some questions regarding the buckling analysis(5.4 of ASME VIII-2)

[YuJie_PV]

hi all experts,

i am looking at para.5.4 of 2023 asme VIII-2, and have some questions regarding the buckling analysis, please shed me some light:

1. "if the applied loading results in a compressive stress field within the component, buckling may occur, and an evaluation in accordance with 5.4 may be required." such statement is mentioned again and again in part 5, but how to determine if there is a compressive stress field? look up the principal stress for negative stress in FEA software like ANSYS?

2. step 2 of method A indicates that "each component’s loads shall be multiplied by its dominating eigenvalue", i perform the eigenvalue buckling analysis for the components ( a cylinder with two heads) in assembly , the eigenvalue from ansys is for the assembly. it's not component-specific, how come i get the eigenvalue of each component ? must the eigenvalue buckling analysis be performed for only one component in a single time? if yes, such analysis must be performed for 3 time in my case, and i think the method is quite hard to apply in reality.

3 . how to "extract the equivalent membrane stress at the mid surface for each component."? is it a linearized stress which shall be extracted by creating a path in ANSYS?

4. i think the rules in para. 5.4 for buckling analysis is so complicated, if possible i would rather choose the the rules in part 4 of ASME VIII-2. could i only use the formulas in part 4 for protection from buckling failure while all other failure modes still be considered per clauses in part 5?

thanks in advance, any reply appreciated.

 

[TGS4]

1. That's for you as an engineer to figure out how to detect compressive stresses. You could plot directional stresses (hoop, longitudinal) or you could plot the max, mid, and min principal stresses. Engineer's choice, really.

2. You will need to request a fairly large number of eigenvalues/eigenvectors to get the ones for each component.

3. Yes, the membrane stress is obtained from a linearization.

4. My opinion is that the difficulty of the Part 4 rules and the complexity of the 5.4 Method A rules are equal. If your geometry and loading is suitable for the Part 4 rules, then I don't think that there should be anything stopping you from using the Part 4 rules in lieu of the Part 5 rules.

 

[YuJie_PV]

thanks for your clarification, @TGS4. still some enquiry regarding point 1&2.

1. let me take the stress state in shell under internal pressure as an example. such state is familiar to all engineers. i plot the linearized min principal stress in the shell removed from discontinuity, and find the min. principal stress still display negative ( absolute value is small) which indicates the presence of the compressive stress field, which hints a buckling analysis is required per ASME rules, which is conflicting to empirical practice.

i am curious if there are any rule of thumb which could be used for a rough estimation to judge if time to trigger the buckling analysis, something like a stress limit?

2. @TGS4, could you elaborate on " fairly large number"? could the eigenvalue for the whole assembly (a shell with two head) be used as the "dominating eigenvalue" which to be multiplied with "each component’s loads"?

Thanks in advance, any reply appreciated.

 

[TGS4]

1. That is the through-thickness stress - entirely predicted from thin-shell theory: the negative of internal pressure on the inside and zero on the outside. This will not lead to buckling. The focus is on hoop and meridional directional stresses. For example, in a torispherical head, under internal pressure, the hoop stress at the knuckle is compressive - this can and does lead to a buckling failure (you can see this in the design-by-rules for heads - knuckle buckling). So, it's not a stress limit, it's using your engineering judgement regarding which compressive stresses can (potentially) cause buckling.

2. Fairly large means enough to observe a buckling mode shape in each component. No, "the eigenvalue for the whole assembly", which I take to mean the first eigenvalue, cannot be used for all components. You need to find the eigenvalue for each component.