error. Since the variables are nonlinear to find the root or the unknown function is bit hard. Thus these nonlinear equations are linearized using guess values and iterate them until the actual function is computed as a range between two values. This iteration can’t be run eternally. By stopping the
- 10. 10 chain of events requires inputting another value called the Residual or the tolerance limit. If the differences in values of two successive iterations fall below this residual value the loop ceases. Setting the residual is also challenging. In some cases if the residuals are input to be of very small order, difficulty in convergence occurs. Thus it has to be input by trial and error. 5.3 CONVERGENCE CRITERION Table 5.2Convergence criterion RESIDUAL ABSOLUTE CRITERIA Continuity 1e-8 X velocity 1e-8 Y velocity 1e-8 Energy 1e-8 K 1e-8 Epsilon 1e-8 Figure 5.2 Convergence Curve after the iterations Turning on the FMG initialization, one of the advanced initialization techniques available within the solver, the number of iterations taken to reach convergence has dramatically been reduced.
- 11. 11 CHAPTER -6 RESULTS AND DISCUSSION Following are the results obtained after the iterations For the nozzle with the divergence angle 11.3 degrees Figure 6.1 Pressure contours Figure 6.2 Temperature Contours
- 12. 12 Figure 6.3 Velocity Contours Table 6.1Velocity comparison Section Ax/A* Velocity (m/s) Theoretical CFD Convergent 1.5 169.72 163.17 Convergent 1.2 482.91 478.139 Throat 1 1030.46 1022.64 Divergent 1.2 1335.28 2072.32 Divergent 4 2051.23 2081.47 Outlet 7.142 2387.52 2353.49 Table 6.2 Pressure Comparison Section Ax/A* Pressure(atm) Theoretical CFD Convergent 1.5 87.33 96.68 Convergent 1.2 79.89 88.49 Throat 1 50.96 58.915 Divergent 1.2 32.08 32.87
- 13. 13 Divergent 4 10.98 7.63 Outlet 7.142 1.68 1.34 Table 6.3 Temperature Comparison Section Ax/A* Temperature (K) Theoretical CFD Convergent 1.5 3240.08 3290.36 Convergent 1.2 3194.12 3223.75 Throat 1 2972.98 3012.7 Divergent 1.2 2760.50 2746.02 Divergent 4 2137.56 2154.2 Outlet 7.142 1774.90 1800.5 Figure 6.4 Mach number variation along the axis
- 14. 14 6.1 DIVERGENCE ANGLE WHEN VARIED Initial CFD analysis had been conducted with the nozzle angle pegged at 11.3 degrees. This value has been changed to 13 and 15 degrees and the effects are evaluated. The expected trend would be as the throat area drops the velocity rises and as a result the pressure and the temperature drops. DIVERGENCE ANGLE OF 13 DEGREES Figure 6.5 Pressure contour at 13 deg divergence angle Figure 6.6 Temperature contour at 13 deg divergence angle
- 15. 15 Figure 6.7 Velocity contour at 13 deg divergence angle Figure 6.8 Mach number variation at 13 deg divergence angle
- 16. 16 DIVERGENCE ANGLE OF 15 DEGREES Figure 6.9 Pressure contour at 15 deg divergence angle Figure 6.10 Temperature contour at 15 deg divergence angle Figure 6.11 Velocity contour at 15 deg divergence angle
- 17. 17 Figure 6.12 Mach number variation at 15 deg divergence angle Table 6.4 Maximum and Minimum Parameter changes for 13 deg diverging angle Temperature(K) Pressure(Pa) Velocity(m/s) Min Max Min Max Min Max 1636 3285 1.6e4 1e7 137 2478
- 18. 18 Table 6.5 Maximum and Minimum Parameter changes for 15 deg diverging angle Temperature(K) Pressure(Pa) Velocity(m/s) Min Max Min Max Min Max 981 3279 -6e4 1e7 148.9 2680
- 19. 19 CHAPTER -7 CONCLUSION Following are the conclusion drawn from the analysis. (1) CFD considers the factors like boundary layer effects, shock waves, radial velocity component and so on, which leads to some variance from theoretical results. (2) The variation in the results of theoretical calculations and CFD are quite insignificant. (3) It thus establishes the fact that one-dimensional simplified nozzle analysis is sufficient to predict the nozzle performance. From the study conducted to assess the variation of divergence angle to the pressure, velocity and temperature It has been conclusively clear that as the divergence angle increases there’s a sudden rise in velocity and thus decrease in temperature and pressure.