Structural Design and Manufacturing of a Cruiser Class Solar Vehicle

Cruisers are multi-occupant solar vehicles conceived to compete in long-range solar races that are based on the best compromise between the energy consumption and the payload. They must comply to the race rules regarding the overall dimension, the safety, and the mechanical requirements, while the other aspect as shape, materials, powertrain, and the mechanics can be determined by the designers. In this work, we detail some of the most relevant aspects of the structural design process of a full-carbon fiber-reinforced plastic solar vehicle.

The protocol used for the design of the lamination sequence of the chassis, of the leaf springs structural analysis, and for the crash test simulation of the vehicle are shown. The complexity of the design methodology of fiber-reinforced composite structures is compensated by the possibility of tailoring their mechanical characteristics and optimizing the overall weight of the car. After developing a candidate chassis design, create a finite element shell model.

Import the chassis design into finite element modeling software. Under Materials, select the fiber type to define the properties of a single-carbon fiber-reinforced polymer. Choose the Elastic behavior.

From there, check that the engineering constants are appropriate. Next, view the Hashin Damage parameters. Ensure they have the desired values.

Close out of setting the material properties. Move on to create a Composite Layups section. Here, each carbon fiber-reinforced polymer ply is defined by order in the sequence, material, thickness, and rotation angle.

The next step is to select Mesh to assign the distribution of discrete elements. Check the parameters of the Global Mesh Seed. Again, under Mesh, select Element Type.

Then, select an element of the model. Use the shell element type. Choose the quad-dominated element shape.

If hourglass effects are negligible, select Reduced Integration. Continue assigning mesh elements. When ready to generate the mesh, return to Mesh and select part confirm, that is, OK, to mesh the part.

Once the mesh is complete, under Assembly, create an instance of the chassis to which loads and boundary conditions will be applied. Go to the Steps folder. There, select the analysis procedure.

Ensure the procedure is defined as static. Also, check that the nonlinear geometry behavior is off. Now, go to Loads to begin to apply the prescribed loads.

Under Body force, enter the components and distribution for gravity or constant acceleration. The force direction is shown in the window with the model. Next, identify concentrated forces, such as those due to occupants.

Check that they are applied in the correct positions on the frame. Follow the same steps for the concentrated forces due to the car batteries. After the loads are set, apply the boundary conditions.

Consider the chassis as a supported body acted on by external loads, and identify the constraint locations. Use pinned boundary conditions. To define the output, go to Field Output Requests.

Make the desired selection. Check that the domain is Composite layup. Then, under Stresses, verify the output variables are stress components and invariants.

Also, check under Failure/Fracture. There, the Hashin output data should be selected. Click OK when satisfied.

Under Analysis, begin to set up a job. Name the job, and define the source of the model. After clicking Continue, customize the settings for the computer environment if necessary.

Choose to perform a full analysis. When that is completed, OK the changes in the window. Right-click on the created job, and choose Submit to run it.

Use the output to produce a ply book for a manufacturer. The design incorporates a carbon fiber transversal leaf spring for a simple and light suspension system with reduced unsprung weight. The leaf spring design has to be evaluated as part of the overall process.

Simulate an optimized leaf spring design in the ANSYS Workbench finite element simulator. Within ACP Pre, click on Engineering Data. Then, select the Engineering Data Sources tab.

Go to the Composite Materials folder, and import the carbon, unidirectional, and woven prepregs default material properties. When done, close the Engineering Data Sources tab. Next, right-click on Geometry.

Then, right-click on Import Geometry. Select Browse to find and choose the CAD file representing one quarter of the leaf spring. Now, double-click on Model.

When the new window appears, it will display the leaf spring segment. Select the file under Model. Under Graphics Properties, assign an arbitrary surface thickness.

Right-click on Model to select Insert and from there Named Selection. Use this function to define a layup zone by clicking on the highlighted Geometry field, selecting a region in the model and applying it. Repeat this for each zone required for the model.

When done, right-click on Mesh. Then, click on Generate Mesh to generate the default mesh. Close the Mechanical window to continue.

At the ACP Pre screen, open the Setup window. To define the ply's properties, go to the Material Data folder. Within it, right-click on Fabrics, and proceed by selecting Create Fabric.

In the window that opens, define the material. Then, assign the prepreg thickness. Next, right-click on Stackups, and follow this by selecting Create Stackup.

In the new window, define the sub-laminate stacking sequence by going to the Fabrics dropdown menu and making the necessary selections for the project. Move on to the Rosettes folder option, and right-click on it to create a rosette. In the window, click on Origin and move to the spring model.

There, click along the leaf spring axis to define the element local coordinates. Close the window to complete the task. Go to right-click on the Oriented Selection Set folder, and choose to create a selection set.

For an element set, first select the entries and point. In the geometry, click on an arbitrary point to define the origin. Also, under Rosettes, assign the appropriate rosetta.

Do this for each of the element sets. At this point, open the Modeling Groups folder. The defined modeling group appears.

To create a modeling group, right-click on the folder and choose Create Modeling Group. In the new window, click OK.Right-click on the new group, and select Create Ply. Define an oriented selection set, ply material, and the number of layers for each ply.

Repeat this step for each group of plies to define the full stacking sequence. Close the ACP window. From the Toolbox, drag Static Structural analysis onto the workspace.

Then, drag ACP Pre Setup onto Model in Static Structural, and select Transfer Solid Composite Data. Double-click on Model under Static Structural. Now, apply symmetry and constraint boundary conditions.

Right-click on Static Structural, and select Insert, followed by Displacement. Next, select the constrained surface of the geometry. Constrain the appropriate components by setting them to zero.

Follow the same procedure for the force. Check that the desired symmetries are respected. Click on Solve to solve the model as linear elastic.

At the Project Schematic, go to the Toolbox and drag ACP Post onto Model under ACP Pre. Drag the Static Structural Solution onto Results under ACP Post. Then, double-click on Results under ACP Post.

To create failure criteria, right-click on the Definition menu and choose Create Failure Criteria. In the window that opens, select Hashin as the failure criteria. Select Configure, and set the dimension of the failure mode to 3D.

OK the changes to return to the initial screen. Now, right-click on the Solution menu to select Create Failure. In the new window, select the desired failure criteria.

Also, check the Show on Solids box. OK the changes before clicking on the lightning symbol to evaluate the failure criteria results. For the simulation of a crash, develop a complete CAD model of the vehicle.

The model should include all of the major components, steering and suspension systems, battery, seats, roll cage, and monocoque. From this CAD model, create a half-car model to exploit bilateral symmetry in order to optimize calculations. Start a new project in the ANSYS finite element simulation software.

Under Toolbox, Analysis Systems, go to Explicit Dynamics. Drag it into the Project Schematic. In the new element, double-click on Engineering Data.

On the new tab, under Materials, add new materials and name it accordingly, Carbon Fiber in this case. Drag the material's needed properties from the Toolbox tree. Under Values, insert values obtained previously, including their appropriate units.

Return to the Project Schematic tab. Then, under Explicit Dynamics, right-click on the Geometry in order to select Import Geometry. Click on Browse, and load the STP file with the half-car model into the model environment.

The file also includes the barrier for the crash test. Inside the Project tree, select Mesh. Under Details of Mesh, go to Physics Preference.

Set the value to Explicit. Then, go to Element Midside Nodes. Set its value to Dropped.

Below, under Sizing, go to Size Function, and from there select Curvature. Move on to Reference Center, and select Medium. Set the minimum element size at six millimeters.

Choose the maximum element size to be 30 millimeters. Now, under Project, set the constraint boundary conditions by right-clicking on the Explicit Dynamics. Select Insert and then Fixed Support to define the rigid barrier for a collision.

Choose how the barrier is to be fixed. Then, select the barrier, and apply the choice. Return to right-click on Explicit Dynamics, and select Insert, followed by Displacement.

Apply the changes. Change the Z-axis from free to the constant value of zero. At the top of the window, click on Solve.

Here is a sample map showing the displacements of the chassis resulting from a 5G backward acceleration. This map can be used to assess the structural stiffness at an early design stage. This is the optimized geometry of the leaf spring.

Finite element analysis of the geometry allows the calculation of the failure index according to Hashin failure criteria. It can also determine the stress in the stigma one one direction on the outer surface of the leaf, along its principal direction. The numerical model is validated using a scale model tested to fracture.

This video makes it possible to appreciate the evolution of the stress in the vehicle during a modeled 60-kilometer-per-hour impact. A sample stress map provides a means to assess the vehicle integrity by helping to identify possible failure points that could harm passengers. A map of displacements from finite element analysis for the same impact speed reveals the largest occur at the front of the vehicle and in the roll cage bars that are attached to the seats.

They are a suitable option of reproducing composite structures, as they can simulate the bending stiffness of the thin-wall bodies with simpler mesh than the solid elements. On the other hand, in the leaf spring, where the local stresses cannot be appreciated by the analytical model, are evaluated by the finite element method, and the leaf composite layers are modeled by the brick elements. It is important to notice that, during the crash events, the deformation of the monocoque is minimal, and no components penetrate the other.

Therefore, it is possible to say that the design on the vehicle is safe. Different American models serve for the structural optimization of a solar-powered vehicle have been shown. The vehicle proved to be efficient and won the American Solar Challenge 2018 in its category.