CHAPTER 4 Numerical Models This chapter presents the development of numerical models for sandwich beams/plates subjected to four-point bending and the hydromat test system. Detailed descriptions of the boundary conditions, element types, validation, and the force distribution collection methods are discussed. Optimization measures of the numerical models are also included in this chapter. The finite element software used in the development of the numerical models is I-DEAS Master Series 9m3 [30]. The relatively robust and user-friendly solid modeling and finite element meshing interface are the main advantages of this solid modeling/ finite element software. 4.1 Model Assumptions All the numerical analyses done in this research involves the use of non-linear analysis capability of I-DEAS, including geometric non-linearity and material nonlinearity. With geometric non-linearity, the software takes the effect of shape change into account while calculating the solution. Using material non-linearity the non-linear behavior of the material response (i.e. post yield material properties) is taken into account. It is important to compare and contrast the assumptions made by the theoretical and numerical models in order to achieve meaningful comparisons. Below are the assumptions made for the numerical models: 1. Face sheets and core are perfectly bonded 52
The numerical model assumes no delamination occur between layers. This assumption is consistent with the assumptions made in the classical sandwich plate theory and higher order theory. 2. Face sheets remain elastic at all time Due to the significantly higher yield strength and modulus of elasticity of the face sheets compared to the core, face sheets are assumed to remain elastic throughout the loading for both the four-point bend test and HTS. This assumption is also consistent with the assumptions made in the classical sandwich plate theory and higher order theory 3. Load scenarios are quasi-static The two load cases considered were modeled quasi-statically instead of dynamically. Incremental loadings are applied slowly during the actual experiments. Therefore, the type of analyses done for this research effort is called static, non-linear analysis. 4. Geometric non-linearity has a significant effect Geometric non-linearity is considered to have significant effect on the load distribution on each layer of the sandwich structure. Therefore all the numerical analyses done take geometric non-linearity into consideration. This is the main difference between the numerical models and the theoretical models. Classical sandwich plate theory and higher order theory do not take shape change of the sandwich structures into account. 53
4.2 Four-point Bend Test Numerical Model The sandwich structure in the four-point bend test model had Aluminum 2024- T3 face sheets and a Herex C70.200 foam core as stated in chapter three. The beam model was partitioned into three layers, forming three perfectly bonded material layers. 4.2.1 Boundary Conditions/ Mesh Due to the symmetric nature of the problem, only half of the beam was modeled. The boundary conditions applied to the half beam model are shown in Figure 4.1. The beam has a roller support. Thus the left support of the model is given translational freedom in the X-direction and rotational freedom about the Z-axis. The vertical lines in Figure 4.1 show the partitions made along the beam s length in order to allow element force calculation in the post-processing part of the analysis. Y Region 1 P (Region 13) 2 Region 20 X Roller X translation free Y translation fixed Z rotation free Symmetry X translation fixed Y translation free Z rotation fixed FIGURE 4.1 Sandwich beam boundary conditions and partitions. 54
The partitions split the beam into several volumes which were labeled as Region 1 to Region 20 for convenience in data collection from the left to the right boundary. The element force calculation method will be discussed in detail later. A line load is applied to the top edge of Region 13 (Figure 4.1), simulating the load transmitted from the upper rollers to the beam. The beam is loaded with a set of loads that vary slowly with time, and results are calculated at each load step. Figure 4.2 shows the time variation form. FIGURE 4.2 Setting time varying load steps on I-DEAS. The time intervals between load steps are not important because the model is assumed to be quasi-static and the analysis type done is a static analysis. The finite element software was set in such a way that corresponding solutions are completed at 55
each load step as shown in Figure 4.3. This allows all the analysis to be done in a single run of the finite element model. As a result, the model would take up less memory space because one single solid model and finite element model can be used for all load steps. FIGURE 4.3 Setting multiple solution points on I-DEAS. The numerical model of the four-point bend test utilizes the mapped mesh capability of I-DEAS. By controlling the number of nodes along each edge of the solid model, this function allows total control of the mesh size. The element size is chosen by referring to Miers [14] work in mesh refinement. Miers [14] recommended a core element size of 1.5 mm and face element size of 3 mm in order to achieve convergence in the data obtained. Constant mesh density is ensured with the mapped meshing function. This is important because constant mesh density ensures that data collected from any region of the beam are of the same degree of resolution. Three-dimensional (solid) brick 56
elements are used in this analysis. Second order (parabolic) brick elements are chosen over the first order (linear) brick elements in order to better interpolate the data between nodes. Figure 4.4 shows the meshed model of the sandwich beam with corresponding boundary conditions. FIGURE 4.4 Meshed sandwich beam with boundary conditions. Since the analysis involves material non-linearity, a yield function or yield criteria needs to be defined for the model. Von Mises yield criteria and its associated flow rule are used in this analysis. Isotropic hardening is also used to describe the change of the yield criterion as a result of plastic straining. Only the core elements are assigned a yield function due to the assumption that only core yielding occurs throughout the loading process. The face sheets are assumed to remain elastic at all time, hence no yield function is assigned to the face sheet elements. 57
4.2.2 Validation In order to validate the finite element model, the numerically obtained loaddeflection curve is compared with the actual experimental load-deflection curve (Figure 4.5). 8000 Load (N) 6000 4000 2000 0 Experimental Numerical 0 1 2 3 4 5 6 7 Center Beam Deflection (mm) FIGURE 4.5 Comparison of load versus center deflection for four-point bend test. The numerical result shows good correlation with the experimental result. The slight discrepancy is due to the error caused by the material properties that do not fully define the post yield property of the core material. However, this model is sufficient to achieve the purpose of this research, which is to determine the load distribution within the sandwich beam and the effect of geometric non-linearity on this load distribution. 4.2.3 Element Force Collection In order to calculate the amount of load carried by each layer of the sandwich beam at several locations along the beam s length, the beam is partitioned into twenty 58
different portions. Each portion consists of top face sheet, core, and bottom face sheet, thus there are sixty volumes altogether. By utilizing the grouping capability of I-DEAS, specific volumes and finite element entities of interest can be grouped together and analyzed. The grouped model then functions as free body diagrams, allowing the author to find out the load distribution on the regions of interest. For example, as shown in Figure 4.6, the volumes before Region 16 and their related elements and nodes are grouped together. Full Beam Cut Beam Exposed Surface for analysis FIGURE 4.6 Grouped volumes and finite element entities of sandwich beam. By only showing this group of entities, the cross section of Region 16 can be exposed. The element force, stress and strain contour can be analyzed on that specific surface. In order to see the cross sections of all the sixty volumes of the beam model, 59
sixty groups were created. The groups were labeled as Core Region 1-20, Top Face Sheet Region 1-20, and Bottom Face Sheet Region 1-20. The groupings are like making a cut on a free body diagram. The Region 1 cut would consist of the volume prior to Region 1, Region 2 cut would include all the volumes before the Region 2 cross section, and so on. In order to find out the actual load carried by a particular layer (core, top face sheet or bottom face sheet) at any surface of interest, the load carried by each node on that surface needs to be calculated. To achieve this there are three challenges that need to be overcome: 1. Data search from the data pool The element force data associated with each node can be stored in a specific data file using I-DEAS. However, there is a need to extract the element force data that corresponds only to the nodes on the surface of interest. 2. Nodes of interest identification I-DEAS labels each node with a unique node number in order to make each node identifiable. Therefore each node that is on the surface of interest has a unique node number. There is a need to obtain the list of node numbers that corresponds to the nodes on the surface of interest. 3. Distinguish nodes on different material layer surfaces In the list of node numbers of interest collected, the nodes that correspond to each layer (core, top face sheet, or bottom face sheet) needs to be distinguished. The first step to overcome the above-mentioned problems is to collect the node numbers of the nodes on the surface of interest. In order to do this the author used the info function of I-DEAS to list the info of all the nodes on a specific surface. I-DEAS 60
allows its users to limit the entity selection. In this case, the author made nodes the only pickable entity. I-DEAS also allows a user to pick entities that are related to certain geometry. Therefore if the surface of interest is the cross section of the top face sheet, users can set the options as pick only nodes and related to surface, and then pick the cross section of the top face sheet. I-DEAS will then list the information about the nodes that are on that selected surface on the I-DEAS List screen (Figure 4.7). FIGURE 4.7 Node information on I-DEAS List window. The information listed including node numbers and their x, y, z-coordinate positions. This list of node information can be copied, pasted and saved on a text editor. Same process would be repeated for the cross section of each layers of each of the twenty regions along the beam, resulting a total of sixty sets of node numbers and locations. The next step is to extract the element force data. Element force data is extracted from the sixty volume groups. Thus there are sixty corresponding element force data files for the sixty groups of the beam. By using the Report Writer function of I- DEAS (Figure 4.8), the element force data can be generated and stored as.dat format. 61
FIGURE 4.8 Report writer window. Figure 4.9 shows an example of the element force data file for the region one core, opened using a text editor. The node numbers and element forces are then load and saved in a Matlab file. The information listed on the element force data file are the node numbers, element forces in x, y, and z directions, and moments about x, y, and z-axes. It should be noted that this coordinate system is with respect to the global coordinate system. The importance of this is explained in chapter five. At this point the element force data from the sets of free body diagram cuts and the node numbers sets on the surfaces of interest has been obtained. 62
FIGURE 4.9 Element force data file on Text Editor. The final procedure would be to match the node numbers on the surfaces of interest with the element force data files of each group of free body diagram cuts. A Matlab program (appendix A) was written to match the node numbers of a particular surface and extract the corresponding element force values from the corresponding set of element force data. All node forces can then be summed and the resulting load in the x, y, and z directions of a particular surface is obtained. 4.3 Hydromat Test System Numerical Model The sandwich panel used for HTS has 3003-H14 aluminum face sheets and an Airex R63.50 core. Similar to the beam model, the solid model of the sandwich panel subjected to HTS is partitioned into three perfectly bonded layers. 63
4.3.1 Boundary Conditions/ Mesh The symmetric nature of the problem allows only a quarter of the whole panel needs to be meshed. The boundary conditions used are shown on Figure 4.10. Region 1 Region 10 Y X Simply Supported X translation free Z rotation free Symmetry Y translation free Z translation free X rotation free FIGURE 4.10(a) Sandwich panel boundary conditions, X-Y plane. Region 1 Region 10 Y Z Simply Supported Z translation free X rotation free Symmetry Y translation free X translation free Z rotation free FIGURE 4.10(b) Sandwich panel boundary conditions, Y-Z plane. The two planes of symmetry of the panel have symmetric boundary conditions, where in-plane displacements and rotation about an axis respective normal to the symmetry plane is allowed. A simply supported boundary condition is applied to the two 64
other edges of the quarter plate. This simulates the simply supported condition of the panel resting on the HTS fixture. A distributed load is applied on the top surface of the sandwich panel, simulating the load transfer from the pressurized bladder to the panel. A step pressure model is used in this simulation. The area in which the distributed load is applied is the effective area obtained using equation 2.93. In other words, the contact area changes as the applied pressure increases. This approach is consistent with the theoretical model. Table 4.1 shows the corresponding contact area at different load steps analyzed and the total applied load. The effective contact area was obtained from Eyre s [25] work. Table 4.1 HTS loading details. Pressure Effective Contact Area Total Applied Load (kpa) (m 2 ) (kn) 17.2 0.180 3.10 34.5 0.189 6.52 51.7 0.196 10.14 68.9 0.201 13.83 86.2 0.205 17.63 103.4 0.208 21.55 The sandwich panel is partitioned into ten different regions that are labeled from Region 1 to Region 10 respectively (Figure 4.10(a), Figure 4.10(b)). Distributed loads are applied beginning from Region 4 to Region 10 (Figure 4.11). The effective contact region is assumed to be a perfectly square shape, therefore the aspect ratio between the length and width of the effective contact area is set as one. This uniform aspect ratio ensures the symmetry nature of the loading scenario and allows analysis done on only a quarter of the plate. 65
Region 4 Region 10 FIGURE 4.11 Distributed load applied on the panel top surface. Similar to the four-point bend test model, the elements used in this simulation are three dimensional, parabolic, brick elements. Again the element sizes were chosen according to the recommendation made in Miers [14] work, where a core element size of 1.5 mm and face element size of 3 mm are used. The solid model is meshed using the mapped meshing capability of I-DEAS. The core is assumed to be the only material that undergoes plastic deformation. The core elements use the Von Mises plastic yield function and undergo isotropic hardening. 4.3.2 Elastic Edge During the analysis, localized core yielding occurs due to the simply supported edges. Although a small region of the core right above the support lines is involved, the deformation in these regions were higher than other regions of the core. At the 103.4 kpa (15 psi) load step, excessive localized yielding occurs and halted the finite element analysis. In order to bypass this localized yielding problem, the core region that is 66
directly above the edge support was made elastic. The elastic edge has the same material properties as the foam core except there is no yield criteria assigned to elements of that region. This prevents the core from yielding at the region close to the support lines without changing the plate response significantly. Validation of this method is shown in the next section. Figure 4.12 shows the full elastic edge used for the 103.4 kpa load step. The effect of a half elastic edge was also investigated during the validation process. Half elastic edge simply means only the bottom half volumes of the edge is made elastic, and the top half volumes could still undergo plastic deformation. FIGURE 4.12 Full elastic edge (shown in green) used in sandwich core. 4.3.3 Validation In order to validate the finite element model the load versus center deflection curve obtained from the model is compared with the experimental data. The experimental 67
data is obtained from Eyre s [25] work in 1995. The numerical model shows good correlation with the experimental results. Error begins to grow as the core yielding begins to take place. This discrepancy is believed to be caused by inaccuracy in post yield material properties. 25000 20000 Load (N) 15000 10000 5000 0 Experimental Numerical 0 5 10 15 20 Center Panel Deflection (mm) FIGURE 4.13 Comparison of load versus center panel deflection for HTS. To ensure that the elastic edge added to the core does not alter the overall behavior of the sandwich plate, the 86.2 kpa (12.5 psi) load step was used as a check. The 86.2kPa load scenario was analyzed again for two other conditions, one with a half elastic edge and another with a full elastic edge. The center panel deflection difference between the models with elastic edges and the model without elastic edge were found to be less than 3%. The shear load distributions on each layer of the panel are shown in appendix C. Shear load plots of the three models on each layer of the sandwich panel considered show excellent agreement throughout the plate span. This shows that the elastic edge insert is a viable method and validates the usage of this method for the 103.4 kpa load step. 68
4.3.4 Element Force Collection The force collection procedures used for the HTS numerical model is similar to the four-point bend test numerical model. Load distribution on each layer is collected and summed on each surface of interest. Forces are collected with respect to the global coordinate system. The element forces on each surface of interest are then calculated using a Matlab program. The results obtained are presented in the next chapter. 69