«DESIGN OF AN INTEGRAL THERMAL PROTECTION SYSTEM FOR FUTURE SPACE VEHICLES By SATISH KUMAR BAPANAPALLI A DISSERTATION PRESENTED TO THE GRADUATE SCHOOL ...»
Using the values of variables in the matrix V, the ITPS Optimizer creates a 1-d heat transfer FE model starting with the first combination. This is done by creating an ABAQUS Script File which is written using Python language commands. This script file contains all the geometry commands by which a line is drawn and partitioned into 3 sections - top and bottom face sheets and homogenized core. Then material assignment commands are used to assign the material properties to the respective sections. The properties of the homogenized core are calculated using Equations (3.2)–(3.4). Commands for creating load steps, applying loads and boundary conditions, and meshing commands are also written into the Script File. All these Python language commands are written into the Script File using Matlab M-file commands. The script files are saved with an extension ‘.py’. Once the script file is ready, ABAQUS® is invoked to read the script file. The invocation is achieved using the following M-file statement
ABAQUS® executes the Python commands in the script file and creates a ‘.cae’ file, which is the geometric model. The Script File also includes commands which create an ABAQUS® Input File. An ABAQUS® Input file is a link between ABAQUS CAE and ABAQUS Solver. An input file contains all the node numbers and coordinates, element numbers, node and element sets, material property information, load steps, loads and boundary conditions information. All this information is in a format recognizable by the ABAQUS Solvers. For this research ABAQUS Standard Solver is used. Usually, the input file is modified by the ITPS Optimizer to put in all the desired information. The input files are required to be saved using the extension ‘.inp’. This input file is then submitted to the ABAQUS Standard solver using the following statement
This command is for ABAQUS version 6.5-1. If a different version is used then the command is different. For example the command is ABQ631, if ABAQUS version 6.3-1 is used.
ABAQUS solver solves the FE problem and creates an output database (ODB) file, which contains all the FE solution information. Required information can be extracted from the ODB files by creating and executing other script files that contain suitable output extraction python commands. Temperature versus time output and nodal temperatures at different reentry times of interest are extracted and printed out in the form of text files. Data from these text files is then obtained and the peak temperatures are determined. Also, the nodal temperature data is used to compute cubic polynomials for temperature distribution through the thickness of the ITPS panel at different reentry times of interest.
The ITPS Optimizer process for buckling is similar to that for heat transfer analysis. Script files are created and executed to obtain a 3-D shell model and FE mesh of the panel. The input file contains all of this information. This input file is modified to impose nodal temperatures on the model using the temperature distributions obtained from heat transfer analysis. Since the buckling analysis is carried out at different reentry times, new input files are created for each reentry time containing the nodal temperature loads from the corresponding temperature distribution data. These input files are then submitted to ABAQUS solver and output database files and ‘.dat’ files are obtained. eigenvalues are obtained from the ‘.dat’ files. At each eigenvalue, the nodal displacements are extracted for the output database file by creating and executing scripts files. The nodal displacements are listed in text files from which the ITPS optimizer extracts the data and determines the buckling position for each eigenvalue.
The ITPS optimizer procedure for stress and deflection analysis uses the same mesh and input files as the buckling analysis. However in this case, the buckling step is changed to static analysis and the material properties are also suitably altered to accommodate the temperature dependent material properties. Using script files, nodal displacements of top face sheet and von Mises stress of various sections in the ITPS panel are printed to text files. The ITPS optimizer extracts the data from these text files and determines the maximum values required for the generation of response surface approximations.
Optimization was carried out with a MATLAB code developed for this purpose. The code uses in-built subroutine fmincon ( ). The response surface approximations obtained from the ITPS Optimizer were input into this code to impose constraints. The optimization process was carried out 10 times with a different starting point at each optimization. The different starting points were obtained by Latin-Hypercube Sampling so that they are spread out uniformly in the design space. If different optimized designs are obtained for different starting points, then the design with lowest weight is chosen as the optimized design.
In the previous two chapters, the finite element analyses and procedure for optimization were discussed. This will be followed by optimization and design of ITPS panels in this chapter.
First, the loads, boundary conditions and other input parameters in the ITPS design will be discussed. Two types of designs have been explored – a) corrugated-core and b) truss-core. The design of truss-core structures will be presented in the second part of the chapter. The truss-cores were found to be unable to withstand the large thermal stresses generated in the ITPS panels. A discussion on the difficulties in truss-core modeling and the reasons for these cores being unfit for ITPS panels will be presented in the last part of this chapter.
5.1 Selection of Loads, Boundary Conditions and Other Input Parameters The ITPS design has been performed generically without any specific vehicle in mind.
Although, the future space vehicles are most probably of the space capsule type, most of the data for these vehicles is not available. So the loads considered for this design were typical of a Space Shuttle-like vehicle.
A discussion on the reentry heat flux input for a Space Shuttle Orbiter-like vehicle has been presented in Section 3.1.1. For this research work, metal alloys have been used for the ITPS panels. Therefore, heat flux input profiles that produce temperatures that are below service temperatures of these alloys can only be used. The heat flux profile chosen for the design of the corrugated-core panels has been shown in Figure 5-1.
The radiation equilibrium temperature (see Section 3.1.1 for details) for the peak heat flux is 946 K for an emissivity of 0.8 and ambient temperature of 295 K. The peak temperature of top face sheet is usually close to the radiation equilibrium temperature. Therefore, titanium alloy (TiAl-4V) has been chosen for the top face sheet and web material. For the bottom face sheet, beryllium alloy has been chosen. Temperature dependent material properties have been listed in Appendix. Further discussion about material selection and recommendations for choice of materials will be presented in the Chapter 6.
Heat influx rate, Btu/ft2-s Figure 5-1. Heat flux input used for the design of corrugated-core structures.
The bottom face sheet of the ITPS panel is assumed to be perfectly insulated. Some of the other input parameters for the heat transfer problem are (See Section 3.1.1 for more details)
• Emissivity of the top surface: 0.8 Coefficient of convection on the top surface after landing: 5.0 Wm-2K-1 •
• Ambient temperature for 0 to 450 sec: 213 K
• Ambient temperature for 450 to 1575 sec: 243 K
• Ambient temperature for 1575 to 2175 sec: 273 K
• Ambient temperature after landing: 295 K
• Initial temperature of the structure before reentry: 295 K Aerodynamic pressure load on a Space Shuttle-like design is shown during reentry in Figure 5-2. The external pressure is close to zero during the reentry phase and becomes equal to atmospheric pressure after landing. Therefore, during the reentry phase, the pressure load on the external surface is taken equal to zero. Usually, the crew compartment is separated from the outer shell, which is the TPS. The crew compartment is under pressure suitable to human comfort. The space between the crew compartment and the outer shell is assumed to be vented to the outer atmosphere. Therefore, before reentry, this vented space would be at zero pressure (pressure in the Space). During reentry phase the pressure load on both sides of TPS is zero and hence there is no pressure load applied on the ITPS panels during reentry phase. After the vehicle lands, the outside pressure is equal to the atmospheric pressure. Even though the space between crew compartment and the TPS is vented to the atmosphere, there will be a certain lag time before the pressure on both sides of the TPS becomes equal. During this lag time, there is a pressure load on the outer surface. Taking the worst case scenario into consideration, the pressure load on the outer surface is considered equal to 1 atmosphere or 101,325 Pa. To summarize, the pressure load on the ITPS panels is equal to zero in all buckling and stress analysis cases before landing and is equal to 1 atmosphere after landing.
Another mechanical load on the ITPS is the in-plane inertial load during the reentry phase.
The inertial load is compressive in nature during the reentry phase because the vehicle is slowing down due to aerodynamic braking. Typical weight of space capsules is estimated to be around 10,000 kg and maximum estimated load due to aerodynamic braking is 5g, equal to 5×9.8 = 49 m/s2. Therefore, the total load on the back shell of a space capsule is equal to a maximum of 490,000 N. Assuming that the space capsules have a diameter of 5 meters, the in-plane load on the backshell of the space capsule can be obtained by dividing the total load by the circumference of the backshell and is approximately equal to 30,000 N/m. This in-plane load is applied to the ITPS buckling and stress analysis only during reentry phase. After landing, no inplane load is applied on the ITPS.A summary of the pressure load and in-plane loads in presented in Table 5-1.
Figure 5-2. Aerodynamic pressure load on the TPS for a Space Shuttle-like design. The pressure remains close to zero during reentry phase and becomes equal to the atmospheric pressure after landing.
The boundary conditions for the buckling and stress analysis cases are dependent upon the way in which the ITPS panel is connected to the vehicle. For this research work, it is assumed that the bottom face sheet is connected to the stringers and frames of the vehicle. Usually, an allowance in the connections is provided in such a way that the bottom face sheet is allowed to expand so as to minimize the thermal stresses developed in the structure. So, simply supported boundary conditions are imposed on the bottom face sheet edges of the panel.
Table 5-1. Summary of mechanical loads applied on the ITPS panel for buckling and stress analysis cases.
No pressure load on the top surface In-plane load of 30,000 N/m Reentry Phase Pressure load of 1 atm on top surface No in-plane load After Landing The top face sheet is usually the thinnest section of the ITPS panel. Excessive thermal compressive stresses can cause the top face sheet to buckle. Therefore, a good design would allow the top face sheet to expand freely. However, the free edges are susceptible to buckling if left free. It is assumed that the panel edges are closed out by a thin metal foil connecting the top face sheet to the bottom face sheet. These foils help in containing the insulation material within the panel. The mechanical properties of the metal foil are assumed to be negligible. However, the foil applies certain restraint on the top face sheet edges. This restraint is approximately simulated by restraining the rotations on the edges of the top face sheet. Such a constraint would apply mild restraint on the top face sheet edges while precluding the development of large thermal stresses.
Thus the panel edges on the top face sheet are restrained in rotations and no constraints are placed on the displacements.
It is clearly evident that there are a number of assumptions involved in the various input parameters, loads and boundary conditions on the ITPS panel. One of the most important reasons for these assumptions is because this design process is for a generic ITPS panel as there is no specific vehicle for which it is being designed. Most of the assumptions were made in order to obtain a reasonable ITPS design. It is almost impossible to proceed with the design process if all the parameters were to be close to reality, because not all parameters are well defined for the design problem at hand. The significance of all these input parameters is studied by individually varying these parameters and observing their effect on the ITPS design. The results for these analyses will be presented in the Chapter 6.
The following 6 geometric variables completely describe a unit cell of a corrugated-core ITPS panel, as shown in Figure 1-2 and reproduced here as Figure 5-3,
7. Thickness of top face sheet, tT,
8. Thickness of webs, tW,
9. Thickness of bottom face sheet, tB,
10. Angle of corrugations, θ,
11. Height of the sandwich panel (center-to-center distance between top and bottom face sheets), h,
12. Length of a unit-cell of the sandwich panel, 2p.
Figure 5-3. A unit cell of a corrugated-core ITPS panel illustrating the 6 design variables.
An additional design variable introduced here is the number of unit cells, n, in one panel.