Max principal stresses 1

[saja11]

Hei,

I have two queries. I want to get max value of maximum principal stress at each time point. I want to know that what does this mean? Are these max principal stresses in each node of element and single value is their averages at centroid?

Secondly, I want to get a max value of max principal stress by averaging max principal stress value around this element (from surrounding 4 elements).

 

[FEA way]

These are the values at the centroid of the element but without averaging - just taken directly from nodes of this element. In Abaqus (not mentioned in your post but can be easily recognized) you can change averaging options in Result —> Options.

 

[saja11]

Thank you for your response. Ok so I got that the single value is from centroid but are the 8 values of max stresses from 8 nodes of same element? Also it is not good approach to get max value from single element from centriod so I want to get average of centroid values from neighbouring four elements. Right now with idx+1 and idx-1 I can get two elements on the two sides of our element with max value but I want to get 4 elements surrounding this element with max value of max principal stress? I hope I am making sense.

 

[FEA way]

There are three chapters in Abaqus documentation that may be very helpful for you:
- "Understanding how results are computed"
- "Understanding result value averaging"
- "Understanding probing"

They explain in detail how Abaqus postprocesses the results before displaying them and how probing tool actually works. For example it is explained that for elemental output Abaqus obtains probe results on an element-by-element basis without averaging.

 

[rb1957]

be careful about what data you have and how you're plotting.

the data can be element centroid data or it can be nodal (corners, averaged for the different elements).

then you can plot this data as either elemental (centroidal) or nodal (corners) and the s/ware interpolates.


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

 

[Coreform_Greg]

Something to be aware of is that Abaqus uses a C⁰ formulation (at least for most cases). This means that while the solution variable (displacements in your case) are continuous at the element boundaries (i.e. nodes) -- meaning that there is one and only one solution value at each node -- that stress being a derived value (i.e. proportional to derivatives of the solution) is discontinuous (C^-1) at the element boundaries -- meaning that each element that shares a node provides its own unique stress value at the node. This is why Abaqus uses a volume-weighted average in its contour plots to make stress appear continuous, when in fact it isn't. This is one of the reasons why it is typically recommended to query stresses from quadrature points. As a side note, from theory it's clear to see that derived values will converge at slower rates than solution values - if you would expect displacement to converge at a rate of h^p+1 then stress would converge at a rate of h^p -- so you need a lot more elements to converge to stress than are needed to converge to displacement.

Anyways, I've never heard of the advice to "average the centroidal stresses of the neighboring elements" because "you can't trust results from a single element". The truth is, for a well-defined FEM-problem you absolutely can trust the results from a single element as you can show that the best-approximation property holds for derived values. The caveat to this is contained within well-defined as stress-singularities, elements at a boundary-condition, locking, etc. can have issues to be sure. What I typically advise is to look at a quilt plot of stresses and if you see a region that has either oscillatory stresses or a stress that qualitatively looks out-of-place compared to its neighbors, to then explore further to see whether you have a singularity, locking, or haven't yet converged to accurate stress results.