Nodal stresses vs. Element stresses in Structural FEA

[Francesco Bro]

Hi,

I am running into a structural verification criterion for an aerospace component, and as we know FEA packages offer the ability to show either nodal stresses and element stresses (at the centroid for instance).

I realized that the nodal stresses values are much higher than the element ones. If we use nodal stresses because they are extrapolated to the "free surface" of the part being analyzed, aren't we being too much conservative?

What is the standard procedure in the FEA industry? Which is the correct variable to look at when verifying the structural MoS? Pros and cons of each output? When is used each variable?

I am not talking about averaging, since I understand it is a matter of the mesh discretization and FEM convergence principle, but on the nodal vs. element stress output.

BTW, I am using NX Nastran FEA solver with Simcenter Pre/Post GUI.


Thank you!

 

[rb1957]

I'm surprised with "the nodal stresses values are much higher than the element ones". This indicates a significant stress gradient, which means ... proceed with caution.

In a typical structure (an axially loaded rod, a beam in bending) there should be only small differences between nodal and centroidal stresses ... in the tension rod none at all (if no area change), in the beam in bending only small (predictable) changes (due to the change in moment , or M/I).

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

 

[centondollar]

The answers should be similar if the mesh is fine enough. Remember that in FEA, the only thing directly solved are the nodal degrees of freedom (displacements and, for some engineering dimension reduction models, also rotations), after which the displacement field inside elements is interpolated (using the same interpolant that was used to solve the DoFs), and the last step is to calculate internal forces and stresses using their definitions.

Only in special cases can "superconvergent" points (points that give "more accurate than expected" stress values) be found, and those are located at integration points (Gauss integration points) inside the element, not at the nodes. In addition, for frames, deflections can be "exact" at frame corners for suitably simple loading. In general (for conforming element formulations and suitably regular geometry, loading and boundary conditions), accuracy is gained by reducing element size or changing the polynomial degree of the element displacement (and possibly rotation) interpolant.

What relative differences are you witnessing in the solutions?

 

[SWComposites]

Nodal stresses are extrapolated from element stresses, so in many cases are less accurate. The average of nodal stresses from multiple elements at a node can be fairly accurate, depending on element type and mesh.

You need to run representative test cases at varying mesh densities to sort out the appropriate results to use.

 

[FEA way]

FEA software extrapolates the stresses from the integration (Gauss) points where they are the most accurate to nodes and then performs averaging. So when looking at stress contour plots we use extrapolated values (sometimes without averaging to find problems). However, when checking particular locations we use stresses directly from integration points to ensure proper accuracy.

 

[rb1957]

"However, when checking particular locations we use stresses directly from integration points" ...

how do we do that ? I've never seen stress output at integration points ?

why are nodal stresses so "bad" ? whether we average across elements (from centroid to centroid) or use nodal stresses (averaging across the different element results at each node) ... is it really that different ?

FEMs are not Truth, but are (sometimes) a really good approximation of reality. To argue which approximation is better is IMHO somewhat pedantic.

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

 

[FEA way]

Abaqus has a query tool that can be used to check stresses (and other variables) at various locations, including integration points. Maybe choosing this location is not so important but we do it out of habit to make sure that potential inaccuracies due to extrapolation are not of concern.

 

[rb1957]

ok, that explains it ... never used Abaqus, only Nastran.

still surprised that you think that integration point stresses are so much more reliable than nodal (or centroidal).

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

 

[NRP99]

Results are computed at integration points and then extrapolated to the nodes for nodal results. Elemental results are obtained by averaging/extrapolating the nodal results/integration point results at centroid of an element. This may vary from software to software.

Nodal results represent smooth "flow" of result (which is actual case since material is somewhat homogeneous) and elemental results represents "discontinuous flow" of result.

All result information is still "approximate" since FEA is approximate and no information is reliable unless GIGO is avoided. If the behavior is representing the actual physics, checking the nodal results is most appropriate. Most of the time nodal stresses are sufficient. But yes the amount of discretization error can be pointed out by comparing nodal results to elemental results.

 

[rb1957]

both nodal (averaged) stresses and element centroid stresses produce smooth results. One could say element centroid are more reliable, if you consider discontinuities in the structure (skins of different thickness, steps). I just don't get that integration point stresses are "so" superior to either centroidal or averaged nodal stresses, but meh.

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

 

[Francesco Bro]

Thank you all for the answers!

I guess rolling back to my original question, it is not standard in the industry which stress value to look at for MoS computation (except NRP99 who mentioned nodal stress as the ultime value to take, assuming the FEA model has a proper mesh representation and the results correlate with the real problem).

I was asking as a standard procedure, best-practice, that some guru folks may add to the discussion.

 

[rb1957]

best practice ... don't take stress from a FEM, use the FEM for loads and then hand calc these loads on the structure.
This has some real sense for large scale structures where FEMs can't (couldn't ?) account for things like diagonal tension or effective width (in compression) or for coarse grid models (like a fuselage with a single element frame-to-frame, stringer-to-stringer) when pressure loads are not properly reacted by the skin.

Of course, if you have a 3D solid FEM of a machined part I would use FEM stresses (but then this wouldn't be "best practice" as above).

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

 

[Frederic Martin]

In (NX) Nastran you should look at the elemental stresses to be on the safe side. The elemental stresses are directly derived from the Gauss points (aka stress integration points) mentioned above. When your mesh is sufficiently refined, the difference between the nodal and elemental stresses will be minimal, which makes it a great way to find out if the mesh is refined enough in the first place.

 

[IceBreakerSours]

A not-totally-irrelevant tangent: If you go through the book by Oberkampf and Roy, one realizes that skeletons can easily hide in the FEA/CFD/FVM/.. .. software code closet and it takes a fair amount of effort to uncover those. Whether you need to go through some level of that trouble depends on the risk calculation.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083