mesh convergence with stress concentration

[ygsygs]

Hello Everyone,

I am currently working on a linear static FEA with stress concentrations. I have not refined the mesh on the stress concentrations. The average stress in another region/surface without the stress concentration from 2mm-9mm mesh size has shown consistent output of about 30MPa, so i know the mesh setup has converged except on the stress concentration (represented by the max stress) which is showing a different behaviour. Trying to understand this behaviour.

My point of view is that, from 2mm - 5mm, the stress concentration is starting to be more pronounced and is growing exponentially in the results,
while from 5mm - 7mm, i believe this is a region where the stress concentration is not growing exponentially yet ( I can use results from this region),
while at 8mm and 9mm, (details below), I am not sure how to explain it.

Not included in this attaachment is: [mesh size(mm), max stress(Mpa)], [8,15713],[9,14552] which are way off.

Am I interpreting the results properly? What are your thoughts on the results?

 

[GregLocock]

I think you are chasing a never ending refinement, if you stick with a linear material model.

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[rb1957]

i cannot follow your explaination of the stress results. however, if you're trying to FEA a stress concentration with a linear model, it is a "fool's errand"; a linear model will predict a stress over yield.

if your stress concentration is a standard form, then i'd use a coarse mesh and a handbook solution for Kt.

if i did it with FEA i'd use the nodal stress and a fine mesh.

another day in paradise, or is paradise one day closer ?

 

[ygsygs]

thank you all for your replies,

I guess using a linear material model to assess a component with a stress concentration can only be used to identify the stress concentrations or give an idea of how the component behaves under the loads and boundary conditions its been placed on.
or like what rb1957 says, if the stress concentration is standard, and only linear FEA is available, can use a coarse mesh and handbook the stress concentration.

I have tried using a nonlinear material model before on another component, which allows plastic deformations, however, I face the same issues with the stress concentration where the max stress starts to exponentially increase as the mesh size reduces. I have attached the stress vs. mesh size as an illustration. Did you guys go through similar challenges? Could it be I am doing something wrongly?

This would mean using max stress is not the way forward when handling stress concentrations to justify a covergence even if it was a nonlinear material model ? Because through analytical means or considering other sections without a stress concentration on the model, the stresses seem to be stable and can be cross-checked.

So there needs to be a cutoff point if one would want to use the output from the FEA model?, like in this case it would be an 8mm mesh, right before the stress starts to grow exponentially?

Quite curious how guys in places where stress concentrations are more critical, like the aerospace industry, go about with their stress concentrations. I dont have exposure to the aerospace industry, so I wonder if aerospace design standards has addressed stress concentrations when it is not related to fatique. If you are to place a finer mesh in the stress concentrations region, you would just get a higher stress at that place.

 

[corus]

Stresses at a geometric stress concentration will converge. I suspect your stress concentration effect is due to a point load or restraint, or perhaps a right angled corner where the fillet radius is zero and the stress concentration factor is infinite. Perhaps a picture of your results at this stress concentration would help.

 

[rb1957]

what stress are you showing us ? element average ? nodal ??

have you considered using fatigue analysis codes, like ncode ?

a pic of the model would be nice.

as corus has posted ... is this at a point load, or a fastener ? is it a model "artifice" or real geometry ??

another day in paradise, or is paradise one day closer ?

 

[ygsygs]

corus :

just to clarify myself, geometric stress concentration are the ones as in handbooks, exp: a rectangular block with a hole in the center?
could you elaborate what you mean by a point load and restraint causing a stress concentration? any examples to illustrate?

the picture in my 2nd post is the stress at where the the stress concentration is at. it is where the max stress is also at.

rb1957 :

the stress i am showing is nodal. if it was the element average, would it change the convergence behaviour of the model?

not necessary for me to consider fatique because the model is only to see a particular static loading. but that's cool, didnt know there is a softwares like ncode specializing in crack growth, lifespan etc.

i can't really show the model, but a snapshot of where the stress concentration is coming from is as attached.
in this case, the snapshot appears like a standard hole, but i struggled to match it with any of the cases in the handbook.
there were many reasons,the feature(notch or hole,because stress concentration appeared as a notch), the loadings, the comparing dimension, geometry ( there is a flap of material on the upper side of the hole) etc. it would be clear if i could show the whole model but unfortunately thats not possible.

 

[rb1957]

you really have the counterbore breaking the edge ?

nodal stresses are correct if you're trying to see the Kt.

if you're interested in a static load, running a linear model into the root of a Kt is pointless (as the linear model will predict a ficticious stress). the material at the root of the notch will yield, without affecting the performance of the structure ... unless the yielding becomes massive in comparsion to the size of the part, which would be evident without a super-small mesh.

another day in paradise, or is paradise one day closer ?

 

[corus]

The picture doesn't show the stresses, only the geometry. Each of the bore holes has a 90 degree corner though, where as I said above, the stress concentration factor would be infinite. If the maximum stress was at the inner radius of the hole then it would be a different matter. However, as you're not concerned about fatigue and the stress concentration would contribute to a peak stress component, then there's little need to find out exactly what that stress is.

 

[ygsygs]

thanks all for your replies, getting more clarity out of these discussions.

rb1957 :

yes there is a counterbore breaking the edge

this model is different from the first stress figure we were discussing about, i used a nonlinear model for this. agree that linear model for this is not the way forward.

corus :

i have attached the picture of the stress, its red at the edges. youre right that the max stress is at those 90 degree edges. so its infinite.


why i would like to know the exact stress at that point?

the acceptance criteria for a elastic-plastic simulation in ASME BPVC Div 2 only permits a certain amount of plastic strain on the model.
so, if the stress is infinite on a portion, like the example above, would that mean its plastic strain is infinite as well? and cant meet the criteria?

alternatively would that mean i should just take a suitable cut off point from the results and move on ?

any of you came across any research done regarding infinite stress concentrations and material performance/integrity?

 

[csk62]

Why are you looking for a stress in an area of infinite stress?
As many have pointed out before, it is ridiculous to extract stresses in the immediate vicinity of certain boundary conditions, applied point loads, and geometries which produce infinite notch factors.

 

[jhardy1]

Any discontinuity in load, restraint or geometry will tend to produce an indefinite stress (i.e. tending to infinity as you refine the mesh in a linear elastic analysis).

Think about it:

The contact stress under a point load (or point support) is the result of a finite load over an infinitesimal area; that is, infinite stress.

If you have a sharp re-entrant corner which the stress / strain field has to "flow" around, the stress has to deviate through 90 degrees in an infinitesimal distance, and must therefore mathematically be infinite at the point of the corner.

Refining your mesh in these scenarios will only take you closer and closer to the theoretical solution of infinite stress!

In the real world, there are no "point loads" or supports (they all have finite area), there are no "sharp corners" (they all have some finite radius at some microscopic scale, and the micro-structure of the material means the assumption of isotropy is invalid when you get down to a small enough scale), and there are no linearly-elastic materials (they all show some sort of non-linearity when the stress gets high enough).

You need to accept the limitations of linear elastic analysis of isotropic materials with idealised (simplified) geometry, and apply other methods to resolve the peak stresses (e.g. classical solutions for stress raisers), or else you can try much more sophisticated modelling techniques to resolve the singularities and non-linearities, but this approach is rarely employed in global FEA models.

http://julianh72.blogspot.com

 

[rb1957]

"yes there is a counterbore breaking the edge" ... well, there's your first problem ... refine the transition (so you don't have that sharp point of "nothingness").

"its red at the edges. youre right that the max stress is at those 90 degree edges." ... your second problem ... how are you going to make a sharp corner (at the edge of the counterbore) without a fillet rad ? and if you removed the fillet rad to simplify the model ... well, that'd be your third problem.

"a certain amount of plastic strain" ... if you're running a linear model, your 4th problem ... how would you work from an elastically calculated stress beyond yield to an amount of plastic strain ? if you're running a non-linear model, then it'll work things out for you ??

finally, i think we're dealing with highly localised yielding that won't affect the performance of the structure. we're only seeing these stresses in calculations today 'cause it's easy to run FEA with very fine meshes.




another day in paradise, or is paradise one day closer ?

 

[corus]

I'm no expert on ASME codes, however their design criteria are similar to other pressure vessel codes. In that respect I'm surprised they consider the plastic strain in a static analysis as stresses are limited to within yield stress, or in the case of secondary stresses to twice yield but again based upon an elastic analysis. I suspect plastic strain only refers to fatigue assessment and as such wouldn't be of concern as yours is a static analysis. As I said before, the stresses are at a stress concentration and as such are classed as a peak stress component and would only be of concern in a fatigue assessment. As such they wouldn't come into your assessment.

 

[ygsygs]

csk62 & jhardy1 :

guys i understand what you guys mean, it was pointed out by rb1957 & corus. thank you for further emphasis regarding the matter. i was trying to introduce a new facet to the thread. i should reword the statement,

"why i would like to know the exact stress at that point?" to "why before i tried to know the exact stress in that region?",

i am not searching for the stress now, i have used a cut off point( not sure if it was the right thing to do, but it seems, it is an infinte stress area and is a tiny region after all. should not affect the overall performance of the component) and moved on, just following up on some knowledge gap i had during that time regarding stress concentrations.


rb1957 :

refine the transition (so you don't have that sharp point of "nothingness") --> yes, means i transition the mesh so that i get more curvature?

your second problem ... how are you going to make a sharp corner (at the edge of the counterbore) without a fillet rad ? and if you removed the fillet rad to simplify the model ... well, that'd be your third problem. --> if i could show the entire component, it would show how, a half circle of the counterbore started earlier on an extruded material, later the other half came in on the main body, therefore it appears as such, btw not the design engineer who worked on it)

if you're running a non-linear model, then it'll work things out for you ?? --> agree linear not going to solve it, i dont think nonlinear can solve it too, because the stress there is infinite, but elastic-plastic is there to try to meet the standard's criteria regarding plastic strain.

finally, i think we're dealing with highly localised yielding that won't affect the performance of the structure. we're only seeing these stresses in calculations today 'cause it's easy to run FEA with very fine meshes. --> agreed

Corus :

sorry corus just checked, it was an ISO standard which referred to ASME's elastic-plastic method. the ISO standard is the one which gives a criteria for the local plastic strain to be less than a certain percentage. (cant remember what ASME BPVC says about this, i think you're right, it only comes in during fatique, however i remember reading something about 'protection against plastic collapse' when using elastic-plastic analysis in BPVC's part 5 : design by analysis ). i dont really have expertise in these standards to clear this out, i need to re-read part 5 again. best leave it for now for someone with expertise to comment on this. if i find something, i will post it out.

thanks guys for your contributions, got a clearer picture of stress concentrations, FEA and where to dig on next. feel free to add on suitable things to the the thread regarding stress concentrations. as for now,new year's coming. =) hohoho and merry christmas.

 

[csk62]

Regarding the acceptable level of plastic strain in a given design, I have seen some in house standards for steels (non ASME) which state that the plastic equiv. strain will be less than half the strain at rupture for a uniaxial test. It is also multiplied by certain correction factors.

This plastic equiv strain is analagous to the formulation of von Mises stress, however I think that it must take into account that the poisson ratio changes in certain directions with relation to the yield surface, as the part plastifies.

This was for a simple quasi-static analysis; no fatigue considerations, strain-hardening, or load ratcheting effects. Just an example that I remembered.

 

[corus]

csk62, that test sounds suspiciously like the criteria for 'infinite' fatigue life but I've seen it as limiting the stress to approximately half the UTS value and the correction factors are for surface finish, size, etc. Quasi static may refer to stresses from shafts in bending where dynamic effects are negligible and an infinite fatigue life is required using results from a static analysis.

 

[rb1957]

you've noticably side-stepped my "1st problem" ... ie the counterbore cutting though the edge, leaving a sharp point. maybe this is part of your problem, maybe it isn't, but it is bad design.

do the counterbores have sharp corners or fillets ? it is veryquite difficult to machine a sharp 90deg corner, and noramlly there'd be some fillet radius (which it looks like you don't have in your model). if you deleted the fillets to simplify the model ... don't !

a non-linear model will not predict an infinite stress at the root of the notch, because a non-linear is smart enough to realise that the the maximum stress in a part is ftu. a linear model is dumb, in that it'll extrapolate stresses beyond yield (and ftu).

i'm not sure what your "cut-off" stress means in a linear model. and i really didn't "get" your reworded problem statement ?



another day in paradise, or is paradise one day closer ?

 

[tbuelna]

Based on the local geometry around the counterbored holes and the global element size/SAG properties used for the model mesh, you would expect to see significant local stress concentrations. You can either ignore them or you can refine the mesh around each of the counterbored hole locations.

 

[stressebookllc]

Clearly fatigue is not an issue for you, if it were, then this probably would be a nightmare to deal with for fatigue life. The design has to change in my opinion.

If the design cannot change, As far as statics is concerned, then as you refine the mesh around the edges of the hole and the fillet, the concentration will get worse and worse.

But this is not necessarily a bad thing. You can demonstrate that the high stress concentration area gets smaller and smaller with mesh refinement and you could consider the stresses an element or two away as more realistic. If you can indeed run an elasto-plastic material, then you will see there will be some plastic strain there. But the difference in the overall part deformation will show whether that plastic deformation is too much or acceptable. Especially for ductile materials (steel), it should be OK if the plastic strain there is less than a few percent. Because they are 'tough' meaning they can take load beyond yield and still not fail or fall apart on you depending on how much more load you apply.

http://www.stressebook.com

Stressing Stresslessly!