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 ?

 

[gwolf2]

The stresses at the integration points are the most accurate. They occur inside the element and may not be the highest stress in the area; for example around a fillet radius the free surface stress will be higher than the integration point stress.

The element shape function is used to extrapolate the integration point stresses out to the element nodes - these are in a useful location like a fillet radius free surface or a hole edge.

Adjacent elements combined with their shape functions will predict different stress values at their common nodes. The question then arises which stress do you believe? Most FE packages average the stresses for each element at the node.

If the unaveraged stresses are within a few percent of each other I go ahead and use averaged nodal stresses. If the unaveraged stresses are significantly different, I use peak unaveraged stresses, or refine the mesh to get a better result.

IN ALL CASES, UNAVERAGED NODAL STRESSES MUST BE CHECKED BEFORE USING AVERAGED NODAL STRESSES.

WHEN USING SHELL, BEAM, OR ANY OTHER ELEMENT FOR WHICH RESULTS ARE PRESENTED IN SOME FORM OF LOCAL SYSTEM, AVERAGED NODAL STRESSES SHOULD NOT BE USED UNLESS YOU REALLY KNOW WHAT YOU ARE DOING.

I can't count the number of expensive fatigue errors which I have seen as a consequence of averaged nodal stresses.

Amen

 

[prost]

gwolf2 and others: I have often heard the statement in this forum that "stresses at integration points are most accurate." Can anybody provide proof (say a refereed journal article, a section of a book, or a study you have made which has enough details to repeat the study ourselves) of that assertion?

It seems intuitive that this statement is true in a nonlinear analysis because you use the stresses at the integration points in the nonlinear iteration (say a Newton Raphson iteration is used to solve the nonlinear equations). However, the 'truth' of this 'stresses are most accurate at the integration points' statement doesn't seem so obvious in a linear analysis, since all you are doing is solving Ku=f, and there is no need to calculate the stresses at the integration points until you perform the post processing.

 

[rb1957]

i think it's because FEA calculates stresses at the integration points of the elements and extrapolates these to the nodes, and averages across adjacent elements.

 

[btrueblood]

Depends on what you mean by accurate, I'd interject.

If "accuracy" means "correct for the linearized, discretized system of equations that was created to approximate a solid body deforming under load", then, yes, the stresses are correct only at the integration points, and are extrapolated to the edges of each element. A whole bunch of assumptions are built into the FEA element models, some of which imply that the stresses change only modestly from element to element. Thus, we conduct convergence studies, to show that stresses in a region of interest converge to a single value as the mesh is made finer and finer within the region.

If "accuracy" means "correctly reflecting the real-world solid mechanics which are being modelled", then we've got a whole 'nother can of worms to open...

 

[rb1957]

OFGS, don't bring the "real world" into it !!

 

[gwolf2]

ditto,

Opethian, do it my way and all will be well with your world.

Do it any other way and learn to enjoy confusion, fear, late nights........................................

If you want to know why it is the way it is then read a book on FE theory, it's about masters level but not that bad if you are mathematically competent.

Alternatively if you have ABAQUS for example you can get it to print results at integration points, unaveraged at node, averaged at nodes etc. This is a good way to understand the differences. If you combine this with a good postprocessor like PATRAN you will also be able to look at the many different ways in which stresses can be dispayed as both contours and numerics and relate this to the numbers in your printout file.

 

[opethian]

ditto
FEA is undergrad level course in my country and do not worry i passed several FEA courses . My question was about post processors mostly. If you have used hyperwork and abaqus post processors you will be confused soon for sure you will be confused about the programs. Best is to write your own post processor i guess.

 

[rb1957]

OFGS (again) ... we don't want to be doing That ! how many ways are there ? i agree that making a code of your own is something you understand, but what about the rest of the world ? how much confidence would you have in someone else's post-processor ? ok, it makes pretty pictures ...

that's why (well, one reason why) there are canned programs. everybody knows (ok "knows") how they work and so it's "just" the application of the software to the particular problem that's the issue.

i agree you need to understand what the post processor is doing. run some simple patch tests. on a different level, i don't particularly care how the FEM extrapolates from the integration points to the nodes. i know that the stresses reported at the nodes are accurate for some cases and very inaccurate for others, depending on the program and the loading; this leads to increasing the mesh density to resolve the known issues (eg, put a single CQUAD4 in bending, it doesn't like it, so we don't do it !).

only MHO ...

 

[johnhors]

gwolf2 - just curious, in your last post are you inferring that Patran is a better post-processor than Abaqus/Viewer?

 

[btrueblood]

Sorry, RB, you're right. This is FEA we are talking about, not engineering...

 

[gwolf2]

johnhors,

No, I've never used ABAQUS viewer. I gave PATRAN and ABAQUS as an example. ABAQUS results output type control is outstanding (meaning you can see exactly what is going on in the .dat file if you wish), and PATRAN can display combined numeric and contour plots at averaged, unaveraged, and integration points - just what you want if you be sure what's going on.

gwolf2

 

[prost]

IMO you still need to differentiate what goes on in FEA software for linear vs. nonlinear solutions. In linear solutions (no iterations, material linear, no contact, etc.), stresses are never calculated at the integration points UNTIL you do the post processing to extract them. In a linear solution, you calculate only the displacements (your solution vector), and all you to do is invert the big stiffness matrix K. In a nonlinear solution, which requires a nonlinear iteration method such as Newton method, you need to calculate the stresses in the previous iteration to get your new solution vector. Because you calculate the integrals in the FE method not exactly, but by the Gauss approximation, in which the quantities in the integrals are calculated only at the Gauss integration points, at least in principle it appears to me that stresses are most accurate at the integration points but only for the nonlinear solutions, NOT for the linear solutions (since stresses are not computed as part of the linear solution procedure).

Since it isn't often you know the exact solution, I would define 'accurate' relative to the numerical convergence of the stresses--any quantity is more accurate at a (first) location relative to another (second) location if its numerical convergence is quicker for the first location relative to the second. Now maybe this is dependent on your particular software, the way in which stresses are calculated--but the statement "...the stresses are correct only at the integration points, and are extrapolated to the edges of each element...." is incorrect in general (unless you can present proof otherwise). Stresses are calculated from the strains, which are just the spatial derivatives of the displacements (see, for instance, Szabo and Babuska, Finite Element Analysis--which is up to $190 on Amazon! When did they start gilding the pages?). Again, in a linear solution, there is no need to calculate stresses at the integration points, until you are finished solving the Ku=f equations. You can calculate stresses ANYWHERE in any element using just the solution vectors and the spatial gradients, and are not restricted to calculating stresses at just the integration points and extrapolating.

Unless of course that's just a restriction (stresses are computed directly only at integration points and are extrapolated to edges) your FEA software places on your analysis.

 

[btrueblood]

prost wrote:

"the statement "...the stresses are correct only at the integration points, and are extrapolated to the edges of each element...." is incorrect in general (unless you can present proof otherwise). Stresses are calculated from the strains, which are just the spatial derivatives of the displacements "

Yes, but no. Saying that the strains are calculated, and not the stresses, is pretty specious, since they differ by only the constitutive model (which for linear problems is a linear factor difference). The strains are no more calculated (again speaking of linear FEA) than the stresses are - both are buried in the FEM formulation, and thus are calculated implicitly whenever the K[x] = f matrices are solved. Backing them out and printing them or coloring the charts is more of an excersize in computation, not calculus. The calculus came in formulating the elements' stiffness matrices.

More importantly, in linear FEA, the displacements are known at the nodes, which are at the boundaries (generally the corners) of the elements. But the strains (and thus stresses) can only be calculated between the nodes, since the strain is derivative, i.e. the difference in displacements between two or more nodes. All element formulations I've ever seen and/or derived, have an implicit (assumed) stress distribution across the faces of the element (typically constant for linear elements), which allows the stresses and strains to be derived and the element stiffness matrix formulated. The result is that the stresses are known only by derivation from the displacements, which in linear models implies that the stresses or strains are "known" (in the sense of how they were modelled) in the center of the elements.

This basic idea, that the nodes (where the displacements happen) and the interior of the elements (where the strain and stress happen) is why you need to refine meshes to keep the difference in stress from one element to the next, is what we should all take away from this.

Textbook reference would be The Finite Element Method in Engineering Science, Zienkiewicz, O. C., 1971, 1977. Might be a bit dated, but I doubt very much that they've changed how to compute derivatives in the last 40 years or so.

 

[btrueblood]

Sorry, this

"This basic idea, that the nodes (where the displacements happen) and the interior of the elements (where the strain and stress happen) is why you need to refine meshes to keep the difference in stress from one element to the next, is what we should all take away from this. "

Should've been:

This basic idea, that the nodes (where the displacements happen) and the interior of the elements (where the strain and stress happen), are different (one is a point in space, the other a volume, thus they physically cannot be the same) is why you need to refine meshes to keep the difference in stress from one element to the next, is what we should all take away from this.

 

[btrueblood]

ARGGhhh....3rd time's the charm:

This basic idea, that the nodes (where the displacements happen) and the interior of the elements (where the strain and stress happen), are different (one is a point in space, the other a volume, thus they physically cannot be the same) is why you need to refine meshes to keep the difference in stress from one element to the next as small as practically possible to avoid errors, is what we should all take away from this.



...and if anyone knows how to avoid errors in posting, save iterations, please tell me.

 

[pja]

The reason that the statement is often made that stresses are more accurate at the Gauss points, even for linear problems, is that for elements like Q4 and Q8 the stresses are superconvergent and their accuracy is comparable to the accuracy of computed displacements.

For example impose on an element a displacement field f whose degree is one order higher than the highest-order complete polynomial for the element interpolation. Then obtain the nodal dof by evaluating f at the nodal locations. Next if you seek locations in the element to evaluate the B matrix (used with the nodal displacements to compute the strains) such that the strain as calculated from f is the same as that calculated from B*d where d is the vector of nodal displacements, those locations will be at the Gauss integration points for lower order elements which are most commonly used and slightly different for higher order elements (which are seldom used).

 

[prost]

What is the basis for the statement "stresses are implicitly calculated from the solution to Ku=f"? In a linear solutions, where are stresses (or strains for that matter) in "K," "u" or "f"? No, stresses are calculated AFTER you compute the displacement vector "u", by computing, as you know, the spatial derivatives. Stresses and strains are calculated with the postprocessors. If your FE software does it differently, I'd sure like to know the reason, since no stresses or strains (other than at the boundaries, in which case stresses are known because they are imposed by the user) are needed in the matrix "K," or the vectors "u" or "f" in a linear solution.

As far as stresses being superconvergent, I doubt that's even numerically possible, since stresses are derivatives of the displacements (which can be superconvergent, depending on the formulation), and anyone who has ever tried to compute derivatives of anything knows how crazy derivatives of apparently smooth data can look. I would be most appreciative if you would supply an actual reference, say a published paper, and not a statement from a User's manual for the FE software. I have accepted anything's possible, but it would be nice to have proof found in the open literature.

 

[btrueblood]

Prost,

How is the stiffness matrix derived for a given element?

To derive the algebraic equations for a given element's stiffness matrix, one must first solve implicitly for the stress and strain fields internal to the element. This is done by making certain assumptions about the boundary conditions (small displacements, linear constitutive model, constant tractions at the boundary faces, etc.) and then applying complex transforms to solve the stress/strain fields directly via numerical integration.

Thus, after actual load and displacement vectors are solved for, the strain and stress can be backed out from the stiffness matrix formulation as algebraic sums. The stress and strain were already solved for, by the person who computed the equations for the stiffness matrix. All FEA models report element stress tensors based upon the element stiffness model, and these stresses are calculated at, and are most "accurate" at, the integration points used to derive the element stiffness model. If you try and apply your own "stress calculation" to derive the stress field from the solved displacements, you will have a result that is less accurate than using the already solved equations to find the stresses at the integration points that were used to derive the element stiffness.

So, fine, Mr. Prost, you are technically correct in the statement "stresses are calculated AFTER you compute the displacement vector "u",". Yes, generally, the stresses are computed after first inverting and solving the Kx=f matrices.

But, the rest of your statement "...by computing, as you know, the spatial derivatives." is not correct, at least not for linear solutions; the stresses in a linear FEA again, are found from implicit equations, not by recomputing the difference equations that you've already solved by integration. So, I and others, are also correct. And the reference I gave is a textbook, one of the original ones for FEA, that describes the above in excruciating detail. I should know, as I used it for many years to write and solve my own FEA codes.

 

[pja]

Prost,
The superconvergent-like behavior of stresses at Gauss points for Q4 or Q8 elements is shown to be true in many textbooks..for example look on page 231 of Cook fourth edition. My example gave the reason for this and was actually taken directly from Cook.