AnsweredAssumed Answered

Surface stress interpretation

Question asked by Peter MacDonald on Mar 17, 2014
Latest reply on Mar 19, 2014 by Peter MacDonald

Like • Show 0 Likes0
Comment • 10

I am unsure what conclusions to draw regarding the stress concentration in the attached picture.

The picture shows a sectioned view of Von-Mises. The peak stress at the surface region indicated is around 415 Mpa, so about 60Mpa above the yield strength. As can be seen, the stress decreases very rapidly through the thickness of the material, reaching acceptable levels a mere millimeter or so beyond the surface.

The part in question is 12.5mm thick S355.

Considering the material thickness and the acceptable stress just beyond the surface, is this stress really a concern?

How should I conclude the results in this region?

Much appreciated,

Peter

Attachments

Surface stress.PNG89.0 KB

No one else has this question

Outcomes

10 Replies

Shaun Densberger Mar 17, 2014 4:17 PM
Mark Correct
Correct Answer
It's somewhat hard to tell with the image given, but I does look like your stress gradient is on the steep side. However, this doesn't necessarily mean that your high stress values are due to a singularity. Did the stress results in that area converge? Can you provide more information on the model definitions (load, constraints, analysis goals, etc.)? Can you provide more information about the design and its intent? Are you using FEA to help hone in on a good design prior to doing physical testing, or are you trying to avoid any physical testing by using FEA?
Like • Show 2 Likes2
Actions
Mikael Martinsson Mar 17, 2014 4:28 PM
Mark Correct
Correct Answer
Well, it's really difficult to answer your question with the information given, and you hopefully will get some answers from more experienced users, but here's my two cents...

If we assume that the stress has converged, and that the fixtures, loads, contacts, material data, temperature e.tc. is chosen in a way that reflects the reality as close as possible, then you have a stress concentration in this area of your part.

The stress concentration goes above the materials theoretical yield limit of 355 MPa. If this is a linear static simulation, the results above yield are wrong and a non linear simulation is necessary to give your a better answer.

Normally the stiffness decreases when material yields, so the maximum stress you see, 415 MPa, will probably be lower if you do a non linear simulation. The change of stiffness in this limited area, due to yielding, will then cause the flow of forces to move to stiffer areas inside this section of the part.

The main risk with a stress concentration like this is problems with fatigue. If your part experience repeated loading, this area could probably be the initiation zone for a crack that propagates and in the end causes failure of the part.

I recently got a presentation from a customer who had a design with calculated stresses above yield in a very localized area. The conclusion of the simulation result was that it was ok because of the static nature of the load (self weight) and that the yielding was localized. This was a non linear material model and the max stress was above yield but well below UTS.

In reality, some dynamic movements unforeseen, made the part fail in field due to fatigue with cracks forming in the exact area where the stress concentration was predicted.

So in the end it's up to you to decide if your setup and results are believable and if your design is ok in the working environment of the part.
Like • Show 3 Likes3
Actions
- Ugur N. @ Mikael Martinsson on Mar 18, 2014 4:17 AM
  Mark Correct
  Correct Answer
  very helpfull informations, could you look at this post and give your opinion please. Thanks https://forum.solidworks.com/message/416736#416736
  Like • Show 0 Likes0
  Actions
Jared Conway Mar 18, 2014 12:53 AM
Mark Correct
Correct Answer
depending on the loading condition, i'd say that is probably somethign to be worried about rather than ignored like a singularity

check your setup
check your mesh
both look potentialyl suspect before you go interpreting results
Like • Show 0 Likes0
Actions
- Nathan Manio @ Jared Conway on Mar 18, 2014 1:52 AM
  Mark Correct
  Correct Answer
  I wouldn't ignore it either.
  How many elements are across the cross section? Is the mesh refined on the surface or by depth? Are the elements in the region overly distorted?
  
  The area between the nodes of the elements' is a mathematical interpolation based on ideal elements, so it will not be accurate if the elements are distorted.
  Like • Show 3 Likes3
  Actions
Peter MacDonald Mar 18, 2014 5:18 AM
Mark Correct
Correct Answer
Thanks everyone for the input.
How many elements are across the cross section? Is the mesh refined on the surface or by depth? Are the elements in the region overly distorted?
Mesh is only refined on the surface. See attached pic. Admittedly I now see that there are not enough elements in the area, but I don't think they're too distorted.
The stress concentration goes above the materials theoretical yield limit of 355 MPa. If this is a linear static simulation, the results above yield are wrong and a non linear simulation is necessary to give your a better answer.

Normally the stiffness decreases when material yields, so the maximum stress you see, 415 MPa, will probably be lower if you do a non linear simulation. The change of stiffness in this limited area, due to yielding, will then cause the flow of forces to move to stiffer areas inside this section of the part.

The main risk with a stress concentration like this is problems with fatigue. If your part experience repeated loading, this area could probably be the initiation zone for a crack that propagates and in the end causes failure of the part.

Very useful information. I'll try a non-linear simulation. Fatigue is a serious concern with this part. The loading applied in the simulation is a worst case scenario, but there will still be frequent dynamic forces applied to this part.
Did the stress results in that area converge? Can you provide more information on the model definitions (load, constraints, analysis goals, etc.)? Can you provide more information about the design and its intent? Are you using FEA to help hone in on a good design prior to doing physical testing, or are you trying to avoid any physical testing by using FEA?
Hopefully the attached pic gives a better view of the area in question, now that I've removed the section plane. The thick gussets have not been quite as beneficial as I'd hoped!
As much as it will pain you to hear, we do not plan to do much physical testing with this part. Therefore I need to be fully confident that the design is suitable. An appropriate safety factor has been considered. With regards to the design intent, as said above it will need to withstand frequent and potentially significant dynamic forces. Around 115kN is being transferred through the member indicated in the picture. As a very rough guide, what we want to see is no stress higher than around 220 Mpa.

So I need to:
- Refine mesh through the thickness
- Try a non-linear study
- Check that the stress in the area is converged
Many thanks,
Peter
Attachments
- Mesh.PNG101.3 KB
- Fixtures.PNG53.4 KB
Like • Show 0 Likes0
Actions
- Peter MacDonald @ Peter MacDonald on Mar 18, 2014 8:22 AM
  Mark Correct
  Correct Answer
  Another quick query whilst I'm here.
  
  In the attached pic the curved surface has a mesh control applied.
  
  Why might singularities develop at the edge of a mesh control? I understand their occurance when re-entrant corners are involved, but not here.
  Attachments
  - Singularities.PNG381.0 KB
  Like • Show 0 Likes0
  Actions
  - Jared Conway @ Peter MacDonald on Mar 18, 2014 10:24 AM
    Mark Correct
    Correct Answer
    You have a sharp model edge there too. So if it is being torn in either direction could develop a singularity. Improve the mesh. Really dependent on loading.
    Like • Show 0 Likes0
    Actions
- Mikael Martinsson @ Peter MacDonald on Mar 18, 2014 2:19 PM
  Mark Correct
  Correct Answer
  I'm not sure if i interpret your pictures correctly, but your picture "fixtures.png" says "fixed rear face". If you mean that the complete face is fixed in all degrees of freedom this is not a very realistic boundary condition. It's similar to the part being surface-glued or surface-welded to a perfectly rigid wall.
  
  In your other picture "singularities.png" it looks to me like the high stress is in this area where the radius meets this perfectly fixed wall. If this is the case, your boundry conditions probably causes the singularity. The highlighted edge in your picture is the border where, on one side (radius) the part can deform naturally, and on the other side (flat fixed) the part is totaly fixed.
  
  I recommend the approach where you add one "layer" of components to your FEM model to get better stress readings on the part of interest. In this way you capture the stiffness/elasticity of the structure in a better way and also move the unrealistic fixtures to parts where you don't have to care about singularities.
  
  Good luck.
  Like • Show 1 Like1
  Actions
  - Peter MacDonald @ Mikael Martinsson on Mar 19, 2014 4:23 AM
    Mark Correct
    Correct Answer
    Very true, I realise the fixed face is unrealistic. I did however completely forget about that fixture when looking at that singularity! Now I understand it.
    
    I'll probably do as you suggest and add another part to the model to move the fixture away from more important parts.
    
    It may or may not be of interest, but I've managed to improve the design. There's no longer a bend in the part, just gussets welded to a single flat plate. It works surprisingly well. However, I've now got a different problem area to deal with.
    Like • Show 1 Like1
    Actions

Surface stress interpretation

Attachments

Outcomes

Attachments

Attachments

Related Content

Recommended Content