Stress Singularity Causing Problems for Obtaining Values for Fatigue

[Mechman77]

I've searched eng-tips.com and also have spent quite a bit of time googling my issue, but for now, I'm not having any luck.

The attached pictures best explain the issue I'm dealing with. I'm sure it's stress singularity in the model as I've refined the mesh the stress increases in same location, however the high stress values stay within the elements in contact; the elements adjacent to the one at the singularity drop off.

Due to the location, I'm sure there will be a rise in stress, however, because I'm dealing with fatigue I'm not able to assume plastic deformation and because of this and I'd like to be able to determine what the approximate stress value is for my fatigue calculations.

Any help is appreciated.

 

[Mechman77]

Additional info: elements are bricks with midside nodes turned on, using Autodesk Simulation 2012

Also posting additional image.

 

[ESPcomposites]

Contact stresses are compressive, which do not cause fatigue in metals.

If you get a singular tension stress you will need to do a fracture mechanics solution (not a fatigue analysis).

Brian

http://www.espcomposites.com

 

[rb1957]

i'd start with a material non-linear run, to see how much material yields (before becoming singular).

 

[corus]

For fatigue you should be looking at maximum principal stress, and the range of this stress through the load cycles.

If you have significant compressive stresses above yield then you can get cracking with the residual temsile stress as it's unloaded, and/or the residual stress from manufacturing or welds. How that crack propogates in a compressive field I wouldn't know.

 

[rb1957]

however, stresses beyond the proportional limit are ficticious, and if it's an area of interest/concern then you need NL stresses.

 

[Mechman77]

Thank you ESP, corus, and rb1957 for the replies.

I wanted to post a picture of the basic area of interest I'm dealing with. Hopefully this will better explain what I'm after.

The blue plates (both sides) are welded to each other, same for the red plates. However, the connection between the blue and green plates and red and green plates is a bolted connection that will be slip critical; for simplification of the model and to make things run more efficiently, I've modeled the connection as bonded.

Basically I'm checking the fatigue of the bending of the green plates, with the area of concern being the portion that is in between the red and blue bolted plates.

I've included the arrows to show what type of forces this joint will be experiencing; this is fully reversible.

 

[rb1957]

sorry, can't open pix at work (something about blocking 3rd party hosting sites) ...

the "area of concern being the portion that is in between the red and blue bolted plates" ... is this the weld material itself, or the plates between the welds ?

if it's the welds you're looking at, i'd use the FE to tell me the bulk load being sheared at weld, then use weld fatigue data it understand if i was ok or not.

if it's the parent material (near the weld), again i think i'd use the FE to tell me the load, and use welded material fatigue data to understand it. If it Had to, and if it was Really important, i'd do a simpale fatigue test, using the load from the FE.

if the linear (elastic) FEA is producing inelastic stresses then you Need to run a NL (Elastic-Plastic) analysis if this is your area of interest.

 

[Mechman77]

--------------------------------------------------------------
Continuous Plate ( * )Bolted Connct. to Below (Modeled as Bonded)
--------------------------------------------------------------
---------------------- ------------------
Welded to Below | -Gap- |Welded to Below
------------------------ --------------------
Welded to Above |Gap| Welded to Above
------------------------ --------------------
/\/\/\/\/\/\/\/\/\ |||||||||||||||||
||||||||||||||| \/\/\/\/\/\/\/\/\/\/
Force Opposing Force


So the above may or may not help you rb1957....

My area of concern is the bending between ( * ) on the continuous plate. I've modeled the bolted connection as bonded as it's a slip critical connection. The stress singularity is occurring at the corner between the continuous plate and welded plate below; which is a bolted connection.

After editing my post more times than I'd like to admit, I can see how this may be more confusing than helpful...

 

[rb1957]

i appreciate the effort ... maybe using fixed pitch font would help.

 

[corus]

You' ve modelled the plates as being bonded, which is probably correct in compression, but on the opposite side wouldn't the plates tend to part and so the tensile stresses there would have less of a singularity as the contact area becomes more rounded. For certain, around the bolts you can be assured of contact being retained, but at the free edges of the plate this is unlikely to occur. To model this, though, you'd have to include contact, and the bolt loads, which would be more difficult.

Most fatigue design standard use the nominal stress, which you could work out by hand. For your analysis I would have thought the welds would be of greater concern than the plain metal between the bolted connections. For this you could only use nominal stresses.

 

[Mechman77]

I agree about the tensile stress having less of a singularity if the connection was modeled as bolted. However, this area is in one portion of a pretty complicated structure.

I haven't spent much time in the way of sub-modeling so I was a bit hesitant to do that.

In reference to your comment about using nominal stress for fatigue, I'm unsure whether you're implying I'm obtain those forces by hand using information from my model, or doing a straight hand calc of this connection.

 

[corus]

Nominal stresses are those away from any details. In this case I'd just consider it as a composite beam in bending and work out stresses by hand. These should be similar to the stresses in the model away from the singularities.

 

[inline6]

extrapolate using values 1.0t and 0.4t away to the actual area of interest and use that value. Sometimes called hot spot method and used often for welded structures

 

[rb1957]

sorry, but i gotta vent ...

why extract stresses remote from an improperly modelled detail ? why not pick a number ??
an elastic FEM predicting inelatic stresses is Wrong. there's an option that you can say the peak stress (beyond yield in the FEM) would be redistributed in a real piece and may be acceptable; what you're saying is "if i ran a NL FEA i'd get good results".

if the inelastic stresses are in your area of interest, and you don't like the hand-waving above, then you need to do a NL FEA. picking stresses "near" the detail as "near enough, good enough" would only be ok (IMHO) if you'd do a ton (or tonne) or analysis and test to validate the method ... ie the stress picked outside of the Kt region, manulipated this way, gets a good result.

sorry, but i've had to deal with this type of situation in real life.

off soap box ...

 

[corus]

rb1957, it's not extracting stresses at some arbitary point away from the detail, but using values away from the region of interest to extrapolate to the weld. In general you should see a non-linear change in stress up to the stress singularity. 'inline6''s method is a way of defining which points away from the weld you use to extrapolate to the weld. Personally I'd just draw a graph and estimate what the 'linearised' stress was at the weld if the peak stress due to the singularity of the geometry was removed.
Note that for fatigue evaluation of stresses at a weld then the stresses from an elastic model are used.

 

[inline6]

I am a little confused the OP mentions contact stress as reason for high stress but later there is talk of welds and bolts in another post. I am not clear on what is happening on the OP analysis. If it is just a contact problem then the mesh is far too coarse and maybe a classical solution might exist (FE is not always the best way). I wont add anything else on this side of things until it is clear.

My previous post was me thinking it was a welded connection and l'll add the following. If the stresses in that immediate area are at a singularity it doesn't make sense to pick a value close to this area. There are widely recognised standards used internationally across numerous industries that use the approach i mentioned in my previous post for assessment of steel structures particularly welds.

If we are talking about a ductile material we don’t always need to do NL to judge if the result is a singularity or not. If the region is too large to be purely due to a singularity an experienced analyst should be able to judge if the mesh is fine enough to capture the plasticity and how much elastic material is in the vicinity to “support” the inelastic area to know that redistribution will occur and gross failure will not be an issue. To err on the safe side it is always interesting to do though. You need a much finer mesh to capture true effects of plasticity and this makes nonlinear analysis even more time consuming. Though these days with more demands on structures it is the norm for me. I know of far too many disasters caused by analyst carrying out linear static analysis without an understanding of solid mechanics and carrying out simple calculations.