The methods for dealing with stress singularities are:
- add fillet
- include plasticity
- ignore it and read results from different location
In this case you considered all these approaches. But keep in mind that the analysis with plasticity included is not unrealistic as in real life notches like that will also cause large stress concentrations and local yielding. But usually this yielding is limited to really small area and doesn’t indicate failure.

There are also special methods for weld assessment designed to bypass stress singularities. These approaches include hot-spot stress method and structural stress method. They are very useful when determining fatigue life of the weld.

FEA way, thanks for your reply.

Perhaps i was not clear enough, but what i mean is that according to paragraph 5.3.3.1 (see image) the local failure criteria must be met for all points in the model, this includes de weld edges.



Since the plastic strains near the edge are too high, this criterion will never be met there.

if you model the weld as a chamfer with linear material, then yes you'll see an "issue". the quotes are there 'cause it isn't a real issue, but we won't tilt that windmill today.

if you model the weld as a (circular) fillet (rad) then even with linear material I doubt you'll see an "issue".

if you model with non-linear material and a chamfer then you'll see highly localised yielding at the weld transition (kink).

"at every point" is something that'd be written in a textbook. "at every significant point" is more real, but opens the discussion to "what's significant ?"

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

You can find the answers to your questions in this paper: https://asmedigitalcollection.asme.org/PVP/proceed...

TGS4 as i can see from the abstract, that paper talks about how to compute the strain limit in the nodes being that the finite element results are given at the gauss points. but my question has to do with the singularities that arise from modeling welds with sharp edges.

if you want to look at that detail (the very edge of the weld, then why model it in a manner that'll give the worst possible result ?

Would you model as a weld sitting on top of the plate, 2 solid elements ... a brick and a wedge, or would the weld material be essentially part of the plate, 1 solid element ... a tapering brick ?

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

fem.fan - trust me, it's the same issue.

Plus, at your "singularity" point, one of the principal stresses is zero, so your triaxiality is low.

How are you calculating your limiting plastic stain, or better yet, how are you calculating your SLDR (strain limit damage ratio)?

TGS4 - i am defining a "user defined result" in ansys with the formula provided by the code (i uploaded an image in a previous post). The program calculates the SLDR at each gauss point. Then i can extrapolate the results to the nodes.
i´m not sure if this answers your question

At least you are following a preferred method.

From the paper:

Quote:

Conclusions
A mesh that appears to be sufficiently converged for both stresses and strains may not necessarily be so for SLDR. In general, a much higher mesh density is required for determining SLDR. This effect may be even more pronounced around discontinuities.

However, provided that the mesh density was sufficiently high, the Ductile Damage Material Property and Calculate at the Gauss Points and Extrapolate methods produced similar results. The Calculate at the Nodes and Interpolate method was the outlier. Accordingly, the Ductile Damage Material Property and Calculate at the Gauss Points and Extrapolate methods are both considered suitable implementations of SLDR.

The best method to test whether or not the mesh density is sufficient appears to be to compare the averaged and un-averaged results. Special attention should be paid to the un-averaged results to determine if the SLDR results appear highly discontinuous or not. Furthermore, if the value of SLDR is negative while plotting the un-averaged SLDR, this too would indicate that the mesh is insufficient. More rigorous test methods may be available, but this simple check appears to suffice.

So, are you following the advice recommended in the final paragraph I quoted above?

Correct, it is an intrinsic problem of singularities, rather than a problem of mesh refining.

I have never run into this problem myself. Can you provide some additional details?

Let me explain with a simple example. I have run several simulations of a simple 2D model to avoid the large computational costs of modeling the nozzle for "investigation purposes". The following is an image of said model:



the following images shows the Plastic strain and the SLDR respectively:

Plastic strain (zoom in the zone of interest)


SLDR


As you can see, there is a zone with SLDR values greater than 1. So i modeled a 0.1 and 0.2 mm raidus but still the SLDR was greater than 1 there. Only with a 0.3 mm radius the SLDR was greater than 1 at each point.

My conclusion is that, when analyzing local failure, modeling the fillet radius is a must, otherwise you can´t be sure that he criteria is satisfied near the weld edges.

when you say "plastic strains", are you modelling non-linear material ?

Nice idea, modelling simple examples. Have you tried different angles ?
For example, how about adding a chamfer to the corner (to simulate the weld).

How are you modelling the non-homogenous nature of the weld ... the parent material, the heat affected zone, the weld material ??

What's "SDLR" ?

This is the impracticality of "at every point". Every structure has always had details beyond yield. Only they are highly localised and had viable loadpaths around them and so do not hazard the safety of the structure; unless it fatigues.

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

rb1957 - a non-linear material, taken from ASME Section VIII, Division 2, Annex 3-D would be the curve.

SLDR is a term that I invented, called the Strain Limit Damage Ratio, which is the ratio of the calculated equivalent plastic strain divided by the limiting plastic strain, as described in Equation 5.6 of ASME Section VIII, Division 2, Part 5 (and shown above in one of fem.fan's posts.

This relates to a very specific failure mode where, under certain stress states (high triaxiality), the material behaviour transitions from ductile (and represented by the elastic-plastic stress-strain curve) to be more brittle (the limiting plastic strain decreases). It needs to be assessed everywhere, because brittle fractures can occur spontaneously with only one application of a load. I'd be happy to discuss the failure mode in greater detail, if you would like. It's rather fascinating.

fem.fan - please provide additional details of your material model and α_sl and m₂.

Cuurently i am using a bilinear curve (first line to yield stress and second line from yield to UTS) due to licencing limitations. (we plan to upgrade de licence for commercial cases to be able to use a multilinear model of the ASME curve).
the material is SA-516 Gr. 70

αsl = 2.2
m2= 0.2784

FYI, the following image shows the SLDR of the exat same model with the only difference of a 0.3 mm radius.

Your uniaxial strain limit is too low by a factor of 10.

Is your 2D model really 14mm x 7mm with a 7mm x 3.5mm chunk cut out? And a 20N force?

Details, please.

The big square is 6mm x 6mm the rectangle is 6mm x 3 mm. thickness 1mm.

The uniaxial strain limit is 0.381. Why do you say it´s too low? i computed it from table 5.7
the force is 80 N (i changed it because i also changed the yield strength that i had reduced for testing purposes).

updated results:

SLDR


Plastic strains


Strain limit:

Now i see what you mean, i´ve corrected the value of uniaxial limit strain and the SLDR is below 1 everywhere. thanks for the correction. However, don´t you consider that generally speaking one needs to model the radius? otherwise, the strains results there are not real at all.

The elastic-plastic method is surprisingly forgiving for poor geometries, including singularities such as what you have modeled.

Have you done a comparison of the averaged and un-averaged plots of SLDR? Is you mesh converged for SLDR? Remember that apparent convergence for stress and stress does not equate to convergence for SLDR.

I wil admit that I have not run into this problem in my 15+ years doing these types of analyses. Don't forget that your load factor for checking local failure is not β, but only 1.7.

Thanks for keeping the discussion, it´s very enriching.

The mesh is converged only "certain distance away" from the singularity. In this particular example let´s say 0.2 mm, but you will never get convergence on the singularity and it´s near vicinity by definition, the stress and strains grow indefinitely there. This is a numerical problem, no matter what load factor you use.

Remember that i made this simulation only as an example, my concern is general.

How does the 3rd pic relate to the other two ?

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

SLDR = plastic strains / strain limit

Notch geometries are very real when it comes to Local Failure. The geometry that you used as an example is real when it comes to the inside of a air cooler header box wrapper plate (for example). These locations can actually experience local failure. We can just do our best, and try to follow the guidance in Seipp 2013 with respect to convergence for SLDR.

One additional note - I do not believe that a bi-linear curve is appropriate here. You will need to upgrade your software. But good for you for trying out the elastic-plastic analysis method.

Happy to help in any way.

rb1957 - some things that you might find interesting about this failure mode...

If you go to metal forming (deep drawing, wire extrusion, etc) formulae, you will find very similar equations for strain limits. In conditions of high compressive triaxiality, the strain limit can be many multiples of the uniaxial strain limit. (Think of successively drawing a wire from a rough billet). However, in conditions of high tensile triaxiality, the opposite happens - the strain limit decreases until the material is effectively brittle.

This condition is relevant because in the limit of pure triaxiality, the stress invariant (which is based on the difference between the principal stresses - could be von Mises, could even be Tresca) collapses to zero, even though there are non-zero principal stresses. At the limit of pure triaxiality, when the material is ideally brittle, the stress of interest is no longer the invariant (usually von Mises in a ductile material), but the maximum principal stress. However, you need to be able to figure out when that switch-over happens. The ASME Code has a prescribed limit, defined in Equation 5.6. There have been real failures that can be attributed to this failure mode - hence its inclusion in the ASME Code starting in the 2007 Edition. However, the numerical issue (invariant going to zero) was recognized waaaay back when the ASME Code first introduced Design By Analysis in the inaugural (1968) Edition of ASME Section VIII, Division 2 and ASME Section III.

I haven't thought much about this detail, but I would have thought that the differences between parent metal, weld filler, and heat affected zone would be (in reality) more significant than the precise geometry of the toe of the weld.

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

TGS4 - i´ve been thinking and the problem was "solved" because it was a 2D plain stress simulation and consequently the triaxality too low. so i gave a third dimension to the problem and a pressure of 100 MPa (i chose this value trying not to produce generalised plastic strain) and as i expected, in the singularity the SLDR is greater than 1. you can see tha this happens only there because the plastic strains and stresses are unreallistically large.



SLDR


Plastic strain


limit strain



the same with 3mm radius

SLDR


plastic strain


limit strain

fem.fan,

I'm late to this discussion, but I've run into this as well. I once ran a model of a lightly loaded sharp inside corner down to an absurdly fine mesh size and found that the stress and plastic strain increased slowly and steadily at an increasing rate with diminishing element edge length, but the plastic strain is extremely localized. I generally ignore this unless there are more generalized triaxial stresses in the area.

Of course, sharp inside corners in ugly welds do cause failures. Typically undercut, overlap, convex fillets, moreso than sharp toes on 45 degree fillets. My advice is that you focus on getting good welds, and don't worry too much about the numerical singularity. If there is a larger volume that is near the strain limit, I might grind the weld toe to make sure I get a smooth transition. If it's a critical service, I might also do a fracture mechanics calculation to understand how likely a crack is to run from the weld toe. Fracture mechanics is better suited to dealing with the singularity.

-mskds545