Looking for Alternative to Stress Linearization for Solid Model FEA?

[croy2]

There has been a bit of discussion of the merits/methods, etc. of stress linearization through a section of interest to extract equivalent membrane and membrane + bending stresses to compare to ASME Sec. VIII Div. II allowable values.

Someone had suggested looking at the stress intesity at both "endpoints" along the stress classification line and getting a rough idea of the true numbers from that. It was correctly stated by another person that there is a chance, albeit small, that such a derivation could be non-conservative.

I was given a program that could reportedly perform this analysis on a 3D structure from Cosmos/M data. I was elated since I am unaware of any software that can do a decent job of this (looking at Algor, Cosmos (only axisymmetric), NE Nastran, and Ansys). I was really disappointed when learning it could only work with Tet4 elements. (Secondary question: should Tet4 elements never be used for establishing bending stress distributions through sections regardless of the number of element layers?)

Does anyone have a conservative (not hyper-conservative) methodology of staying within the Div. 2 membrane/bending guidelines for solid models without relying on stress linearization, or know of a third-party add-on to CosmosWorks/Cosmos that will do the job?

 

[TGS4]

The answer to your first question is rather straight forward - plasticity. See all of article 4-136. A limit-load analysis is all that is required to satify the 1.5*Sm requirements - if the solution converges, then the 1.5*Sm check is met. There is no need to perform any linearization.

To answer your second question regarding tet4 - 4-node tetrahedral elements are (to quote the ANSYS manual) "not recommended".

But I'll ask another question - why bother with this 3rd party program? If your software can output the component stresses as a function of the through-thickness dimension, then you can import that into MathCAD (or something similar - like Excel) and perform the linearization yourself. I use Option 3 from Table C-1 of Appendix C of WRC 429.

That said - PLASTICITY is the way to go - forget about stress linearization.

 

[croy2]

TGS4, thanks for the reply. I'm familiar with 4-136 and the related methodologies outlined at:

http://ped.eurodyn.com/jrc/jrc_design.html

However, the problem is that I've got potentially dozens of different sizes/thicknesses of equipment to design and each of these might require a few iterations. Instead of minutes, I could be talking more like hours in certain cases for non-linear solutions to converge.

In Cosmos, I am unable to get the component stresses through the thickness along a line. I used to use Ansys and seem to recall that when you defined a stress classification line that it took 40+ points along the line to get the stress linearization (lsecplot or something like that was the command). The other problem with Ansys is that the lsecplot command only works node to node. If you happen to have a nice brick mesh through the section then you can be pretty confident you are getting a good SCL, otherwise going node to node in a tet mesh would give you a questionable SCL.

Does anyone have a way of extracting component stresses along a line (on a 3D structure) in Cosmos? Doesn't it get a little tricky with element shape functions with higher order elements to interpolate the stress values along a line from neighboring nodal stress components.

 

[prex]

croy2
IMHO linearization through a line segment traversing a 3D model should simply not be used (the guidelines you referred to are at least partly along this line of thinking).
The point is that with a line you will find only very local stresses, missing the redistribution that could occur around the line: and this redistribution is the very basic reason for making the linearization!
As suggested by those guidelines, a plane cutting the model should be used for 3D models, but then how to limit the cut area where linearization is performed? (and of course the calculation may become really cumbersome).
However I can't see an alternative to the plastic analysis as suggested by TGS4: only there you'll find a definitive answer, if you want to be consistent and conservative (but not too much).
However, again IMHO, if you are trying to linearize stresses in a 3D model (3D elements, 3D geometry) you are simply in the wrong place: 3D models should be used only for peak stresses and linearization should be limited to 2D models (axisymmetric or thin shells).
I know of course that some geometries may be fully represented only as 3D, but it is a matter of analysis to simplify it in perhaps a few 2D models: the error in evaluating stress indices will probably be smaller (with the exception of 3D plastic analysis of course), the model will be better meshed and will calculate faster!

prex

http://www.xcalcs.com

Online tools for structural design

 

[croy2]

Prex,

The geometry I am considering is a relatively thick walled cylinder (welded to another thick structure) and I would naturally consider lines not a single line through a cross-section of interest. The loading is such that the maximum stresses will definitely occur on the same plane as the load, so only one cross-section need be considered and a few SCL's calculated. This would, in effect, reduce it to a 2D problem. Also, I think that the major premise of WRC-429 is stress linearization in 3D FEA models, so I'm not clear on why this method is inappropriate for 3D analysis. Also, I don't know how I can reduce this to a series of 3D models, or if this is even possible. If it could be reduced to a series of 2D problems, would the necessary assumptions involved result in any less accuracy than using a simplified look at the stress intensity and maybe go with 1.3 instead of 1.5 *Sm for B+M and 0.9 instead of 1.0 for membrane stress, or something like this that would always be conservative?

You probably agree that sometimes it makes economic sense to possibly reduce by many hours the analyis time for a problem by spending a little more money on thicker material, more welding, etc. by taking a very simple conservative approach to a problem instead of analyzing it to death over the course of days to reduce the thickness of a part by 1/16".

By "simplified look" I am referring to a previous post in which "cab1990" estimated the membrane+bending stress distribution by just looking at the SI at the cross-section surfaces. I think that you replied to the post that the actual linearized stress could be higher, which of course is correct.

I'm no FEA guru by any means, but I do believe that plastic analyses would result in analysis time orders of magnitude greater than a linear analysis.

 

[TGS4]

A few comments:
1) In ANSYS you can define an arbitrary class line, using the path commands and then mapping the component stresses onto this (arbitrary) path. It does not need to coincide with nodes. Unfortunately, I do not think that COSMOS offers this option, so you have to be particularly judicious in your mesh.

2) w.r.t the time issue, one of the strengths of the plasticity method is that you actually need a less-refined mesh to achieve a reasonable limit load. When you include the (mostly manual) post-processing that needs to happen when using stress linearization, I could argue that the time difference is about a wash between the two methodologies.

3) Croy2, you mention that you are looking at a relatively thick-walled cylinder. Specifically, what is the D/t ratio. If, in any region it is less than about 10, then stress linearization is simply NOT appropriate. At these D/t ratios (and smaller), the theoretical stress distribution follows the Lame equations, which are quadratic. Stress linearization is therefore bound to give you unconservative results.