PREX & TGS4 - Could you both please help with some Stress Linearization? 2

[AFG03082015]

Hello Prex, TGS4 and anyone else who may be able help!

From reading several other posts you both seem highly informed when it comes to stress linearization and was hoping you could help me out a little...

I am completing an FEA analysis to support an ASME VIII Div.1 vessel by completing the analysis to ASME VIII Div.2.

I have attached screenshots that show my 1/4 model and also the location of my SCL (The highlighted line in the centre of the three)

I have also attached the results file stating the six component stresses at each node's location along the SCL.

Would either of you be able to enlighten me as to how to proceed to calculate the Membrane Stress & Membrane + Bending Stress?

Any help would be greatly appreciated,

Thanks for your time...

 

[Soave]

OK TGS4, I think that I understood.
I corrected my calculation consider the lenght (dx).

but I can't find the bending stresses along the path, like ansys show at table.

 

[TGS4]

Where in the ANSYS documentation are you getting this?

 

[Soave]

http://files.engineering.com/getfil...c=212727627.5.1475537305662&__hsfp=2605326849

 

[TGS4]

I would ignore the intermediate points. They are merely points along a straight line. The intermediate points are not calculated by anything other than y=mx+b. Figure out how to do the linearization first.

 

[Soave]

TGS4,

I corrected my calculation, and the values are equal to Ansys, I calculated with the following:

Sm=((Σ[sub]1[/sub][sup]n-1[/sup](S[sub]ij[/sub])+ S[sub]ij[0][/sub]/2 + S[sub]ij[n][/sub]/2)/n

Sb=[(Σ[sub]1[/sub][sup]n-1[/sup](S[sub]ij[/sub]*(t/2 - X[sub][/sub])/t)+ (S[sub]ij[0][/sub]*(t/2 - X[sub][0][/sub])/t)/2 + (S[sub]ij[n][/sub]*(t/2 - X[sub][n][/sub])/t)/2]/n

But I'm confused if the bending calculation is according to ASME VIII Div.2 formula (5-A.2) and described in 5-A.4.1.2(c)

 

[TGS4]

Great!

Now that you have figured out how to properly linearize a through-thickness stress distribution, there are a couple of more things. First, you have now calculated the linearizations of the component stresses, which need to be rounded up into an invariant (such as von Mises, if you are using the latest Edition of VIII-2). To do so, please pay special attention to my post of 2 Aug 16 16:12. How ANSYS calculated the bending invariant is WRONG when it comes to compliance with Annex 5-A (I've only been fighting with ANSYS for 17 years to fix it, but that's another story).

Furthermore, I am going to ask a much more fundamental question. You say that you are doing this for a graduate thesis. My impression of university graduate-level work is that it should be relatively on the cutting-edge of technology. Why, then, are you using a technology (linear-elastic stress analysis using stress linearization/categorization for demonstrating either Protection Against Plastic Collapse or Protection Against Failure From Cyclic Loading: Ratcheting) that is 50 years old, when a perfectly good modern technology (elastic-plastic stress analysis) that doesn't suffer from the same complications and constraints exists?

 

[Soave]

I will pay special attention to your post!

For your second advice, I answer: I will upgrade my studies to a elastic-plastic stress analasys of course, but first I wanna understand the beginning.

Thank you again.

 

[Soave]

At last, other question:

About the peak stress (Sp), Is the calculation below correct?
Sp[sub]0[/sub]=Sij[sub]0[/sub] - (Sm+Sb)
Sp[sub]t[/sub]=Sij[sub]t[/sub] - (Sm-Sb)

(I thought very simple)

 

[TGS4]

Yes. The peak stress is the value of the actual stress subtracted from the membrane plus/minus bending.

 

[ksbhatt]

Hi Soave,

As you mentioned that your calculated values are matching with Ansys result values.
Can you please show me the same for Bending stress calculations according to "Sb=[(Σ1n-1(Sij*(t/2 - X)/t)+ (Sij[0]*(t/2 - X[0])/t)/2 + (Sij[n]*(t/2 - X[n])/t)/2]/n"?

 

[Soave]

Hi ksbhatt

I calculated acc. formula (5-A.2) and described in 5-A.4.1.2(c).

The spread sheet is attached. (you can also see peak calculation in this sheet).

 

[ksbhatt]

Hi Soave,

Thank you very much for sharing the spreadsheet. It helped me a lot.

As I am observing, there is difference in ansys results and calculated results for bending stress values in my case.
According to spreadsheet Von-Mises bending stress is 247 Mpa and in Ansys it is 198 Mpa.

 

[Soave]

ksbhatt


Sorry for confusion. That spreadsheet does not refer to ANSYS calculation above (it was used to other vessel).
Please, check with any your ANSYS calculation.
And as explained by TGS4, the intermediate bending stress values is just calculated by y=mx+b (My spreadsheet dos not consider it, since this value are not helpful).

I'm new about ASME Div. 2, therefore if I'm wrong, please someone correct me! =)

 

[ksbhatt]

Thank You Sandip,

It is really nice post on Stress Linearization.

Now I am pretty clear about the differences of Ansys and ASME code in terms of stress linearization.

I have one question,
why ASME Sec VIII Div2 Annex 5.A.4.1.2 neglects the local component stress parallel to the SCL or in-plane shear stress?


Thanks

 

[AFG03082015]

Sandip,

Can you explain to me why you used Simpsons Rule to Calculate The Stress Tensors please?

Thanks