Mesh size dependance of ASME Div.2 analysis for elastic stress method

[Paulettaa]

Dear all

I am reviewing an elastic stress analysis of legs to shell junction for protection against plastic collapse. The vendor wants to show that the stress results for the analysis are free from mesh size. First he has reduced the mesh size from 100 mm to 50 mm and the maximum stress has increased from 88 MPa to 101 MPa. Then he has reduced the mesh size to 40 mm and the stress increased to 115 MPa. He then has concluded that the stresses are stabilized with respect to the mesh size and the results with this mesh size are reliable. I cannot accept it since he has decreased the mesh size by 20% while increasing the stress by 15%. This does not look like any stability in results. However, I do not have any reference or criteria to tell me what is the reliable answer with respect to the mesh size. Is it 3%? Is it 5%? And this with respect to how much reduction in mesh size?
On the whole, I want to know if there is a remedy to meet this problem. Should I simply shift to elastic plastic method? I have had this problem especially when working with shell elements. Do you think using solid elements would help? And finally I was curious if there were problems using shell elements in elastic-plastic models.

Thanks in advance

 

[marty007]

One resource I've used in the past is AB-520 (Finite Element Analysis (FEA) Requirements Regarding the Use of FEA to Support a Pressure Equipment Design Submission) from the Alberta boiler branch (ABSA).

They discuss the following approach in the section titled Presentation of Results:

Presentation of Results
4) Plot with element stress and copare nodal (average) stress vs. element (non-averaged) stress (If the small difference is less than 5%, the accuracy should be OK);​

Cheers,
Marty

 

[cbPVme]

This seems like too much of a difference between the final two mesh iterations. We typically look for less than 5% change in stress. But where are they measuring the stress? If it's the maximum stress in the model that occurs on a sharp corner, this is a singularity and the stress will perpetually increase as the mesh size is reduced.

You should not have convergence issues with shell elements. If the element size is appropriate, the stresses will converge.

 

[Paulettaa]

When I have solid elements I can handle sharp edges with some fillets with some radius. But I do not know how to remove this issue when I have shell elements where the stresses will not stop increasing by reducing mesh size.

 

[TGS4]

Are you focusing on peak stress or membrane stress in this comparison? The latter is usually all that is needed for Protection Against Plastic Collapse. Also, how close to the limit are you?

 

[Paulettaa]

I am not concerned with peak stresses. Actually I do not understand how peak stresses can be extracted from shell element. I thought the stresses at the middle layer are membrane and at the top or bottom are membrane plus bending and no indication of peak stresses in shell elements. Nevertheless, it does not matter how close I am to the limits since I finally pass the limits by reducing the element size to some enough level.