Von mises stress

[mvg1982]

1. Do we have to look into Von mises stress always even if the material is not yielding ? What other parameters can be seen to justify the level of sress in the component ?

2. There are lot of opinion of limiting the stress value like we have to limit it to 2 element depth ot 3 element depth. Why can't we limit the stress to yield and judge the stress level ?

 

[rb1957]

1) von Mises is a failure criteria, for combining different stress components together to compare to a uni-axial (standard coupon) test result (ie fty). Use it when you have ...
a) multi-directional stress components (sx, sy, shear xy, sz, ...), and
b) failure defined by von mises (you culd also use principal stress, octahedral shear stress, etc).

2) not really sure what you're on about here ... maybe how many elements to put across a stress gradient?

 

[mvg1982]

Thanks for your reply...
When we have the results the stress SMX is a numerical value and can be very high, but usually we come up with an absolute value which will be less than the SMX and say that is the maximum stress in the component.
In gist, How do you say what is the maximum stress in the component and I hope it is not SMX ?

 

[corus]

I guess that the software is showing SMX on the contour plot at the position of the maximum stress. Your question implies that you can disregard that and choose your own maximum at some arbitary number of elements away from that position.
Although in practice it is common for some human interpretation of results from a finite element model, usually this is done in a logical/reasoned fashion. In your case you may have some high stress at a point load or a restraint, for example. In such cases you cannot interpret the results at that position nor can you opt to choose a stress at x elements away from that position as it would be highly unlikely that your point load represents the real situation. Either you will have to represent that part of the model more accurately or totally disregard the stresses at or near that position knowing (in a reasoned way) that in real life such stresses would never exist.

Tata

 

[rb1957]

what code are you using ? ... i don't recognise "SMX"

how do you come up with "an absolute value less than SMX" ??

 

[mvg1982]

@ Corus... you are right. The node at which the SMX falls can be ignored if it can never occur in the real life situation. Now further on do you just see the range of the stress values to undertsand what the component is subjected to ?

@rb1957... I really did not get you on code ? SMX is in Ansys and am not sure what it is in any other software.

 

[rb1957]

ok, you're using ANSYS.

now, thx to corus' intuition, you've got a high stress peak in your model due to either a load input on a grid or a constraint. if it's a constraint, you can release some of the stiffness by attaching a spring to the model and placing the hard fixed grid off the model. in either case, you've got "some" license in interpreting your model and you should have some logic for this.

i've had cases where the detail modelling was bad (= coarse) so the local results were bad (= high) and we were directed by the job owner to use the stresses in an element 2 bays away ... but i never liked it ...

 

[corus]

Another simple method is to categorize the stress as per their location and load type. In a case of a point load then the stress due to that point load is classed as a peak stress component, whereas stresses elsewhere may be classed as primary or secondary. For a peak stress component you would assess that stress (or range of stress) against fatigue damage criteria. If your stresses don't cycle, or have a very low number of cycles then you can reasonably ignore the fatigue damage criteria and hence reasonably ignore the stress due to the point load. How far away you can go from that peak stress before you can start assessing stress levels is a difficult question and best avoided by modelling the object correctly in the first place.

Tata

 

[EngAddict]

If you are using solids you can linearize the stress across the thickness and separate peak from bending and membrane. I know this can be done in Ansys for you but don't ask me how. What you can't do is assume it will alway be a set number of elements from the stress intensifier. However there are methods for calculating stresses at set distances from fillet welds. Mainly concerned with fatigue though but worth a look, ref PD5500.

 

[mvg1982]

Cool....! those where very nice reponses. Thanks to all.
I have few more in line.... Will post soon.