Folder Path
Saved locally on Connor’s computer
Context
I suspected that the gussets would need local mesh refinements to avoid discretization errors (as opposed to the beam elements, which are essentially 1-dimensional and likely don’t require as much resolution). This suspicion was not supported by technical knowledge, just intuition. And some mech advisors agreed during a recent review. Thus I tried a few different options while I was familiarizing myself with running static structural simulations in ANSYS.
I used an older CAD model (2020-10-13 Chassis) in the front bar collision scenario with point masses for the passengers, battery box, and bulkheads/dynamics.
Results
Case #1: Default Gusset Meshes
I started with a moderate element size of 20 mm (based off of Tommy’s mesh independence study) and used default mesh settings for the gussets.
After running a simulation, the maximum deformation was only 47 nm. This seems unrealistic in a 5G crash scenario. The maximum combined stress in the beam elements was 361.4 MPa.
Case #2: Tetrahedral Gusset Meshes
The first change was to switch the gussets from rectangular elements to tetrahedral mesh elements. The element sizes were kept at 20 mm.
| Expand | ||
|---|---|---|
| ||
This was an arbitrary decision based on previous experience using tetrahedral elements for CFD simulations. However, in CFD they are commonly used for isotropic behaviour whereas rectangular elements are typically reserved for cases where a parameter is mainly acting in a specific direction. Since I don’t know the direction of the forces acting on the gussets, I thought it would be best to use an isotropic element. |
This time there was significantly more deformation in the chassis model. The maximum deformation was 4.2 mm, which is many orders of magnitude greater than the default mesh case. The maximum combined stress in the beams was still 359.3 MPa, which is close to that of the default case.
From here, I conducted a gusset mesh independence study where I tested a few sizes of tetrahedral elements on the gussets while maintaining 20 mm elements on the beams and bulkheads. Despite some variation, there are not likely to be any dramatic improvements from using smaller elements.
Discussion
The choice of mesh elements seems to have a large effect on the deformation in a simulation. This is very important for future simulations for 2 reasons. First, the regs state that the chassis must not deform by more than 25 mm so we need to be able to accurately predict how the chassis will deform. Second, the deformation of the chassis will likely impact the stresses in the chassis. It might seem like the results presented here contradict that, since the maximum stresses do not significantly change when different types of elements are used. However, the maximum stresses in this collision scenario occur right above the collision object. I would argue that the gussets have a very minor role in protecting the chassis from this collision scenario and that it is likely that greater stress differences will be seen in other collision scenarios.
How do we know that the tetrahedral elements are more accurate/realistic? And why is there such a large difference in deformations? I would say that I intuitively believe that the chassis will deform by more than 47 nm in such a collision. Although I cannot say if 4.2 mm is accurate, I think that number is more probable. As for why, I found this article from SimScale that discusses meshing practices. They discuss a concept called “locking” which is where improper modelling of certain features limits their mobility. In our case, modelling thin features with a single layer of linear mesh elements can lock them and prevent them from bending. This artificially increases the stiffness of the thin elements (the gussets), which I’m thinking reduces the overall deformation of our chassis. Tetrahedral elements help with this issue slightly by creating 2 layers of elements but it would help even more to switch to higher order mesh elements.
ANSYS has the capability to use quadratic elements, so I ran a simulation where the gussets were represented by quadratic tetrahedral elements and the bulkheads were represented by quadratic rectangular elements. The max deformation increased slightly to 4.33 mm (only 3% difference from linear elements) and the max combined stress increased to 368 MPa.
Conclusions
Having 4.2 mm of deformation makes more sense to me than 47 nm. I would be interested to hear what others think of this but for now I will continue using tetrahedral mesh elements to model the gussets. Even though this study focused on the gussets, if this is indeed a thin feature locking effect, these results could also apply to bulkheads and any sheet metal reinforcements as those are also thin features which are only being modelled by single layers of mesh elements.