perpendicular shells 9

[chaboche]

Hi,

I have four shell elements connected perpendicular to one another (in a cross). One face of the cross is subject to a bending load, the other is fixed at one end. A stress concentration is calculated at the interface. Is this a valid stress? It seems very high.

Any comments are welcome.

 

[GBor]

You need to refine the mesh in that area and see by how much the stress changes. I suspect you will still see an elevated stress in that location and that it is a valid stress, but right now, you have greater than a 10% stress gradient across a single element. There is a lot happening in that location and it should be very stiff with all of those plates running to that single spot. It will carry a good portion of the load through that area, but refine your mesh and see what happens.

 

[Stringmaker]

You'll probably see higher and higher stress as you refine the mesh in your model. If you only care about determining the structure's stiffness or dynamic response the model you have should be suitable. If you require detailed stress output the best option is to submodel the area of interest. You should see good results by doing so.

Good luck.

 

[SWComposites]

Is the stress shown valid? No - the mesh is way too course to get an accurate value in the stress concentration area. However, the use of plate elements may not be appropriate for a very localized stress concentration. Do you have to consier the high stress? - maybe - depends on the material, loads, application, etc.

Can you post of figure showing the real part/structure? And a figure showing the loads and boundary conditions applied to the model?

 

[rb1957]

at this detailed view, are the parts joined accurately ? FEA welds the things together at common nodes, are there discrete attachements instead ?

 

[crisb]

You cant expect realistic peak stresses using shell elements. In real life the load will spread through the thickness of the horizontal fin and then through the vertical flange. Mosts codes allow a 45 or 60 degree spread. If you want realistic peak stresses you will need to use 3d elements.

 

[corus]

I don't know if I'm not seeing it properly but the stresses appear discontinuous across the web and flange at a hot spot. Whether this is because of a change in thickness or material isn't clear, but I'd check to make sure you have no gaps in the model.

As has been said, you can't class the stresses there as peak and assess for fatigue damage, but you could class them as being secondary stresses (occuring at a structural discontinuity) with a limit on the stress range of twice yield.

corus

 

[prost]

I don't work with shells very often--is it normal for shells to be used when the stress fields are so obviously three dimensional, such as where the shells are crossing and presumably connected? Shells, because of their formulation, normally perform poorly in regions where stress fields are three dimensional.

That being said, I would also guess that refining the mesh would just increase the max. stresses to infinity, since this looks to be a singularity at this connection point.

The question I have is are you modeling reality adequately? Are these pieces going to be welded together? Bolted together? If they were connected as shown, with loads that cause the stress to go to infinity at this connection, then that could indicate problems with the modeling of the connection itself. Is the way you have modeled it realistic? If you really need the stress at the connection point, then you have to do a better job of modeling what is really going on at that connection point. If you are interested only in stiffness (that is, how much it deflects for a given load), what you have might be adequate but you can't trust the stresses at that connection point.

 

[cbrn]

Hi,
I'm with Stringmaker and Prost when they say that refining the mesh more and more will show higher and higher stresses. In fact, the hot-spots you are seeing are in geometric "edge-discontinuities" (triple- or multiple-corner in one case, T-corner in the other. These are the typical cases for "mesh-paradoxes".
The stress distribution, imho, can makes sense (as far as I can guess because there is no indication about the restraints and the loads). If you plot S1 instead of SEQV, you should find that the stress at the "external appendix" T-joint is in compression, while the hot-spot in the I-beam is in traction.
Where I see a possible problem, as Corus says, is in the discontinuity web/flange/appendixes. You should check that the nodes are merged etc...
Anyway, as "the" solution to your problem if you do are interested in the "realistic" stresses at the junction, I'm with Stringmaker in proposing "Submodeling" (with Ansys which you are using, you can even perform shell-to-solid submodeling without problems). In your solid submodel, include all realistic features and, possibly, avoid any sharp edge discontinuity between concurring elements.
Regards

 

[chaboche]

First of all, thanks very much for all of your posts, I'm overwhelmed by how many responses I have recieved, all very helpful.

The structure being assessing is a reel, composed of various steel sections which is why it has been modelled with beams and shells. A stress assessment is to be performed to determine the capacity.

I understand that the mesh is coarse, however this is just a small segment of the model, and unfortunately due to the loading conditions, I cannot exploit symmetry. I have performed a mesh sensitivity check and the stresses away from the concentration are unaffected by further refinement.

I need to consider the stresses at the concentration to ensure they are within the allowable of the code. The structure is to be used offshore and therefore I am performing the assessment according to DNV Rules for Marine Operations.

The shells are joined at common nodes, however they are composed of different thicknesses which adds to the discontinuity. It is all the same material. In reality, the shells are welded together.

I will try submodelling using solid elements; in order to quantify the peak.

Thanks for your help, I will keep you posted.

I have attached a figure of the model. I shall add additional posts showing further detailed plots.

 

[chaboche]

further plot at the link below

 

[chaboche]

further plot at the link below (2)

 

[chaboche]

further plot at the link below (3)

 

[chaboche]

further plot at the link below (4)

 

[chaboche]

further plot at the link below (5)

 

[chaboche]

further plot at the link below (6)

 

[trainguy]

You should be very careful in how you've set your averaging, because at shell element corners, some of your stress results should NOT be averaged, especially if they're in orthogonal directions.

tg

 

[chaboche]

Thanks trainguy,

I will be careful with stress averaging at the intersection. Is there an easy way to stop averaging at the interface? I guess I could set up different materials for each shell.


I have built a 3D submodel, though intial results show peak stresses at the sharp corners, to be expected. I will add appropriate fillets and rerun.

 

[chaboche]

I have now run the 3D submodel assessment. I encountered high stresses along the cut boundary. I think these are due to the shell/solid cut boundary interpolation, as they mainly occur at the juncture between perpendicular shells.

Stresses in the submodel away from the cut boundary are similar to the global results, indicating a successful transfer.

The results on the submodel show high stresses at two locations, both are internal corners and I have added appropriate fillet radii. The maximum concentration is ~550MPa, much higher than yield (355MPa). This concentration is a secondary stress localised on the surface of the model.

Corus mentioned that I could get away with assessing localised results against twice yield. I can see that the stresses through the section away from the concentration are less than yield, and therefore will provide support against failure. I know that it is acceptable in some codes to exceed yield locally, as long as the structure is not compromised.

Does anyone have experience of justifying why such a stress concentration would be acceptable, or can point me in the direction of a reference to a section in a code that deals with such stress concentrations?

Any further questions, please ask. Thanks for your help.

Below is a link to a plot showing the global and submodel stresses.

 

[rb1957]

not sure that last file linked properly ... just got a blank, vacant stare from the screen ...

a stress peak higher than yield means there is some localised yielding going on. if you can rationalise that this is indeed a localised behaviour then go for it. if you can't, how difficult is it to do a material non-linear analysis ? this would give you a "definitive" answer.