ASME VIII, Div 2 - Part 5 Design by Analysis

[engpes]

I have a high pressure vessel that I am analyzing per ASME VIII, Div 2 - Part 5 with a design pressure of 10,000 psi. I am using elastic stress analysis method an have a question in regard to the local nozzle analysis.

The nozzle is having high bending + primary stresses at the radius of the base of the nozzle. I am linearizing the stresses across the thickness SCL that produces the highest bending + primary stresses and getting stresses over the allowable limit. I have added a repad to account for the overstressing, and my questions are as follows:

1.) My worst case scenario when linearizing the stresses is the angled hoop / meridonial stress SCL (ASME Figure 5-A.3). Are there any cases / exceptions where the bending + local primary stresses can exceed the 1.5 x Sm allowable limit?

2.) Is it acceptable per ASME to linearize the stresses taking into account the repad thickness?

See attached image to get an understanding.

 

[TGS4]

1. DO NOT use elastic stress analysis in this situation. Please refer to 5.2.1.2, 5.2.1.3, and 5.2.1.4.

2. Even if you did use elastic stress analysis, your SCL is wrong. The SCL in 5-A.3(b) is there to demonstrate the difference between monotonic and non-monotonic ONLY. The location is completely inappropriate (we have an action to revise these figures, but it won't be ready for the 2017 Edition, but hopefully it will be ready for the 2019 Edition) And yet even if your SCL were to be right, what criteria are you using to judge whether or not the stresses are excessive. For Protection Against Plastic Collapse, the limit is on P_L < S_PL. In your location, there is no P_b. Therefore, there is no limit (for your specific Load Case Combination) on the membrane-plus-bending stress. However, for Protection Against Failure From Cyclic Loading: Ratcheting, the limit on the range of P+Q would be S_PS.

3. Judging by your stress plot, your discretization is inadequate. You need more elements in there. I would recommend using quadratic hexahedral elements - in that location I would make sure that I am using a minimum of at least 7 but preferably 7 elements in the through-thickness direction. If your software can't do bricks, but only tets, then mesh the heck out of this, but ensure that you have at least 7 elements in the through thickness direction.

 

[NRP99]

Based on the question and your stress linearization location, I feel you need to understand basics of stress linearization. Just search this forum and google about it. You will get plenty of information about stress linearization which will help you decide the stress linearization location and the stress categorization(P_m,P_L, P_L+P_b and P_L+P_b+Q) at that location. I will recommend to go through following sections and reread it again and again until you get general idea.
ASME Section VIII Div 2 Part 5: Para-5.2.2.2, Para-5.2.2.3, Annex 5-A(Go through all the figures Figure 5.A.1 to Figure 5-A.11. Especially Figure 5-A.11.), Table 5.6, Para 5.12, and Figure 5.1.

If you feel that stress linearisation is providing ambiguous results and you do not trust the classification(which is your case because of thick vessel. For thick vessels, the through thickness stress distribution is not linear but quadratic.), you can completely avoid it by using Para 5.2.3:Limit load analysis method and 5.2.4:Elastic-Plastic stress analysis method, as TGS4 suggested.

 

[engpes]

TGS4:

1.) Yes I understand the R/T<4 so elasto-plastic is required for this case.

2.) If this was a "thin-wall" vessel and the elastic method was applied, there would be no bending limits at this corner. However there would be stresses due to moments created in the nozzle neck/shell wall at this angle. Annex 5-A.3 states that the SCL should be oriented to the normal to contour lines of the stress component with the highest magnitude and references Fig 5-A.3 (a). Am I correct that only the Sps (3.0 x Sm in this case) would need to be evaluated at this nozzle corner for primary + secondary for fatigue / ratcheting? This is a gross structural discontinuity per table 5.6 right?

3.) Yes I know that the mesh is very large. I am still running the rough results before I set up the refined mesh.

Thank you very much for your help!

 

[TGS4]

Regarding 2), the limit on the range of P+Q is indeed S_PS. See my blog post on the topic -

http://becht.com/blog/asme-section-...ic-analysis-discussion-collapse-vs-ratcheting