×
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

Elastic-Plastic Stress Analysis Method in ASME VIII.2

Elastic-Plastic Stress Analysis Method in ASME VIII.2

Elastic-Plastic Stress Analysis Method in ASME VIII.2

(OP)
Hello All,

I am trying to understand the Assessment Procedure and the Acceptance Criteria for the Elastic-Plastic Stress Analysis Method.
I've already create the Stress-Strain curve, based on ASME VIII.2 Annex 3-D and I know how to define the material in the FEA software.

What I don't understand is how to know if my design meets the requirements of the Code.
5.2.4.4 stated that: "if convergence is achieved, the component is stable..." but how do I know if convergence is achieved?

PTB-3 Example for this case only shows the von-Mises stress plot and the Equivalent Plastic Strain and stated that "convergence was achieved" so, for me, it's not very helpful.

Thank you very much.

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

With the factored loads applied, one performs the analysis with the specified materia stress-strain curve. The analysis either converges to a statically-permissible solution or it doesn't.

What software are you using?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

(OP)
I'm based on Appendix 46-4 for applying the Design By Analysis requirements of Section VIII, Division 2 Part 5 in Section VIII, Division 1 Vessel.
Therefore, as per 46-4(c)(1)(-c) the factor shall be 3.5.

I am using the Non-Linear simulation module of SolidWorks.

I think I didn't understand the meaning of: "The analysis either converges to a statically-permissible solution or it doesn't."

How do I know if this happen or not?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

The software will either give you an answer at that load factor, or it won't.

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

(OP)
Do you have an example for it?
I have found this example: Link
but it only stated that: "The analysis converged for the given load and thereby satisfy the global acceptance criteria"

The example only shows Stress and Strain plots, nothing more.

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

How familiar are you with the concepts of LRFD?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

(OP)
Not much, but I am not sure I can use it when using Section VIII.1 Appendix 46 which stated that the factor need to be 3.5.

Is there something like the Assessment Procedure of 5.2.2 in 5.2.4?
So I can tell if the stresses is above or below the allowable stress?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

No. The software/computer does all of the work for you (hence the brilliance of the E-P method).

Have you run the analysis yet?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

(OP)
Haven't run it yet. I wanted to make sure I understand what I need to do before I starts.
As I said, I started with define the stress-strain curve, based on Annex 3-D.
Than, I looked at the Assessment Procedure and the Acceptance Criteria for the Elastic-Plastic Stress Analysis Method, but I didn't understand it I guess.

From what I know, convergence mean that there will only small effect on the stress results when the mesh is refined.
But I'm assuming that it is not the meaning when talking about the Elastic-Plastic method..

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

Do you have a mentor that you can connect with? We are reaching the end of what can be provided, for free, over the internet. I would also encourage you to look into taking a technical training course on the topic.

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

(OP)
Unfortunately I don't have any mentor for this subject.

Do you, or anyone else in this forum have any example and/or FEA report he or she made using the Elastic-Plastic Stress Analysis Method which he or she can share?

PTB-3 and the examples which I found only say that The analysis converged for the given load, but does not provide any other explanation.

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

Not with your software.

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

(OP)
So maybe with other FEA software?
I just want to know what I need to look for.
Does "convergence" mean there is a solution and the analysis come to an end?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

Effectively, yes.

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

(OP)
So, if I am running a FEA study with the correct Stress-Strain for the material under consideration and I get a solution, that's mean the analysis has convergence and the Code requirements have been meet?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

Correct

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

(OP)
Thank you very much for your help.

So, let's say I run a FEA study for a shell made of SA-516 Gr. 70, stress has convergence but I get a maximum von-Mises stress of 450N/mm^2.
The stress is much higher then the allowable stress per Section II-D, is it OK?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

This would be at the fully-factored loads? Then yes, I would expect that the stresses would be well in excess of the allowable stresses. Potentially by a factor of at least 3.5 (you did mention that you were doing this for a VIII-1 vessel, right?)

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

Hi
Nice discussion.

TGS4, what if I choose an elastic perfectly plastic material model? Is it possible that the results show a Von-Mises stress that exceeds the yield stress?
I understand that the strain can be higher than the yield strain but the stress should not go higher than yield. However, when I run FEM using elastic perfectly plastic model there are points at which the Von-Mises stress is higher than the yield stress that I defined for the material. Is it because of interpolation (or extrapolation) inside elements or is it something about the flow rule?
Actually I could not understand how to assign the flow rule to the software at all ( I use ANSYS).

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

Yes, it's possible. But with adequate refinement of the mesh, such occurrences should disappear.

The Associated Flow Rule is the default in most major software, including ANSYS.

Are you able to attend my training class next month in Houston?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

TGS4, unfortunately I am in the middle east and cannot attend your courses.
I have another basic question regarding elastic-plastic method for evaluating protection against plastic collapse.
What should be considered as the yield strength in the material model? Is it the Sy as mentioned in Sec.II tables or 1.5 times the allowable stress?

Are there any rule of thumb for preference of Limit Load analysis over elastic-plastic analysis or vice versa in different situations?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

(OP)
TGS4, Yes, it was with fully-factored load (3.5*P) according to Mandatory Appendix 46.
Another problem I have is that the stress is increasing with mesh refine, but maybe is a singularity problem and not a stress problem.

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

Paulette - the rules in 5.2.3 state that the effective yield stress to be used in the Limit Load Analysis for demonstrating Protection Against Plastic Collapse is 1.5*S. (the exact reference is 5.2.3.5, Step 3.)

There are no situations where I prefer the Limit Load Analysis method. I generally prefer the Elastic-Plastic Analysis Method in all situations. It has the added bonus of being able to satisfy Protection Against Local Failure using the Elastic-Plastic analysis method, and the exact same model with the same material properties can be used for demonstrating Protection Against Failure From Buckling.

IdanPV - once you get into elastic-plastic analysis, you really need to stop looking at the stresses. I kn ow that it's difficult, because most of us are accustomed to using stress as the language for communicating. However, in elastic-plastic space, the language needs to shift to strains. And the strains at the factored loads are going to be much more theoretical than anything that you would expect, mostly because you are looking at a large factor of the loads which will put you fairly far to the right in the stress-strain curve - perhaps even to the perfectly-plastic portion of the curve after the true ultimate stress.

In your specific situation, it is likely a singularity problem, but one that will likely not affect the elastic-plastic analysis results. Don't think too hard or look too hard at the results from the factored loads. That it converged is sufficient from demonstrating Protection Against Plastic Collapse.

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

TGS4, in the assessment procedure for elastic-plastic method it is mentioned in 5.2.4.4 that a material model that includes hardening or softening, or an elastic perfectly plastic model may be utilized. My question is that in the case of elastic perfectly plastic model what should be the yield stress?
is it the same as limit load analysis 1.5*S?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

No guidance is provided in that regard and I would not recommend using a elastic-perfectly-plastic material model for the elastic-plastic analysis.

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

(OP)
TGS4, Thank you for your help.
One more question regarding the Elastic-Plastic Stress Analysis Method.
The material model for this kind of stress analysis is non-linear and required true stress-strain curve as input.
Section VIII.2 Annex 3-D gives the required model for the stress-strain curve.

This Link provide an example for the Elastic-Plastic Stress Analysis Method of Section VIII.2, 5.2.4.

The stress-strain curve in the link above use the Plastic Strain data for the stress-strain curve nor the Total Strain data.
Which data I need to use for the material model - the Plastic Strain or the Total Strain?

RE: Elastic-Plastic Stress Analysis Method in ASME VIII.2

That's a question specific to your software. For example, Abaqus requires the plastic strain only.

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! Already a Member? Login


Resources

White Paper - The Evolving Landscape of Commercial Battery-Powered Trucks
What’s driving the evolving landscape of truck electrification? What are the barriers, motivators and strategies for accelerating the electric transition? What insights and resources are available for today’s design engineers working to achieve industry disruption and evolution? For answers to these and other pertinent questions, read this white paper. Download Now
eBook - Rethink Your PLM
A lot has changed since the 90s. You don't surf the Web using dial-up anymore, so why are you still using a legacy PLM solution that's blocking your ability to innovate? To develop and launch products today, you need a flexible, cloud-based PLM, not a solution that's stuck in the past. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close