I was working on a simple static load test on a bolt in a slotted hole of a plate, such that the load direction is perpendicular to axis of the bolt and plate area vector as well. BC- just fixed plate at one end , load is concentrated point load on one node on bolt edge in direction mentioned with (hard contact surface interaction between slot cut inner surface and circular cylinder (bolt dummy)) However, when saw result, in displacement the cross-section of round bolt become oval, (it should but in opposite orientation- see the attached image). The ovality, where (major axis of the oval cross-section is getting larger on increasing scale factor), Not getting how does this happened. Am I doing something wrong or its usual? Seeking comments……
Ok, but it’s hard to say what’s going on without seeing the model setup. Apart from the fact that the mesh of the bar is rather coarse and that if it’s a point load on just one node then it’s a bit risky in terms of potential artificial stress concentrations. It would be better to distribute the load on the whole end face or at least some small partition at the top.
Also, the displacement is large. If the load is not unrealistically high, it might be good to enable Nlgeom.
Ok, so here are some remarks after checking the file:
The mesh of the bar definitely needs refinement, especially in the contact region. You may also need some fillets for this nasty edge-to-edge contact region with large stress peaks:
And better use an extruded hex mesh (try C3D8R elements).
As I’ve mentioned, force should be applied to a surface (not necessarily the whole cylindrical surface, you could make a partition in CAD software) instead of a (midside) node:
Just don’t use concentrated force load for that - there’s Surface traction load available.
There are large deformations in this analysis. You may need to change the material model (linear elasticity is valid only for small strains up to ~5%) to hyperelasticity or add plasticity.
Large deformations may also require Nlgeom for realistic results, but keep in mind that it may cause non-convergence.
At least for testing, you could replace this nonlinear contact with tie constraint. This would improve convergence.
Here’s your file with the most relevant of the aforementioned modifications (see if you need other too):
Most likely too coarse mesh and linearity of the analysis. Check if it still occurs (likely just to a small extent, at least with true scale deformation) in the file I shared. If yes, try adding the aforementioned nonlinearities one by one.
Hi there, I checked your edited file, Actually its looks good for real scale in both case with and without Nlgeom in step. However, when increasing scale its going toward ovality. see this image, is it just visual or something that I should think and have concern about?
Such artificial deformation effects may occur in linear analyses, especially with higher scale factors. I would focus in true scale, but also try adding Nlgeom. It may fail to converge then so try reducing the load or adding material nonlinearity too so that it behaves more naturally.
