stress evaluation in critical areas

[meher634]

hello,
I did a simple fea test (analogous to cantilever beam),I am to evaluate the region of critcial stresses in the beam,I find that the stresses are high at the constrained end.I refined the mesh to as fine as possible,but my question is should i consider the stress-concentration region (constraint-end) as the critical region when reporting the stress value.

 

[jhardy1]

Firstly, for a cantilever beam, you would expect your maximum stresses to be at the constrained (fixed) wend.

However, you might want to check your boundary conditions and geometry etc are realistic. If you have over-constrained the end of your model, and/or you have modelled a geometric discontinuity (eg a sharp re-entrant corner) and/or you have a point load, then no amount of re-meshing will make the apparent stress concentration go away. (Theoretical stresses at a sharp re-entrant corner are singular, so will report as very high stresses, regardless of how fine your mesh. Theoretical stresses immediately under a true “point” load are infinite.)

If the maximum reported stresses are unrealistically high, consider remodelling to get rid of the over-constraint, geometric discontinuity, or load discontinuity that is causing the problem. E.g. consider using elastic restraints with a high spring stiffness rather than fixed nodal restraints, and make sure you restrain the whole end face of the beam, not just the corner nodes. Eliminate sharp re-entrant corners by modelling a fillet, and eliminate point loads on plate / shell / solid models by applying as a surface pressure load over a finite area of elements, rather than as an isolated nodal load. (There is no such thing as a truly fixed restraint, or a zero-radius corner, or a true point load in the real world.)

 

[bvi]

If you have a cantilever beam, what is wrong with Mc/I????
You can calculate the moment and section modulus with hand, or very simple computer assisted calculations. The stress is very simple to calcuate. If you have stess risers, such as re-entrant corners, this is a fatigue concern,not an issue normally of concern in structural design.

 

[gurmeet2003]

me634,

It seems to me that you have a sharp corner at the location of constraint. Stresses at a sharp corner are theoratically infinite and FEA can not calculate them. Another possible way is to look at the stresses a small distance away.

Gurmeet

 

[jetmaker]

meher634,

JulianHardy is spot on in his remarks. Most likely, you will have a discontinuity at your boundary condition. Check the stress gradient in this area. If it is changing rapidly, then try a different constraint and see if the results are similar.

Gurmeet makes a good point about checking the stresses a small distance away. However, keep in mind, that the effect of a singularity can propagate into the body for quite aways. A rule of thumb is that the stress due to a singularity should be disappated by the 5th/6th element away from the singularity. Of course, there are many exceptions to this rule.

Regards,

jetmaker

 

[meher634]

Thank you julian,gur,jetand cb4,i agree with you all that its better to omit that particular node,and chk the stress values a little far from that node.