Limit load analysis - ASME 2010
Limit load analysis - ASME 2010
(OP)
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
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





RE: Limit load analysis - ASME 2010
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.
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?
RE: Limit load analysis - ASME 2010
RE: Limit load analysis - ASME 2010
RE: Limit load analysis - ASME 2010
RE: Limit load analysis - ASME 2010
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?
RE: Limit load analysis - ASME 2010
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.
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.
RE: Limit load analysis - ASME 2010
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.
RE: Limit load analysis - ASME 2010
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.
RE: Limit load analysis - ASME 2010