FEA Analysis of 3D Printed and Fiber- or Mylar-clad Foam Parts
Properly stressing the 3D printed SLS nylon and the fiber- or Mylar-clad foam elements is probably best left until the detailed design stage, but if preliminary results are required for these elements, some steps can be taken without reaching for a fully featured design. For example, to limit design effort and computational cost, the 3D printed nylon parts can be modeled as thick-walled structures. To do this, we simply adopt a specified equivalent thickness having calibrated the resulting weights and stresses against our experience of the performance achievable from a more fully detailed structure; see Figure14.14 where a 4-mm-thick wall has been created using the shell commands of the CAD package. Although this model is more complicated to build and mesh, the resulting mesh has fewer elements, which can be used to better effect; meshing fully solid parts with a fine mesh rapidly increases the element count. When this approach is used to study the forward SLS nylon boom supports, it reveals that
Figure 14.12 Deformed shape and von Mises stress plot for full Decode-1 spar model with locally refined mesh under wing flight loads taken from XFLR5 together with a load factor of 4 plus elevator and fin loading based on Cl values of unity.
the peak contact stress with the tail boom is now predicted to be locally 57.8 MPa but that this falls rapidly away from the fine edges. At the same time, the peak contact stress with the main spar is only 5.6 MPa, while the stresses in the spars are hardly changed from before, see Figure 14.15. Reducing the equivalent wall thickness to 2 mm raises the peak nylon stress in its finest area to 84.6 MPa and that near the main spar to 24.2 MPa, see Figure 14.16, suggesting that 2 mm wall thickness is probably more appropriate for an equivalent stress model in this case. Note, however, that thin-walled structures notoriously suffer from local buckling, and thus far our Abaqus analysis, though dealing with contact stresses, does not allow for buckling (or nonlinear material properties). It is inadvisable to push this kind of simplified structural analysis model too far; the final part will contain rib-stiffening to control buckling and the SLS nylon will undoubtedly suffer from local yielding where it is in contact with the CFRP spars.
To model the aerodynamic surfaces, we need to model both the lightweight foam core and its cladding. Again, a simplified approach is possible, and we proceed as before but join the inner surface of the cladding to the outer surface of of the foam with tie constraints all over. The foam is also created using the shell commands of the CAD package plus suitable fillets, here with a 10 mm wall thickness which is typical of the sort we manufacture. The foam parts are easily meshed with standard 3D brick hex elements, see Figure 14.17. The cladding is created as a very thin shell surrounding the foam, and we use continuum shell elements to model it in
Figure 14.13 Deformed shape and von Mises stress plot for full Decode-1 spar model with fully refined mesh and reduced boundary conditions under wing flight loads taken from XFLR5 together with a load factor of 4 plus elevator and fin loading based on Cl values of unity.
Figure 14.14 Simplified Abaqus thick-walled structural model for Decode-1 SLS nylon part. The mesh for this part contains 25 000 elements.
Abaqus. These allow direct meshing of the solid body produced by AirCONICS despite the very thin nature of the cladding, here 0.1 mm - continuum elements allow for the extreme aspect ratios produced when elements are this thick while being 10 mm and more in the other
Figure 14.15 Deformed shape and von Mises stress plot for thick-walled nylon part in full Decode-1 spar model with fully refined mesh and reduced boundary conditions under wing flight loads taken from XFLR5 together with a load factor of 4 plus elevator and fin loading based on Cl values of unity.
directions, without the need to switch to traditional surface-based shell models, which are less easily constructed from CAD models. Suitable material properties can be found in Tables 18.3 and 18.4, although we always reduce the Young’s modulus value for the glass fiber to allow for the reduced fiber-to-resin ratios achieved in very thin claddings. A value of 25 GPa is a reasonable approximation that is borne out by the results of experimental vibration testing of wings.
It is important when using continuum shell elements that sweep meshing be used to build the mesh and the through-thickness direction is correctly specified as the sweep direction. To do this, we partition the cover into separate parts using the Partition commands in the Tools menu: first, the main upper and lower surfaces are separated at the leading and trailing edges with face partitions; and then, if sharp trailing edges are in use, the upper and lower trailing edges are split off using the “sweep edge along edge” process to further partition off the trailing edges, which are then triangular in cross-section. If a truncated trailing edge is being used (perhaps because a flap has been cut from the section), the part is partitioned at the truncation points. The main upper and lower covers are next meshed using swept medial axis hex meshes with the stack directions defined by selecting the outer faces. If a sharp trailing edges is adopted,
Figure 14.16 Deformed shape and von Mises stress plot for 2 mm thick-walled nylon part in full Decode-1 spar model with fully refined mesh and reduced boundary conditions under wing flight loads taken from XFLR5 together with a load factor of 4 plus elevator and fin loading based on Cl values of unity.
the two resulting wedge sections are meshed using hex wedge elements. These are compatible with the continuum shells, and the fact that we are not using shells in this very small region will make little difference, see Figure 14.18. If a truncated trailing edge is used, this may have to be meshed using tetrahedral solid elements linked with tie constraints.
The foam parts are coupled to the rest of the structure via contact interactions with the spars and also with lugs added to the SLS nylon parts, see Figure 14.19. Pressure loads are then applied to the outer surface of the cladding that surrounds the foam, using values taken from the XFLR5 analysis, and these replace the body forces previously applied to the spars, see Figure 14.20. The pressures are applied using an Abaqus-mapped field created through the “tools - analytical field - create” option, which allows the data from XFLR5 to be entered from a comma separated file with X, Y, and Z coordinates taken directly from the XFLR5 output and the Cp values converted to pressures by multiplying by 0.5pV2. Note that the data entry dialogue box has a “mapper controls” tab where the tolerances used to do the mapping can be set. Then, when creating a pressure load, the analytical field can be referenced along with a value of 4 for the load magnitude to simulate the 4g loading. Obviously, the XYZ pressure
Figure 14.17 Abaqus model of foam core created with CAD shell and fillet commands and meshed with brick hex elements.
Figure 14.18 Abaqus model of glass-fiber wing cover created with CAD shell commands and meshed with continuum shell hex elements. Note the wedge elements used for the sharp trailing edge.
Figure 14.20 Pressure map on Decode-1 foam part under wing flight loads taken from XFLR5.
Figure 14.19 Abaqus assembly with foam parts added, highlighting the tie constraint between the foam and the SLS nylon support.
data must be in the same geometric locations as the AirCONICS CAD model used to create the structural model.
Note that XFLR5 only supplies mid-surface aggregated pressure loads unless a full 3D panel analysis is carried out; such analyses are currently only possible for wing alone configurations in the code. Thus to get the desired pressure loads for the mold line surface, one first sets up the full aircraft with elevators, fins, and so on, to establish the desired flight conditions and then re-analyses the wing alone at the desired speed and angle of attack to generate the pressure loads for the wing (these then being suitably scaled to simulate the desired load cases taken from the Vn diagram). The resulting analytical field inside Abaqus can be used to load multiple parts in the FEA, as Abaqus can correctly work out which part of the field needs to be used for which surface when defining the pressure loads. If pressure loads are required for the elevator, this has to be set as the main wing in XFLR5 and an approximate angle of attack and speed have to be deduced by trial and error so as to get to the same net forces as seen on the elevator for the full configuration. This is a tedious process and rarely warranted for structural analysis of the elevator foam parts, as they typically see smaller stresses than the main wings (though they can flex noticeably if the hinge spars are too small in diameter, something that can adversely affect controllability).
Figures 14.21 and 14.22 show the resulting deflections and stresses in the foam, cover, and supporting SLS nylon part when a section of the main wing foam is analyzed in this way. Here, the peak stresses in the foam are 0.45 MPa, those in the cover 38 MPa, and those in lug region of the nylon 35 MPa. Thus there are small regions of the foam that are close to the material limit in this model, while the nylon is acceptably below its limits and the glass-fiber cladding well below its ultimate strength. Note, however, that the failure mechanisms seen in tensile and compression tests of woven glass-fiber-reinforced plastic specimens are rather different from those we have observed in our airframe parts: ultimate failure of our wing foam parts is caused by delamination of the cover where the adhesive layer between the foam and cover fails locally, followed by crushing of the foam. A much more detailed FEA model would be required to study this kind of behavior since the resin layer between the glass fiber and foam would need to explicitly modeled and a very fine mesh used in the foam element. Moreover, the nonhomogeneous properties of the fiber reinforcement would also need to be allowed for.
Pressure loads can also be extracted from runs of Fluent by using the file export solution data capabilities of the code: an ASCII space delimited file should be created for cell center static pressures on the bodies for which loads are required. This will create a (typically very large) text file with a header row and five columns of data (cell number, x-coordinate, y-coordinate, z-coordinate, and pressure). Before these can be read into Abaqus, the header and any blank trailing rows have to be removed along with the first column. Once read into Abaqus, the size of the original data file does not matter, as Abaqus calculates a loading pattern appropriate to the part the pressure is mapped onto. Because Fluent can be used to study arbitrarily complex geometries, pressures can be applied to all the external surfaces of the Abaqus model in this way, including deflected control surfaces, assuming they both originated from the same AirCONICS (or other) CAD-based geometry definition.
Figure 14.21 Resulting deflections and stresses in foam core and cover for wing under flight conditions.
Figure 14.22 Resulting deflections and stresses in SLS nylon part with foam mounting lug for wing under flight conditions.
-  We find it difficult to make claddings thinner than 0.08 mm, and even this thickness is very hard to achieve evenlyover the whole wing surface.
-  If the “Redefine Sweep Path • • •” option in mesh controls is used, a small red conical arrow is shown defining thesweep direction. This must be normal to the surface of the cover; selecting the outer surfaces as the top surface in the“Assign Stack Directions • • •” option will enforce this.
-  Because the files are often very large (perhaps containing over a million lines), this is not completely straightforward. However, a simple Windows batch file can be written to strip the first column. It should contain two lines: @ECHOOFF and for /F etokens=2-5e %%a in (%1) DO ( echo %%a %%b %%c %%d). Once the data hasbeen stripped in this way, the header line and any blank lines at the bottom should be removed by manual editingbefore it is read into Abaqus.