FEA on ASME Section VIII division 2

[DG4]

Hi,

I'm a mechanical engineer that designs ASME Section VIII division 1 vessels.

There is a situation at the facility I'm working and I would like to have some advice/opinions on how to address the issue.

The production staff wants to use an existing nozzle on a tank in a way that would cause external loads on it. Nozzle was not designed for those loads in the first place.

WRC and FEA tools in COMPRESS both shows that loads are too high on nozzle. No pad would solve the problem.
I'm now considering adding stiffeners on nozzles. Since this configuration can't be pocessed thru Compress, I'm considering making an elastic analysis as per ASME Section VIII division 2.

Below is my methodology.

Software we usually use is Solidworks Simulation with Pressure Vessel linearization tool.

Model: Nozzle is a double fillet welded as per fig UW-16.1(i). The FEA model represents exactly the assembly, welds, gaps between parts, with no fusion between parts that are not fully penetrated. This model as expected causes increasingly high peak stress in local discontinuity areas.

Fatigue: This is an occasional, non cyclic loading. Fatigue evaluation is excluded(will have to be agreed with my AI).

The point is, since fatigue will not be evaluated, Model will be evaluated only for plastic collapse and local failure. My intention is to check model convergence for membrane stresses and bending and disregard incrasing peak stress at the local discontinuities.

So I would do the following steps in order to check model and results.

1) Make the FEA model.
2) Run a first analysis with a unrefined meshing.
3) Select SCP and linearize through the correctly selected SLCs.
Note the general membrane stress, local membrane stress, and bendings.
4) Refine the mesh, run analysis, note stresses
5) Repeat until verifying convergence (Disregarding local peak stresses)
6) Run final analyses, combine loadings, compare with allowable stresses.

So, I would like to know, is my assumption to disregard peak stresses acceptable if fatigue need not to be evaluated?
Moreover, the software I use only creates tetrahedral elements. Is there a limitation in ASME codes that prevents the use of those elements?

 

[fegenbush]

I have found that the simpler solution can be the more cost effective one. In this case, that would mean adding an expansion joint to the piping attached to the nozzle in question. This cuts down on the engineering time paid for by the client and avoids an R-Stamp on the vessel. If there are other circumstances which negate this option, please let us know so we may provide an additional option.

 

[DG4]

Hello fegenbush.

Thanks for your reply. Even if there would be workarounds for solving this problem by other means, I would like to take this opportunity to know if my understanding of ASME section VIII division 2 linear analysis is correct. It is a problematic for my own company, with no major cost/time limitations, so I think the timing is right.

And FYI, I would also make a hand calculation for weld strength, and a WRC 107 calculation using modified Inertia of new section made by pipe with stiffeners.

 

[TGS4]

First off, welcome to eng-tips.

There is no inherent problem with tetrahedral elements (unless you're using linear tets - you're not, right?). The important thing is to ensure that you consistently have at least 5 (7 or more is even better) nodes in the through-thickness direction.

I will caution you that, based on my experience, the built-in linearization tools in most software are not compliant with 5-A.4.1.2. If you are doing this as a learning experience, I would recommend that you perform the linearization yourself.

Be careful with how you categorize the various stresses.

I have an article that I wrote about using FEA to satisfy U-2(g) for a Division 1 vessel. It's good that you have dealt with fatigue. You still need to consider ratcheting and buckling (at some point, your vessel will likely have a vacuum condition that will need evaluation).

Your approach for achieving convergence seems appropriate. Good on you for considering that - it's a critical aspect that many engineers miss.

Feel free to come back here with questions.

 

[tankman64]

Have you tried rerunning your pipe stress using the flexibilities from the FEA in order to reduce the loads? I find this works in about 90% of cases.

 

[DG4]

TG4,

Thanks for your article about using FEA to satisfy U-2(g) for a Division 1 vessel.

One point you indicated in this article is that "The allowable stress for all product forms except bolting needs to be from Section II, Part D, Table 1 and Table 1A (i.e. the allowable stress for Section VIII Division 1 construction)."

I fully agree that using those values fits with the “as safe as” the rules otherwise provided in Section VIII, Division 1 requirement.

However, I would like to know if there is an official document, code case or other, stating ASME recommendations on the matter, mandatory or not.

I might very well end up in a situation where the difference between allowable stresses of division 1 and 2 make the difference, and I would like to justify my selection with official documentation

 

[TGS4]

Right now, there is nothing official. There is some work in the Code Committees to codify something (as a supplement to U-2(g)), but it is taking a long time.

There is a bit of engineer in judgement in "as safe as", but what I have written is the current practice accepted by most AIs.

 

[DG4]

Thanks everyone for your help

I completed a few elastic FEA analyses on my double fillet welded nozzle model , starting with the P + L condition.

Results indicated that my maximum stress is in the nozzle wall, next to the inner fillet weld, in the shell longitudinal axis. Stresses are much lower along the shell circumferencial axis.

I suspected that a major part of the stress was caused by the constraint of shell to nozzle. So I ran another analysis and put live loads on nozzle, pressure on nozzle but 0(gauge) pressure inside shell.

The stress results were completely different, much lower, with maximum values not located at the same places as before.

I'm now condiering how to correctly classify this stress.

On one hand, after verification. It is clear that this stress in nozzle wall is due to constraint of adjacent parts. So secondary would be the correct classification

However, on the other hand, this stress on nozzle by shell is indirectly caused by pressure, which is not self limiting.

How would you classify this load.

 

[DG4]

By the way I'm using ASME Section VIII division 2 2010 edition because it was the applicable year when vessel was fabricated.

After reading 5.6 and table 5.6 once again, there might be another way to classify this load.

Shell on nozzle stress may be considered as a discontinuity stress.

 

[jte]

By the way I'm using ASME Section VIII division 2 2010 edition because it was the applicable year when vessel was fabricated.

This is a time to use the latest (2013) edition. You have no oblication to use 2010, and there have been lots of corrections (not "changes") to Part 5.

Consider taking one of TGS4's classes - he seems to know what he's doing.

jt