Interpretaion of 3D FEA study with ASME VIII 1

[MarkCopland]

Help..

I have perform a pressure vessel analysis using FEA pro/mechanical (3D solid p-elements, tetra) under pro/e as a cad modeller,

I have obtained some results of the max shear stress in my model (because my vessel is quite thick (r/t = 8) and also it has got some unusual geometry changes that produce stress concentration in this areas.

I can see that every body talk about some topics (as linearization etc), which are not cover in the ASME VIII div 2 in the appendix 4 “Design based in stress analysis”.

I am comparing the stress that I have got in my analysis with the allowable stress from the code, (following the classification of stress for some typical cases Table 4-120.1 form this code):

The level of stress that I have got close to discontinuities are less that 1.5Sm and the Maximum shear stress that I have got in the general body of the vessel (which are not affect for the stress concentration ) I compare with Sm.

Please can somebody tell me, if I am doing wrong my study?…What can I do if a want to perform an study with Linearization using pro/mechanical and then compare the results as you propose?.

What happen with Div 1… if I want to do or to check a design done with a good FEA practice?.

Matteo.
matteo_1234@hotmail.com

 

[bvi]

One rule you always have to follow, both with Div 1 and Div 2, is that you have to satisfy the basic equations for wall thickness that are provided in the Code, regardless of your FEA results. Use FEA for the local details, not for determining the required thickness of general shells of revolution.

 

[cab1990]

Matteo,

First let me agree wholeheartedly with cb4. You should be doing a hand calculation to check your fea. For instance, you can look at the radial stress and check that it equals the internal pressure at the inner wall.

Also, you can check your hoop stress and axial stress away from any discontinuity using thick cylinder calcs. This will go a long way towards assuring your analysis is done correctly.

Finally, when you are viewing a stress distibution from FEA, you will find that near locations where the load path changes direction(for instance, at a change in wall thickness or at a head), the stress distribution will be composed of a membrane component, a bending component, and possibly a local peak component. These must be separated to comapre the FEA results to the code limits. This is why linearization has come into use. Linearization is the only route to decomposing an FEA stress distribution so that you can obtain numbers to check against code limits.

In areas where there is no dicontinuity, the stresses should match your hand calcs and you will quickly realize that no FEA was needed.

By the way, Ansys and Patran both have accurate linearization routines and print out the membrane and bending stress range numbers automatically. Be careful not to include peak stresses in your stress classification line or you may overestimate the bending component. But thats a whole other subject.

Good luck

cab