Problem with results of Ansys analysis

[erga]

Hello,
I am doing a analysis of a tubing support, a guide, that works like a hold-down too.
In this analysis I put the vertical positive force on the right face of the guide and like I expected it produced a stress concentration.
The stress concentration isn't my problem, my problem is when I try to refine the mesh, the stress increases a lot, and the more I refine, the more the stresses increases.
I have done a fillet in the stress concentration area for being like the real situation, but the problem remained.
I would like to know if I have done something wrong and/or there is a secure number of elements, or a size of elements that given a real result.
I attached the photos showing better the situation.

ps: Where do I click for seeing the attachments?

Thanks.

For the first analysis:

http://files.engineering.com/getfil...148f-4a98-9389-0d2f1b49a0b6&file=ansys_11.JPG

http://files.engineering.com/getfil...aff5-40b1-b332-3d23d1c01878&file=ansys_12.JPG

For the second analysis: (more refined one)

http://files.engineering.com/getfil...6c4-4085-a610-16f732d87b98&file=ansys_2-1.JPG

http://files.engineering.com/getfil...a32-49fa-bfe3-7ce47033ae72&file=ansys_2-2.JPG

 

[gurmeet2003]

Erga,
Your problem is that you have not got mesh convergence. Radius you have added is really small. In order to get a realistic stress number you need to put at least approx. 3 elements through the radius. Better way is to keep reducing your mesh size till you get convergence (till your results stop changing). How you will use this information in practice is another story. It will depend on whether you have fatigue load or static load. But that is a topic for another thread.


Gurmeet
Time is an illusion. Now is the only thing there is.

 

[erga]

That's the thing I have more doubts... How many elements to put? And what is the size of the radius? What are the criterion for choosing it? How can I know it?
Because, the more I refine the mesh, the more the stresses increases.

 

[erga]

No one can help me with my problem?

 

[rb1957]

are you looking at element centroid stress or nodal stress ?

refining the mesh will cause bigger changes to element centroid stresses than the stress at the edge of the stress concentration.

another thing to consider is that you're chasing an impossible target. you're using linear FEA (i assume) and the model is predicting stress beyond the elastic limit (i'd expect), and you're trying to get the exact peak. if you're concerned about the stress concentration, use the nodal stresses. if you're concerned about the rest of the structure, use element centroid stresses, and some story to explain what's happening in the stress concentration area.

 

[erga]

Thank you for yours answer rb1957...
I am looking at nodal stress,
I realize that the more refined is the mesh, the bigger is the stress,
I am not wanting to get the exact peak, I want to take a safe result that I can say to my boss "That's the bigest force that it can hold.".
The problem is that no one gives me an answer that explain why theses results only improve.

 

[erga]

Just for fix some errors that I did...

"That's the biGgest force that it can hold.".
The problem is that no one gives me an answer that explain why theses results only INCREASE.

 

[rb1957]

i think that as you refine your mesh you're getting closer into the stress concentration and so th emodel is telling you higher and higher stresses (assuming you're looking at element centroid stresses). if you're looking at nodal stresses the peak stress (at the edge of the radius shouldn't be changing that much as you refine the mesh.

the problem with FEA is that it detects these highly localised stress peaks that may not be completely relevent to the capacity of the part. the FEA is linear elastic (i'm assuming) and it's predicting stresses beyond yield (i'm expecting). The real world is not linear elastic (when it comes to small details like stress concentrations); yielding occurs so the high stresses predicted by FEA don't appear in the real world.

sure you can run NL FEA (allowing the model to yield). for your stress peak, i'd look at it so see if the high stresses are local to the surface (not much of a problem) or all the way though the thickness (a real problem !).

 

[erga]

Ok, I will try the nonlinear analysis, but I would like to know if there isn't other ways to solve this kind of situation...
Maybe some considerations or things like that, because the nonlinear analysis is difficult for doing and more complicated... And I think this little structure is so simple for it.
Thanks for the answer!

 

[IceBreakerSours]

How many elements to put? And what is the size of the radius? What are the criterion for choosing it? How can I know it?

You'll know it when the stress stabilizes (or reaches a steady-state or stays within a narrow bound).

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[rb1957]

one of the things i notice between ansys_12 and ansys_2-2 is that the fillet looks to be remeshed in the first model it looks pretty coarse, the 2nd looks very detailed. the max stress changed from 15 to 19(ksi?) ... not much of a change considering the change in meshing. if that is the ture stress, then not much yielding happening !? but i suspect you're applied a unit load ?

if model 1 had 1 element on the fillet, and model 2 has several, then model 3 with more shouldn't change much (from 2).

 

[erga]

Hello rb1957, thanks for yours answers... I did what you tell me, I refined the mesh on the fillet but the stresses increased a lot. It got 30! And the units are kgf/mm².

The elements:
Your file's link is:

http://files.engineering.com/getfil...cb6-40d7-9cd0-f420f34791f5&file=ansys_3-1.JPG

The results:
Your file's link is:

http://files.engineering.com/getfil...0c7-463d-8507-73ef2fff1245&file=ansys_3-2.JPG

 

[rb1957]

your mesh is Horrible ... make the elements squarer ... element aspect ratio nearer 1 ... in a rapidly changing stress field you need small square elements.

 

[rb1957]

now i notice your meshs (sorry, at first glance your pix looked like blue blobs) ... you first mesh won't capture the stress concentration (replacing the radius with a fillet, one element long). your 2nd and 3rd track around the radius well enough, but the aspect ratio is way too high (if you're trying to capture the stress concentration). to accurately capture the stress concentration (a highly localised stress peak, you need more elements than your 2nd model, and smaller aspect ratio.

have you done a Kt calc ? what result are you expecting ??

(why use such a horrible unit ? kgf/mm2 is about dN/mm2, why not Mpa = N/mm2 ?? ... i know, i know ... it's what your company or customer use.

 

[erga]

How can I do this Kt calc in this situation? Why I need square elements? I have almost no experience in FEM, smaller aspect ratio means smaller elements?

Thank you a lot for your attention with me!

 

[rb1957]

"How can I do this Kt calc in this situation?" ... from a book of stress concentrations, like Petersen.

"Why I need square elements?" ... 'cause they are more correct (have less error) than rectangular ones.

"I have almost no experience in FEM" ... in that case learn by learning, not by doing; without knowing the body of knowledge your pictures of model results are just that, pictures.

"smaller aspect ratio means smaller elements?" ... a square has an aspect ratio of 1, a rectangle greater than 1.

maybe you refined the mesh along the side of the part with the fillet. it'd be better to refine the mesh, dividing each element into 4 ... refine the mesh along all sides of the part.

 

[erga]

Im sorry for my lack of knowledge about this subject...
Would you advice me about some good theory or something that can me teach this things better?
Why the square elements are better than the retangular? When we use the others one?
I was looking at the book you said, and at page 160 (3rd edition) we have something like my problem, but that's not exact my problem, how can I use something from there? I was thinking about doing an analogy multiplying the factor by 2, because I have just one curve at my drawing, what do you think about it?

And again, thanks a lot man, you are helping me a lot!

 

[IceBreakerSours]

If you are interested in modeling ONLY, then you don't need to worry about the "why" question. What you do need to pay attention to is that the mesh refinement and quality must be good for stress analysis in Standard and very good in case of Explicit. It would be good to know the answer to the "why" question.

However, if you are interested in finite element analysis itself, then I'd recommend grabbing a good book on FEA and work out the problems - one by one. As convenient, interesting, and helpful they might be, watching videos on YouTube will not translate into learning.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[rb1957]

Peterson 3rd Ed, pg160 ... symmetric shoulder under a moment load ... as opposed to pg 151 loaded by tension ?
i would not factor by two if you're trying to account for your situation being 1/2 of Peterson's model ... i'd use the figure directly, showing the stress concentration of the tension stresses due to the applied bending. i don't think there's much effect due to the 2nd fillet (if the far side was straight, i think the stress concentration on the near side would be the same). model the part as seems fit to you, note how Peterson determines the reference stress.

to understand why square elements are better than rectangular ones, ...
1) get a FEA text, or online resources (MIT opencourseware), or
2) make some models of your own ... use a web 10" by 1", cantilevered at the LH corners, loaded with 1000 lbs shear at the RH end (so the web is in bending). model with 1 (single) element, 2, 5, 10, 40 elements, ... compare the results with what you'd expect from hand calc.

consider swapping in QUAD8 elements (with mid-side nodes)

 

[erga]

Well, I have a doubt about doing this calc, my support is fixed at the bottom side and not at the left one... Peterson determines the reference stress by our classic stress formula, Stress= My/I, and I still thinking that this model couldn't be used as mine, because at my view, when you have 2 bends, the stress due the moment applied will be divided through them, If I have just one, all that moment will make a stress in this only one bend, right?
I have downloaded this videos, and I'm watching them bit by bit =]
And some questions, how would you do this support? (mine) What considerations would you make?
Thanks a lot for your help and attention.