Stress Linearization (ASME Section VIII Div-2)

[MDKARMD]

Can anyone explain why stress linearization required and how it is doing with ANSYS??
pls suggest any literature for FE Analysis as ASME section VIII Div-2

 

[TGS4]

For the "why", refer to ASME PTB-1 and WRC 429. For the "how", Annex 5-A is self-explanatory. For the ANSYS question, please pose that specific question in the ANSYS forum - however, please be aware that the default linearization scheme in ANSYS is not compliant to 5-A.4.1.2.a).

 

[MDKARMD]

thnks..

 

[Maud35]

that the default linearization scheme in ANSYS is not compliant to 5-A.4.1.2.a).

I looked to ANSYS help, but it did not make it clearer especially about the "2D Behavior".
I wish to "Ignore the thickness-direction bending stresses" but for that I should use "Axisymmetric Straight", which I do not clearly understand. Could you help me on that?
Thanks

 

[TGS4]

Please post a link to the exact part that you are unclear about. And then describe your problem, and exactly what you are unclear about.

 

[Maud35]

Could it become compliant by using “axisymmetric straight” as 2D behavior with “through thickness bending stress” ignore for the non-axisymmetric (due to bolts) 3 D model , as it is mentioned in the help : “These choices are available to any type of geometry (for example, you can choose Axisymmetric Straight for a 3D model)”

(// Mechanical User Guide // Using Results // Structural Results // Linearized Stress)
(// Theory Reference // 19. Postprocessing // 19.4. POST1 - Stress Linearization)

I do not understand what are those different 2D behaviors so I am unsure if it s the good way.

 

[Maud35]

Actually, You wrote that the "default linearization scheme in ANSYS is not compliant", so I was hoping it could become compliant with specific settings, but maybe I misunderstood.

 

[Maud35]

I tried to verify myself, not sure how good it is (I did calculate by components first )
It seems to me and at least for this example that ansys is not doing that bad?

 

[TGS4]

You need to ensure that the bending is calculated using the membrane+bending using the hoop and meridional directions only, and the membrane for every other
component.

The default in ANSYS (and Abaqus) is to use the M+B for all of the components.

You need to do this regardless of whether you have 2D-axisymmetric or 3D.

 

[Maud35]

Thanks for your answers.

Could you explain why is it so important to exclude the bending stress component parallel to the classification line. Isn't it conservative to include all of the components? or what is the reason behind it?

 

[TGS4]

It may not necessarily be conservative to do so. And, the hoop and longitudinal directions are the only ones with physically-meaningful directions for through-thickness bending stress components.