Unsmoothed Von Mises 530MPa and Smoothed Von Mises is 334 MPa (Solid Element)

[tibor121774]

Hello all!!!!I have attached a sample file (solid element)....In this sample file (case "Secondary Operating W+P+T) have a result of 334 MPa (smoothed value) and 530 MPa (unsmoothed Maximum value)....I have refined the mesh to 8mm but the difference is still large...Hope someone can explain why this value cannot be reduced to an acceptable value say 20Mpa difference?....I've got no problem with a plate element...Many Thanks for your time...I've read from one of the essay regarding smoothing options that it is better to use an unsmoothed result with a difference of acceptable value to smoothed result..which can be achieved through mesh refinement...But in this case I've already minimize the mesh as much as possible...But cannot get the two values (unsmoothed and smoothed near each other)....

Cheers!!!!

[tibor121774]

Sorry but the file is too large...Anyway is this difference acceptable in solid element?...Many Thanks...

[AstroJohnPE]

Tibor,

(Warning: it's getting late here, so I may be rambling too much, or my statements may not make sense. 🙂

[1]

What you can do is manually review the stresses provided by all of the elements at the node. The abnormal high stress (530 MPa) will be from a 4-node element that has 1 node attached to the surface. Discard this element because they always seem to be high in this circumstance. (Correction: whenever a high stress point appears on the surface, it seems to be due to a 4-node element. What I do not know is how many times 4-node elements DO NOT produce a high stress; I don't bother to look for these situations :-).

What is the stress range from the other elements connected to the node? The range is probaly much smaller -- maybe even acceptable.

In the ideal world, you would be able to view the unsmoothed results and refine the mesh until the difference is less than some chosen value. Here in the real world, the automatic solid mesher is unlikely to ever create a mesh that comes to a converged solution, in my opinion. It just does not have the intelligence or speed or something to create a quality mesh, throughout the entire volume, with a minimum number of 4-node elements, and keep the aspect ratio of all elements to a reasonable value.  In addition to the aspect ratio, the other things that ideally should be controlled are the angle between two edges (node angle), whether 4 nodes that make a face are in the same plane or how large of an angle it makes.

To get a model where the unsmoothed results converge to a solution would require a hand-built mesh where you can control the aspect ratio (maybe 10 to 1 maximum?), the node angle (maybe 90 +/- 30 degrees?), and planar faces (maybe +/- 10 degrees?).

[2]

I think that smoothed results are acceptable for reviewing the results. After all, does anyone complain about a smooth contour when looking at displacements? The displacements are only known at the nodes, so the contour should be color at the nodes only and no color in between the nodes. The same is true for stresses. The stresses are known at specific points in the model (at the gauss points) and no where else. So, should the software only color the gauss points and have the model be blank in between? Of course not! If the software does it reasonably well, the same type of scheme to calculate the stress in-between the gauss point of adjacent elements should give similar results to extrapolating the results from the gauss points of one element to the nodes and then smoothing those result. Hopefully, the results from adjacent elements connected to a node will have a bell-shape distribution where some results are too high and some results are too low. Viewing the average of these would be closer to the real result. This is why smoothing is acceptable, in my opinion.

If you have reason to believe that all of the results from the elements at a node are too high, then the average would also be too high. In this case, you would want to smooth the display using the minimum stress from the elements connected to a node. If you have reason to believe that the results are too low, then you would want to smooth the display using the maximum stress from the elements connected to a node. Both of these can be done in the software by changing the Smoothing Options.

[3]

The "Precision of von Mises" is a relative amount: the stress range at a node divided by the maximum stress in the model. It may be easier to view the stress difference at each node; in other words, see that the stress is plus or minus 20 MPa at this location and plus or minus 400 MPa at others. If the large stress range occurs where the stress is naturally low, then it doesn't matter. If the large stress range occurs where the stress is high, then you have a concern. This type of result can be viewed by setting the Smoothing Options to "Range". (Actually, the Range would be = maximum - minumum, not (max-min)/2 like I was implying with the "plus or minus 20 MPa" example.)

Also, the precision of von Mises only shows the result of comparing the von Mises stress. You can use the "Range" smoothing for any type of stress: tensors, principle stress, and so on.

This may be a new record fo me: the longest post in my life!

[tibor121774]

Thanks for that valuable wisdom and information...Actually I've tried to use (Compatibility as "Not Enforced") because I've read from a help file that

these elements are formulated using an assumed linear stress field and these elements are most effective as low aspect ratio rectangles. And I've got a maximum unsmoothed value of 366 MPa and smoothed mean value of 310 MPa...These coincides with the plate element result of 367 MPa....I think this is more effective than "Compatibity Enforced" because it can give reasonable result even with not so perfect element (which is hard to achieve in a solid element)....As stated in the help file the compatibility "Enforced"  elements are formulated using an assumed linear displacement field. These elements

can overestimate the stiffness of the structure. In general, a greater mesh density in the direction of the strain gradient is required to

achieve the same level of accuracy as elements for which the Not Enforced option is selected. With this option selected, the elements are formulated using an assumed linear displacement field. So the "Not Enforced" option is a good tool for a little bit distorted element...

Please correct me if my interpretation of the help file is wrong...

Cheers!!!!