Peak stress in solid FE models 5

[Struct71]

Hi all,

Does anyone have any guidelines or philosophies with respect to high peak stresses?

There are several guidelines to for design stress and maximum allowable stress for classic "manual" calculation methods, but I can't find anything for FEM/FEA maximum. How to deal with peak stresses?

Both as an engineer and as a checker I regularly find statements as

* "The high peak stresses should be ignored"
* "The maximum stress is local therefore allowable"
* "The hot-spots are negligible"
* "Due to the local nature of the high stress etc..."
* "Next to the red region there is a green region" (!!!)

As an engineer, this is not very satisfactory. Anybody else finds these situations? Is there a recognised guideline to handle peak stresses? How to evaluate them?

Hoping for a healthy discussion!

Regards,

 

[rb1957]

for myself, I'm ok with "ignoring" localised stress peaks ... tho' i don't think i'd use such wording in a report. i think i'd say that the peaks are acceptable as they are highly localised, and a results tof the linear elastic assumptions of the model. In reality such stress peaks would not occur due to localised yielding. these days i should really use NL codes but ...

 

[GBor]

There are various industry guidelines for handling highly localized stress. A few of them are:

>10% stress gradient across a single element (may need to refine local mesh and rerun analysis)

Peak stress in area of little or no interest (engineering judgement tells you that this isn't the load path, so poor FEA geometry is causing the problem).

peak stress across <10% of the local cross-section

Check with your particular industry. There should be a reason why the statements that you mentioned were made...

 

[crisb]

I usually find these occur because of poor details or poor modelling, and generally try to amend details to reduce these "hotpots".
If they persist a plastic analysis is usually very quick to run, and values of plastic strain will often be found to be very low.

eelco71...I agree with you and dont like the statements described, which are often made to avoid proper consideration of results.

 

[SWComposites]

The statements:

* "The high peak stresses should be ignored"
* "The maximum stress is local therefore allowable"
* "The hot-spots are negligible"
* "Due to the local nature of the high stress etc..."
* "Next to the red region there is a green region" (!!!)

without a detailed explanation show that the FE analyst has no clue what they are doing. And yes, these are all too common.

Evaluation of peak stresses depends on:
- material (not all exhibit plasticity)
- structure
- stress state at peak (tension, compression, combined, etc)
- loading type (static, cyclic, thermal, etc)
- application
- applicable codes and regulations

So there is no universal guide. Please provide more detail of the specific situation.

 

[corus]

Peak stresses aren't ignored, unless it's a particular aspect of your modelling that you're aware of such as a concentrated force or restraint in an area that you're not interested in.
Usually you consider the peak stresses for fatigue damage but if it's purely a static loading with no cyclic loading then you can ignore it. Refer to design standards such as those given in pressure vessel design codes, usually in the Design by Analysis sections, which give details of stress classification and their appropriate limits.

corus

 

[jte]

eelco-

If you're looking for a code or standard which provides some acceptance criteria for dealing with peak stresses in metal structures, I'd suggest you meander on over to your local pressure vessel engineering outfit (or tech library). Take a look at ASME Boiler and Pressure Vessel Code Section VIII Div. 2 Appendix 4 (pre 2007 ed). The 2007 ed (part 5) and its companion, API 579-1 / ASME FFS-1 (Annex B1) deal with nonlinear analyses better but are first edition with the customary errors associated withfirst editions. For what its worth, the 1968-2006 VIII-2 is more of an ASD philosophy while the 2007 version has jumped to a LRFD type approach.

jt

 

[Struct71]

Few reactions to the healthy discussion above and a wrap-up:

The statements mentioned are just as meaningful as just shouting that the analyst has no clue of what he is doing. It would be good if there could be a proper objective unambiguous way to justify these stresses.

In my experience there are several types of peak stresses:

* due to modelling in regions that you are truly not interested in. Those stresses can be ignored.
* due to modelling in regions where you want to know the stress. To get accurate stresses you should change your model by changing element type (eg quadratic volume elements) or changing mesh size
* truly occurring stresses, where changing the mesh size does not significantly change the result. Element results and average results are more or less similar.

I hope to constrain this discussion to the latter cases.

Classic allowable stress according to most codes is of order magnitude 60%-75% yield. Although I understand how to input plasticity and how to interpret the results, it does not solve the problem as plasticity only occurs around yield stress.

In case it wasn’t clear, material in my case is usually steel, could be S355 or A572 gr 50. Plastic properties are obtained using Ramberg Osgood. Application is not a pressure vessel.

To me it is clear that in some cases “high peak” stresses in “small local” regions cause no problem because of redistribution of stress due to plasticity. At the same time I realise that due to the undefined nature of “high peak” and “small local” this becomes very very slippery.

Anyone has any idea on how to define maximum values of “high peak” and “small local”?

Thanks!

 

[feajob]

Hi eelco71,

I usually use Neuber's Rule to transform the peak stresses of a Linear FEA. In other words, I return those points back to the real strain-stress curve by Neuber's Rule.

You can get more details by checking the following thread:
Linear Finite Element Analysis & Neuber’s Rule
thread727-210076

But, if I have enough time then I will go with Nonlinear FEA.

A.A.Y.

 

[gurmeet2003]

If we have expereince with the product and know the failure modes, some of the stresses could be neglected, with proper explanation. However if I have any doubt I go for non-linear analysis using abaqus. Run time is longer, but the if the model size is not large it is not a problem.

Before doing the non-linear analysis, I would debug the linear model.

Gurmeet

 

[Struct71]

feajob, gurmeet,

I have mastered the non-linear plasticity, it takes a bit longer to run, but that's OK.

If the peak stress in linear calculation was higher than yield, it will now be smaller but still higher than yield. Not surprising.

Now what? Is higher than yield now OK? Are the hot-spots now negligible because next to the red region there is a green region?

The statement by GBor is intresting peak stress less than 10% of the local cross section is a good definition of "local". Is there any reference?

What we need now is a good definition of "peak stress"...

 

[cbrn]

Hi,
eelco71, imho you should properly understand a pair of points:
1- why you run a plastic analysis in cases you find higher-than-elastic-yield stresses
2- what is the real meaning of a "local", a "secondary" and a "peak" stress.

Let's begin from the simplest of the two points:
2- even if you don't deal with pressure vessels, ASME B.P.V.C. VIII-2 App.4 / 5 (edition 2005 - I don't have the 2007 edition which, as it can be seen in another thread, has considerably changed) give very good indications / explanations on what and where you can consider local, secondary, peak. By the way: for an elastic linear analysis, ASME criteria allow for limits which are considerably higher than yield for "local primary + secondary stresses" (limit "Sps"), but in this case of course you are obliged to perform a fatigue analysis any time it is needed.

1- As for the plastic analysis... except if you already have exact knowledge of a case-figure exactly similar to the one you are analyzing, seeing a load redistribution will give you very little information "per se". First of all, if you really want to go in the "inelastic route", then congratulations, it's certainly the very best way to go, but it will be VERY time-consuming. In fact, you will have to check not only for plastic collapse (using a purely-plastic constitutive law), i.e. check that the redistributed stress can be held by the net section without "frankly" collapsing, but also for PROGRESSIVE collapse, i.e. if you have a variable load you must check that successive load / unload cycles won't make the plasticized zone grow indefinitely until the section will no longer be able to sustain the load itself. The check is now "in control of strain" instead of "in control of stress", since you will have to check that no point of the part has a total strain higher than a given limit (it depends on the Norm you use).
These things are well defined in the first code which explicitely allowed for the elasto-plastic "direct" analysis without stress categorization, i.e. EN-13445. As far as I know, the 2007 edition of ASME updates its methods to almost the same level of completeness.
Warning: depending on the field you work in, you may have VERY BIG problems to have your customers accept the "inelastic route"...

Regards

 

[Struct71]

Hi CBRN, Thank you for your helpfull post. You hit the core of the problem. I studied the ASME code you described, there it mentioned the acceptance of "peak stress" in "local" regions due to model discontinuities.

I could not find a numerical definition of "peak" and "local". The plastic calculation I perform is just to try to get a better grip on what is happening, I can switch it on or off in a blink. Wether the calculation is elastic or plastic, the evaluation still comes to the same thing. If higher than allowable stresses are acceptable over a small region of the model, then where is the limit?

The last (plastic) model I had had a maximum stress of 101% yield, with approximately 4% of the load bearing area above the allowable 75% yield. So yes, it is probably OK, but now I need to find a renown document to prove it...

At this point I cannot even convince my colleagues, let alone clients and - in case something happens - insurance.

Note that most of our items are for one temporary use only, no fatigue needs to be concidered.

Thanks,

 

[trainguy]

eelco71,

Your questions exactly echo my concerns about FEA. i.e. When is a hot-spot OK?

Maybe the answer is to do some hand calcs for certain regions, to convince yourself or your clients that things are probably OK.

I've heard some very experienced FE people dismiss many peak stresses when they were near a load or other stiff boundary condition. Usually, these people have extensive testing experience to corroborate this.

One thing I have also seen, was (very qualified) people extracting nodal forces from the FE then performing a hand calc (such as My/I) to determine local stresses.

More often than not, in my industry, the controlling failure mechanism is buckling, which is not even captured by linear static FEA, thereby requiring still more hand calcs.

tg

 

[cbrn]

Hi,
ASME code has a way to guide you in order to reckon if a stress can be treated as "local": the main dimension of the area where the stress is 10% higher than the "general" limit should not extend more than SQRT(R*t) and two successive "local" regions can not be closer than 2.5*SQRT(R*t). It's in ASME VIII-2 App.4, 4.112 (i).

Regards

 

[gurmeet2003]

eelco71

In my opinion here is how the non-linear analysis helps. If you see high local stresses more than yield. After the non-linar analysis one has a more realistic picture of stresses and also the extent of high stress zone. In your question you mentioned that you are talking about static loads and fatigue is not involved.

Once we rule out fatigue, the failure mode is yielding through the section. ASME code is a very good document if you are involved with pressure vessel design. However if you are designing products other than pressure vessels, which also look very different, I do not think it is necesary to go back to ASME code after the non-linear analysis.

Stress concentrations are sudden changes in geometry, such as corners, fillets, holes or steps etc. If the gross stresses are much below yield, the high stress zone would be confinded to a small neighbourhood near the stress concentration. The word 'small' is compared to the geometry of the part; thickness, diamter etc. (a 10%) figure sounds pretty reasonable.

If there is still some doubt remaining, one could calculate the limit load for your part. I usually consider that load as the limit load, which causes yielding through the thickness.

I would avoid putting one stress concentration on the top of the other; a hole on fillet.

Gurmeet

 

[corus]

A paper by R.Seshadri (

http://cat.inist.fr/?aModele=afficheN&cpsidt=16873436)

gives a method for determining the acceptability of hot spots by caclulating remaining strength factors. Although the method is for hot 'hot spots', ie. those caused by temperature, the method assesses not only the stress but also the extent of the 'local' hot spot and its acceptibility. This could be extended to hot spots as defined by geometric stress concentrations. This would then give you an assessment based upon not only the value of stress, but also the size of the region. It's a 'Level 2' assessment, ie. a hand calculation method, but it could probably be extended to results from a linear FE model where the full non-linear elastic-plastic 'Level 3' capabilities weren't available. There's probably a thesis there for anyone wishing to take it up.

corus

 

[Struct71]

CBRN, thanks again,

if you do the math with max dimension of stressed region of sqrt(Rt) (and assume it is circular) and the cross sectional area of pipes it turns out that the region could be maximum 1/8 = 12.5% of total area. Intresting, now this could be applied to any area.

Few more issues with this definition:

1:
the code states that the region is a peak stress only when it is 110% of allowable stress. So how about stresses between 100% and 110%?? This stress is higher than allowable, but it is not classified as peak stress.

2:
Is there any limit to the height of the peak stress? even if the region is smaller than the sqrt(Rt)=12.5% I would expect that there would also be a maximum peak stress.

3:
How about when the area is loaded with bending moments as well as axial forces? Peak stresses (due to geometrical discontinuities) will occur at the outer fibres (My/I, but then including stress concentrations)

Calculating the limit load as Gurmeet suggested could be intresting. Just investigating when the entire section is yielding.


I know, this is getting complicated, that is why I feel FEM together with correct interpretation should provide a solid answer.

Thanks all,

 

[cbrn]

Hi,
1- there is a little confusion. In the chapter I mentioned, ASME code is talking about LOCAL, not peak stresses. It means that, when you see a region where the stress intensity is higher than the "primary general stress" limit, you can compare it to a higher (1.5 times higher if no secondary effects are involved) limit, provided that you verify that this "high-stress" zone effectively has the characteristics to be considered "local", i.e. the "SQRT(R*t) for over-110%" criterion. If it doesn't respect that, i.e. if it extends more, then for safety's sake you must consider it "general" stress (not local any more) and so consider the verification failed. Consider the hot-spot stress you have, and "draw" (physically or ideally) two markers at 0.5*SQRT(R*t) from the hot-spot. Now "draw" two other markers where the stress begins to be higher than 110% of the "primary general" limit. Are these two last markers inside the first ones? If yes, the region IS a local stress; if not, bad luck, you have to consider it failed for the primary general stress criterion. IF it is LOCAL, THEN the hot-spot stress must be lower than the "primary local" stress limit, i.e. 1.5 times the primary general.
If you are in a zone where secondary effects arise, then the limit is higher again. Secondary stresses are self-limiting, i.e. they will tend to be "confined" by what happens around. In other terms, they will never be the direct cause of a frank failure of the section where they happen. In order to know that, ASME gives some examples. Other ways to reckon a secondary stress zone is... experience. Another way is the plastic analysis, especially in your case where, as far as I understand, the load will be applied only ONCE and then never removed-and-reapplied again.
So, in YOUR SPECIFIC case, most probably the plastic check against direct collapse is a sufficient verification. You will have to input a "pure-plastic" constitutive law if you want to be safe, as stated by EN-13445.
2- No, not with purely-linear-elastic constitutive laws. You will have to ensure that you can not initiate a damage (crack propagation theory) if you have a traction stress. However, if the peak stress gets too high, most probably you will see a "more-basic" criterion fail BEFORE (primary general, or primary local. If the hot-spot is extremely high (even higher than ultimate stress) but ALL other criteria are respected in the same time, then 99% probably the hot-spot is not "true", i.e. it is a numerical artifact.
Due to the fact you can do it with little expense, in this case a pure-plastic analysis is a good verification.
3- I don't see a conceptual difference in this case.

I'd add: if you run a plastic analysis, the determination of the limit load is easy: it's the lowest load for which the solution doesn't converge any more (be careful to be somewhat restrictive in the convergence criteria, or it will take very long !!!)

Regards

 

[chaboche]

Hello,

I have experienced a similar problem recently. A static stress assessment of a steel structure calculated a stress concentration where several members are joined together. I originally modelled the structure with shells, but had to build a solid submodel to find the results in more detail. The results are shown in the attachment below.

As can be seen, there is a stress concentration at the fillet radius. The yield is 355MPa, and the results indicate the maximum stress concentration is ~550MPa. I do not believe that the entire section will yield, due to the support offered by the surrounding structure. The problem is, how much support is offered by the surrounding structure, and therefore when does the stress concentration turn unacceptable?



I also have past experience with ASME III DBA, and have performed non-linear plastic analysis. A limit load assessment using linear-perfectly plastic properties can be used to gradually increase the load until convergence does not occur.

A full non-linear plastic shakedown analysis of a component requires that the number of loadings above 1.5Sm are known. The model is subject to repetitive cycles of the intended loadings, and the strain is calcualated. This is then compared against the ASME limit below:

According to ASME III, Subsection NB-3228.4:

The limits on thermal stress ratchet in shell (NB3222.5) and progressive distortion of non-integral connections (NB-3227.3) need not be satisfied at a specific location, if, at the location, the procedures of (a) through (c) below are used.

(a) In evaluating stresses for comparison with the remaining stress limits, the stresses shall be calculated on an elastic basis.
(b) In lieu of satisfying the specific requirements of NB-3221.2, NB-3222.2, NB 3222.5 and NB-3227.3 at a specific location, the structural action shall be calculated on a plastic basis, and the design shall be considered to be acceptable if shakedown occurs (as opposed to continuing deformation). However, this shakedown requirement need not be satisfied for materials having a minimum specified yield strength to specified minimum ultimate strength ratio of less than 0.70 provided the maximum accumulated local strain at any point, as a result of cyclic operation to which plastic analysis is applied, does not exceed 5.0%. In all cases, the deformation which occurs shall not exceed the specified limits.
(c) In evaluating stresses for comparison with fatigue allowables, the numerically maximum principal total strain range shall be multiplied by one-half the modulus of elasticity of the material (Section II, Part D, Subpart 2, Tables TM) at the mean value of the temperature of the cycle.


I have long sought where the 5% strain value comes from, and also as to what type of strain it refers. I believe it to be a 'membrane' strain though the section, as this section guards against progressive plastic collapse.




Incidentally, you can also perform a fatigue assessment using the results of the non-linear assessment, to remove conservatism.


I don't want to perform a full non-linear shakedown analysis for this static asssessment since it takes a long time/would have difficulty defining the inteded loads over the lifetime. I'm also not sure if I should mix rules from a pressure vessel code with a strutural design code.

What would be useful would be some guideline for when a stress concentration in a load bearing memeber becomes a mode of failure. Any suggestions?