In solid elements, linearization is done across the thickness to get the membrane stress (avg stress, wch is a horizontal line), bending stress (linear), and peak stress (the left over in the curve). But shell elements give the stresses only at the mid surface . Stresses are assumed to be linear through the thickness. Thus the peak stresses are neglected when shell elements are used. But total stress = membrane stress + bending stress + peak stress + secondary stresses(due to thermal...).

I don't understand your question : what do you mean by "peak stresses" ? In FEM, you obtain stresses at integration points, and then various extrapolation methods can give you stress at nodes. This is true for static as well as dynamic analyses ...

So you can compute "peak stresses on the element" (max value on the element, depending on the extrapolation method), and "peak stresses during the time history" (max value during the loading cycle). I use fatigue analysis daily with shell elements, and really do not understand where your problem lies ...

It would if you defined what you mean by "peak stresses".

Are you referring to stress variation along the thickness?

You should have a look at DNV RP 203 standard. They are freely available on the internet. You'll find there a detailed description of the procedure to determine the Hot Spot Stress, summarizing you should use an element size less then the shell thickness.

In solid elements, linearization is done across the thickness to get the membrane stress (avg stress, wch is a horizontal line), bending stress (linear), and peak stress (the left over in the curve). But shell elements give the stresses only at the mid surface . Stresses are assumed to be linear through the thickness. Thus the peak stresses are neglected when shell elements are used. But total stress = membrane stress + bending stress + peak stress + secondary stresses(due to thermal...).

I'm sorry but I still don't understand what you mean by peak stresses.

Membrane stress and bending stress are available for shell elements. So you can have (at least in the FE codes I know - Nastran, Abaqus, Pamcrash) stresses on the top and bottom surfaces, and not only on the mid surface.

Which software are you using ?

BTW, you can also have non-linear material behaviour via through the thickness integration ("section points" in Abaqus). But it is usually less useful for fatigue analysis, at least in an S-N approach.

Taking residual (secondary) stresses into account is of course another challenge, which implies coupled analyses.

You are right Rosy according to API, ASME or ISO-13628-7standards you get a stress classification at concentrated stifness variation (due to linearization)

a) Membrane

b) Mem+Bend

c) Mem+Bend+Peack

and with a shell model you cannot get the "peak stress" across the shell thickness but you can get the "peak stress" induced by an in plane geometric variation in your structure (see DNV)

So if in your structure the geometric changes are localized in a thichness sharp change (as in an axisymmetric structure) you "shoudn't" use shell element, you should use solid element. API report an example of use of ANSYS in doing such calculations.

Ján Kudlovský- peak stress it is very important fo calculation for example low cycle fatique and so on. . They are stresses at discontinuties.

An excellent tool for getting the stresses through the thickness is VAPAS. See http://www.neng.usu.edu/mae/faculty/wenbin/ht_docs/vapas.html.

Dear Rosy reading again your question usually for fatigue calculation you need "to extrapolate" from your results the stresses at the weld toe.

Many standards give guidelines about how to extrapolate the whole stress (Mem+Ben+Peak) according to the FEM mesh results that can be from both SHELL or SOLID lements.

For this reason probably the answer could be more effective if we refere to a specific geometry instead of a very "general" configuration

Rosy,

By default the shell elements stresses are never displayed for midsurface. Depending on the program, it's reported for top, or bottom, or maximum of them.

If your stress is a result of step change in thickness, in shell model pay attention for averaging of stresses between different thickness areas (can be on/off, various algorithms of averaging). It can have great influence on the result values.

Most of the shell elements (thick or thin) are based on the Reissner-Mindlin postulates, which assume that a plane transverse section remain plane during loading. An obvious implication of it is that only bending stresses and membrane stresses will be calculated. An extensive treatment of such elements is given in the book- FEM (Vol II) Zienkiewicz and Taylor. It is also well accepted that the shell elements will not give stresses correctly at discontinuities, such as corners, sudden change in section or notch, which are vital for fatigue analysis. To evaluate the total stresses at such locations full solid elements should be used with sufficient subdivisions along thickness. This will place huge demand on computational resources. A mix of solid elements (in locations of discontinuity) and shell elements elsewhere could be used if the particular software being used permits this. This total stress will be the sum of membrane, bending and peak (due to discontinuity) stresses. Such analysis using mixed elements is quite common. For better results second order solid elements 27 node cuboid , 10 node tetrahedron will be more suitable as solid elements.

In shell element the stress just get distributed all along..simila as in surface tension in liquid bubble, no peeking in stress it just expodes

There are bridging techniques to couple shell and 3D elements like Arlequin method (H. Ben Dhia, G. Rateau, The Arlequin method as a flexible engineering design tool, International Journal for Numerical Methods in Engineering 62

(2005) 1442–1462.). Unfortunately there are not available in commercial codes (perhaps in Code ASTER that is free)

It is very funny to read "......UNFORTUNATELY (capital letters mine) there are not available in commercial codes (perhaps in Code ASTER that is free)...".

I shall say "..fortunately from the point of view of the science the method is available under the form of Software in a code distributed under the GPL licence"

The bridging technique can be replaced by so called submodelling.

Area of interest in the shell model is substituted by detailed local solid model.

The displacement field on the boundary of the area of interest is automatically transferred from the solved shell model to the new, local, solid submodel (as a boundary conditions). Calculation of stress field in the solid submodel gives us all details of stress field, including peak stress.

This method is fortunately/unfortunatelly (select what is your favorite one :) ) available in commercial codes like ABAQUS or ANSYS.

Hello,

currently I'm working on a method for analysing welded structures with the help of FEM, Patran/Nastran (v2012). The structure I'm analysing is a T-piece with a double sided fillet-weld, modelled by QUAD4-shell elements. In the pre-processing, I've considered all requirements which are in official documents: like the edge-length of the elements with 0.5*t (t=thickness) and the thickness of the inclined lines with t. ( http://web.mscsoftware.com/patran/current/html_patran/Fatigue%20Theory%20Guide/images/DTG-081.png ) The inclined lines are made to model the fillet weld.

My approach is to estimate the so called "hot spot stress" for fatigue analysis but unfortunately, there is no non-linear stress increasing of the nominal stress near the weld! The only change of the stress is in the last element, in front of the weld root. The stress should look like this: http://ars.els-cdn.com/content/image/1-s2.0-S1350630798000259-gr2.gif but like I've mentioned, the nominal stress is constant unti the weld root. A refining of the mesh didn't work either. Does anyone of you has some advices why the notch effect does not appear in my calculations? Thank you.

(Some screenshots can be seen in the attached pdf-file)

Here is the file, sorry for the double post.

Your vertical shell seems to be not loaded. this method is intended to find actual stress in complex stress field. For simple tension, there will be no stress concentration, because vertical and oblique elements are not carry out the load at all - this is a reason for lack of stress changes.

Try to add some bending load on vertical element, you will see that stress will change in the neighborhood of the weld.

Thank you for your reply. Well, actually you are right, there is no stress increasing near the weld toe when only normal stress (tension) is applied. I've checked it also with a solid model with atleast 3 elements along the thickness. The non-linear stress increasing appears only, when bending is introduced.

Dear Mustafa,

I analyzed the same joint geometry in a degree thesis of one of my students. We obtained similar results as you (no stress raising effect). The reason is that this type of joint is not very appropriate to check the "hot spot" approach. In fact, the "hot spot" approach captures the stess increase only due to global joint geometry (i.e. weld bead geometry excluded). Your joint has not macro-stiffening effect. Only a small stiffening effect is present due to the lateral poisson contraction that is blocked by the welded attachement (this effect, however, is of second order and then negligible).

This joint would give good results with a plane 2D model with the weld bead modelled explicitly. For shell elements, try for example to study a joint with longitudinal non-load carrying attachment. You will find the stress increase, as expected.

Best regards

Denis

Hello Denis,

thank you for your very usefull hints. Could you please describe the 2D-joint more detailed? :) I don't understand how to deal with the non-load carrying attachment...

Is it possible to get access to the thesis you've analyzed? If yes, it is in english? :)

Best regards,

Mustafa

Dear Mustafa,

enclosed please find two documents that describe the 2D-FE modeling of welded joints for hot-spot calculation. You can find further guidelines to reports by the IIW - International Institute of Welding (look for documents by Dr. E. Niemi).

Unfortunately, the thesis is in italian.

Best regards

This the second...

Hello Denis,

thank you very much for your answer and sorry for the late reply. I will go through the papers as soon as possible.

Best regards