Limit load analysis - ASME 2010 1

[Pawel27]

I would like to ask about Limit-load analysis method (ASME 2010 sec. III, div.2, 5.2.2). This method is one of Plastic Collapse
Protection. At this plastic collapse load plastic region appears. This is not yet ultimate load, but something before ultimate
strength.

In 5.2.3.4 There are Acceptance Criteria. There is mentioned that: "The plastic collapse load is taken as the load which causes
overall structural instability". I didn't find anything about plastic strain value. I guess I must continue numerical analysis
until there will be problem wigh convergence. When I have problem with convergence - this is limit load. Am I right?
Comparing ASME 2010, sec.VIII,div.2 with EN 13445-3- in EN there is Gross Plastic Deformation Method. Plastic strain 5% is
allowed. From my tests, headers in boiler can carrry only a bit more than load related to this 5%. Quite fast problem with
convergence appears.

This method from EN seems to be similar to the method in ASME. Note - in 5.2.3.1 of ASME there is mentioned that limit load
analysis failure mode is gross plastic deformation.

I just would like to confirm that in case of ASME I must reach problem with convergence. That is all. Of course
some experience in FEM program is necessary ;-)

 

[TGS4]

I didn't find anything about plastic strain value.

And you won't. What is important to understand in a limit load analysis is that the ONLY stress-strain curve that can be used is elastic-perfectly-plastic (EPP). And, small-deformation MUST be used. These are the definition of a limit load analysis. You can do other things, but they are not a Limit Load Analysis.

With the EPP stress-strain curve, the magnitude of strain has no physical meaning. Therefore, it makes no sense to place a limit on a meaningless quantity.

I guess I must continue numerical analysis until there will be problem wigh convergence. When I have problem with convergence - this is limit load. Am I right?

Right.

Note that there is ongoing discussion about including a strain limit in the elastic-plastic (EP) analysis - 5.2.4. However, for the time being, consider the analysis method in 5.3.3 an effective strain limit.

On that note - when you perform a limit load analysis, you are still required to perform an evaluation per 5.3, either 5.3.2 (Elastic Analysis) or 5.3.3 (Elastic-Plastic Analysis). You are doing that, right?

 

[Bobfromoh]

So where do I find a EPP stress strain curve?

 

[TGS4]

5.2.3.5, Step 3.

 

[Pawel27]

Ok, so now I have confirmation of my interpretation

 

[VonFea]

I'm new whit limit load analysis and I have few questions:

small deformation theory = The full load is applied in one step, and there is no change in the stiffness matrix

How can I find limit load with only one time step?

What does convergence mean?
How can I recognize problem with convergence in practical basis? Does fea program give for example an error?

Is it totally different situation if I have:
- Bi-linear material
- Load is added by time steps (final load for example 1000 N)
- Large deformation is set off (no changes in stiffness matrix)
- If the load is big enough, Load factor approaches to single value (after many iterations) For example 0,9
- Analysis is stopped with "fatal error" and I get results only in area 0 - 0,9 (time steps)
- with timestep/load factor 0,9 stress is reached yield limit and plastic strain is very large compared to previous time step.
- Maximum load that structure can sustain is now 0,9 x 1000N = 900N. Is this the limit load?

 

[TGS4]

small deformation theory = The full load is applied in one step, and there is no change in the stiffness matrix

How can I find limit load with only one time step?

Not quite. Small deformation theory means that the stiffness matrix is not updated as the structure deforms. For most FE programs, that is the default, and you need to turn on large deformations or non-linear geometry, or something like that. It doesn't necessarily mean that the load has to be applied in one time step, or in one increment, or anything like that.

What does convergence mean?

Convergence means that your FE program has determined that your structure plus your loads achieves a statically-permissible solution. However, if your structure does not converge to a statically-permissible solution, that means that for a tiny (determined by you when you set the solver tolerances) increment of load, a solution cannot be obtained.

How can I recognize problem with convergence in practical basis? Does fea program give for example an error?

This is an issue to be discussed with your software vendor - unless you care to share your specific software, in which case knowledgeable members of this community may be willing to assist.

With regards to your example, my only question is: is your bi-linear material elastic-perfectly plastic? If so, then yes, you are correct.

 

[VonFea]

Thank you for your reply. The fe program I use is Femap with NX Nastran.

Analysis type I use is "nonlinear static". With this analysis type Nastran bulk data options: LGDISP is ON by default
With static analysis LGDISP is OFF by default, but with static analysis you cant't use bi-linear material.
Can someone confirm that this LGDISP is the right setting in Femap to deside between small/large deformation theory?

Bi-linear material I use have small tangent modulus (=1). So it's quite close to elastic-perfectly plastic material model.
I have heard that it's better use small tangent modulus than zero for mathematical reasons.

 

[TGS4]

I don't use that software, so I can't comment on the specifics.

However, I will say that your material needs to be perfectly-plastic. Even a small tangent modulus is incorrect. If you have issues in your software with that, I recommend taking that up with your software vendor.

 

[Pawel27]

I use Ansys and I have similar problem. I must set small tangent modulus 1, because many headers often cannot reach convergence. When 1 is applied then calculations converge very fast. It seems to be then artificial numerical problem. There will be rather no failure in reality.