Stresses At Boundary Locations 2

[meher634]

Dear FEA Gurus,
I think there was lot of discussion before on the topic i am going to post it now .
1.FEA analysis is performed on curved beam, and the boundary conditions are identical to the curved cantilver beam.
2.The geometry is somewhat comlicated to be calculated with hand calculations.
3.The stresses at the boundray locations (where the beam is fixed) shows very high stresses always.
4.The stresses are very low say 2 mm away from the boundary location and is more uniform, I am just curious if the high stresses at the boundary locations are due to local stress error.
5. The cross sectional area at the boundary location is identical to the cross-sectional area at 2mm away from the boundary location. Ideally one would expect the stresses to decrease gradually rather than the sudden drop in stresses.I am still confused if my assumption is true.or should the stresees at the boundary locations are accurate?
6. Stresses at the boundary location is about 100 Ksi while the stresses at 2mm away from the boundary location is about 35-40 Ksi and the stresses thereafter show smooth transition.
I would appreciate if any one has suggestions.
Again Many Thanks
Meher.

 

[GregLocock]

If you apply a point load to the tip of the beam then the stress distribution at the the base should be fairly easy to estimate by hand.

It does sound as if you have unrealistic fixity at the base. In the real world it is very hard to get a truly encastre (fixed) foundation, and if you do then there is local yielding as the thing sorts itself out.

Can you describe your boundary conditions?



Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[corus]

Sometimes it's useful to look at the stress components rather than the 'stress' which I presume you mean the stress intensity. The component stress value S11, S22, or S33, may well equate to values obtained fom a hand calculation, whereas the stress intensity may not - due to shear compnents at the restraints for example.
Another problem may well be that the stresses are related to the mesh, rather than to the geometry of the problem. It's quite common for people to quote the maximum stress whatever the computer spews out even though that stress is due to a badly shaped element or a point load/restraint.

corus

 

[johnhors]

Meher

You can disregard the stresses at your fixity positions, they are fictitious. As Greg pointed out, fully clamped boundary conditions are almost impossible to achieve in practice. You can either try and soften the fixity by replacing the fixed supports with springs to earth, but choice of a realistic spring stiffness is very difficult, or you can partially model the support structure. Anyway, unless you have a fully load balanced model with a set of minimal determinate supports, you cannot trust results at or near the supports.

 

[cdbajpai]

Hi Meher,
Do not much rely on the stress values what you are getting at fixed point as by fixing you are suppressing all possible dof which may not be the case in real life. you can simply imagine the variation from 100ksi to 40ksi. This much of variation is indicating that it might be because of singularity issues.
So your main focus should be how to report true stress in your model. There are several ways to do that:
you can take a path plot considering some 4 or 5 grids along the stress flow and ignore the value which are corresponds to Ist higher slope and consider the value based on 2nd higher slope that could be your true stress value.
Also if you have any isolated node having highest stres. you can ignore it but for that you have to make sure that the adjacent node's stress value is far away. The basic logic behind this a single peak stress will not lead any failure for static analysis point of view.(for fatigue you can not ignore this isolated point)

cheers,
BAJPAI C.D.

 

[rb1957]

personally, i'd not suggest to ignore the end stresses ... they are telling you something. they may be unrealistically high because the nodes are unrealistically constrained (eg every node on the plane being fixed). or the constraint may be unrealistically confined (maybe you're constraining only one node, so the local stresses are unrealistically high).

soapbox time ...
i don't know your experience, but i'm assuming that you're leaning FEA. don't casually ignore anything in FEA. certainly there are things to ignore ('cause of the way the structure's been modelled) but you must understand why. if you start ignoring things ('cause the numbers are funny) then you may ignore things that you shouldn't, and (possibly worse) you might not understand FEA, but accept it on faith.
i go now ...