Stress concentration problem in FEA 1

[Diegoaest]

Hi all,

I have a problem of stress concentration or singularity. Stress is increased as mesh size is decreased. There is no convergence, so results are unreal.

I have learned a lot about this problem in other threads of the forum. But in this case I am not interested in knowing if the peak stresses in small regions are acceptable or not. I want to know the stress in that area. I mean, getting results with an acceptable accuracy. In addition, I can't ignore those peak stresses because I consider fatigue damage later.

Tests were performed and I know the real results. So, my objective is setting the FEA analysis or modelling correctly (or some other measure) to get convergence, checking the results are valids. And then, with that correct setting, I will be able to carry out other analysis changing geometric parameters of the piece (for a optimization purpose).

Is it possible getting real results or that area can't be studied due to the stress concentration?
Is it possible getting results ignoring the peak stresses and working with the surrounding node or element stresses?

My case is a 3D model and the problem is caused by a boundary condition, a fixed support, in the surrounding area of one of the edges of the face where is imposed. This conflicting area is a thread zone, like a nut.

Measures I've already tried unsuccesfully:
1- Trying different mesh settings. I work with ANSYS Workbench and I have used tets elements with midside nodes, although I have tried with bricks too.

2- Remodelling the shape of the CAD model where is the boundary condition, to decrease the stress concentration. This have influence but don't avoid the problem.

3- Changing the fixed support into a elastic support (more realistic). Here I don't know what foundation stiffness (in N/m^3) I can introduce and, anyway, I always get this warning: "One or more bodies may be underconstrained and experiencing rigid body motion. Weak springs have been added to attain a solution."


I think I'm making a mistake somewhere, probably related to the FEA model.

I would appreciate your help,

Regards

 

[GregLocock]

Take a step back and think what a fixed support really means. Think what happens to the stress gradients in the structure as you physically approach that impossible but mathematically convenient constraint.

I'd run with option 3, and would devote substantial energy to finding out what a realistic foundation stiffness is. I'd also figure out appropriate additional constraints myself rather than letting the machine decide.

In the automotive world anyone who tells you they've got anything stiffer than 50000 N/mm to bolt up to probably hasn't measured it very well (there are exceptions, eg cylinder heads in their own right).

Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[oneintheeye]

i think your error message may be due to the soil stiffness k value only putting spring in vertical with no horizontal restraints hence structure is free to move. The program may be putting 'weak' springs in this direction to allow a solution. My program crashes unless inputed myself yours might be different. Obviously this is not definate as your program is different.

 

[gwolf2]

The only way to get an accurate fatigue stress around a fastener using FE is to model the joint in detail with contact, friction, and pre-load.

If you work for a big aerospace company you can do it via loads at a point restraint with appropriate springs and then use well tested in-house empirical software to come up with a fatigue life.

If threads are the fatigue hot spot then empirical or test is probably best, although if you have the time and skill you could sub-model the thread interaction with contact.

I have yet to see a fatigue problem which can not be eliminated completely by trivial design modifications. These problems usually arise because the component is the wrong shape for the loads in the first place.

Try looking at this problem in different ways. I say this because I doubt that Ansys Workbench will allow you the sort of detail needed.

good luck.

gwolf

 

[Diegoaest]

First of all, I´m very grateful for your help.

Yes, I realised the problem is bigger than I thoght. Firstly, the objective wasn't solving this subject, in fact that part of the piece wasn't going to be analyzed by FE since tests were performed. However, I'd like to make sure I can't model it approximately (I suspect I could do something else with ANSYS but I don't get it), otherwise how can I justify the difficulty of the analysis? I have no idea about contact or friction problems applied to FEA, would you know any reference?

Regards

 

[gwolf2]

> I have no idea about contact or friction problems applied to FEA, would you know any reference?
Sorry no - as you have Ansys you could start with the user guide, it can probably do it but it probably won't be easy or intuitive.

You could try extracting loads from the point restraint and perform some hand calculations with suitable KT factors but beware! Most of these book methods (e.g. Bruhn, Niu) are based on limit or ultimate load and smear the stresses via plasticity. Not what you want for fatigue. The heel-and-toe effects and friction on the bolt head are important at lower loads - this is why aerospace companies for example have specialist programs filled with correlated test data to do this job.

Try a hand calc, be pessimistic in your assumptions and see where that gets you. If the stresses are very low and the fatigue life very high (say 10^8-9 cycles and you only needed 10^4 cycles) then maybe that is good enough and you proceed at risk.

gwolf

 

[gurmeet2003]

Diegoaest,

You said you have a problem of stress concentration or a singularity.

These are not the same. A stress concentration represents a real physical situation, where as a singularity represents an incorrect physical model. For example:

A fillet or a hole in a stressed area is a stress concentration. But a sharp corner is not. A sharp corner is a singularity becuase if you use an elastic material model, the stress will tend to go to infinity as the mesh is refined further and further. However if you use a non-linear material model, which includes yielding, the singularity will go away as material will begin to yiled and stiffness in the material will go down substantially leading to very small rate of stress increase beyond yielding.

You said,"Is it possible getting real results or that area can't be studied due to the stress concentration?
Is it possible getting results ignoring the peak stresses and working with the surrounding node or element stresses?"

A good way to judge whether the area is a possible casue of failure would be to look for expereince in similar equipment. But if you are concerned about the area ignoring the peak stress and looking at surronding nodes is a not an acceptable method. To identify whether the problem is real or not, first step is to carry out a convergence study. If you can get convergence then your stress is real (based on your model). It leave the question of BCs still to be decided by testing.

However you have indicated that you did not get mesh convergence. A fixed boundary condition is likely to give areas of high stress in the neighbourhood. You have indicated that your high stress area is in the nut. Have you modeled the threads? What is the application?

I deal with lot of bolted joints in gas compressors. But usually these joints are preloaded. The stiffness of the joint protects fatigue load from being transmitted to threaded areas. This protection is necessary because threads are very poor in fatigue due to high stress concentration at the thread roots.

Also if you are looking at stress in thread roots the chances are that the thread exceeds yield strength of the material. How do you propose to account for yielding in your fatigue calculations?

Gurmeet

 

[Diegoaest]

Hi,

Thanks for the explanation, I realised I was confusing terms which are different (stress concentration/singularity). I could not get convergence, so I was talking about a singularity caused by a boundary condition. I would have to get a more realistic condition, for example by using springs.

But then you said: "threads are very poor in fatigue due to high stress concentration at the thread roots" And that is exactly the conflicting area. So, I suppose both questions are happening here. (or the convergence study is wrong, but I don't think so) What is your opinion?

The joint is not preloaded. But I am not studying a complete joint, I am only dealing with a piece that, in service, is screwed a bolt below.

I have modeled the threads but only approximately (exact cross section but no threads inclination) since it is a wedge for a small angle of revolution (axisymmetric model).

Although the cases are different, how do you model the thread area in your bolted joints? I have seen structural preloaded joints with the bolts modelled through trusses elements to avoid convergence problems and include the preload effect in the study of the overall behavior of the joint.

As for fatigue, fatigue calculations are carried out with the strain-life method to account for cyclic plasticity. By simultaneously solving Neuber’s equation along with cyclic strain equation, we can calculate the local stress/strains (including plastic response) given only elastic input.


Thank you for your attention

 

[gurmeet2003]

Diegoaest,

Usually I also model the threads using axi-symmetric models. 3-D threads get computationally very expensive. I believe I have seen good results with axi-symmetric models.
I also use non-linear material models.

I think that you are probably right about non-convergence of your results. If there is any doubt you could run another mesh size to confirm it.

Gurmeet

 

[rb1957]

you start your last post saying "I could get no convergence". i assume you have found some way to make the model run (note no references to the Rolling Stones).

as other posters have already said, you need to check the loads in these constraints to make sure that they are not significant.

you're doing an elaborate 3D FEA of a bolt thread (essentially). if this is a fatigue application then you're preloading the bolt. this is an incredibly significant part of the fatigue analysis and you need to appreciate the consequences of the joint gapping (or not).

whether or not you're testing the joint, you still need some assurance that the thing is going to work out as expected; so you ned to do some analysis. do you Need to do 3D FEA, possibly not; me personally i wouldn't rely on 3D FEA of a screw thread. if the structure is complex you may need some sort of FEA to show you the loadpaths, to understand the limit load on the thread. this sizes your bolt and the preload (in either order!).