«DESIGN OF AN INTEGRAL THERMAL PROTECTION SYSTEM FOR FUTURE SPACE VEHICLES By SATISH KUMAR BAPANAPALLI A DISSERTATION PRESENTED TO THE GRADUATE SCHOOL ...»
Other assumptions of note include the assumption of a perfect conduction interface between the face sheets (and webs) and the insulation materials, that is, there is no thermal contact resistance at the interface. The insulation material is usually made of a low density porous material, such as Saffil®, which is made of alumina fibers. Even though this insulation material is assumed to completely block out all the radiation from the top surface to other parts of the ITPS, there is some radiative heat transfer to the interior of the ITPS due to the porous nature of the insulation material [7,17]. Also, there could be a convective heat transfer through the insulation material due to the air present in the pores [7,17]. For the design process, the radiative and convective heat transfer through the insulation material is ignored and only the conductive heat transfer is taken into account.
3.1.3 One-Dimensional and Two-Dimensional FE Models As explained in the previous section, there is no lateral heat flow across the unit cells.
Thus, the FE heat transfer analysis was limited to unit cell analysis, instead of taking the whole ITPS panel into account. Further, a 2-D FE model in the y-z plane (refer Figure 2-1 for the coordinate directions) is sufficient as there would be no temperature variation in the x-direction in this design. The heat transfer FE problem could be further simplified to a 1-D model. This would save considerable time for the transient heat transfer FE analysis. In order to show that a 1-D model can effectively do the job of a 2-D model, a comparative study was carried out. This section will describe the 1-D and 2-D models and show the comparative studies. All finite element analyses for this research were carried out using ABAQUS® finite element software package.
A typical 2-D FE model is shown along with its mesh in Figure 3-4. The solid portion of the ITPS is made of a titanium alloy (Ti-6Al-4V) and the insulation material is Saffil.
Temperature dependent material properties were used for both materials. Eight-node quadrilateral heat transfer element is used for 2-D modeling (ABAQUS element DC2D8). The number of nodes used in the model was 10,149 and the number of elements was 3,306.
Figure 3-4. Typical mesh for 2-d heat transfer problem A) the solid portion of ITPS only, B) complete ITPS including the insulation material in between the webs.
A 1-D FE heat transfer model is just a straight line of length equal to the height of the ITPS panel plus the thicknesses of the top and bottom face sheets. One-dimensional 3-node (quadratic) heat transfer link element (ABAQUS element DC1D3) was used for 1-D modeling. 109 nodes and 54 link elements were used in this model. Figure 3-5 schematically illustrates a 1-D model.
The corrugated-core of the panel is homogenized, while the top and bottom face sheets remain the same as in 2-D model. The homogenized properties of the core are calculated by the rule of mixtures formulas. The formulas below show the homogenized properties for density, specific heat and thermal conductivity.
ρ stands for density, C for specific heat, and k for conductivity. The subscripts 1 and 2 represent titanium and Saffil, respectively, while the superscript * represents the properties of the homogenized core. V* is equal to the sum of V1 and V2. A stands for the cross-sectional area for the heat flow. Multiplying by sinθ implies that, for the titanium webs, the heat flux component in the panel-thickness direction only is taken into account for this calculation. This takes into account the angle of corrugations, θ, of the webs.
Figure 3-5. Schematic representation of 1-D heat transfer model.
Figure 3-6 shows the comparison between the 1-D and 2-D FE heat transfer analyses results for an ITPS panel with dimensions, tT = 2.0 mm, tB = 6.0 mm, tW = 3.0, θ = 82.0, d = 140 mm, p = 75 mm. Heat flux input, boundary conditions and materials selection were discussed in the previous section. Figure 3-6A shows the temperature versus reentry time for two locations on the 2-D model. Loc-1 and Loc-2 are two points on the top face sheet where the temperatures are at the extremes. For example, during the 3 reentry phases when heat flux is incident on the top surface, Loc-1 will be at the highest temperature while Loc-2 will be at the lowest temperature of all the locations on the top face sheet. The 1-D heat transfer analysis does a good job of predicting the top face sheet temperature which is around the average of the temperatures at Locand Loc-2 in the 2-D model. Figure 3-6B shows the temperature variation with time on the bottom face sheet. Loc-3 and Loc-4 are two of the extreme locations on the bottom face sheet.
The 1-D model again does a good job compared to the 2-d model temperatures as the maximum difference is less than 5%. Figure 3-6C shows the temperature variations at 3 different locations on the web. The 1-D model does a very good job of predicting the temperatures at all these locations. An important conclusion from Figure 3-6C is that the 1-D model does a good job in predicting the temperature distribution through the thickness of the ITPS panel. Thus we can conclude that the 1-d heat transfer finite element model computes the temperatures and temperature distributions sufficiently accurately at all reentry times and can be reliably used for the design process.
3.1.4 Temperature vs. Reentry Time and Temperature Distribution Temperature versus reentry time curves for top and bottom face sheets and mid point of web are shown in Figure 3-7 for comparison purposes. As mentioned earlier, the temperature on the bottom surface peaks after the vehicle landing (approximately 2175 sec). These curves were obtained from the 1-D heat transfer analysis.
Temperature distribution through the thickness of the ITPS panel is shown in Figure 3-8 at different reentry times. At 450 seconds, which is the end of the initial phase of reentry, the bottom face sheet is still at its initial temperature. This is the time at which the temperature gradient through the panel thickness is at its severest. The distribution at 1575 seconds is when top surface reaches its peak temperature, at 3455 seconds the bottom surface reaches its maximum temperature and at 1845 seconds the mid point of the web reaches its maximum temperature. Each of these temperature distributions can be accurately represented by a complete cubic polynomial in one variable (z-coordinate) fitted using least squares approximation technique.
Figure 3-7. Temperature variation vs. reentry times for top and bottom surfaces and web midpoint obtained from 1-d heat transfer analysis. Dimensions of the ITPS panel are the same as listed in Figure 3-6.
Figure 3-8. Temperature distribution through the thickness of the ITPS panel at different reentry times. Dimensions of the ITPS panel are the same as shown in Figure 3-6.
3.1.5 Obtaining Temperature Data from the FE Analysis After the 1-d transient heat transfer analysis has been performed on an ITPS model, temperature versus reentry time data at different points on the ITPS can be obtained from the ABAQUS output file (similar to Figure 3.7). Using this data the peak temperatures of top and bottom face sheets can be obtained. As mentioned earlier, the peak top face sheet temperature helps determine the material to be used for the top face sheet. The peak bottom face sheet temperature is used in the design optimization process to impose the upper limit on the temperature attained by the bottom face sheet.
Apart from the peak temperature values, the reentry time at which the peaks occur can also be obtained. The temperature at each node in the 1-d heat transfer model at each of these reentry times can be extracted from the ABAQUS output file. Combining the nodal temperature values with the nodal coordinates (z-coordinate), the temperature distribution through the thickness of the ITPS can be accurately obtained as one complete cubic polynomial at each reentry time of interest. The coefficients of the cubic polynomial are determined by least squares approximation technique. The temperature distribution polynomials at different reentry times can be used to impose the nodal temperatures in the stress and buckling FE analyses.
ITPS panels are to be designed to withstand significant transverse and in-plane mechanical loads and extreme thermal gradients through the panel thickness. In order to make the ITPS economical, it is necessary to design panels which are large in size. This would imply that there would be large unsupported or partially supported sections of thin plates subjected to various kinds of loads including thermal compressive stresses and in-plane mechanical compressive loads. Such sections would be susceptible to buckling. While local buckling, by itself, may not always lead to catastrophic failure, it could contribute indirectly. For example, if the top surface buckles locally it could lead to extremely high local aerodynamic heating which could prove to be catastrophic.
Finite element analysis for buckling is carried out using ABAQUS. In the finite element model, only the solid portion of the ITPS panel is taken into account, which includes the face sheets and the web. The insulation material is not considered to be a structural member. This is indeed true because Saffil insulation is a soft fibrous insulation with hardly any mechanical properties when compared to the properties of the solid material that make up the webs and face sheets. Therefore, it can be safely omitted from all structural analyses without introducing any palpable error.
The ITPS panel is made of thin plates. Therefore, 3-D shell element is the most suitable element for modeling the structure. Eight-node shell element (ABAQUS element S8R) with 6 degrees of freedom at each node (3 displacements and 3 rotations) and reduced integration was used for the buckling FE model. Around 5560 nodes and 1820 elements were used for each buckling model. A typical shell-element mesh for buckling analysis is shown in Figure 3-9.
Figure 3-9. Typical FE shell element mesh for buckling analysis. Two unit cells are shown in this figure. The panel edges are marked A, B, C and D.
In the heat transfer problem a unit-cell analysis was carried out. Unit cell analysis is not possible in the case of the buckling analysis because the boundary conditions for the unit cell buckling problem are unknown. Therefore, the buckling analysis was carried out by including the whole ITPS panel in the FE model. This introduces an additional variable into the problem, which is the length of the panel (considering only square shaped panels). Instead of the length, the number of unit-cells in the panel could be considered as a variable. Either the length or the number of unit cells need to be specified in order to completely define the geometry of the panel.
Figure 3-9 shows one-quarter of an ITPS panel. The panel has a total of 4 unit cells. However, only 2 unit cells are necessary to model the panel by taking into account the symmetry conditions.
The boundary conditions on the ITPS panel depend on how the panels would be mounted on vehicle. For this research, it is assumed that the edges of the panels are mounted on the stringers and frames of the vehicle. Usually, provision is made for the panels to expand slightly when heated. This arrangement precludes the development of large thermal stresses. The top face sheet experiences the highest temperatures and should be allowed to expand as much as possible. For this research work, it is assumed that the edges of the bottom face sheet of the panels are mounted on the stringers and frames and simply supported boundary conditions are imposed. The edges of the top face sheet are fixed with respect to all 3 rotations while allowing the displacements. In Figure 3-9, on Edges A and B are the actual edges of the panel. The bottom face sheet edge on these edges is fixed in z-direction displacement and the top face sheet edge is fixed in all three rotations while allowing all three displacements. Edges C and D are the symmetric edges of the FE model. On Edge C, the top and bottom face sheet edges and the web edges are fixed in x-direction displacement and y- and z-direction rotations to simulate the symmetry boundary conditions. Similarly, the symmetry boundary conditions on Edge D are simulated by fixing the y-direction displacement and x- and z-direction rotations.
The loads for the buckling problem include temperature loads, aerodynamic pressure loads and in-plane inertial loads. Temperature loads were obtained in the form of through thickness temperature distributions from the heat transfer problem. The temperature distributions are cubic polynomials in one variable, the z-coordinate. Using these polynomials, temperature was imposed on each node of the 3-D buckling model. This implies that the top and bottom face sheet temperatures is uniform throughout the length and width of the panel. Although the temperature varies slightly in the x- and y- directions, this variation is very small and can be neglected. The pressure loads are imposed on the top surface. In-plane loads are imposed only in the x-direction of the panel. These loads were imposed on the Edge A on the bottom face sheet only.
The buckling problem in ABAQUS was modeled as an eigenvalue buckling prediction problem. It was used to estimate the critical (bifurcation) load for the structure. The eigen buckling analysis is a linear perturbation procedure in which the objective is to determine the loads at which the model stiffness matrix becomes singular, so that the equation
has nontrivial solutions. K is the tangent stiffness matrix when loads are applied and u is the nontrivial displacement solutions. The buckling eigenvalues or loads are estimated relative to the base state of the structure. The base state includes all the boundary conditions and the noncritical loads called pre-loads, P, if there are any such loads. In the buckling eigenvalue step an incremental load, Q, is applied to the structure. The equation for the buckling problem then becomes