...
Please start by reading the how to FEA section of Frame 101
To preface again, static structural analysis is utilized to analyze the pure structural response to the load cases exhibited in a roll over. This isolates the frame without allowing momentum or energy transfer to the wheels (which would actually happen in real life), which allows us to see the worst case scenario on the frame. Dynamic analysis/LS-DYNA simulation could be utilized in future simulations, to see how the frame reacts to work/impulse over time, which is a useful too in chassis building, but is not directly required by our regulations.
Occupant Cell Beam Element Analysis (for iteration)
For the occupant cell load cases (front, side, and rear), beam element analysis is utilized for the entire frame, to quickly and efficiently iterate the frame design by looking at overall chassis stiffness and deformation. Additionally, we can test torsional rigidity (not required by our regs, but we still should evaluate it) by using beam analysis (potentially with modeled suspension assemblies).
...
Walking through the setup, the focus for this setup is again to quickly give results on the occupant cell load cases. To do this, beam elements are used to generalize the structure and simplify the mesh geometry, in order to streamline load times and give fairly accurate results. The beam elements are set to specific tube profiles, the same profiles they have when you select outer diameter and wall thickness in Solidworks (more on this later).
Looking at the support setup, the 3-2-1 method of supports is used, primarily to constrain the part enough to restrict rigid body motion, but not enough to restrict any deformation/stress as a response to the load case. This is done by selecting a suspension node at the back of the car, in which all 3 DOFs are restrict, then moving along the Z axis, restricting another suspension node at the front of the car, this time only with 2 DOFs (only x and y because we moved along the z axis), and then finally one on the back right side of the car, only restricted in 1 DOF (only y because we moved along the z and x axis).
...
You can constraint the frame in another way, primarily by fixing each individual suspension point, which mimics the way the frame is actually constrained when combined with the dynamics assembly. However, this support setup is rather conservative, as it over constrains the frame and adds nodes of infinite stiffness that are not present on the actual car. Because of this, we opt for the 3-2-1 method, again to constrain the part as minimally as possible.
In terms of force setup and placement, the regulations for each of the load cases calls for “5g”. All this means is that the force exerted on the frame must equal five times the weight of gravity exhibited on the car. To clarify, this means the entire car, and not solely the frame, meaning you must have an estimate for the full mass of the car. Take that mass, multiply by the gravitational constant, multiply by five, and then you have the force exerted on the frame. Fairly self explanatory. As far as force placement goes, we place the force vector around a 150mm diameter contact patch, meaning the frame must have a split section that is at maximum 150mm large in diameter. This type of split can be done in Ansys Spaceclaim or Solidworks.
Otherwise, this sim setup is fairly simple and gives results typically within a minute. The setup accurately represents the deformation of the frame under load, as deformation is accurate with beam element analysis. Because of this, you can iterate the frame based on a desired stiffness (i.e. you can set an arbitrary goal stiffness, take the force exerted, take the shown deformation, and use the spring formula of F=kx, to work backwards and calculate the stiffness). Because your exerted force is not changing, your stiffness is directly proportional to the deformation shown, meaning that less deformation gives a higher stiffness. Therefore, you can iterate the frame as many times as needed to lower the deformation enough to get close to the desired stiffness (within reason with design choice and weight goals of course).
Additionally, there is a cool feature within Ansys, where you can directly change the beam profile without having to go back and forth with Solidworks, meaning that if you want to iterate the frame by just changing tube OD/wall thickness and not geometry, you can do that directly in Ansys and immediately be ready to sim. I recommend this for quick and easy results.
Lastly, you can use the beam tool to give you a general idea of maximum/minimum combined stress, which is useful for iterating your design, but not super accurate, given the generalization of the beam elements. Because of this, you can use the change in stress values across the sim as a basis to see if your changes are working or not, but do not use the stress values alone to gauge whether a design is passing regulation or not. This is why we utilize a full solid analysis in order to get von-mises, max principal, and min principal stress values, which are accurate (when using a small mesh size), because of the complexity and representation of the frame design as thousands and thousands of nodes.
Occupant Cell Solid Analysis (for final results)
...