stress linearization in abaqus in transition areas 2

[farzad1]

hello friends

i am doing an stress linearization in a perforated region of a connection of shell to tubesheet.

i have read the similar threads but it did not exactly solve my problem.

i want to discuss numerically.

my problem is that the stress i see as a total von mises , )not by stress linearization) is 218 Mpa .

1- i have to mention that tubesheet yield is 218 Mpa and the shell is 250. in stress analysis i see maximum stress of 218.2 around transition area and a small plastic deformation. but when i choose my SCL for stress linearization in the region (both in tube sheet or head or exactly on material transition line ) the maximum amount of membrane+ bending is 260 MPA !!!

my question is that between the amounts 218.2 which is total and 260 , which is Pm(or Pl) + Pb + Q ? and why the membrane plus bending which is part of total stress has exceeded than 218.2 which is the total stress ?

2- what is the method to understand the amount of secondary and primary from results of FEA ?

3- why abaqus rotates the axes of stresses (the x axis in direction of SCL ) ? what is the necessity ? why not calculating in global directions ?

thank you

 

[TGS4]

Are you performing this analysis in accordance with Division 2? If so, follow the guidance in Annex 5.A.

 

[farzad1]

hello;

thank you TGS4 , i have read that annex , it is just the procedure that the software does it . i mean i have extracted membrane and mem plus bending and my problem is that the maximum value of membrane plus bending is higher than the total von-mises stress. i need to know why and how should i interprete it ??

 

[prex]

As noted in another thread, your situation is perfectly possible, and you should use M+B, if you trust your calculated values, for stress checking.
If you want to understand what happens, you should plot the stresses along the SCL and graphically draw the membrane and the bending components across the curve.

prex

http://www.xcalcs.com

: Online engineering calculations

http://www.megamag.it

: Magnetic brakes and launchers for fun rides

http://www.levitans.com

: Air bearing pads

 

[farzad1]

hello prex ;

thank you very much for your valuable answers , i have uploaded the result of total stress as mises and the membrane plus bending also , i have not used thermal analysis , i have evaluated the effect of temperature on young modulus and i have no heat source in the model.

also i decided to persume that when i calculate the total stress , there would be no secondary and only primary stresses M+B are taken into acount , and when i get the membrane plus bending diagram , i should assume that the membrane here is a combination of primary and ssecondary , i mean that the software doesnt show the secondary stress in total stress and the 218.2 doesnt include Q but the membrane plus bednig which is 250 ,includes Q . is this assumption true ?

 

[farzad1]

also here is the membrane plus bending and membrane diagram.

 

[prex]

What you should look at is the through thickness diagram of the equivalent (vonMises) stress: that distribution should show, with the M and M+B stresses superimposed, how it comes that the local maximum stress is smaller than the M+B stress.
Consider however that in a 3D model it is not easy to define a representative SCL , as local effects might govern: a comparison with a thin shell model and an axisymmetric one would assist in evaluating the results.
Concerning the classification into primary and secondary categories, you should consider the following:
- the calculation of M and M+B stresses from a general stress distribution is a matter of geometry and can be automatically performed by a computer code
- the classification of stresses into primaries and secondaries cannot be done by a (linear) computer code, as this classification involves determining the self limiting character of secondary stresses and only an elastoplastic analysis can do this
- that classification is generally done based onto engineering judgment; as an example, the stresses at the interface of two different structures (the shell and the TS in your case) are generally secondary stresses
- primary stresses are normally determined by simple formulae or simplified models of single structures: a tubesheet will generally be analysed as an equivalent plate supported at the periphery, a shell as a shell (?), etc.

prex

http://www.xcalcs.com

: Online engineering calculations

http://www.megamag.it

: Magnetic brakes and launchers for fun rides

http://www.levitans.com

: Air bearing pads

 

[TGS4]

In addition to what prex has said (all of which I agree with), I would also add that you need to be absolutely certain that you are linearizing the stresses at the component level, and that you are calculating the M+B following the rules in 5.A.4.1.2.b.1. To accomplish this, you need to orient a coordinate system along the hoop-circ-axial directions of the vessel, transform the stresses into that coordinate system, and them perform the linearization. Be careful, because the procedure in 5.A.4.1.2.b.1 is NOT the default for your software.

The situation that you are describing is possible, and not unheard of.

 

[farzad1]

thank you all ;

as what I have known about what the software does is as follows :

the software asks two points as the start and endpoint of the SCL line , normally I choose one of the points at the node inside vessel (maximum stress) and the other one outside in a way that if the points are connected with a line , the line will be normal to section ( towards the vessel center ) in this case the software (According to its manual) chooses the x axis of the stress linearization coordinate system along the SCL line , then defines the other tow axises with some transformation. so the stresses as s11 s22 and etc given in this procedure are not like the same stresses s11 , ... of global coordinate system ( I have checked it ) . but there is something , the total , M and M+B stresses in diagrams uploaded are all as von mises . isnt von mises stress independent of coordinate system ?

I found something else also : when there is no special case like material or structure change or there is no plasticity , the M+B is equal to total stress , but in regions that plastic deformation (even small like in my problem ) occures , there is this problem, and when the plastic deformation gets significant , the software is unable to calculate the plasticity ,

any way , I think that according to prex that was sure that there is secondary stress in M+B , so the Q should exist also in total stress and maybe 250 of M+B is a numerical error , but both have to be compared to 3*f , this is what I judged . please correct if i am not right.

 

[TGS4]

Have you actually read 5.A.4.1.2.b.1? Do you understand what it means? The default ABAQUS methods for calculating M+B are NOT in accordance with 5.A.4.1.2.b.1.

You seem to have a misunderstanding of how to calculate linearized M+B equivalent stress. FIRST, you calculate the linearized M and M+B for all 6 components. Then, you combine it per 5.A.4.1.2.b.1. The results are HIGHLY dependent on the coordinate system chosen, so be careful.

but in regions that plastic deformation (even small like in my problem ) occures , there is this problem, and when the plastic deformation gets significant , the software is unable to calculate the plasticity ,

Are you actually including plasticity in your model? All of the stress linearization techniques are applicable ONLY to linear elastic analysis.

Please note that all of the calculations in 5.5.6 must be performed when comparing the P+Q stresses to any value. You are calculating the stress RANGE between two stress states, checking for ratcheting. Therefore, you need to follow the rules in 5.5.6 very closely. This is NOT the same as some random check of P+Q<3S anywhere in your system.

Please read 5.5.6 again, and also 5.A.4.1.2.b.1.

 

[farzad1]

hello ;


thank you very much Dear TGS4 ;

first , yes , i have actually read it , 5.A.4.1.2.b.1 : "stress linearization procedure" .

this is what abaqus does for stress linearization : for example membrane stress is calculated as the integrration of stress along the thickness ( abaqus chooses a coordinate system which its x axis is along the SCL line ( Thickness ) and calculates all of the 6 components of M by this integration . since just the formula of integration is exactly the same as Div.2 I doubted about this : do you mean that I have to for example use S11 of the calculated membrane as sigma ij in 5.A.4.1.2.b.1 and so calculate the sigma ij,m ? you mean integrate a membrane stress to gain membrane ?
excuse me , if you know the difference between abaqus methods and Div.2 , could you mention it please ?

2- thank you very much about the 5.5.6 , about delta Q , i doubted how to calculate it . is it exactly multiplication of thermal expansion co efficient in temperature difference ?

3- Yes , i have defined plasticity. shouldnt I ? are the stress results valid if i use only elasticity ?

thank you and best regards.

 

[TGS4]

3- Yes , i have defined plasticity. shouldnt I ? are the stress results valid if i use only elasticity ?

OK, I'm going to stop right here. Elastic stress analysis and stress linearization and stress categorization are all about ELASTIC analysis. Per 5.2.2, an elastic stress analysis is all about the analysis being ELASTIC. Nowhere in 5.2.2 does it say that you are to define plasticity. Why would you do that? If you want to perform an elastic-plastic analysis, then by all means go ahead and do that, but follow the rules in 5.2.4.

2- thank you very much about the 5.5.6 , about delta Q , i doubted how to calculate it . is it exactly multiplication of thermal expansion co efficient in temperature difference ?

I don't even know what you mean by this. Do you understand what ratcheting is why it's a failure mode that needs to be protected against?

 

[farzad1]

hello;

tank you very much . but about racheting no ! it is new to me , i read all of the sec.5 elastic . elastoplastic and other approaches. i think i got it. but about the exact concept of racheting i am not sure.

 

[TGS4]

I'm at a bit of a loss about how to help you from here. (For free that is - if you want to pay me to teach you, then that's another matter...).

I would suggest you purchase this book -

http://catalog.asme.org/Codes/PrintBook/PTB1_2009_Section_VIII.cfm

and read it and absorb all of the technical background information.

I use ABAQUS, so I am intimately familiar with the stress linearization techniques, and the "defaults" are NOT in compliance with 5.A.4.1.2.b.1. However, I would suggest that you start a new thread in the ABAQUS forum to discuss that, so we don't bore or scare away the non-ABAQUS users.