Maybe an earlier look at the documentation would help in this regard:
It is essential to be aware of the limitations of any solver (open-source or not) if you plan to deal with other people’s lives and safety in your calculations. The engineer must take this care and is unfortunately not the common approach nowadays. Hopefully, we are here discussing ways to raise this awareness so that everyone can better use FEM tools.
you should flip master and slave
In my model, master is the one with a coarser mesh. Ties seem to be working properly. The model could be further improved but it was just a quick setup to bring the discussion on the right track.
Yes I understand and it’s very useful. It’s just another check that’s worth thinking about as described below.
I cannot comment on Nastran but with the master and slave as provided, the influence of the support of the leg extends beyond the leg geometry too much.
swapping slave and master gives
and a deflection of 16.32mm or 0.64 inches
Perhaps tied contact could provide even better results here.
i checked again, it seems non-alignment of surface between neighbor is not the source of problem in this case. Probably, since rib plates are in membrane stress dominant.
deflection results did not have significant different between linear & quad element, similar problem is replicate using Step file available.
Btw. Abaqus has a nice feature that visualizes ties:
Can be really useful for debugging when ties aren’t working as expected.
This might have been useful to compare at the beginning and might be the source of most of the original issue. Flipping the slave and master on the very original model posted achieves 0.56 inches max deflection so 8% from the Nastran solution. Not sure how the “tie” is handled in Nastran, but can’t imagine it’s much different,
Congratulations! You stiffened the structure just to get the same result to make me look stupid? Serious…
I agree with you. Like I said earlier… apples to oranges.
please don’t take seriously and getting sensitive, in the past i submit a bug in C3D8I element directly by email to the author. So i do investigate further about the problems.
Well, an explanation would be helpful.
Could you please share your NASTRAN model?
no, studying thickness parameter from 20mm, 10mm and 5mm shown consistent in result of both element type. As an early state, i guessed something problem in the models, not the element itself.
*edited
sorry i miss to set element order, below correct ones from S4. Discrepancy is below ten percent compared to quadratic at the same number of element.
I did some testing using your model. To accomplish this, I’ve removed the feet of the table and used a fixed boundary condition on one side while the other side is just supported in the vertical direction to avoid overconstraining. The idea is not to reproduce exactly the OP model but to work in a reduced problem with fewer things that may cause issues. I did not use linear elements, just quadratic trias and quads. The goal is to check convergence.
table_no_supports.pmx (2.3 MB)
I tried 5 configs: one using the original mesh (about 60mm) and 4 fine meshes. The max displacement seems to converge, but the max stress does not. I did not investigate further the reasons behind this, but the idea is to show that the original model is far from converging. It would be nice to check this behavior in Nastran and Abaqus, however, I don’t have access to them.
It seems to be a singularity. The cause of this is the sharp edge, created by the connection between the top plate and the web. In comparison with code aster, calculix results with S8R elements are closest to code asters with coque_3D elements (these have 8+1 center nodes).
My first thought was that this could be some issue with knots, but didn’t investigate further. Nice to know that other solvers are having similar behavior, even with true shells
below an interesting article for real cases of thin part. As i understand in general conclusion are; invest hardware (memory), prefer to use solid element (linear/quadratic) & properly set layered trough thickness. Some element of shell formulation (thin) shown less accurate in capturing, another ones need proper setting.
image from Rotter & Sadowski (2013)
