This is a referenceable document that walks through the Ansys Mechanical FEA setup for the 24-26 chassis. The Ansys Mechanical setup was created by me, Noah, in order to streamline the simulation process and get accurate results with relatively low runtime. We will walkthrough the entire setup so you can understand what is happening and why I chose to do it that way.

Please start by reading the how to FEA section of Frame 101

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 with modeled suspension assemblies.

Occupant Cell Solid Analysis (for final results)

For the occupant cell load cases (front, side, and rear), solid element analysis for the entire frame is utilized as final verification to ensure our frame design meets regulations for the occupant cell (max and min principle stress, Von-Mises/equivalent stress, total deformation, and factor of safety).

Roll Cage Solid Element Analysis (for iteration and final results)

For the roll cage load cases (all 10), solid element analysis for the roll cage is utilized to iterate and use as final verification to create and ensure our roll cage design meets regulations (max and min principle stress, Von-Mises/equivalent stress, total deformation, and factor of safety).

To start, because only the roll cage will be utilized for solid element analysis (due to the runtime concerns of a full chassis as solid elements), we need a way to accurately model stress propagation from the roll cage to the rest of the chassis, without actually having the chassis modeled. We will do this by creating deformable joints at each tube coming from the roll cage while utilizing a specifically calculated stiffness matrix for each joint. Additionally, weak springs are turned on, to ensure the model will be constrained just enough to not have rigid body motion occur. This allows each joint to accurately deform itself, while acting as if stress is propagated to the rest of the chassis, which is more accurate than utilizing fixed supports, that would act with infinite stiffness and create a more conservative simulation process (which means we would end up overbuilding our frame).

Splitting the frame is the first step in setting up this simulation. You can achieve this by creating planes in SolidWorks that are then used to split the roll cage from the rest of the chassis. Ensure that a small section of the propagating tubes from the roll cage are left on the model, to give a starting point for the stress propagation and ensure that our joint calculations are accurate.

Next, utilize this MATLAB file, in order to calculate the respective stiffness matrix to be imported into Ansys for each joint. You will need material properties (that can be found from ANSYS), as well as properties of each tube. This includes, elastic modulus (E), shear modulus (G), tube outer diameter (OD), tube wall thickness (WT), as well as the length of each tube not modeled (meaning the length of the tube that was cut off the design, as each joint represents a point on that tube acting as a cantilever beam). All of these inputs need to be made in imperial units (this follows the unit convention from our tube sizes).