stress concentration factor - fine mesh FEA 1

[magicme]

hello

i can't get any universal agreement on this question, and it seems it should be simple.

i have a finite element model (ANSYS) of a hollow stepped shaft with a fillet at the root of the step. i model a fine mesh (at least 10 elements from OD to ID ) and looking at bending and torsion in the shaft. the mesh is very fine when compared to the radius of the fillet (3").

i argue that the stresses output by the model are valid as-is, while some of my partners say i need to add stress concentration factors on top of the ANSYS stresses. i think they are wrong --- if the mesh is fine, the stresses will implicitly include "stress concentrations".

i have searched the previously asked questions and can't put together a direct answer to this question.

any comments would be appreciated.

regards

magicme

------------------------------------
"not all that glitters is gold"

 

[jerzy]

Hello magicme,

I agree with you: as mesh is refined, FEA model stress will approach real world stress (most of the time, we hope.)
Recall how stress concentration factors are defined: simple expressions that ignore the stress concentrating effects are used to give a value which is then corrected for the ignored effects. In the FEA models the geometry includes the stress contcentrating details (if the model has not been "de-featured").


jerzy

 

[Stringmaker]

If you have a well converged solution in the fillet then you should be good. Otherwise you may want to use some stress concentration factor reference, such as Peterson's, to calculate this factor. I'd probably try and verify my FE results to an analytical case just for my own piece of mind anyway.

Good luck,
-Brian

 

[cbrn]

Hi,
if the analytical table you are using for SCF has been correctly defined, and if your geometry is truely corresponding to that table, then FEM will give you almost exactly the same result as the table (errors less than 1%when you properly build models to compare to Peterson's or Roark-Young's cases). This has been verified many and many times.
The problem is that, being the SC a very localized effect, you have to be extremely careful in how you mesh the zone where you expect the SC to occur (size AND type of elements...). If you are investigating a non-tabulated geometry in order to obtain the SCF (in order to apply it over a simplified general model, for instance when you perform shaftline analyses and you have to determine fatigue life), I'd say that you need "exaggeratedly-fine" mesh in the zone of the SC (I mean, elem size is about 2 orders of magnitude less than in the "far-away" zones). Mesh transitions must be smooth, elements must not be distorted, etc... And also, be sure to apply boundary conditions "very far" away from the SC zone...
Regards

 

[corus]

If you can use hand calculation methods to determine the scf and hence the stress at the detail then I'm not sure why you bothered modelling it. However, if you have included the detail in your model then obviously you don't need to include a scf on the stresses from the model. Why don't people just use simple common sense and look at the results they get?
Personally I try and validate or verify results from a FE model each time. In your case I'd use the hand calulcation method to see if you get a similar answer. It doesn't have to be exactly the same as you may have other features close by which could influence the result. It would show you're in the right 'ball park', to use an american euphonism, and you haven't made an obviously stupid mostake, which quite often happens.

corus

 

[cbrn]

Corus,
what I wanted to say is that many times we deal with very complicated models for whom it would be impossible to include all the details. I mean, simplifications such as sharp edges instead of fillets, etc. So, the general, complicated, FE model will produce erratic results on these stress raisers. In order to correct these situations, it is, I believe, very common to sub-model (or model separately) the SC zone if its geometry doesn't fall into a tabulated analytical case. Think of a stepped shaft with polycentric fillets: this case is mentioned in Roark-Young but no table is provided. So, a dedicated axisymmetric model properly built and meshed can give you the SCFs (for axial, bending and torsion) for the polycentric fillet. The shaft model can remain without any fillet, and it will be far better since, unless you use extremely huge quantities of elements, it won't have sufficiently fine a mesh in order to give the correct value in the SC zone. With this method, for example, I will be able to use a beam formulation for my shaft static and dynamic analysis (which is sufficient and computationally efficient), and still have correct results for the stresses at the shaft steps... Of course, if you prefer making a shaft analysis in full-3D with 564287900 elements, you are free to do it...
If you think this is not "simple common sense", please educate me...

 

[corus]

Well cbrn, the comment about common sense was meant for your colleagues, however I am pleased to educate you where I can.
For a stepped shaft then you can find SCFs in Peterson Stress Concentratio factor book, if it's not available in Roark. For a polycentric fillet (which I presume you mean has a fillet made up of 2 radii) then just be conservative on the scf from the book, and use the small radii. Otherwise if you are to model it then use a 2D axisymmetry model instead of a 3D model. For asymmetry loading such as bending, you can still use a 2D axisymmetric model instead of 3D, but just use asymmetry loads. Of course you can still always use a 3D model but reduce the model size with symmetry for that partticular loading, wherever possible.
You can then apply the scf you get by whatever means to your beam model.
I hope that helps

corus

 

[magicme]

thanks to all for the replies.
i understand the cautions involved with meshing these areas, but feel better now that the very fine mesh will closely capture the true stress field without the need for an additional SF. (to be true, i usually add my own "comfort factor", knowing all the uncertainties of applied loads, etc etc)

regards

magicme



------------------------------------
"not all that glitters is gold"

 

[cbrn]

Corus,
sorry I have misinterpreted you. It seems in reality we both agree 100%. What you describe in your latest post is exactly what I usually do.
Where I have to depart a little is on your statement "... just be conservative and use the small radius". Apart some rare exceptions, it's a thing I can not do. The behaviour of a polycentric (can be 2 radii, but sometimes we have 3 radii or a spline law) can be tricky and we can not be over-conservative, so the best way is to actually analyze the fillets in axiharmonic-2D. It's a 5 mn task since I have built a parametric APDL.

Btw, and to return to the o.p., sometimes also the tables are subjected to variations / updates which continuously ameliorate them: Peterson's book is out-of-date for some stress raisers, for which several "corrections" have been proposed.

Regards

 

[rb1957]

I would use petersen to check the FEM result (remembering that the stress conc. factor is the local stress divided by the remote stress).

I would never apply Kt on top of an FEM result, unless i didn't model the conc. (maybe a hole), so the FEM was essentially telling me the remote (ie unconc.'d) stress at the point in question.

remember too that the stress conc. peak is Very shape. you need the surface node stress (rather the average of the surface element).

 

[prost]

magicme: It just occurred to me after reading your last post that what your colleagues were talking about was 'Safety factor'--SF in your last post. If my interpretation is correct, then of course you must use a SF that you would divide the max. stress by to get your max. allowable stress. Safety factors are an integral part of any engineering analysis; Safety factors are engineer's insurance that the numerous uncertainties intrinsic to any analyses don't reach up to grab us and cause the structure to fail. What are the sources of uncertainty? Assuming your FE solution is converged to within your a priori error bounds, you still have many uncertainties in material properties, loads (what's the phrase? FE analysts try to compute the 3rd significant figure, loads engineers are happy with the correct sign? Someone out there knows the correct expression, my apologies for botching it), geometry definition (could be the difference between 'as designed' and 'as manufactured'), manufacturing anomalies such as nicks and scrapes introduced during the making of the structure. Even if your FE solution is perfect, you still all those other uncertainties, most of which you can control only to a limited extent.

 

[magicme]

prost

no, what you say is not correct.... some of my colleagues are definitely saying that they would apply "Peterson"-type kt's and kb's to FE stress results. and my argument is that a very fine mesh of a well-shaped model (holes and fillets in detail) has already captured a very accurate stress picture and no stress concentration factor needs to be added.

i think their position goes back to crude models (maybe plate elements, no fillets, etc.)

but we all do agree that a Safety Factor (i called it a "comfort factor") is generally necessary. this helps you sleep at night, given all the uncertainties of the "specified operating conditions", material properties, etc etc.

(which reminds me to post a comment on optimization in another posting.)

regards

------------------------------------
"not all that glitters is gold"

 

[rob768]

Compare stress in the straight shaft, multiplied by the stress concentration factor with the stress as predicted in the fillet. they should compare well.
We're doing FEA in order to do away with stress concentration factors, so no need to do double.

 

[prost]

If you model the notch properly, and your colleagues are still saying you use a "Peterson" type kt and kb to 'hit' the FE calculated stress concentration factor, that's double bookkeeping, and it's a wonder to me that you can afford to make anything with such an analysis approach. Certainly you couldn't afford it with airplane designs. Safety factor is one thing, but essentially squaring the Kt of the notch sounds like bad design practice to me, and unnecessarily conservative.

 

[corus]

My guess is that your colleagues are suggesting you apply the factor to the nominal stresses away from the stress concentration, rather than the value obtained from the model at the stress concentration. This may be a reasonable approach as FE tends to underestimate stresses, however the approach would only be applicable if the detail was the same as in Peterson. Probably the best way is to compare the FE result with the nominal stress x the factor and choose the biggest stress.

corus

 

[magicme]

thanks for the added comments

i am sure now of how to proceed; and i'm pretty certain that the people wanting to add SCF's to the results are based on their history with simplistic modeling (course mesh, plate elements).

we actually have 2 "camps" on this issue and the guys who are saying "no added SCF to fine mesh models" are going to win this one.

thanks for the valuable support.

magicme.

------------------------------------
"not all that glitters is gold"

 

[FEAHappy]

I believe a stress concentration multiplier should not be applied to a FEA result in a radius. (assuming a fine mesh)

The question I would pose regards the depth of the stress.

If the stress decreases by 30 %, .010" below the surface in a 4" shaft, .25" R, I wonder which stress to use.

 

[cameprak]

Hello,

relevant to this thread, i have a doubt. small fillets are avoided in big plastic components analysis which are normally not a standard structure. How to interpret the stress values near sharp corners. what are the considerations and factor of safety.

 

[gurmeet2003]

As clarified in many posts above SCF can not and should not be applied to FEA results.

One should take necessary precautions in quality of mesh to ensure that mesh is appropriate. Also in recent past I have become a fan of using mesh convergence to check the adequacy of the mesh. A second run is made with either half or double the first mesh density in the area of interest. The results are compared. The difference between the results gives a good check on whether the mesh is fine enough.

Cameprak asked a question about how to handle sharp corners. Many products have sharp corners. Sharp corner is a singularity, therefore refining the mesh at a sharp corner will not work. It will keep on giving higher stress as the mesh is refined. However one can judge from a preliminary analysis if a sharp corner is important or not. If the stress in a sharp corner is less than one third the maximum stress in other regions, it can probably be ignored. Also check if there is any significant dynamic stress in the sharp corner. Sharp corners are susceptible to fatigue failures, whereas a monotonic stress will be releived by plastic flow. However if it appears that a sharp corner is important, put a fillet on this corner and analyze it.

Gurmeet

 

[corus]

gurmeet,
You can't make a preliminary analysis of a stress at a sharp corner by comparing it with other stresses, when you've just explained that the stress is at a singularity, therefore the value there has no meaning.

corus