Stress peaks in plate analysis 3

[BMart006]

I am starting to learn FEA and have noticed a trend in many of my analyses where at fixed areas and corners I have high peak stresses on the magnitude of 5 to 20 times the average stress. I decided to test the theory on a fairly simple model to see if it still occurs. I modeled a rectangular bar stock, fixed one end and loaded the opposite end with a evenly distributed pressure. At the corners of the plate on the fixed end, I end up with stresses about 8 times higher than the average. I realize that in real world applications, this plate would be fine, so how does one explain away such occurrences or correct them in a simulation? Thanks!

 

[rb1957]

it's over constraint.

if you fully constrain every node on a face (like at the end of your bar, I assume) you prevent the bar from contracting (poisson effects). constrain all nodes axially (z, reacts Fz, Mx, My); then carefully minimally constrain the other freedoms (Fx, Fy, Mz) ... constrain 1 node, constrain 2 nodes with Fx on one and Fx and Fy on the other so that the two Fx react Mz (ie separate the nodes in y).

on the plate if the four corners are fixed (maybe only in the 3 translations) the the plate is prevented from small deflections. Better to support the plate on finite stiffness (I use three rods) and constrain the rod nodes.

another day in paradise, or is paradise one day closer ?

 

[gravityandinertia]

There's a few factors at play here:

1. Your model likely has perfectly sharp corners on that rectangular bar stock. In reality there is no such thing. there is some radius/transitioning geometry on there that could be finer than your eye can see, but it's there, therefore in the vicinity of this, your model is likely wrong.
2. Nothing is ever fully fixed. Everything is flexible, however, how much flexibility or lack thereof, determines on whether or not we can leave out a larger portion of the model and replace it with a fixed boundary condition. In reality, whatever you are connecting to would have more give relieving some of the stresses. Right now, at your fixture, the part wants to spread out in two directions due to poisson's ratio of the material, however it is restrained from doing so at the boundary, giving a stress increase.
3. In all likelihood at 20X the average stress, you are probably exceeding they yield strength of the material. In a linear analysis, whether or not you exceed the yield, the stress keep increasing on the same line. In reality, material behavior passed the yield is non-linear, you will get larger deformations than predicted in linear, but with lower associated stresses. In general, what happens for things like metals, is that after yield, the material stiffness decreases, and the load redistributes to the areas that haven't yielded yet.

All in all, there are probably more factors at play here than this, but I don't have a lot of time at the moment.

 

[klaus.]

In FEA the results can never be 'better' than the input
This means you need to know the quality of the input so you know how 'good' result can be


best regards
Klaus