ASME VIII Div 2 Part 5 Elastic-Plastic vs. Limit Load Results

[Russ A]

Hi all,

I seem to have found an unusual situation (from my experience anyway) whereby Elastic-Plastic results are more onerous than Limit-Load and only slightly better than ASME VIII Div 1 hand calcs. I am using ANSYS and have tried many different solver settings, mesh etc. (and have had discussions within ANSYS with regard to the issues I am experiencing) and am reasonably confident that the ANSYS result is what it is and is likely a reasonably reflection of the physical system.

The issue I am having is that the FEA model fails to converge before utilising the full elastic-plastic material model i.e. the material would appear to have more load capacity that is not being utilised, as it fails to converge at about half the plastic strain of the plastic strain at true UTS (i.e. well within the bounds of the material model). Failure is also due to strains in the plain cylinder rather than e.g. a nozzle, where high strains would normally be expected. The pressure at which non-convergence occurs is lower than the pressure at which a limit load analysis fails to converge.

From running various test cases I believe this is related to large deflection being activated for elastic-plastic cases, which it is not for limit load (small displacement theory assumption). My question is that has anyone else experienced this situation (limit-load potentially non-conservative)? Is my interpretation of the code correct, that large deformation (non-linear geometry) does not need activated for limit-load analyses?

The material is A-516 Gr 70, so not exotic, but it does have a relatively high UTS/yield ratio which results in higher than usual (in my experience) plastic strain at UTS (ASME VIII Annex 3D for material model setup), which appears to be contributing to the issue.

Any thoughts or pointers appreciated.

 

[TGS4]

Russ A - please provide more details. What is your ultimate tensile strain (what does your elastic-plastic stress-strain curve look like)? What sort of geometry do you have, with what types of loadings?

In my experience, the only time(s) that I have had an Elastic-Plastic analysis fail to converge, where I expected it to out-perform a Limit Load Analysis, is when there was a state of compressive stresses and the solver was (correctly) detecting a buckling situation.

The Limit Load Analysis is small deformation, by definition.

 

[Russ A]

Hi TSG4.

Thanks for your response. UTS = 410 MPa, 572 MPa true stress. It is a multi-linear elastic-plastic curve in accordance with ASME VIII Div 2 Annex 3-D.3. Yield is 184 MPa. It is a simple vessel with elliptical heads and saddle supports. Two nozzles, close to the heads at each end. The non-convergence (high residuals) occurs at the middle of the vessel, between the saddle supports in the plain cylinder (this has been confirmed with a sub model of just the plain cylinder).

Currently I am only applying internal pressure. I am deliberately applying a high pressure so taking the model well into the plastic region.

"The Limit Load Analysis is small deformation, by definition." - that is how I understood it. But if in the real world large deformation is likely (due to material, loadings) does the Limit Load still stand up? Without running an elastic-plastic analysis the analyst is unaware of the effect of large deformation. I believe in this instance large deformation is resulting in an exponential rise in stresses (due to the interaction of the load with the deformed geometry), which is not captured with small deformation. Of course I may be wrong, but this is what I am currently thinking based on the cases I have run.

In your situation, how did you determine that it was buckling that was being detected? I don't think I have a buckling situation here, but I may be missing something.

 

[TGS4]

I generally detect buckling by looking at the component stresses (or principal stresses). Elliptical heads may have compressive stresses in the knuckle region.

Limit load has withstood the test of time, so I have great confidence in it.

Can you perform a simple cylinder analysis with the EP model and get it to align with the hand calc burst pressure?

 

[Russ A]

I had run a sub model which was effectively the plain cylinder only. The hoop stress is considerably higher for a given pressure than the hand calc hoop stress, I believe this is purely a function of the non-linear geometry. At high strains the radius increases significantly enough that stresses are a lot higher than expected for a given pressure. Further more the elastic-plastic model pressure at non-convergence is only just higher than that used to calculate the ASME VIII Div 1 thickness.

There are high compressive stresses (all principal stresses -ve) at the knuckle, however, the sub model model suggests that the non-convergence is not due to any potential buckling of the head i.e. the plain cylinder sub model (with pressure end loads rather than head modelled) fails to converge at essentially the same load as the full model.

 

[TGS4]

What are your exact dimensions?

 

[Russ A]

579 mm OD, 10 mm wt, 3 mm CA, 2:1 elliptical head, 4500 mm between saddle supports, 6445 overall length.

One thing I should have been clearer about, this is a FFS of an older vessel using API 579-1. Therefore the Beta load factor is 3.6 (M of 4 x RSFa), which means the benefit of using elastic-plastic is reduced (compared to design a vessel to the latest code), since the load factor is 2.67 times higher than that applied to limit-load.

 

[TGS4]

What's your temperature? For SA-516-70 - there is no temperature where the UTS=410MPa and Sy=184MPa. UTS=410MPa @ 450°C, but Sy=184MPa @ 387°C.

 

[Russ A]

I'm not at my computer to check, but I've potentially given you values adjusted by E, but I've also ran E = 1. It's 200degC so no derating if I remember correctly.

 

[Russ A]

Hi TGS4, thanks for your responses so far. Do you have any further thoughts on this?