Stress at integration points or at nodes ? 7

[opethian]

Think of that you have a 3-D model and you simulated some forces acting on it. And get a Stress contour ? it should have normally the most accurate results at integration points (or not)? but then you have 4 integration points so should we extrapolate the results to the nodes ? or for this element which value should we take ? how about the stress results at nodes arent they realistic ?

 

[prost]

If I am indeed calculating strains/stresses when I solve the FE equations, then shouldn't I be able to directly extract stress as say Node 1 (or some other points) without any more work? I can do this with the displacements--the "u" in Ku=f is my solution; therefore (if I used isoparametric elements), once I solve for "u," I know the displacements at every single node in that mesh. You cannot say the same thing about the strains or stresses. Even after solving the FE equations, don't you have some more work to do to compute the strains/stresses at any point in the mesh, superconvergence or not?

 

[rb1957]

prost,

"I still don't think you need to know anything about the stresses to compute the displacements."

i think you need to read what you type, or maybe think alittle more about what you're typing ...

you can't have displacement without stress (nor stress without displacement, generally). Basic FEA assumes a stress distribution in the elements, and determines displacements so that the resulting internal stresses balance the applied loads.

 

[prost]

What 'stress distribution' is assumed in the elements a priori? The only "distribution" that is assumed is the form of the displacement field. You start with pointwise equilibrium of the spatial derivatives of the stresses, which is not the same as assuming the stress distribution itself.

 

[rb1957]

ok, maybe i should think before i write !

elements typically assume a displacement field (there were some early on that assumed a stress distribution). and after a bunch a math it solves for those displacements, and then derives strains and so stresses.

but i could contend that if you assume a constant displacment field then you are also assuming a constant stress field (assuming a constant thickness element).

 

[EdR]

rb1957:

Think a bit more....For a linear displacement field (two nodes) the strains are constant (eps = du/dx, etc.); thus the stresses are constant......thus a constant displacement field would give zero strains and stresses......

Ed.R.

 

[outpost11]

just a few more words on this issue....
stress based elements (actually the assumed field is a force distribution) were initially developed for the aircraft industry and they work very well in that environment because the important parameter across element boundaries is equilibrium of forces (i.e. shear flow). There is no enforcement of strain compatibility across element boundaries and it would be like having cracks along adjacent edges between nodes. Strain compatibility (enforced by displacement based elements) was considered more important by others in the field who were not necessarily dealing with semi-monocoque structure. Displacement based elements give better representation of stiffness, if used appropriately.
However, displacement based elements have their problems too, i.e. excessive stiffness of full integration elements, shear strain locking, hour glass modes, etc. Thankfully a number of commercial programs have developed "softening" features over time to minimize these issues.

 

[cbrn]

Hi,
I also add my two-cents... for what they are worth of...
In FEA packages (and by consequence in FEA literature) there are A LOT of different formulations for the same "kind" of element. Some hypothesize a stress field, other hypothesize a displacement field, some have auxiliary nodes at the edges' midsides, other have auxiliary nodes "inside" the element, and so on and so on.
However, for every 3D element I am aware of, there is always an hypothesis made on the (internal)force/displacement fields. The undirect demonstration of this is, for example, when you launch the solution with ANSYS: the first solver message before starting the equilibrium iterations is the output of a "force norm", determined on the basis of the [F] matrix AND the force-field coming from the elements' formulation. If stress/force didn't come into play in the computation of the equiibrium, there would be no way to decide the solution has come to convergence (i.e. there are simultaneously an equilibrated force field and a compatible displacement field).
Even if you use a direct solver, the internal matrix depends upon the element formulation, for the exact same reason: you MUST give an equilibrated force field as a response of a compatible displacement field, and vice-versa.

So, IMHO, to return to the original question: the Gaussian results as regards stresses are <generally> considered "the most accurate" from a numerical point of view simply because the element formulations are <generally> based upon these points and not upon the corner nodes. OK, there is also to say that the positions of the Gaussian nodes DO ARE calculated AS A FUNCTION OF the nodes' positions, so there is IMHO no point in saying that they are "more realistic" or not.
Just to make another example, in the case of the components/assemblies I usually analyze, the UNAVERAGED nodal results, by someone considered as a "must-be", are complete rubbish. I know of other situations where, instead, averaging like I do may lead to dangerous under-estimations.
Literature makes a good work in telling which kind of results, and in which applications, should be sought from the integration points, which instead from the nodes, which from the overall element, and so on.

AFAIK, there is no univoque answer to the original question.
"Gaussian better than Nodes? It depends..."

Regards

 

[outpost11]

Gauss Points or Node Points for stress interpretation ....
In my experience of displacement based elements I find that nodal extrapolation of element stresses give higher stress values for many structural applications. Although the mathematical correctness of stresses and strains at gauss points is true ... it really stops there when it comes to the interpretation of a continuous structural domain. Higher stress levels are usually associated with outer and inner structural boundaries (however, it is load type dependent). For 2D elements it is imperative that nodal averaging is only carried out for similar materials, and similar thicknesses, etc....
Nodal extrapolation for linear material analysis is appropriate and more prudent. However, non-linear material analysis is where nodal averaging becomes more complicated. Again, since the stress/strain levels are correct at the gauss points it could mean that nodal extrapolation will generate stresses in excess of the non-linear material definition described in the data file (over and above those for "true" stress adjustment). I feel that in non-linear material problems it is more appropriate to use gauss point values for stress interpretation but nodal extrapolation for interpretation of strain. Strain is a better result to interpret in non-linear material problems.
For 3D problems, again boundaries give the highest stress levels (in general). Extrapolation to nodes is again more appropriate (conservative) but it may prove more beneficial to "skin" the solid boundary with 2D elements and only plot the results for the "skin" elements.

 

[johnhors]

"it may prove more beneficial to "skin" the solid boundary with 2D elements and only plot the results for the "skin" elements."

outpost11 - could you please expand on or explain your reasons for this statement?

 

[outpost11]

No problem Johnhors ..
A useful approach for interpreting stress levels on the boundaries of 3D solids is to "skin" the boundary with 2D face elements. However, you do need a pre-processor (like PATRAN) to achieve this if it is a complex solid. The idea is to create 2D face elements on the exposed faces of the solid elements i.e. QUAD on the exposed faces of a HEX model, or TRI on the exposed faces of a TET element model. The nodes on the boundaries must be compatible i.e. use TRI6 with TET10 etc. One should never use a TET4 model other than some preliminary guideline analysis. Assign some very small thicknesses and/or material props to these "skin" elements without ill-conditioning the problem. Remember, you must have strain compatibility between the 2D and 3D elements so the stress levels in the 2D elements will be what you would expect to find on the surface boundaries of the 3D solid elements.

 

[outpost11]

A clarification on the previous point
I have always used the same material property for the 2D elements as the solid elements but small thicknesses for the geometric properties. If you use a different material property you need to make adjustments to the thicknesses to arrive at the same material constitutive equation (stress/strain relationship) which is messy and not recommended. It is the strains that match to the solid so the same material with small thicknesses would give the best result.

 

[johnhors]

Do you attach shell elements or membrane elements? In either case aren't you are attaching elements with incompatible shape functions?

But the main point of my original question was, why is this beneficial?

Assuming you are comparing surface stresses of the 3D solid where there are no applied pressures, no supports and no contact and thus only a 2D stress field exists, would you really expect the shell element stresses to yield more accurate stresses than those given by the solid elements?

 

[outpost11]

I would use membrane elements, if possible, but there may be issues with these in terms of acceptable warp if the solid shape has complex curvature. Otherwise, I would use shell elements because they are more liberal in accepting geometric issues.
Having similar nodal boundaries addresses the compatibility issue. It is the solid that dictates the strain ... the 2D element goes along for the ride (small thicknesses) but it is a convenient way of outputting results.
You may find that this approach is useful for addressing stress concentrations (for fatigue problems) in complex solid geometry. If a 3D automated TET10 mesh is used there can be issues associated with nodal extrapolation and nodal averaging. Irregular shaped TET elements are common and the locations of some gauss integration points for adjoining elements may be inconsistent in relation to the boundary position. This can lead to poor nodal averaging or even un-averaged peak values.

 

[johnhors]

outpost11 - yes I follow your argument I have heard it before, especially in relation to fatigue (let me guess nCode?) and with respect to poor tet elements. I would argue that skinning a solid of poor or bad solid elements is no substitute for re-meshing the solid with better quality elements. I find it hard to accept that this process can transform poor results into good, since the "good" results of the skin rely completely on the bad results of the solid! I was kind of hoping that you may provide a more plausible reason, hence my deliberately open question in the first place.

 

[outpost11]

The reason to do this is not to help resolve poor solid meshing. A 3D solid element calculates the stress away from the boundary and extrapolation is required, no matter what!
My point is merely an approach to assist in getting stresses calculated on the boundary itself. That's all.
If can also be very useful in keeping output result files (and post-processed) much smaller in size. If one has a number of load cases that can surely add up.
Just a suggestion ... employed by many analysts out there!

 

[johnhors]

Have you compared stresses at nodes in the skin element with stresses from the solid element at the same nodes?

 

[outpost11]

I have found smoother stress gradient results from this approach in the past i.e. if you look at un-averaged values.
However, I have also had difficulty at times trying to get this to work in non-linear problems (i.e. surface contact and large displacement) mainly due to the 2D elements away from the area of interest producing undesirable performance etc....
For complex CAD solids the local mesh refinement can get very challenging, especially with PATRAN.
PATRAN can give "unknown failure" for solid meshing. The most dreaded response in the program......

 

[gwolf2]

Interesting sub-thread on skinning. I've tried it, works fine. The only way to get a good quality stress concentration is a 'nice mesh of hex elements around the corner' using mapped meshing. But then I'm something of a dinosaur perhaps.

I find that with the appropriate tools (mentioning no names)there is often little difference in speed between hand crafting the right hex mesh the first time and iterating a couple of TET meshes. We are of course talking about the 1-2% accuracy range here for fatigue. - and I don't hand craft everything these days, often using hybrid hex/tet meshes.

I remember when this was all fields.....................................

gwolf

 

[btrueblood]

Gwolf,

Were the fields arrayed as far as the eye could see?

 

[gwolf2]

Indeed