first principal stress? 2

[ch1]

All,
I am working on a simple model. it a beam fixed at one end and pulled horizontally with a force at the other end. the middle section of the beam thins out.
I have a converged nonlinear solution in ANSYS. I am trying to decide which results from ansys to use. I got results for first principal stress but when I also plot a nodal solution for shear-xy, I also get a value.
Should I trust my results for the 1st principal stress since first principal stress is the max stress when there is no shearing???

 

[EnglishMuffin]

Check the Von-Mises stresses and compare them with tensile stress data for the material.

 

[ch1]

I checked the stress in x-direction/first principal stress against the von mises stress. They are pretty much the same. does this validate the solution? and why? Is this what you meant...or did you mean to compare it to experimental data for tensile 'strength' of the material?? (if this is so, the experimental value is much larger than the force being applied in this model). will appreciate the help.

 

[EnglishMuffin]

The Von Mises failure citerion is as follows :

Sy = sqrt{((S1-S2)^2+(S2-S3)^2+(S1-S3)^2)/2) where S1,S2,S3 are the three pricipal stresses and Sy is the yield strength in a uniaxially loaded bar - in other words if you calculate the "Von Mises Stress", and it is greater than the tensile yield strength that you can usually look up, failure will occur. The "Von Mises stresses" given by your FEA program are calculated from this equation. This criterion is generally accepted as being the best "theory of failure" for ductile materials - such as a piece of mild steel. If you have brittle behavior you should use maximum normal stress theory. (I should have mentioned this in my all too brief original answer).
In ductile materials, it is the shear stresses that cause failure. If the three priciplal stresses are not all the same - you've got shear. If, for example, you have pure hydrostatic compression, nothing will happen, however high the pressure becomes - all the principal stresses will be the same and the Von Mises stresses will be zero. The same thing would be true in tension - which would cause the criterion to fail in the extreme, because the atoms would eventually have to be pulled directly apart - but I don't think anyone has ever figured out how to do this in practice, and it would involve an enormous stress.
In your case - it appears that S2 and S3 are zero - in other words you have pure tension - and the Von Mises stress is the same as the first principal stress S1 (study the equation). So in this particular case, you can compare your tensile stress directly with that present in a normal tensile test. Hardly worth doing an FEA was it ? You can gain a better understanding of all this by looking at the Mohr stress circle. Look in a book about elementary strength of materials - it should help you. Since you are doing an FEA, you should not need to consider stress concentration factors - but you may need to consider fatigue failure if you have cyclic loading. As a rough guide, you can look up the endurance limit (assuming the material has one - not all materials do).You also need a factor of safety in all designs - but from what you say you may be OK in that respect.

 

[EnglishMuffin]

I should probably have added that I think your maximum shear stress should be about half of S1, on a conical surface at 45 degrees to the direction of your applied force. In a tensile test, that's exactly how ductile materials fail.

 

[EnglishMuffin]

And it also occurs to me - after re-reading your original question, that since you are doing a non-linear analysis, you are likeley to be dealing with a material that is a bit out of the ordinary - in which case none of my remarks may apply. They are valid for most ductile metals - but these don't normally require a non-linear analysis.

 

[dollarbulldog]

Which kind of nonlinear analysis have you used (material-only or with large displacement option)? Shear stress always occurs if element is distorted caused by necking in this case (this effect will not be seen in small displacement analysis even with isotropic plasticity model). What Englishmuffin told you is exactly tresca yield criteria which is also valid for metal but it is not popular for programming caused by nonunique corner effect (tresca hexagon-note for nonunique plastic flow direction at corner). However, to compare with experimental model, the definitions of stress and strain measurement must be concerned, ANSYS uses corotational cauchy stress (via Jaumann rate) and logarithmic strain for most elements with large displacement (NLGEO,1) formulated on current configuration (Updated lagrangian). Please see more in help. Try to use higher order elements or turn on special EAS option to avoid shear locking. But I wonder why don't you have S2 for some parts that are distorted (by necking effect)???

key words: logarithmic strain, Jaumann rate, updated lagrangian,logarithmic strain,Cauchy stress

Bests,

 

[dollarbulldog]

More about stress, Jaumann rate will necessary only for rate constitutive like hypoelastic-plastic. Otherwise corotational stress called rotated-Cauchy stress via deformation gradient is applied since Cauchy stress is not invariance by rigid body rotation.

Bests,

 

[EnglishMuffin]

dollarbulldog:

Actually, the Tresca yield criterion, (or maximum shear stress criterion) is not exactly the same as the von mises criterion, although they are close. It is a certainty. though, that if you have uniaxial tension, which is what ch1 appears to have, you will have a lot of shear stress, regardless of what kind of analysis you are doing, or even the shape of the part.

 

[dollarbulldog]

Sorry EnglishMuffin, I should stated that your 5th answer is based on Trasca not above which is surely VM

 

[EnglishMuffin]

Not quite sure what you are saying. Do you nean my 3rd answer (5th post) ? This 3rd answer isn't actually based on anything specific, just a rough guess based on the fact that the Von Mises and first principal stress are almost the same. My 5th reply isn't really an answer- just a comment. I also don't see how there could be plastic deformation in this problem if the applied stress is so low - as ch1 seems to be implying in his second answer- although his stetment is ambiguous, but maybe there is a stress concentration or something. When he says "the middle of the beam thins out" in his first post, that might be before the load is applied. I wonder if ch1 is still reading this. I hope its not one of those student posts.