Solid element with integration points co-located with corner nodes

[aerovf]

Does anybody know whether such an element available in Ansys? I mean solid element with integration points at the same locations as corner nodes. Seems like there is one in Abaqus, but what about Ansys? This question is related to extraction of results on surface, rather than inside of the element. Any techniques other than "skining" are available?

Thanks

 

[johnhors]

"Seems like there is one in Abaqus" - really! what is it called?

What's wrong with using results extrapolated on to a surface from the integration points? Assuming the mesh is sufficiently refined (mesh convergence) then the error induced by extrapolation will be negligibly small.

http://www.Roshaz.com

quality, cost effective FEA solutions

 

[btrueblood]

I don't think a solid element, or any element, can have its integration points (which are functions of the enclosed volume) located at the edges/boundaries of the elements. Unless, perhaps, you are analysing klein bottles.

 

[mechfeeney]

If you probe values (using the Tools->Query) option, can you select values on the surface of the elements? Or the corners?

 

[ESPcomposites]

I am guessing he is confusing the difference between an integration point and a point a which to extract results?

The integration need not (and won't be) at the corners. The use of the shape function will still allow you to determine the results at the corners.

Brian

http://www.espcomposites.com

 

[aerovf]

Thanks to all for your responses. I'll dig a bit more tomorrow about Abaqus (per topic of course).

But my vision on that is as follows (I'll refer to Solid elements only). Because the highest stress are always on surface (well, if not always, then in most cases are) and the most accurate stress values are calculated at integration points, then it does make sense to have integration points as close to the exterior surface of Solids as possible. Otherwise, extrapolation using element shape function is needed (not the end of the world, but still extrapolation, i.e. accuracy etc).

From another side, numerical integration used in FEM is the most accurate at the Gauss integration points. I'm talking about brick-shaped elements; integration within tetrahedral elements can easily be done analytically.

On attached picture there are formulas for numerical integration. Coefficients are given for Gauss integration points. However, as far as I understand, the points of integration can be chosen not necessarily at Gauss points (for 3rd order of integration +/-0.77 and 0), but at, say, +/-1 and 0, that is 2 corner nodes and centroid (or close to). The question would be about ksetta (or whatever it is called) coefficients for each C (see attached picture).

I don't know, may be I'm mixing stiffness calculation vs stress calculation. But in any case it is still numerical integration used, that means points, at which integral is calculated, could be chosen anywhere (agree that Gauss is the most accurate).

So, I think it is a trade between inaccuracy of integration at non-Gauss points and extrapolation outside of integration points. What do you think?

Sorry for being so wordy and correct me if I'm wrong.

 

[ESPcomposites]

I think you are getting too theoretical. Your more likely to introduce error via discretization, setting boundary conditions improperly, or just plain old inaccuracy of the inputs. All engineering problems suffer from the fact that they are not in a lab and don't adhere to "perfection" of the loads, geometry, materials, etc.

Brian

http://www.espcomposites.com

 

[mechfeeney]

Just out of curiosity, why is this useful information? Why are you trying to find the values at the integration points? If you are concerned that your model is not picking up the "true" maximum stresses on the surface (because they are interpolated values from the integration points), your results will not improve (or become more accurate) by somehow being able to probe the integration points. Your results will improve by having a sound model with a converged mesh. Furthermore, it's really unlikely that an engineering problem would require values from the integration points. If you find that your peak stresses are X Newtons, you don't design the object to fail at X Newtons (you design it to X + E where is E is some factor. (you know all of this i'm sure...).

And just to clarify, in case you didn't know: the integration points are inboard on the element (i.e. not located at the surface or the corners). The values that are reported are on the surface and the corners and are interpolated from the inboard integration points.

gl hf.

 

[aerovf]

sorry, didn't manage to get element name from Abaqus people. All in vacation, you know...
But I promise I'll get back to you.

mechfeeney, why "skin" technique is used? Why those who use this technique don't simply ignore the difference between FE results
in skin elements and results extrapolated from integration points of solid elements to which skin elements are attached?

Stress/strain are the most accurately assessed at integration points? Theoretically, if we had integration points
at surfaces of the solid elements, would it be better for the assessment of surface stress/strains without skinning?

And, let us leave fine meshing and mesh convergence alone. Skinning is not a substitute for a mesh convergence.
I am trying to get rid of extrapolation, if it is possible. Hope you agree that extrapolation, though giving you
data at points you need, adds uncertainty. Therefore dropping extrapolation works towards more accurate results, agree?

"X + E where is E is some factor" - that is the point. The more accurate FE results, less E I'll add, and other way around.
Isn't it?

And mechfeeney, with all due respect, did you open the picture I posted? What do you think it is about? Can't you find
even coordinates of integration points for the 1st, 2nd and 3rd order of integration?
These coordinates inside of the element, or outside?

I am not trying to convince FE community in something. I was just asking if Ansys has FE element with integration points
co-located with corner nodes, because I heard from Abaqus people that they have. I have not got any argument
that it doesn't make any sense of such an element to exist so far.

 

[btrueblood]

aero,

I think you really need to review a little more of FE theory.

You suggest that having integration points at the surface of an element will give a "more accurate" knowledge of the state of stress at that point.

In reality, the state of stress for an element is known for that element, throughout its volume, once the displacement and forces at the nodes is computed. The Gauss integral is not an approximation of the integral, it is exact, provided certain limits of the element shape are not exceeded. How is that possible? Because very strict assumptions are used in the model of the element (constant or linearly varying tractions on each face, etc.), and are carried through in the analysis - i.e. your input boundary conditions of force and displacement are discretized at each element and averaged at each node. This discretization of boundary conditions is, in and of itself, its own source of errors in modelling.

What is not exact in FEA, is that the stresses from one element to its neighboring elements will always be slightly different in all but the most trivial cases. When these discrepancies are very large, one should (must?) increase the discretization (refine the mesh) to determine if the stress magnitudes are being correctly modelled.

The alternative is to use boundary element analysis methods. BEM will give exact results for the surface state of stress at its integration points. The problem is that, for most structures, it is computationally inefficient (solution matrices are fully populated, rather than being banded as in FEM).

 

[mechfeeney]

Aero,
I wasn't trying to be brazen or rude (and yes I looked at your picture...it looks exactly like the ones in my books). btrueblood explained it pretty well. It's still unclear to me as to what exactly you are asking...and I think that's largely due to the fact that you may not know what you are asking (but I could be wrong and I mean no disrespect).

The picture you provided shows the effect of increasing the order of your interpolation function (shape function). This is pretty standard knowledge...showing how higher order functions can map the curve more accurately. There are two approaches to increasing the accuracy of FEA. First of all the inaccuracies are dominated by the Shape Functions (or interpolation functions)...which are assumed functions describing how the material displaces at the nodes and throughout a given element. If these functions are low order, than...in some cases, the displacements won't be accurate. We have either 'h' or 'p' refinement:

- h refinement: increase the density of the mesh (i.e. reducing element size)
- p refinement: increase the order of your interpolation functions

There are obvious trade offs...but I guess an analogy could be seen with calculus and Reimann sums. If you have a curve, and you are trying to estimate the area under the curve, you can add up rectangles under the curve with the principal in mind the smaller the rectangle width...the higher the accuracy. Now imagine having only a few rectangles under the curve, but instead of flat tops, the rectangles had a higher order curve top piece. This is, in principal, what happens with these two refinement methods.

I sincerely hope this helps clarify some confusions (if there are any). Good luck out there.

 

[mechfeeney]

then* not than* (line 7)

 

[aerovf]

At first, let me say that I feel sorry for being exasperated while answering to mechfeeney. I am a bit stressed last weeks, I apologize for that. Your explanation of integration is clear and easy to follow, I appreciate it.

Ok, per topic, once more again, the whole story briefly. I've got the information (verbal so far) that Abaqus introduced solid element with non-standart location of integration points. That's it. I don't know any details of that element. I don't know even if it is true or just my simple misunderstanding. Before getting more information about this I decided
to ask community a question about similar element in Ansys.

My question initiated a discussion, and by the way, I want to thank everyone who responded. Again, I don't know any details of that element and my curiosity is based on the following points (now I suspect that what I thought of as a definite fact may turn to be wrong, therefore revising theory would be a next step; btrueblood, I'll never argue with your note to review FE theory, fully agree.

So, the points I knew:
1) our organization uses skinning technique every time, when we do analyses to support tests (skin elements resemble gauges)
2) item (1) makes me think that usage of thin shells on top of exterior faces of solids gives more accurate results than extrapolated results on solid faces at corner nodes (given that everything else is the same, like mesh, for example, which has been proved on convergence study),
3) item (2) gave me a reason to think, that if solid element had integration points at corner nodes, then stresses at solid faces would be assessed somewhat close to what skinning gives and no skin elements are needed anymore.
4) at last, info from Abaqus about such an element

Hope this clarifies the nature of my question.

btrueblood, if I understand you right, the source of error is in discretization, but not in the position of an integration point.
I.e. stresses, regardless whether they are calculated at integration points or extrapolated to nodes, are equally accurate or non-accurate depending on discretization. However, while referring to BEM, you are saying that BEM will give exact results for the surface state of stress at its integration points. Why not at corner nodes now? To me it's not logical.
It's an interesting discussion, but may be off-topic.

By the way, I agree that BEM is computationally inefficient, but I am not sure about populated matrices in contrast to banded FEM ones (as far as I remember, matrix size in BEM is significantly smaller because number
of elements and nodes on surface of 3D solid structure is much less than in 3D volume of similar FE model).
I am not sure, but it has something to do with BEM inability to work with non-homogenous structures (absence of information inside the body). But again, it's just my opinion, I never programmed and tested BEM, just read articles about it.


So, to conclude this thread. Nobody can confirm existence of finite element with weird location of integration points in Ansys (key word is Ansys). Even more, this element probably does not exist at all, including Abaqus.

I do appreciate your time and opinion given to me. Thank you.

 

[corus]

I have to disagree with btrueblood. BEM (Boundry Element Methods)doesn't give exact solutions at the surface. BEM is another approximate method of solving the equations of state, just as FEM and finite difference methods are approximate. All depend on the level of disretisation used. As far as I recall, BEM solves the integral equations for the equations of state rather than the partial differential equations. It's debateable whether BEM is more efficient or not, as it only meshes the surface of the domain rather than FEM which meshes the whole volume. As has been said though, BEM populates the full matrix, whilst FEM is a sparse matrix which may or may not require less storage and computational effort. The other downside to BEM is that only constant material properties can be used.

Tara

http://tinyurl.com/4ydjg7m

 

[johnhors]

"usage of thin shells on top of exterior faces of solids gives more accurate results than extrapolated results on solid faces"

- no they do not, "skinning" a solid model will not yield more accurate results. The quality of the results is determined by the quality of the solid model alone, you cannot make a bad 3D model good simply by "skinning" it. If this was true then don't you think it would have become standard practice to skin every 3D model?


Abaqus have a "special" modified ten node tetrahedral element developed specifically for contact analysis. However its performance in contact is not that great and it should never be used as a substitute for the standard element in non-contact models.

http://www.Roshaz.com

quality, cost effective FEA solutions

 

[btrueblood]

Corus, aerovf,

Sorry, I was not being clear. BEM doesn't give exact answers to the problem, my point is that - at the integration points of the surface elements, the equations of the state of stress are exactly satisfied for the given problem statement. I.e., there are still discretization errors in BEM. The only difference is that there are no extrapolations required to find surface stresses.

 

[mechfeeney]

So are you looking for a solution to a surface inaccuracy issue? Currently your method is applying shell elements to the surface (skinning) to populate the surface with an element that "does better for thin sections"? Now you are looking at solid elements with modified or, simply, more integration points?
I'm fairly confident (although johnhors explained the 10-node tet) that the answer to this problem is to apply a denser solid mesh at the surface and a gradient to a coarser mesh towards the inside of the body. This is assuming you are having computational time issues. You should really do a comparison test between your (1) skin technique, (2) a dense solid mesh throughout the body, (3) dense mesh at surface to a coarser interior. Where, assuming proper convergence, (2) is the "correct solution."

 

[aerovf]

Thank you, totally agree. The skinning technique is very new for me and I didn't have much time to play with it thoroughly. Thanks for Abaqus element, now it's clear.