Structural Design and Manufacturing of a Cruiser Class Solar Vehicle

NOTE: The design process of a solar vehicle is a quite complex task, involving multidisciplinary aspects, so it is not possible to cover them all here. In order to guide the reader, the logical process in which the described protocols are embedded is shown in Figure 1.

Figure 1: Design flow chart. The interactions between the different parts of the design process are depicted. Please click here to view a larger version of this figure.

1. Lay-up of the Main Chassis Design

1. Determine the load distribution in the worst-case scenario.
   1. Multiply the passengers’ and battery pack mass distributions by the design’s vertical acceleration to obtain the main design load.
   2. Consider the position of the seats and the different possible battery locations.
2. Calculate the reactions on the leaf spring joints. The vehicle is considered as a simply supported a-beam.
3. Determine the diagrams of the bending moment and shear.
4. Find the maximum allowable shear stress on the core material. Its value can be read in the core technical sheet or found by means of experiment on suitable specimens. In this case, the delamination stress of the core plies can be determined.
5. Calculate the sandwich core thickness based on the shear resistance^17,18 (where is the width over which the shear force is applied and is the core thickness).
   
6. Find the tensile and compressive strength of the available CFRP plies. Their value can be found in the plies’ technical sheets.
7. Determine experimentally the bending strength of the sandwich composites¹⁹.
8. Determine experimentally the ILSS for the possible combinations of materials^20,21.
9. Take into consideration the different sections of the vehicle, whose shape is designed in a trade-off between aerodynamic requirements and functional needs.
   NOTE: There are three critical sections in the chassis—the one with the highest bending moment, and the two ends, where the area is dramatically reduced due to the presence of the wheel-suspension systems. Moreover, in these two reduced sections, the shear must be transferred from the leaf spring to the chassis.
10. Make an assumption about the lay-up in the three sections considered and in the different parts of the sections, taking into consideration that the technological minimum¹⁷ is at least 10% of the fibers in each direction (0° [i.e., longitudinal], 90° [i.e., transversal], and ± 45° [i.e., diagonal]), the most important load acting in the specific part of the section, that the number of plies is integer, and that the thickness must be kept to a minimum.
11. Calculate the maximum tensile and compressive stresses according to the sandwich theory^17,18 and compare them to the allowable ones (where is the width over which the moment is applied and and are the thickness of the core and of the plies, respectively).
    
    1. Modify the lay-up, if necessary, and go back to step 1.9.
12. Make a finite element shell model in the software Abaqus and apply the impact-equivalent loads prescribed by the regulations²².
    1. Create the chassis in a CAD modeler.
    2. Import the chassis in the FEM software as a shell or solid part by clicking on Import | Part. If it is imported as a solid, use the Geometry Edit tool to transform it into a shell part.
    3. Define the properties of a single CFRP ply as Elastic material with type Lamina or Engineering Constants; select the elastic moduli and Poisson’s ratios of the material. Notice that engineering constants parameters are needed if the out-of-plane behavior of the shell is analyzed. Choose Hashin Damage Criterion to implement a failure criterion for the composite ply²⁶.
    4. Create a Composite Layups section by defining the stacking sequence of the laminate. Assign each ply its orientation and thickness in tabular form.
       NOTE: The post-curing thickness must be considered for the CFRP plies.
    5. Assign the distribution of discrete elements of the part by Mesh Seed. Use the Partition Face tool and Bias seed to increase the number of elements at the critical locations. Choose the Quad-dominated element shape and the Shell element type. Click on Reduced integration if the hourglass effects in the model are negligible; otherwise, use nonreduced integration.
    6. Create an instance of the chassis in the Assembly module. This is the one to which the loads and boundary conditions will be applied.
    7. Define the analysis procedure in the Step module as Static. Choose the settings of the solver. Select Nlgeom: On to activate nonlinear membranal behavior.
    8. Apply loads that are equivalent to the ones prescribed by the regulations as Body force loads on the chassis. Apply Concentrated forces at the batteries’ and occupants’ positions to take into account their lumped weights.
    9. Apply the BCs on the instance. Consider the chassis as a supported body acted upon by the external loads, with Pinned BC at the constrains’ locations.
    10. Define the outputs in the Field Output Requests module. Select Domain: Composite layup to extract the outputs at each ply’s location in the laminate.
    11. Create a Job and run the analysis.
    12. Verify the compliance of the results with the regulations’ requirements²². In case they are not fulfilled, go back to Steps 1.9 and 1.12.4 and modify the lamination sequence.
13. Produce a ply-book translating the section-by-section approach of the structural designer to a ply-by-ply approach needed by the manufacturer.
    1. Make special modifications in the sections where specific functional requirements lead to a reduction of the sandwich thickness.
14. Manufacture the chassis in an autoclave.
    1. Produce high-density foam patterns by precision milling.
    2. Guarantee a smooth surface finish with fine-granulometry sandpaper.
    3. Apply layers of sealer and release agent on the foam to assure the detachability of the carbon fiber molds.
    4. Manufacture the molds by assembling pre-impregnated low-catalysis-temperature carbon fiber layers and sealing each part with vacuum bag compression for a further autoclave cure.
    5. Polish the surface of the produced molds and apply sealer and release agents.
    6. Laminate the chassis parts over the mold according to the ply-book and submit them to vacuum bag compression and an autoclave cure.

2. Leaf Spring Design

Figure 2: Loading diagrams of the leaf spring. This figure shows the determination of the shear and of the bending moment acting on the leaf spring. Please click here to view a larger version of this figure.

1. Determine the load distribution along the leaf spring (see the bending and shear diagram of Figure 2).
   1. Evaluate the maximum load applied at the wheels of the vehicle in the worst-case scenario (see Step 1.1).
   2. Calculate the reactions forces (maximum load ) on the leaf spring ends, considering the suspension arm leverages.
   3. Define the supporting and loading points of the leaf spring based on its anchorage points to the vehicle chassis and the suspension ones.
   4. Determine the diagrams of bending and shear, modeling the leaf spring as a four-point bending beam with an equal maximum load applied at the ends (worst-case scenario).
2. Evaluate the maximum displacement of the leaf spring ends in accordance with suspension geometry and allowable space around the vehicle frame.
3. Select the material with the higher specific strain energy-storing capability, .
   
   Here, is the allowable stress, is the elastic modulus, and is the density.
   1. As bending is the dominant load of the leaf spring (the shear load is one or two orders of magnitude lower), keep the fatigue strength of the material as .
   2. For composite orthotropic materials, consider the fatigue bending strength of the FRP along the principal direction (fiber direction) as .
4. Conceptually design the leaf spring shape and lay-up, to maximize its specific energy storing capability.
   NOTE: The leaf spring cross section should be modeled so that the maximum allowable stress state occurs along all the leaf spring.
   1. Focus only on the bending diagram of Figure 2. The shear load is one or two orders of magnitude lower. Based on that, divide the leaf spring in two types of sectors: between the two supports () and between the supports and the leaf spring ends ().
   2. Along , keep the bending load constant and at its maximum; hence, also keep the cross-section constant.
   3. Along , increase the bending load linearly from the load application point to the support; hence, the cross-section height should satisfy the following equation to keep the stress constant on the outer surface of the leaf spring, along all its length.
      
      Here, is the distance from the point of application of the maximum load and is the cross-section width. The formula suggests that along the span, the leaf spring’s cross-section height should be tapered with a parabolic profile. However, for process practice reasons, approximate the leaf spring’s height profile with a linear one.
      ​NOTE: Keep constant to avoid fiber interruption during the lamination process, which will reduce the strength of the composite laminas.
   4. Because bending is higher than the shear load, use a sandwich structure with a linearly tapered core of 0-90 fabric FRP to resist shear loads and confer torsional stiffness to the leaf spring and outer layers of unidirectional FRP oriented with the leaf spring’s principal axis to contrast the bending load. The outer layers have a constant thickness to avoid geometrical discontinuities in the higher stressed zone.
5. Obtain the tensile, compressive, flexural, and shear strength of the selected FRP materials. Their value can be found in the technical data sheets or by means of a test based on ASTM standards (preferred option).
6. Optimize the leaf spring geometrical dimensions by means of an analytical model.
   NOTE: The objective function is to minimize the mass while complying to the imposed constraints; hence, sustain a maximum load with a deflection equal to and keep the stresses lower than the material-allowable ones.
   1. Constrain the condition on the maximum deflection for a specified max load .
      
      Here, is a small value inserted for convergence reasons. Conceptually, the leaf spring is a sandwich with a tapered core in the region. Calculate the deflection at the loading , by means of Castigliano’s method.
      
      Here, and are the flexural stiffness of the leaf spring along and , respectively.
      
      Here, and are the elastic modulus of the core and the outer layers, respectively,
      is the outer layer thickness, and is the core thickness.
      
      
   2. Constrain the condition on the maximum bending stress: (maximum UD fatigue bending stress). Evaluate by means of the Euler-Bernoulli theory.
      ​
   3. Constrain the condition on the maximum core and outer layer shear stresses: (maximum core fatigue shear stress) (maximum core fatigue shear stress). Evaluate and by means of the Euler-Bernoulli theory²⁴.
      
      ​
   4. Use the leaf spring mass as objective function to minimize.
      
      ​NOTE: The geometrical parameters which can be varied are: , , and . If allowed by the design of the anchorage points to the frame, and can also be considered as variables, if the following constrain is respected:
   5. Solve the problem iteratively or by means of optimization algorithms, which can be found integrated in several numerical computing software programs.
7. Perform an FE simulation of the optimized leaf spring in Ansys Composite Pre/Post (ACP). The goal is to evaluate the stress concentration and the out-of-plane loads.
   1. Draw, as a surface, the CAD geometry of only one quarter of the leaf spring, with the surface divided in correspondence with the support point and lay-up variations.
   2. Create a new simulation project in the ANSYS Workbench. Select ACP (Pre) (in the Toolbox menu) by dragging it into the workspace.
   3. Define material properties by clicking on Engineering Data. Select Engineering data sources and import from the Composite materials folder carbon UD and woven prepregs default material properties, by double-clicking on them. Update the material constants in the three principal directions with the ones available on the material data sheet or obtained from experimental results.
   4. Import the geometry while keeping the link with the CAD by right-clicking on Geometry and then on Import geometry. Import it in the native CAD format.
   5. Double-click on Model. Assign an arbitrary surface thickness. Define the different layup zones by using the Named Selection function (right-click on Model and then on Insert). Generate the default mesh by right-clicking on Mesh and then on Generate mesh.
   6. In Workbench, open ACP–Pre by double-clicking on Setup.
   7. Define the plies’ properties in the Material Data menu folder. Select Create Fabric by right-clicking on Fabrics; then, define the Material and assign the prepreg Thickness. Select Create Sub laminates by right-clicking on Sub Laminates and define the sub-laminate stacking sequence.
   8. Define the element local coordinates system in the Rosettes menu folder according to the principal direction of the lamination process (principal leaf spring axis).
   9. Orient the local coordinates of the FEM elements in the Oriented Selection Set menu folder by defining for each Element sets (previously defined in Step 2.7.5) an arbitrary origin Point and the Rosettes set in Step 2.7.8.
   10. Define the layup based on the results obtained in the optimization process of Step 2.7. Right-click on Modeling Groups and select Create Ply. Define the Oriented Selection Set, the Ply material, and the Number of Layers. Repeat it for each repeating group of plies.
       NOTE: Follow the same stacking order of the lamination process.
   11. In Workbench, drag Static structural analysis (in the Toolbox menu) onto the workspace. Then, drag ACP (Pre)Setup on Static structuralModel and select Transfer solid Composite Data. Double-click on Static StructuralSetup.
   12. Apply the symmetry and constrain boundary condition. Right-click on Static Structural and select InsertDisplacement. Select the Edge or the Surface of the Geometry and set the displacement to 0 for the appropriate Component direction.
   13. Apply the Force following the same procedure of Step 2.7.12.
   14. Solve the FEM model as linear elastic by clicking on Solve.
   15. Evaluate the maximum displacement ) of the leaf spring by right-clicking on Solution and selecting InsertDeformationDirectional. If it is low, come back to Step 2.7.10 and increase the number of the outer UD plies; if it is higher, reduce it.
   16. In Workbench, drag ACP (Post) (in Toolbox) on the ACP (Pre)Mode. Then, drag StaticStructural solution on ACP (Post)Results. Double-click on ACP (Post)Results.
   17. Right-click on the Definition menu folder and select as failure criteria Hashin 3D.
   18. Right-click on the Solutions menu folder and select Create Failure …. Select Hashin and check Show on Solids.
   19. Check if the failure criteria are always below one. If they are not, go back to Step 2.7.7 and increase the number of plies in the zone identified as critical, orienting them as necessary.
   20. Write the ply book.
8. Test a scaled model of the designed leaf spring.
   1. Design, by means of the analytical model of Step 2.7, a 1/5- to 1/10-scaled leaf spring, tuning the outer layers and core thickness to have the same ratio between bending and shear stress of the real component and a similar curvature for the maximum load.
   2. Laminate the scaled leaf spring.
   3. Test it with an ordinary four-point bending test fixture.
   4. Analyze the maximum load and displacement and the failure mode.
   5. Optimize the design of the leaf spring based on the conclusions of the experimental test.
9. Manufacture the optimized leaf spring.

3. Full-Frontal Crash Test Simulation

Figure 3: Cruiser geometry. This figure shows the general shape and dimensions of the vehicle. Please click here to view a larger version of this figure.

1. Draw the geometry of the vehicle (Figure 3).
   1. Create and name a new Part project in the CAD modeling software.
   2. Model solid parts using the resources Extrude, Revolve, Swept, and Loft to ensure full contact between different vehicle parts (such as chassis, seats, and roll cage). When necessary, click on the tab Surface, Reference Geometry, and Plane to draw a reference plane.
   3. Repeat Step 3.1.2 until the geometry is complete with monocoque, doors, roll cage, seats, battery, wheels, tires, wheel hubs, suspension arms, leaf spring, steering system, and rigid solid barrier (2 x 2 m).
   4. Exploit the bilateral symmetry to optimize calculations and use a half-car model. Under the Utilities tab, click on Symmetry Check and select the Automatic Symmetry Split command. Then, click on the part of the body that will be kept and confirm by clicking on Split Part.
   5. Convert the solid bodies into surfaces: select the faces related to the thickness of the bodies and click on the Surfaces tab and, then, on Delete Face.
   6. Click on Save as and select the STP format.
2. Set up and perform the simulation.
   1. Create and name a New Project in the ANSYS Workbench Finite Element simulation software.
   2. Drag from the Toolbox – Analysis Systems to the Project Schematic an Explicit Dynamic window. Double-click in Engineering Data and add new materials, dragging their necessary properties from the Toolbox tree and inserting the values obtained in Section 1 of this protocol, naming each material accordingly.
   3. Right-click on Geometry to Import Geometry. Click on Browse and select the STP file generated in Step 3.1.6.
   4. Double-click on Model under Explicit Dynamic to open the Model environment.
   5. Once inside the Model environment, right-click on Geometry to insert Point Mass for 3-D elements or in Layer Section for 2-D elements, to define concentrated masses or the composite layup, respectively. For each component under Geometry, the proper material and thickness of the surfaces should be assigned under Detail-Materials.
   6. Right-click on Model to insert Symmetry – Symmetry Region. The YZ symmetry plane defines correct geometrical symmetry in terms of the future results giving proper boundary conditions.
   7. To correctly set up Connections, delete all automatic connections and leave only Body Interactions, defined as frictionless.
   8. Under the details of the Mesh Explicit Method (Figure 4), drop the Elements midside nodes and set up the Sizing function on Curvature with Medium Relevant Center. Set up the Maximum Element Size to 30 mm with a minimum of 6 mm.
   9. Set the Number of CPUs for parallel processing under the Advanced tab of the Mesh section.
   10. Set the Velocity as an initial condition under the Initial Conditions tree of the Explicit Dynamics tab.
   11. Set the constraint boundary conditions by right-clicking on the Explicit Dynamics tab, selecting Insert, and picking Fixed Support to define the rigid barrier and Fixed Displacement to prevent that the wheel moves on the Z-axis.
   12. Under Analysis Settings, set up controls in terms of End Time (to 0.3 s) and Maximum Number of Cycles (to 2.5 x 10⁵), the necessary inputs to obtain velocity, and the Kinetic Energy (equal to zero).
   13. Under Solution, right-click on Solution Information to insert Kinetic – Total – Internal Energy to track these results. On the other side, under Solution Information, Solution Output can be tracked in terms of Energy Summary, Time Increment, and Energy Conservation.
   14. Click on Solve and analyze the outcome results in terms of Total Deformation, Stress, Strain, Total, Internal and Kinetic Energy, and Acceleration.

Figure 4: Mesh of the finite elements applied to the half-vehicle model. This figure shows the discretization of the model, done of on half of the vehicle due to symmetry. Please click here to view a larger version of this figure.