ASME vs FEA 1

[rmerlob]

I tried posting this yesterday and somehow it just didnt get posted, here it goes:

I posted this on the autodesk forums:

So, im trying to compare results from calculating a torispherical head according to ASME VIII with the model dimensions, with an 8 mm thickness the ASME calculation validates it to 250 psi, running Inventor FEA doesnt, Im doing a symmetrical analisys for 1/4 of the head, I get a stress of 334.5 MPa .

Material is A516 gr 70, 260 MPa YS, 485 UTS, since its over 70 ksi UTS , ASME recomends allowable stress 20000 psi for their formula (see spreadsheet attached)

I would expect FEA to actually predict what SF ASME is going for with the formula but since Im getting a stress higher than yield, something must be up.

Any insights?

EDIT: simulating the entire head with a fixed constraint at the bottom head gives the same results as the 1/4 head, 351 MPa max Von Mises

Link:

http://forums.autodesk.com/t5/Autod...nd-Inventor-FEM-results-analisys/td-p/3281429

Discussion at that forum practically concluded that fea is not giving inaccurate results, but somehow, ASME code clears this head for 250 psi while FEA doesnt

So could anyone check the spreadsheet over there and comment?

Is hard for me to believe that ASME code will allow for yielding in a pressure vessel head, yet i cant see where im wrong.

Thanks

 

[vpl]

This would probably be better posted in forum790 as on that forum you will get people that use Inventor while people who read this forum could be using a number of different programs. If you do decide to post over there, come back here and either red flag this post and ask for it to be deleted, or post a reply linking to your new thread. The thread number can be found directly under the title and is in the format "threadxxx-xxxxxx". Note that there is no space after the word thread.

Sorry I can't help further, but I don't use Inventor.

Patricia Lougheed

******

Please see FAQ731-376: Eng-Tips.com Forum Policies for tips on how to make the best use of the Eng-Tips Forums.

 

[rmerlob]

Im sorry if im being rough but did you read my post?

Im asking if someone could check THE SPREADSHEET on that forum, it relates only to asme code calculations. All of the FEA/Inventor stuff is already checked in different software and by people who do use Inventor, I want someone with ASME BPVC knowledge to chime in with their opinion.

Thanks for your response though.

 

[TxAg78]

rmerlob-
The calculations in your spreadsheet look correct to me. I added another equation to calculate the required thickness for the 250 psi pressure. The result is t=0.3149. That's a good sign.

After looking at the images of your Inventor results (and reading the other forum thread), I'm curious:
Are you trying to analyze this problem with ONE Tet element thru the thickness? If so, I think that's your problem. One element thru the thickness isn't going to capture the displacment and stress distribution for most problems. I recomend no LESS THAN 3 elements thru the thickness.

I did a quick analysis (using axisymmetric elements and another analysis code). I put 5 elements thru the thickness. I don't get anywhere near 335 MPa (48,500 psi). My analysis shows 13,435 psi (~92.6 MPa). That's consistent with ASME allowables. See attached PNG for the stress results across a cross-section of my model.

Now, caveat emptor. I did this in my easy chair while watching a basketball game. So, it's possible there's an error. However, you definitely need to refine your mesh and see how the stresses change.

 

[TGS4]

I'm going to agree with TxAg78; that is a poor excuse of an FEA. Something tells me that I wouldn't be surprised that those are linear tets.

Why are you doing the FEA, again? Why are you not doing a 2D-axisymmetric?

Note that when you finally evaluate your FEA, I would recommend that you follow the rules in ASME Section VIII, Division 2, Part 5.

 

[TxAg78]

rmerlob-
Something's still bothering me about your FEA model. Like TGS4, please, please don't tell me those are linear tet elements (eg tet/4). Generally when a mesh is too course (either due to mesh density or element type), the structure is too stiff, and the displacements and stresses are too low. Your stresses are WAY to high. So, the issue is more than just a problem with mesh density and/or element types. Also, the FEA results should show smooth axisymmetric bands. Yours clearly don't. This is another sign there's aproblem with your FEA model.

I realize this is mostly an intellectual study to see how FEA results compare to Sect-VIII, Div-1 hand calculations. It's safe to say that ASME Div-1 equations are conservative, and won't create a design with primary stresses above yield. Since your equations appear to be correct, assume the error is in your FEA analysis. Where exactly, I don't know. But you shouldn't see that magnitude of difference between the two. So, now this an opportunity for you learn how to do FEA analysis correctly.

Things to check:
1) Since you're converting between in-lbs and SI, make sure all Inventor inputs are correct.
2) Check your boundary conditions!!! The Inventor reoport lists 3 sets (good), but doesn't indicate the type. The each plane should only restrain the normal displacement. Also, check the ractions. You should be able to hand calculate the total force on the section and compare to FEA results.
3) Check the length of the cylinder away from the head. You need to provide enough distance so your boundary conditions don't influence the head response.
4) Check FEA stress components to see if you have the expected stress response. For example, in the cylindrical section the hoop stress should approach PD/2t, and the axial should be about 1/2 of that.
In addition, you would expect PD/4t in the center of the spherical section of the head.

I'm sure there are other things to check, but that should keep you busy for awhile.

 

[rmerlob]

Thanks for your responses,

I believe the order of the tet elements used in Inventor is higher so from what I've read they should be able to model this stress scenario with one element thru the thickness, I ll check anyways

About the stress distribution not being smooth I believe thats because the color bar is set to discrete sections not smooth changes, but I'll check that too

All in all you guys have mentioned good things to consider I'll do it when I have some time to spare and report back.

Thanks

 

[TGS4]

Just as a note, one element through-thickness (tet, brick, whatever) regardless of whether or not it is linear or quadratic, will give you an incorrect result.

You are trying to simulate a through-thickness stress distribution that is, at best linear, and at worst, strongly nonlinear. My default is to start with no fewer than 3 quadratic bricks through-thickness (that gives you 7 nodes through-thickness - 6 linear bricks through-thickness will give you similar results), and to increase that mesh density where I expect high stress gradients.

Unless I am completely stuck with an impossible geometry (has happened about two, maybe three times in the last 10 years), I avoid tets like the plague. You simply never know how many you will get through-thickness. And with our good friend Murphy, you know that where the mesher gives you fewer elements through-thickness, that's exactly where you'll really need them.

 

[JStephen]

It is possible that if you do your analysis to the nth degree of perfection, that you won't be matching the ASME designs very well, anyway- don't assume it's YOUR analysis that's off. I was thinking those head equations were around a long time before good analysis methods were.

 

[fegenbush]

I haven't even looked at your calculation or FEA result, but I can tell you that and ASME F&D head generally does not hold up to rigorous analysis. From what analysis I have done, the knuckle buckling will be the failure mode. This can be more easily calculated using Section VIII Division 2 or API 579 (ASME FFS). This is one of the reasons that ASME F&D heads are not used on Division 2 vessels.

 

[rmerlob]

Thanks for the responses,

Inventors simulation is quite limited and Im quite sure you cant change element type, so Ill do it on another package when I have time, If youre interested in more info the thread over at autodesk is still alive.

Im sorry english isnt my first language what do you mean by an F&D head?

 

[TGS4]

Ok - your posts have intrigued me enough to actually run this as an analysis (quite the feat, I might add, so kudos to you). Using the dimensions and loads that you provided (L=32.48in, r=3.15in, t=0.315in, P=249.5psi), I ran a 2D-axisymmetric analysis.

My stresses had a similar pattern to yours. However, my peak stress was 53,730 psi(370.5MPa) - higher than yours.

That's not the full story, though. In order to determine the acceptability of the stresses, you need to use the methodology presented in ASME Section VIII, Division 2, Part 5.

So, if I create a SCL at the location of maximum stress, I calculate local membrane stresses of 29,726psi, and a maximum membrane-plus-bending stress of 52,523psi. (Note that stresses in excess of yield do not invalidate the analysis and evaluation method).

The maximum-permissible local membrane stress is 1.5*S, or 30,000psi. You just barely squeak by, but still OK. The maximum permissible membrane-plus-bending stress is 2*Sps, which is the larger of 3*S or 2*Sy. Assuming that your head is at room temperature, then Sy is 38,000psi, and Sps is 76,000psi. The calculated value is well below that.

So, in summary, the hand calculation and the FEA match up exceptionally well. I guess that we can add this to the large body of evidence that the Appendix 1-4 calculations work.

A couple bits of free advice:
1) Never model a component with the boundary condition at the end of the component (such as the head). Always leave a minimum of 5*sqrt(r*t) at the end for a straight cylinder to accurately capture the discontinuity stresses.
2) Use at least 5 nodes through-thickness to capture the membrane, bending, and peak values of stress. Always do a mesh discretization study to ensure that you have enough elements through-thickness - the value of stress asymptotes to the "true" answer "from below", so more elements will generally leave you with higher stresses.
3) The interpretation of FEA stresses to the ASME Code is a science in and of itself. I've spent the last 15 years doing it, am involved in the ASME Code Committees myself, and I learn something new every day. For starters, read ASME Section VIII, Division 2, Part 5. Read ASME PTB-1. Read WRC-429. Read as many papers as you can on the topic.
4) Come back to eng-tips if you have any more questions. We're glad to help.

 

[rmerlob]

Thanks thats probably the answer that was needed, I'll be sure to read ASME Section VIII, Division 2, Part 5 when I get access to it

In the mean time:

Could you maybe explain in words what's the principle behind ASMES's method of evaluating FEA results, i mean why's equivalent stress not adequate?

Also, what info can I get from the fact that the head just "squeaks by" when evaluating maximum permissible local membrane stress, and its way safe when evaluating maximum-plus-membrane?

In another words, what could we interpret as ASME's intended ''safety factor'' if you will.

 

[LSThill]

rmerlob (Mechanical)

PLEASE READ PART 5 OF ASME PTB-3 VIII-Division 2 Example Problem Manual American Society of Mechanical Engineers

DESIGN BY ANALYSIS REQUIEMENT PAGE 5-1 to 5-59

L S THILL

 

[TxAg78]

TGS4,
Thanks for running the analysis. I reviewed my quick & dirty (and WRONG) model, and found a dimensional error. However, after correcting, I'm still off (SIGE = 43.6 vs your 53.7 ksi). That's not "close enough" in my book. I ran several reasonable mesh densities, and only see a very small change in results. So, I'm scratching my head (thinking I still have an input error).

Can I verify dimensions used:
t=0.315in (constant thickness)
L=32.48in (vessel OD and hemi-head inside radius)
r=3.15in (knuckle inside radius)

Thanks.

 

[TGS4]

I used:
t = 0.315in (constant thickness)
L = 32.48in (crown IR)
r = 3.15in (knuckle inside radius)

The resulting vessel IR is 18.782in (I didn't specify it, I just specified the crown inside radius, a constraint that the top of the crown was perpendicular to a vertical line, tangency to the knuckle inside radius, and then tangency to the vessel wall, which is constrained to be vertical). As I mentioned above to use 5*sqrt(r*t) for a straight length of the vessel - so I ended up using 15in.

I also used E=30e6 psi and nu=0.3. P=249.5psi.

 

[TGS4]

Could you maybe explain in words what's the principle behind ASMES's method of evaluating FEA results, i mean why's equivalent stress not adequate?

The criteria are very well explained in ASME PTB-1.

Also, what info can I get from the fact that the head just "squeaks by" when evaluating maximum permissible local membrane stress, and its way safe when evaluating maximum-plus-membrane?

The reason that there are essentially two different answers here is that we are dealing with very different failure modes. When one evaluates the membrane stresses (and local membrane stresses), you are dealing with the global failure mode of plastic collapse. There are margins in the Code that are specified against this failure mode (typically 1.5 against yield or 2.8 against ultimate for VIII-2 or 3.5 against ultimate for VIII-1). These margins are well documented (and modified with time) since the ASME Section VIII Code was issued.

When one evaluates the membrane-plus-bending stresses, you are dealing with the failure mode of ratcheting (incremental plasticity every cycle that accumulates and does not shake down to repeated elastic action). This failure mode needs to be protected against for two reasons: 1) ratcheting will eventually lead to loss of shape and exhaustion of ductility and eventually rupture, and 2) shakedown to elastic action is required to perform a valid fatigue analysis.

There are additional failure modes that need to be considered, including buckling and "local failure" (which is caused by high local triaxiality and is the failure mode that underlies sharp notches (among other things)). Of course, there is also fatigue itself that has to be included in the evaluation (if the loads are cyclic).

As you can see, using FEA for pressure vessels is not as simple as comparing an equivalent stress to an allowable. It never was, and it never will be. Please be sure to share with your friends over on the Inventor that FEA for pressure vessels is extremely complex and should only be attempted by engineers experienced with not only FEA, but with the ASME Code, as well. Remember that any FEA code is just a tool, but it takes a well-trained and experienced engineer to properly use that tool. As an analogy, it doesn't matter if I use hand-held screwdriver or a cordless, high power, drill, if I use it wrong, then it's wrong.

 

[TxAg78]

TGS4-
Thanks. It's scary, when I used your dimensions above, I get a maximum VonMises stress of 53,706 psi. Way too close to your answer! Almost makes me suspicious.

So, I'll show my ignorance of torishpherical heads (something new, which intrigued me to begin with).

It seems (to this naive observer) that one can fit a given head and knuckle radius to most any vessel IR (assuming IR < (L+r)), and still meet the tangency requirements. No?

 

[corus]

The results from the FEA are obviously wrong. You just have to look at the contours to see that the mesh is inadequate. Never use tet elements as they generally give rubbish answers, particularly in bending. For that model you'd have got good answers using quadrilateral thin shell elements where the bending is linear, and the model would have been easy to develop.

 

[jharris3]

You can also consult thin shell theory.