FE-Weld Fatigue mesh insensitive- Battelle 2

[deanflinn]

I was wondering if anyone has had any experience or completed work using the Structural Stress FE-Weld Fatigue mesh insensitive approach as defined from Battelle?

Continuing from an old previous thread - Fatigue assessment without the fudge thread 727-155500 - the topic was discussed but since there has been a commercial package released, (Verity) and also included in the ASME Section VIII, Division.2 , anyone found good results from it?

Has anyone had success with applying the theory to their weld fatigue, or even defined they own Master S-n Curve?
What are your thoughts

 

[corus]

Having read the blurb on

http://www.safetechnology.com/fe-safe_verity.html

I'm a little surprised that ASME has included the method as it seems a simplifcation too far. It makes sense that the stress in a particular direction, either along the weld, or across the weld toe, would have an effect on fatigue life, just as any of the weld classifications would. This has been shown by the Welding Instutute (TWI) whose test data provided the basis for the fatigue design code BS7608, or whatever its equivalent is these days. To ignore this and just use a single master curve for all welds seems a mistake to me. The problem with the weld fatigue curves and classification was in determining the reference/nominal stress, but a method, albeit laborious, had been decided upon where the stress was interpolated to the weld toe, removing any non-linearity for the stress concentration effect. I'm surprised that the method of using nodal forces is also mesh insensitive as the mesh density effects the relative stiffness of the finite elemnt model, and hence the nodal force distribution. Me thinks people are just getting lazy these days.

corus

 

[johnhors]

Corus,

Can you please explain the reasoning for your statement "the mesh density effects the relative stiffness of the finite elemnt model" ?

 

[TGS4]

I have used the Structural Stress Method in calculations. It works well, and appears to correlate with some real failures that we have investigated.

The one caveat that I would put on the mesh-insensitive part, is that the mesh needs to be sufficiently refined to avoid the issues that corus refers to. However, beyond an "adequately" refined mesh, because the method calculated the membrane and bending stresses using nodal forces, it has less sensitivity. The way I understand it is that forces are primary variable in the F=kx equations, whereas stresses are derivatives of x.

 

[corus]

johnhors,
It's my understanding from early days looking at the theory that the coarser the mesh then the stiffer the overall model, such that convergence with increasing mesh density tends from only direction, rather than oscillitating about the true solution.

To me the assumption that the method is not mesh sensitive will result in people having as few a number of elements in a model as they can get away with. I'd have serious concerns about results from such 'insensitivity'.

corus

 

[johnhors]

Corus,

For accurate stress results a fine mesh is certainly a requirement. However to see a degradation in overall stiffness you would have to generate an absurdly coarse mesh! The whole basis behind sub-modelling for instance is that the refined sub-model has the same stiffness as the coarsely meshed complete model, otherwise it simply wouldn't work. Models made purely for dynamics and natural frequency analysis can be relatively crudely meshed and still produce accurate results, because their stiffness and mass distributions remain correct with a coarse mesh.

 

[corus]

The problem is johnhors, with a method that claims to be mesh insensitive then you will get people producing absurdly coarse meshes!

Of course if an absurdly coarse mesh produces a degradation in overall stiffness then perhaps a mildly silly coarse mesh would produce less of a degradation in overall stiffness, but still a difference in stiffness that this method relies on. To say that the method is not mesh sensitive seems a little dangerous to me and I'd prefer to see mesh sensitiveity tests to verify the results before relying on it.

corus

 

[johnhors]

If the fine mesh occupies the same volume as the coarse mesh (as would be the case where all sides are planar), then the overall stiffness of the volume is the same in both cases.

Stiffness changes will only start to occur when curved surfaces become poorly defined as they take on a facetted appearance, but even then the difference will be very minimal indeed.

Thus any method which relies on the stiffness in the surrounding structure and not stress, is by definition going to be mesh insensitive.

 

[corus]

My recollection is that if you take a 2D rectangular section, for example, and apply a load then the displacement will be less for a coarser mesh, and will tend to the true solution as you increase the mesh density. ie. the model is stiffer for a coarse mesh, even though the volume remains unchanged.

I still have my doubts on the method and would prefer to see sensitivity studies on the method before accepting it.

corus

 

[johnhors]

Attached is a simplistic analysis for a cantilever, which shows that the percentage error with regards to the analytical solution is 0.62% when just five elements are used and that the error reduces to 0.50% when five thousand elements are used.

Thus the fine mesh shows a 0.12% error reduction over the extremely crude mesh. This change in error being less than a quarter of the total error for the fine mesh.

I think that it is fair to say that the overall stiffness of the block is practically insensitive to mesh density.

 

[mcclain]

johnhors,
Do you know what the error would be for the five element case if using linear elements (8-node) instead of quadratic (20-node)?
Thanks

 

[johnhors]

McClain,

I get a displacement of 0.4959 using five eight node bricks (with Calculix) , thus giving an error of 0.082%

 

[Denial]

Corus, you are correct that a coarser mesh will always predict smaller displacements. This is because the mathematical functions that represent the displacement state are approximate, and the coarser the mesh the more approximate the representation.

Thus the FE process itself can be viewed as applying additional restraint to the structure, albeit a mathematical restraint ("you will deflect according to this set of equations") rather than a physical one.

 

[corus]

Well.. I'm not sure johnhors example is a good one as he takes a beam in tension (not a 'true' cantliever under bending) and I doubt mesh refinement has that much of an effect, as was shown. I only remember the days when the theory was taught to me and it was shown that the convergence was monotonic(?). If there are papers on the method with validation, and whatever caveats may apply, it would be interesting to read. I have seen the program FESafe for fatigue assessment demonstrated before but that seemed to concentrate on solid structures, and the method for weld fatigue assessment seemed to be the same fudge self assessment that comes with any FE program. Maybe it's changed since then.
The method in british standards, such as BS7608, is to classify each type of weld, it's location, and principal stress direction. This method seems to disregard that and imply that you can get away with any kind of mesh to get results. I have my doubts.

corus

 

[TGS4]

The mesh-insensitivity comes about because the method uses nodal forces rather than stresses. The wizardry of the method is not in the calculation of the weld stresses or S-N curves, but rather how the method collapses (reduces the scatter) of the fatigue test data.

As I said before, the method is an accepted method in ASME Section VIII, Division 2 (2007), with the standard caveats that the FE mesh needs to be adequately refined so as to avoid the issues that corus is referring to.

And my recollection, too, is that convergence is monotonic from below. If your model is too coarse, then whatever results you take from it are lousy. That said, with this method, you don't need 10 quadratic elements through the thickness and 1000 elements around the circumference of the nozzle weld either...

 

[johnhors]

Attached are results for a cantilever in bending, modelled using 20 node bricks. The very crude mesh with 10 elements is just 1.22% different from simple theory whilst the very fine mesh with 10000 elements is in error by 0.05%

Whilst the error does decrease with mesh density, the accuracy of the very crude mesh is still very good.

The displacement functions used in these elements are very good at describing deflections, the better they are the fewer elements are required for displacement analysis (not stress !). For instance, beam elements which use a cubic displacement function are a perfect match with simple beam bending theory in linear statics, one element of length 250 gives the same result as 50 elements of length 5 at the end of a cantilever (unfortunately this doesn't apply to natural frequency and buckling mode shapes)

 

[corus]

For fun I ran the same analysis using Abaqus with 8 noded linear elements and the error was 33% with 100 elements and 1.7% with 12500 elements. A bigger difference than john's but this was using linear elements. Maybe time to switch to Calculix?

Of course the method relies on the reaction/nodal forces which must equate to the input forces. It's the distribution of such forces in a more complex model I'd be concerned about and at least ASME has included the necessary caveats to maintain standards of modelling techniques. It'll be interesting to see if the european standards include the same method.

corus

 

[Denial]

I recently had a need to assess the fatigue strength of some fillet welds. I used the approach that is detailed by Det Norske Veritas in their document DNV-RP-C205, "Fatigue design of offshore steel structures", August 2005, in particular section D.8 of that document.

The key points about the method are:
» It allows stresses predicted by an appropriately modelled FE analysis to be used directly against an S-N curve.
» The S-N curve to be used is given in the document. It is
For N<10^7 log10(N) = 13.358 - 3.0*log10(S)
For N>10^7 log10(N) = 17.596 - 5.0*log10(S)
where S is in MPa.
» Reentrant corners in the weld must be modelled as "notches" with a root radius of 1mm.
» For quadratic elements (which are preferred) element spacing around the root radius must not be greater than 22.5 degrees.
» Elements of approximately that size must be used for at least three elements in from the notch surface.
» The analysis should assume linear elastic behaviour.
» The stresses to be taken from the analysis should be surface stresses rather than "integration point" stresses, calculated by extrapolation if necessary.

The S-N curve given (and reproduced above) is based on "mean minus two standard deviations", and thus embraces 97.6% of the experimental data considered.

The application of this method is quite straight forward, and able to be done using pretty much any FE program.

As for my results, I'll have to wait forty years to find out whether I got it right.

Does anyone have any experience of / views on this method?

 

[corus]

I downloaded the standard from

http://exchange.dnv.com/OGPI/OffshorePubs/a4.htm

and the advice there is very good. I'm not sure I'd go as far as they recommend with modelling notches at the weld, but the general method of extrapolating to the weld is fairly common practice. The methods of incorporating the weld stiffness is very good though and I'll pass it on.

corus