Fatigue evaluation with equivalent STRAIN method 2

[M.hmk]

Do you think fatigue evaluation with use of equivalent STRAIN method ( such as those mentioned in Para. 5.5.4 of ASME Sec.8-Div2-part 5 or para. T-1420 of ASME III-NH appendix T) could be a solution when there are many problems to obtain the exact value of STRESS in singular points?

there are no exact stresses at a singularity. But how about STRAINS near and at singularities in an elastic plastic analysis?

Thanks in advance.

 

[EngDesServices]

Hey M.hmk,

Can you clarify your question some? What are you trying to accomplish, specifically.

Are you trying to calculate stress/strain at a singularity for a specific purpose or are we theory-crafting?

If you're interested in this area, I would recommend checking out a book about fracture mechanics such as Fracture Mechanics - Fundamentals and Applications by T.L. Anderson. It is a wealth of information that would be impossible to cover completely in a post but could help you better understand this area of study.

Michael Hall, PE (TX) PMP - President
Engineering Design Services LLC

http://www.engdess.com

 

[M.hmk]

I want to perform fatigue evaluation with FEA.The maximum stress of my model is at a singular point(such as toe of a weld). Indeed I have not modeled the radius for the notched corner because it is not known.As you know the exact value of stress can not be obtained at singularities.
I want to know is it possible to perform fatigue evaluation using equivalent STRAIN method with elastic plastic material model?

With this method, The exact strain will be obtained at toe of the weld and therefore fatigue assessment will be performed without the need to obtain the amount of stress at a singular point.

What is your idea?
The comments will be appreciated.

 

[IdanPV]

@M.hmk,

Fatigue Assesment using equivalent strains is applicable only when using the Elastic-Plastic stress analysis.

But, I have found this article:

https://pveng.com/home/fea-stress-analysis/asme-viii-2-permissible-cycle-life/

Which demonstrate several ways to calculate permissible life cycles for pressure vessel, even at singularities

 

[M.hmk]

@IdanPV

I read the article and thank you so much for sharing. Two methods have been recommended for singularity problem that one of them is well known for me.
one is hot spot with SSE(Surface Stress Extrapolation) and another is something like the method that was recommended by kalnins(passing an SCL through the weld toe with sharp corner will give converged membrane and bending stresses while the stresses at singular point rise to infinity).

However, I want to know if the elastic-plastic method and obtaining equivalent strains, that I mentioned in my first and second posts, could be a solution for fatigue evaluation at singular points, or not?

The comments will be appreciated.

 

[TGS4]

It could be. Do you have a cyclic stress cyclic strain curve for your material?

 

[BJI]

Why not use the structural stress method, this doesn't require the notch peak stress and is relatively mesh insensitive (for stress extraction).

 

[IdanPV]

@N,hmk,

The SCL method through the weld toe can be found in ASME.VIII-2, Figure 5-A.1.

As for the using of equivalent strains and Elastic-Plastic stress analysis, did you check in ASME PTB-3 Example 5.5.4?

 

[M.hmk]

@TGS4
So, Do you believe that unlike stresses, the strain will converge at a singular point and the required value for fatigue evaluation could be obtained? Would you please explain me what is the reason ?

about the material model: It's easier for me to use Twice yield method and therefore a single loading step(as mentioned in para.b of 5.5.4.1 of part5).

Thanks for your help.

 

[M.hmk]

@IdanPv
I have already checked the example 5.5.4 of PTB-3. But there is no singular point in that model.
My concern is whether the amount of strains in singularities are valid or not.

 

[IdanPV]

@M.hmk,
One of the advantage of using Non-linear analysis (e.g 5.2.4) is that it can "ignore" area with high strains.
You can read more about this issue here:

https://enterfea.com/difference-between-linear-and-nonlinear-fea/

(You can start reading in "Concentrate on the solution")

Did you run the non-linear analysis yet?

 

[M.hmk]

@IdanPV
I'm not experienced in FEA but I usually use elastic-plastic analysis. because I no longer have to deal with the problem of stress linearization and categorization.

 

[mskds545]

Equivalent plastic strain will not converge at an inside corner. Equivalent stress will converge at the plastic limit. Equivalent principle stresses will not converge. It’s hard to find places where this is written down explicitly – many people know about the stress singularity with elastic analysis, but seem unaware of the strain singularity with elastic-plastic analysis. Of course, if it were not true, we would not need elastic-plastic fracture mechanics. It is also very easy to prove to yourself. Make a small 2D model with a sharp corner, decrease the mesh size several times, and make a plot of log(element edge length) vs equivalent plastic strain. The divergence should be obvious. If you use an elastic-perfectly plastic material, it will be more obvious with a coarser mesh, but it will also show up with a strain hardening material model.

Arturs Kalnins sort of mentions this in “Fatigue Analysis in Pressure Vessel Design by Local Strain Approach: Methods and Software Requirements,” but he doesn’t come out and say the strain is singular: “The local strain approach is applicable to cases in which all structural features that affect fatigue damage are defined and can be modeled with sufficient accuracy. It is not applicable to cases in which some structural detail is known to affect fatigue damage but cannot be modeled, either because its geometry is unknown (e.g., flaws at the weld toe of an untreated weld) or because its model is unreliable (e.g., very sharp notch). Such cases require approaches that incorporate the unmodelable details in the test data, such as, for example, those described by Maddox for weld joint classes, and more recently by Dong et al.”

Thankfully for fatigue analysis, there has been an enormous amount of experimental and numerical research to come up with the statistical fatigue strength of weldments based on local stress analysis. Follow Kalnins' advice and the advice of previous posters and use a method based on an SN curve fit to test data (master SN method, smooth bar method with linearization and FSRF, PD5500 structural stress, etc). If you use the smooth bar curve with FSRF, read WRC 432 and pay attention to the data they used. It only went up to about 500k cycles, right before the SN curve changes slope. You might also read BS7608 Annex C. If the stress field isn’t amenable to linearization (e.g., rapid thermal transient with nonlinear temperature gradients through the thickness at the weld), you could consider surface stress extrapolation (though if you are doing a Div 2 design, that code doesn’t recognize this method). Alternatively, grind the weld to a known radius and use the local notch stress.

In areas other than fatigue and collapse, technology has not come as far. The plastic strain limit for ‘local failure’ in Div 2 will not converge at a sharp inside corner. Same with stress intensity at the ends of a semi-elliptical crack calculated with the weight function method for an arbitrary stress profile. This, unfortunately, requires a heavy dose of judgement (i.e. guesswork). Failures due to high hydrostatic test are not particularly common, but cracks at weld toes unfortunately are.

In general, if you’re not certain that your model is converged, run a convergence study. Weld toes are a particularly sticky wicket when it comes to local effects, but an elastic-plastic model can also overestimate the collapse load if the mesh is too coarse. Run a convergence study, and then you’ll know, because the internet is often wrong.

-mskds545 at gmail dot com

 

[TomLee777]

A general practice is to model an 1 mm radius at the toe of the weld to avoid singularity. This practice matches the reality that absolute "sharp' edge does not exist in welding.

 

[mskds545]

@TomLee777 I have seen many welds with a toe radius smaller than 1 mm. Is there a code reference or any literature you can cite that endorses using a 1 mm toe radius if the toe is not ground and the radius is not measured?

 

[M.hmk]

@mskds545
Thanks for you reply.

 

[M.hmk]

@TomLee777
I doubt your suggestion would be a suitable solution since the stress values are strongly dependent on the radius value.

 

[DriveMeNuts]

After reading through all the comments, it does look like you are trying to force the real world to comply with the theoretical world, as eluded to in your first reply from EngDesServices.
It appears that the error that you are making is that you think that you "no longer have to deal with the problem of stress linearization and categorization".
If you are insistent on using a "theoretical" singularity in your model then you will need to use a stress linearization method on your FEM result to translate it for use in the "real" world.

 

[TomLee777]

I agree that the stress values are strongly dependent on the radius value. However, in the FEA model, an 1 mm radius bring an infinity stress to a sensible level, which makes the analysis useful. The actual radius varies greatly in reality. The radius will be different even at different spots along the length of the weld. We need to make an assumption to make the analysis feasible. I don't know if there is a standard for this, but it is rather arbitrary.

 

[TomLee777]

I do find a reference about the 1 mm radius, follow the Link and scroll to the very bottom of the page.