×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

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

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

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

(OP)
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...

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

In such a monoblock vessel, I would submit that linear elastic analysis is not appropriate.

If you are bound and determined to do so anyway, please be aware that I do not provide advice on SCLs or linearization - see 5.2.1.2, 5.2.1.3, and 5.2.1.4. And linearization is covered in Annex 5-A.

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

As TGS4 suggested, thick vessels(monobloc vessel in your case) tend to behave differently than the thin vessels for which the stress linearization may lead to some wrong interpretation of results. I guess Monobloc vessels have nonuniform stress distribution.

Anyway you want to know stress liniearization in general please read this post-thread794-410119: Clarification of Stress Classifications (Primary, Secondary, Peak etc.)

Stress linearisation is very complicated subject and only experienced engineers could be able to do that.

Keep in mind the quote and suggestion from above thread from TGS4. He has very extensive experience in this field.

Quote (TGS4)

If you want my unvarnished opinion it's this: DO NOT use elastic stress analysis for demonstrating Protection Against Plastic Collapse and the subsequent considerations of stress linearization and classification.

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

AFG03082015 is just asking how to do the linearization of the stress results, the use he will do of it is up to him.
Now, as you have the stresses at constant intervals along the SCL, the membrane stress compnents will be:
Smx=(ΣSx[i]-(Sx[0]+Sx[36])/2)/36
and the same for the other 5 components. The only trick contained in the above formula is that the end values need be counted only in half. A more general formula, giving of course the same result and explaining that trick, is:
Smx=(Σ036(Sx[i]+Sx[i+1])/2)/36
or in a more general form (dx BTW is wrong in your table), valid also with non constant dx (with t=X[n]-X[0]):
Smx=(Σ0n(Sx[i]+Sx[i+1])/2*dx[i])/t
Now for bending, according to App.5.A, the stress Sx is not considered, and the same for the shear stresses (as your model is axisymmetric, there can't be torsion of the SCL: do not ask me why it is done so, I can't understand, personally I would check whether considering all the stress components gives a more conservative result, as I would expect BTW).
So, using the fact that dx is constant through the thickness, for Sy (the same for Sz):
Sby=(Σ036(Sy[i]+Sy[i+1])/2*(18-i))*6/362
This is for X=0, sign changed for X=t.
If dx was non constant:
Sby=(Σ0n(Sy[i]+Sy[i+1])/2*dx[i]*(t/2-X[i]))*6/t2
Now you have all the membrane and (summing up at both ends of the SCL) the membrane+bending stress components, and you calculate the principal stresses and the equivalent ones at the ends of the SCL.

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

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

(OP)
Thanks All For Your Input, Advice & Help.

Prex Are you saying that dx would be 0.5mm at each node? and not a running addition at each node (0.5, 1.0, 1.5 etc...) as it currently is?

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

Yes, correct. More exactly dx is 0.5 mm for each increment from one node to the following one: you have 37 nodes and only 36 dx increments.

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

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

(OP)
Thanks for your help Prex,

Once I have calculated Smx, Syx, Szx Etc... I use these as stress tensors to calculate the membrane stress?

I've got a litte confused because I found the following online that seems slightly different to the equation you stated before (Smx=(ΣSx-(Sx[0]+Sx[36])/2)/36)

[i]The distance between each node along the SCL is the dimension dx. dx usually varies between nodes depending on how the model is meshed. Sum (integrate) dx*Sn over the length of the SCL from i to j. Repeat for each of the other 5 local stress components. This produces 6 stress components (Snm, Stm, Shm, Tntm, Tnhm, Thtm). These 6 components are either fed into a Tresca routine (ASME VIII-2 2006 edition) or von Mises (ASME VIII-2 2007 edition). The output is a single value for the membrane stress.


When the items are fed through a Von Mises routine, is the membrane stress the resultant Von Mises stress or the greatest difference between the principal stresses?

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

You need to understand that the local value of stress to be used for the integration is not the nodal one, instead it is the value pertaining to each subsegment of the SCL. So the local value is (Sx[i]+Sx[i+1])/2: with this is mind you'll be able to understand the formulae (BTW I made some mistakes with the indices, but if you understand the formulae, you'll be able to figure out what to do).
And I don't know what exactly is a Von Mises routine, but from a Von Mises routine you should get a Von Mises stress, and from a Tresca routine a Tresca stress? ponder

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

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

Hello Prex / AFG03082015,
I am working on something similar myself and have come unstuck in calculating the bending stress,
Did you manage to calculate it AFG03082015? If not could you talk me through it in more details Prex? In the ASME Div. 2 code (5-A.4.1.2) it is stated as...

Stress{ij,b} = 6/t^2 Integral Stress{ij} (t/2-x)

Is this the same as what you stated Prex?
Thanks

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

Yes, nearly.
Assuming:
n as the number of subsegments in the SCL
X[i] (i=0..n) the linear distance of the subsegment's ends from one end of the SCL
dx[i]=X[i]-X[i-1] (i=1..n) the length of each subsegment
t=X[n]-X[0] the length of the SCL
then
Sby=(Σ1n(Sy[i]+Sy[i-1])/2*dx[i]*(t/2-(X[i]+X[i-1])/2))*6/t2

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

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

To ensure compliance with 5-A.4.1.2, it should be noted that

Quote (ASME Section VIII, Division 2, Annex 5-A, 5-A.4.1.2 Step 2 (a))

Bending stresses are calculated only for the local hoop and meridional (normal) component stresses, and not for the local component stress parallel to the SCL or in-plane shear stress.

So, when calculating a von Mises membrane-plus-bending stress, so would use the membrane-plus-bending for the hoop and meridional components ONLY and then the membrane stresses for the other normal components (through-thickness) and the shears.

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

(OP)
TGS4,

are you saying the following would be my six stress tensors at end i of my SCL?

Snm+Snb, Stm, Shm+Shb, Tntm, Tnhm+Tnhb, Thtm

where
n= Normal
t= Tangential
h= Hoop
M= Membrane
b= Bending

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

No.

You need to orient your SCL so that there is a local coordinate system aligned with a local hoop, meridional, and through-thickness direction. Then, your membrane-plus-bending tensor is:

t = through-thickness
h = hoop
m = meridional

CODE --> tensor-notation

σ_t-membrane   τ_th-membrane               τ_tm-membrane
τ_th-membrane  σ_h-membrane + σ_h-bending  τ_hm-membrane
τ_tm-membrane  τ_hm-membrane               σ_m-membrane + σ_m-bending 

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

Dear TGS4, Prex and all

I'm studying for my graduate thesis about ASME Calculation Section VIII Div.2 and I appreciated and learned a lot with yours posts and helps.
Now I have elaborated my spreadsheet for linerarization of stress.
I have two questions:
1- How Can I obtain the bending stress for each node?
2- My calculations are correct?

I annexed my xls file and my test calculation with ansys.


Thanks for your attention and time

http://files.engineering.com/getfile.aspx?folder=a...
http://files.engineering.com/getfile.aspx?folder=9...

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

(OP)
Hi Soave,

I'm a little confused by the values of L at nodes 1-4.

The nodes should be lined up sequentially along the stress classification line, therefore the value of L should increase in from node 0 up until node 48(just like that seen between node 5 and 48).

Between node 1-4 your value of L appears to increase by the value of 20.834 to 83.336 before dropping back down to 10.417

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

Hi, AFG0382015

Sorry for this wrong, the value at nodes 1-4 shall be divided by 10... So, Node: 1 = 2,0834; 2 = 4,1668; 3 = 6,2502; 4 = 8,336

Thanks

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

Bending stress is not calculated at each node. It is the equivalent linearized stress distribution across a section that produces the same net forces and moments as the actual distribution.

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

TGS4,

About bending stress, How ANSYS Can calculated bending stress at each node?

And my bending stress calculation are correct?

http://files.engineering.com/getfile.aspx?folder=9...


Thank you again.

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

ANSYS doesn't calculate the bending at each node. It linearizes the component stresses along a path, and reports the average (membrane), bending, and peak of each component stresses along the path. Membrane and bending (and peak) are properties of the path, not a specific node.

In your calculation of membrane and bending of the component stresses, you need to consider the actual length fo each location, not the "n" of each location.

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

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

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






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

Where in the ANSYS documentation are you getting this?

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

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.

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

TGS4,

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

Sm=((Σ1n-1(Sij[i])+ Sij[0]/2 + Sij[n]/2)/n

Sb=[(Σ1n-1(Sij[i]*(t/2 - X[i])/t)+ (Sij[0]*(t/2 - X[0])/t)/2 + (Sij[n]*(t/2 - X[n])/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)


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

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?

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

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.

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

At last, other question:

About the peak stress (Sp), Is the calculation below correct?
Sp0=Sij0 - (Sm+Sb)
Spt=Sijt - (Sm-Sb)

(I thought very simple)


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

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

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

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[i]*(t/2 - X[i])/t)+ (Sij[0]*(t/2 - X[0])/t)/2 + (Sij[n]*(t/2 - X[n])/t)/2]/n"?

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

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.

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

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! =)







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

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




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

(OP)
Sandip,

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

Thanks

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources