Mesh changing resulted in stress change

Click For Summary

Discussion Overview

The discussion revolves around the effects of mesh size changes on stress results in a finite element analysis (FEA) model of a concrete dam using ANSYS. Participants explore the relationship between mesh density, surface pressure loading, and resulting stress values, addressing issues of stress concentration and singularities.

Discussion Character

  • Technical explanation
  • Debate/contested
  • Mathematical reasoning

Main Points Raised

  • One participant notes that changing mesh density can lead to significant changes in stress results, questioning the logical consistency of this outcome given constant loading conditions.
  • Another participant explains that increasing mesh density should lead to convergence towards a solution, but if results continue to vary significantly, it may indicate a singularity or divergence in the model.
  • A participant suggests that stress singularities or concentrations may be exacerbated by mesh refinement, particularly near boundary conditions.
  • Concerns are raised about a specific section of the model experiencing stress concentration, with a request for methods to mitigate this effect.
  • It is proposed that local mesh refinement is necessary to accurately capture stress values at points of concentration, while also addressing the need to eliminate non-physical singularities in the model.
  • Participants discuss the importance of modeling techniques, such as using rounded corners instead of sharp edges, to avoid introducing singularities.

Areas of Agreement / Disagreement

Participants express varying views on the implications of mesh size changes, with some suggesting that singularities are a natural part of FEA while others emphasize the need to address them for accurate modeling. The discussion remains unresolved regarding the best methods to handle stress concentrations and singularities.

Contextual Notes

Participants highlight the limitations of their models, including the potential for singularities and the dependence of results on mesh refinement. There is an acknowledgment that certain modeling practices may need to be adjusted to achieve more realistic stress distributions.

amirrezaaj
Messages
4
Reaction score
1
HI
I have a problem in ansys that made me confused...I have modeled a conceret dam and meshed it with solid 45 elements...after that I have assigned the available surface pressure on the dam to the model...in another modeling, I changed the mesh size only and analyzed the the model with the same loading conditions...but the results have been changed? why the results are depended to the mesh size in this situation? is there any relation with surface pressure loading and mesh number...?! what should i do...? with kind regards...
 
  • Like
Likes   Reactions: Rajan Kumar
Engineering news on Phys.org
That is normal for a finite element model. Changing the mesh density can help you figure out if you have any singularities. As you increase the mesh density the result should change less and less each time as it converges on a solution. If the results never stop increasing or decreasing, then there is a singularity at one of the nodes and the solution is divergent. There should be plenty of papers on the web over "convergence analysis."
 
Thanks for your regards dear friend...But there is a point that the mesh change that I mentioned, affects the results considerabley...for example when the number of the elements in the model increase about 2 times in the dam ansys model,the stresses in the model increases about 4 times... Also, when some elements in the model refined in mesh size in one location, the results increase 2 time...I don't understand why this happen in my model since the loading condition is the same in both models...this amount of incease in the stress s value is not logical...
 
It's probably a stress singularity as it get worse with mesh refinement, or a stress concentration near a boundary condition that is breaking the model. So it may or may not be important.

Take a convergence plot at several nominal locations away from boundaries, see how those results are affected.
 
Thanks a lot chris...
I had a section in my model that was wncountered with stress concentration and i excactly want to control and read the stress in this section...this section has a low thickness and is connected to another part that is considered as a constrain for the mentioned section...i check this section and see that changing element size in this section resulted in stress increase...now how can remove the effect of stress concentration in this section chirs...? is there any special method or trick in ansys to reduce the effect of stress concentration...?? thank u some much for your kind regards...
 
amirrezaaj said:
I had a section in my model that was wncountered with stress concentration and i excactly want to control and read the stress in this section
...
is there any special method or trick in ansys to reduce the effect of stress concentration...??


Since you want to know the stress at the concentration, you can't use any tricks to get rid of it. You have to locally refine the mesh until the stress stops increasing much.

However if you have a singularity, that's not physical and you must get rid of it to see the real stress. For re-entrant corners, use their actual radius, don't make them sharp. Also watch out for other discontinuities like the edges of fixed faces - these may need to be radiussed too.

Be aware that singularities aren't a fault in FEA, they're the software trying to model something that cannot exist in the real world. If you approach it in the real world, the stress really will approach infinite, just like the model says.
 
Thank u so much for your kind regards...
 

Similar threads

Confidence in FEA stress values?
  • · Replies 9 ·
Replies
9
Views
4K
Meshing a multi body part as shown below (ANSYS)
  • · Replies 1 ·
Replies
1
Views
3K
Curved Mesh on Symmetry Boundary in ANSYS Maxwell 3D
  • · Replies 2 ·
Replies
2
Views
4K
Automotive Topology optimization of an engine's cylinder block
  • · Replies 14 ·
Replies
14
Views
2K
Problem with the friction model in an Abaqus simulation
  • · Replies 6 ·
Replies
6
Views
4K
Meshing & connection issues for a beam/line solid
  • · Replies 1 ·
Replies
1
Views
3K
Why are the stresses not converging in my Ansys plane stress model?
  • · Replies 4 ·
Replies
4
Views
4K
FEA meshing - why not 2d mesh -> 3d mesh ?
  • · Replies 4 ·
Replies
4
Views
13K
ANSYS Workbench solution problem
  • · Replies 1 ·
Replies
1
Views
10K
Abaqus: write surface mesh element detail
  • · Replies 1 ·
Replies
1
Views
3K