Using Cosmos FEA (Shells) for ASME Section VIII Div 2 Pressure Vessel 1

[greauxpete]

Hello,

I am trying to use Cosmosworks FEA to analyze a pressure vessel using shell elements.

The vessel R/t ratio is 150. The I-beam thickness is also "thin" compared to the width and height R/t = 15.

Am I correct in using shells for this analysis?

The vessel includes only internal pressure and vertical and lateral acceleration loads (wave action on ship).

In Cosmosworks you can output Stress Intensity for:

1. Membrane Stress
2. Bending Stress
3. Top (Bending + Membrane)
4. Bottom (Bending + Membrane)

My question has to do with classifying the Stresses per ASME Section VIII Div 2.

The code says my material is as follows:

Sy = 38 ksi
Sm = 20 ksi


The code mentions:

Pm = General Primary Membrane Stress < kSm = 1.2*20 = 24 ksi
Pl = Local Membrane Stress < k*1.5*Sm = 1.2*1.5*20 = 36 ksi
Pl+Pb = Prim Memb + Prim Bending < k*1.5*Sm = 36 ksi
Pl+Pb+Q = Primary+Secondary Stress Intensity < 3*Sm = 60 ksi

I can output Membrane Stress (Only) in Cosmosworks so I
assume this is "Pm". Is this correct?

If I had a membrane stress (say: around the knuckle radiuus) that exceeded k*Sm could I assume this to be a "Pl" Local Membrane stress and compare that stress to 1.5*k*Sa = 36 ksi?

I can also output Membrane + Bending Stress in Cosmosworks so I assume this is "Pl +Pb" (Prim Memb + Prim Bending).
Is this correct?

My maximum membrane + bending stress is 39 ksi.

In my model, I have a membrane + bending stress in the area of the knuckle radius but this high stress goes away at approximately 34 ksi.

According to the code the allowable for membrane + bending stress is: 1.5*k*Sm = 1.5*1.2*Sm = 36 ksi
So I would be okay here - right?

Also in my model, there is a high stress near a discontinuity where a gusset ties the legs to the lower vessel head. There is a 39 ksi maximum membrane + bending stress that occurs at the gusset head interface. The stress is extrememly local and goes away at 39 ksi.

Since this stress occurs at a discontinuity, can the stress be classified as Pl+Pb+Q = Primary+Secondary Stress Intensity? Which has an allowable of 3*Sm = 60 ksi?

Since this stress is local and at a dicontinutiy it would only be considered for a fatigue situation?

Am I thinking correctly?

 

[corus]

You are correct in using shells though your definition of primary stresses isn't strictly correct as it also depends on location. If my memory serves me well, ASME has a diagram of a pressure vessel which gives examples of stress classification as to location and type of loading. Stresses at a discontinuity are classed as secondary, those at a notch as peak. All stresses should be considered in a fatigue situation. Peak stresses are merely excluded from the primary plus secondary stress limits.

corus

 

[greauxpete]

corus,

Thanks for the advice.
What section of ASME is the diagram?
I looked through it and did not see a diagram fo a vessel,
but I did see a table that list examples of stress at different locations on the vessel. I assume this will serve the same purpose. I woul dlike to see the daigram you are talking about though.

Thanks Again,

Steve

 

[jte]

Steve-

I strongly suggest you seek mentorship. The problem you are dealing with is something which requires experience in vessel design and analysis, not just a SolidWorks training class. Read the Foreword to Div. 2.

jt

 

[greauxpete]

My boss is a PE and he checks my work.
He has 30 of experience with the design,
fabrication and testing of ASME vessels.
However, we occasionally run into a situation
where an FEA analysis is required. The ASME
code is not very helpful (in my opinion) with
dealing with stresses reported in FEA models and my boss
does not have much experience with FEA. His experience is
limited to the closed form methods in ASME.
I wish Cosmosworks had a class that addressed ASME Code.
Can you reccomend some reading that addresses Cosmos and
ASME code? Classifying the stresses seems really complicated and subjective.

I am only trying to educate myself on tis subject.

 

[TGS4]

For starters, I would recommend obtaining and reading WRC Bulletin 429. I provides a good description of the linearization for 3D FEA. As far as classification goes, you are right - it is very subjective. Unfortunately, there is no way around that - I would recommend reading the "Criteria of the ASME Boiler and Pressure Vessel Code for Design by Analysis in Sections III and VIII, Division 2" document published by ASME (if your boss has 30yrs experience, then he should have this...).

Just out of curiosity, if your boss doesn't have experience (and expertise) with FEA for pressure vessels, would this put him out of his area of expertise from the PE perspective? Just something to think about...

Oh, and I'll give the answer that I've given in the past - this topic is something that many engineers have spend (and made) their careers on - don't expect to find the answers overnight, or in a packaged piece of software. I find jte's advise most appropriate.

 

[corus]

greauxpete,

I may be mistaken about the diagram in ASME VIII, it may have been in ASME III (some nuclear code), I'm just going by memory. The table in ASME VIII should be enough guidance though. There is a similar table in the british standard BS5500 (or whatever eurocode it is now).

Unfortunately it is very much subjective and hence the reason why FE codes won't have any means to classify stresses, so's you don't have to fink. Unless the location is very well defined in the codes then err on the pessimistic and choose a lower limit, ie. instead of secondary classify the stress as primary membrane plus bending, with the lower limit.

corus

 

[Mech151]

>I wish Cosmosworks had a class that addressed ASME Code.

I wish cosmos (ANSYS, Abaqus, etc) had a class on how to perform FEA, because they don't. They will show you how to use the software, but the two skills are unrelated.

I just mention this as I have seen many people (engineers and managers) who don't know there is a difference.

 

[rmartin00]

greauxpete,

We do a lot of FEA design of pressure vessels using Cosmosworks (and Geostar), using both shell and solid element models. As TGS4 alludes to, there is a lot to learn on the subject, but here are a few pointers that we follow and may be helpful for you:

1. Meshing with solid elements is typically easier, but membrane and bending can't be separated out (as with shell elements). That's where WRC 429 comes in handy with methods for linearizing the stresses in solid models.

2. Membrane stresses near discontinuities are typically classified as local, and thus are subject to the 1.5Sm (or 1.8Sm in your case) limit. There may also be bending stresses, which are typically classified as secondary, thus you will also have to check that P+Q (max of top or bottom) is less than 3Sm. Note that you only get the 20% increase for primary stresses.

3. Bending stesses are typically classified as secondary unless they are in a flat section (flat head or crown of dished head). In these areas, top and bottom (for shells) is your PL or PM+PB classification, limited to 1.5Sm.

4. General membrane is typically found "away" from discontinuities. At these locations, you should see the membrane value is very close to the top and bottom values.

5. Be very wary of picking values at one node and calling it the max stress. Imagine applying a force to 4 nodes 90deg apart around a nozzle opening (see points ABCD in WRC 107); where do you think the high stress will be? Yep, at those 4 nodes. But look at the adjacent nodes, chances are the stress attenuates rapidly to a much lower (and allowable) value. Choosing the average stress of the nodes surrounding this "point" node IMO is more accurate. Remember, FEA is an approximation.

6. Lastly, note that I use "typically" quite frequently. You will find that there are many different scenarios where these tips might not apply, hence back to TGS4's post.

Hope this helps.