Elements size and Stress distrubution 2

[Ricinus]

Hi,

I used to work with other FEM program.
But I have to use PRO/E Mechanica now.

I had bumped into a problem:
When I am reducing the element size, the absolulte value of stress is increasing.

I know this has to be happened, because of Hook's Low.

My question how can I decide the right element size in order get the real value of stress.

Using:
-solid element type
-Pre/e mechanical

I am looking forward your answare!

 

[Drej]

As with most things it depends. If you have a singular stress (at a point of geometric discontinuity for example) then regardless of the element size the stress will continue to rise. If this is not the case and you have a genuine stress raiser, then you will need to do a mesh convergence check in the area where the stress raiser is located ie you will need to continue to reduce the element size in that area until the stress converges (doesn't change). Continue to do this until the stress remains constant for at least two reductions in element size.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[Ricinus]

Hi Drej!

Thanks Your quick answare.

There is a singular stress, if I reduce the element size stress will be infinite(I think)

 

[rb1957]

i'd've thought that denser meshs were able to follow the stress gradients better and so converge on the "right" solution.

do you mean for your model to have a singularity ?

is it real or a result of modelling or loading ?

in either case, do you think it is real (that you'll get infinitie stress in the real world) ?

have you tried a material NL analysis ?

 

[corus]

It looks like you either have a 'lip' that causes a stress concentration, or you've applied a restraint along a line or applied loads along the same line. In any of the cases you've not modelled what would be a 'real' situation, and in any case the mesh you're using is giving irregular stress distributions which would give me no confidence in any results you produced.

I'd reconsider how you apply the loads or restraints, and also consider how you would assess the stress you come up with at that location, if at all. If it's just a static loading then as a stress concentration it may not be important. If it's varying loads then you might be concerned about fatigue damage and would need a much more intense study of the stresses there. if it's just the way you've applied the loads and are only interested in areas away from that region, then ignore it.

 

[Ricinus]

Thanks rb1957 and corus!

I would like to reconsider how i apply the loads and restraints, that is why i am here, asking.

I would like to modelling as possible as real. So I can accept the stress distrubution as result.

So I could do these, I think:

1. Because I have singularity in modell, where the stress must be infinite (because one of the restraints). I won't see there and near the stress distrubution, because in real the value of stress would be smaller than other locations.

2. The real this restraint is a contact thing, that i couldn't make it work in pro/e. I would do it if i work with solidworks.

thanks

 

[ThisIsMe86]

Ricinus,

You are right in thinking that the stress reaches too high a value when u start refining the mesh. Mesh convergence study would be helpful, but not in singularity case i think.

I would refer to the mesh quality guideline from the client and note the minimum element size required. Then refine the mesh beyond that and observe.

As rightly pointed by rb1957 (Im giving you a star rb1957), stress gradient is also a good measure to see how "close" you are to the right solution.


-This is me

 

[Ricinus]

ThisIsMe,

Thanks

I can not see stress gradient with Pro/E.
I checked it in help center, but I could not find it.

So anyone knows, where is the stress gradient in Pro/E Mechanica

The other thing: there is no minimum element size only maximum

-Ricinus

 

[rb1957]

no, you can see the stress gradient ... it's how the stress is changing from element to element.

2nd, if hard (rigid) constraints are the problem (i can't open your attachment at work) then use "sticks" to soften the constraint. replace a hard (fixed) constraint) in the x-direction with a stick in the x-direction and constrain the far end. this way the model has stiffness in the x-direction, but not infitite stiffness (as per regid constraint). Don't ask what area to use for the stick ... try something, see how it works; don't like it try something different !

clear as mud ?

 

[Ricinus]

rb1957,

That's great idea.

thanks

 

[Bobfromoh]

Mechanica uses a "p" element to solve for stresses? I don't think you can adjust elements (sort of) but you should be able to tell
the software to converge on the stress criteria limit you are using. I haven't worked with Mechanica for awhile so I'm not sure
of the process? Also, maybe you can use stress linerization in the results module to determine peak and bending stresses.

 

[rb1957]

i think Pro/E uses both H and P elements ... since th eOP is refining his mesh, i suspect he's using H elements.

if it's a contact problem, Pro has to have a gap element (everyone does these days !)

 

[Ricinus]

Now,
I can accept the result.
I check the stress, where I am looking forward the value of stress is the biggest far from the singular points.

Pro mechanica uses P-method for convergence.
It was a static analysis and could choose bettween 3 convergence methods
-Quick check(not a convergence method)
-Single pass adaptive
-Multi pass adaptive

I cheked the help, and yes in FEM-mod have gap element, but i didn't use that mod, but i will check it also.

Thanks everyone help.

-Ricinus