ASME Section VIII Div.2 elastic and elastic plastic

[shiraz883]

Hi,

I have run an elastic analysis where the stresses were over the allowable stress values at some local zones (where local membrane > 1.5S). So, in order to see whether these stresses redistribute when yielding occurs I have gone for an elastic plastic analysis using the ANSYS plugin ASME material stress strain curve generator using bilinear kinematic hardening material model. Also since I use the shell model fpr FEA, then for local failure criteria I use the maximum, middle and minimum principal stress (for top/bot option in ansys) and combine them [absolute(s1+s2+s3)] using a user defined formulae and compare with 4S but this criteria is also not satisfied (I have seen everywhere in the model).

My questions:

1) Is this approach valid? elastic and then elastic plastic to see if stress redistribute when yielding occurs
2) Is the Ansys plugin using the data from Annex 3-D for material stress strain curve (I haven't checked it myself but wanted to know if someone has already verified)

I know that ASME PTB-1 mentions the methods of analysis in increasing accuracy and decreasing conservatism as elastic---> limit load---> elastic plastic



Shiraz
Sr. Engineer

 

[TGS4]

There is a serious mixing of failure modes here that is quite concerning.

Firstly, you state that you have, in an elastic analysis, "stresses were over the allowable values at some local zones". Although you also say parenthetically "where local membrane > 1.5S". However, the limit on primary local membrane equivalent stress is S[sub]PL[/sub], not 1.5S - can you please confirm that you mean that the primary local membrane equivalent stress is greater than S[sub]PL[/sub] - meaning that the analysis has failed to demonstrate Protection Against Plastic Collapse using the Elastic Stress Analysis Method.

If that is, in fact, the case, then are you saying that you have chosen to use the Elastic-Plastic Analysis Method to demonstrate Protection Against Plastic Collapse? If so, then you should use the full elastic-plastic stress-strain curve for Annex 3-D. I am not familiar with the ANSYS plugin, but if it is using a bilinear curve, then that would be incorrect, in my opinion. It should be a multi-linear curve. This curve would also be used to demonstrate Protection Against Local Failure using the Elastic-Plastic Analysis Method.

For demonstrating Protection Against Local Failure, you may choose either of the Elastic Analysis Method, or the Elastic-Plastic Analysis Method, regardless of the method used to demonstrate Protection Against Plastic Collapse. However, be aware that the Elastic criteria is based on the linearized primary principal stresses. Unless you are in a location where there is primary bending, you would typically only be using the membrane (middle) principal stresses only. Furthermore, you want to maintain the sign of the algebraic sum of the principal stresses, so I would avoid the absolute value in the formula.

 

[shiraz883]

Hi TGS4,

Firstly, I see that the limit on local primary membrane stress is S[sub]PL[/sub] which is large of the two quantities
1) 1.5*S
2) S[sub]y[/sub], except that (1) shall be used if ratio of min. Y[sub]s[/sub] to min. S[sub]u[/sub] exceeds 0.7 or value of S is governed by time dependent properties.

In my case, material is SS316L (UNS S31603 - 16Cr-12Ni-2Mo), for which the ratio of min.S[sub]y[/sub] to min. S[sub]u[/sub] "does not" exceed 0.7 which means I shall use larger of 1) and 2) in which case 1.5S is larger. If the above value would have exceeded 0.7 then I should have used 1.5S without looking at S[sub]y[/sub]. Correct me if I am wrong in this interpretation.
In any case, this limit is exceeded in my elastic analysis.

Secondly, the curve that Ansys gives is a multilinear kinematic hardening curve of the material. I made a typo there in mentioning "bilinear". Instead, it is multilinear.

Thirdly, it is clear now that I should use the algebraic sum (as also mentioned in the code and answered by ASME interpretation number VIII-2-10-08 - whether you call it a code case) and not the absolute value in determining the sum linearized of primary principal stresses. I have primary bending stresses in the model (meaning that bending is not temperature controlled) so I use top/bottom option in ansys in determining the sum and use in user defined formulae.

You are right in mentioning that the elastic analysis fails to demonstrate protection against plastic collapse (local membrane>1.5S) and local failure (algebraic sum of three principal stress). Hence an elastic plastic analysis is used to accurately assess the above criteria.

Is this also the methodology used by analyst in the pressure vessel industry to evaluate the protection against failure modes? I mean to first evaluate the stresses using elastic analysis methodology and compare with the correspondent allowable and if not satisfied, go down the path of elastic plastic approach. And when an analyst does both, how is it justified to the client? I mean there can be a question that why didn't the analyst modified the geometry, say, for example, increase the thickness of a part and re-run the elastic evaluation to see if the computed stresses are within the limits.


Shiraz
Sr. Engineer

 

[TGS4]

All methods listed are acceptable. Generally, the approach is to apply the "easiest" one first - if for you that is the elastic analysis method, then so be it. if that doesn't work, then you are permitted to proceed to the other methods. The final design report would only contain the one that succeeded.

I would note that with respect to the categorization issue, most bending stresses are secondary - Table 5.6 shows primary bending only occurring on flat plates.

 

[DriveMeNuts]

Agreed. There is no need to make the customer aware that an Elastic protection against collapse analysis was ever done.