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

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).

Open

Sim setup with old frame design

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).

Open

Common example of the 3-2-1 method on a practice part

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)

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).

This setup follows the exact same as the beam element analysis, in terms of force and support setup, it just utilizes solid elements to achieve more accurate values. This will greatly increase runtime but because this is used only for final results, it is used mearly to validate the results of the beam element simulation.

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 on sharepoint), 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).

The output will mimic that of the stiffness coefficient matrix shown in Ansys Workbench on the individual general joints. This stiffness matrix essentially gives the joints of the tube a set stiffness instead of an infinite one, to allow for more accurate stress propagation. I chose to have the MATLAB code directly output the same matrix, so that the only work for you to do is directly transfer the values from MATLAB into the matrix on Ansys.

How the MATLAB code for the RC sims works read this

After inputting the values, you then must ensure that each joint has a proper reference axis and face selected, to ensure that the stiffness values are then utilized in the proper orientation and situation.

Do this for every joint, ensure that weak springs is on, and the support settings for the simulation is finished.

In terms of force placement and calculation, the load cases vary from 5g, 4g, and 1.5g. These are all reliant on the force of gravity affecting the entire weight of the car, which is associated with the total mass of the car. Additionally, these are placed at the top of the roll hoop, for the front and the back, depending on the desired sim. Additionally, you may need to take the cos/sin value of a force value depending on specific load cases that ask for a force at a vectored angle.

Finally, you should now be able to run the sim and get accurate results with in minutes, due to the reduced size of the model while also still utilizing solid elements.