Local Mesh Refinements

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. This generates a single layer of rectangular prism elements for the gussets, with some elements having a visually high aspect ratio. In CFD, high aspect ratios are usually bad unless you know for sure that the gradient of the parameter you are trying to calculate is low. (Maybe this isn’t relevant for FEA?)

Figure 1: Default mesh settings on the B-pillar gussets.
Figure 2: Deformation of the chassis with default gusset meshes in a 5G front bar collision.

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.

This was an arbitrary decision based on previous experience using tetrahedral elements for CFD simulations. However, in CFD they are commonly used for more “isotropic” behaviour whereas rectangular elements are typically reserved for cases where a parameter has a large gradient in a particular direction and a low or non-existent gradient in the other direction. Since I don’t know what kind of stress or deformation gradients will develop in the gussets, I thought it would be best to use a more “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 occupant cell 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 guess that the gussets have a very minor role in protecting this area on the chassis from this collision and that greater stress differences will likely be seen in other collision scenarios.

It should be noted that these tests don’t prove which element types are more accurate, only that there is a difference between them. 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 and hence tetrahedral elements are probably better for modelling the gussets than the default elements. As for why there is such a large difference, I found this article from SimScale that may be relevant. They discuss a concept called “locking” which is where improper modelling of certain features limits their mobility. In our case, modelling thin features like gussets with a single layer of linear mesh elements can lock them and prevent them from bending. This artificially increases the stiffness of the gussets, which I’m thinking reduces the overall deformation of our chassis. Tetrahedral elements help with this issue by creating a greater density of smaller elements but another method that could help is 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 quadrilateral 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 if anyone else has encountered lower deformations than expected in their simulations 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.

 

Update

I also tested different mesh element types on another collision scenario, the top 30 collision. I did not see any difference in deformation or evidence of locking behaviour, so this could have just been an error in my front bar collision setup. Another possibility is that the even locked gussets do not help protect the chassis in a top 30 collision scenario.