×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

mesh convergence with stress concentration

mesh convergence with stress concentration

mesh convergence with stress concentration

(OP)
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?

RE: mesh convergence with stress concentration

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 ?

RE: mesh convergence with stress concentration

(OP)
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.

RE: mesh convergence with stress concentration

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.

RE: mesh convergence with stress concentration

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 ?

RE: mesh convergence with stress concentration

(OP)
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.





RE: mesh convergence with stress concentration

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 ?

RE: mesh convergence with stress concentration

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.

RE: mesh convergence with stress concentration

(OP)
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?

RE: mesh convergence with stress concentration

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.

RE: mesh convergence with stress concentration

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

RE: mesh convergence with stress concentration

"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 ?

RE: mesh convergence with stress concentration

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.

RE: mesh convergence with stress concentration

(OP)
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.

RE: mesh convergence with stress concentration

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.

RE: mesh convergence with stress concentration

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.

RE: mesh convergence with stress concentration

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 ?

RE: mesh convergence with stress concentration

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.

RE: mesh convergence with stress concentration

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.

www.stressebook.com
Stressing Stresslessly!

RE: mesh convergence with stress concentration

(OP)
rb1957 :

yes bad design to have the 90 degrees, and i definitely didnt take out a fillet out of there, the fillet is still there actually. its the way it was manufactured to have that 90 degrees effect. cant manufacture it directly but it can be a byproduct of the manufacturing process? an example of this area is : if you joined 2 rods of different diameters together with a circular weld, at this contact point if you put a small hole through it in such a way that each half of that hole is evenly on each ends of the rod, the center of this hole is at the circular weld. i think then you can have an infinite stress point at this area, because of the hole radius moving in all 3 dimensions, like a helix? well thats what the linear model seems to suggest. <-- hope this is clearer.

i cant really do anything much with the design. can only suggest, im not the product owner.

"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)."
<--> understand. so elastic-plastic will show a non-convergence if the stress exceeds the ultimate tensile

"i'm not sure what your "cut-off" stress means in a linear model. and i really didn't "get" your reworded problem statement"
<--> when doing the linear modelling, i came across a trend as i refined the mesh: as i reduce the mesh, the max stress, initially converged, then about 3 or 4 refinements more it stayed about 5% difference from this converged value, i refined further, then it started to behave exponentially. so i took this converged zone as a "cut-off point" for my elastic-plastic analysis. not sure if this is ok but probably what i was doing was something similar to what stressebookllc says, i was taking an element or 2 away from the elements responsible for the infinite stress. but not sure if i can take a linear conclusion ( the stable/converged zone mesh size) and apply that mesh size to the plastic analysis. what do you think, generally the stress pattern would be the same on the component?


csk62 :

i think when defining the material property, the possion ratio is usually inserted in , so the iterations should be considering the possions ration effect? or would that be another setting in the modelling which needs to be activated?


stressebookllc :

"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"
<--> useful tips, thanks.



RE: mesh convergence with stress concentration

"yes bad design to have the 90 degrees, and i definitely didnt take out a fillet out of there, the fillet is still there actually. its the way it was manufactured to have that 90 degrees effect. cant manufacture it directly but it can be a byproduct of the manufacturing process?" ... this is very confusing ...
1) is there a fillet rad in the real part ?
2) is there a fillet rad in your model ?

"i think then you can have an infinite stress point at this area," ... no, you can never Ever have an infinite stress; stress is finitely bound, a real number that can never be infinite. now the FEM might think it's infinite, 'cause FEM can be stupid. in a linear FEM, any stress above yield is fiction.

"so elastic-plastic will show a non-convergence if the stress exceeds the ultimate tensile" ... no, if the part is going to fail non-linear will tell you this 'cause it won't be able to apply 100% of the load. NL applies the load in increments, and if the last increment tried fails, then is says "oh, well; this is the last increment that worked ...".

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

RE: mesh convergence with stress concentration

ygsygs,

I too struggle from time to time with stress peaks above yield in linear models. It's probably self evident, but one should keep in mind that even if the FEA results can't be trusted at/near singularities (point load/constraints, reentrant corners), the stresses are high at those locations, and it is not good engineering practice to put features with sharp corners etc. in loaded areas of your design.

ASME provides the possibility to use linearized stress results, but I do not have enough experience/knowledge to say if the ASME methodology can be used for dimensioning in a general case. Neither have I seen/understood the justification for ASME's method.

IIW (international institute of welding) have developed techniques to handle hot spots at welds. These techniques are largely based on testing, are relatively easy to use but they are not always applicable in a more general case.

/Mats Lindqvist

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources