acceptable plastic strain in static FEA

[u/Maleficent_Play1092]

Curious what people actually use in practice as a sanity-check threshold for local plastic strain in elastic-plastic static FEA of ductile steel structures, when fatigue is explicitly out of scope
I know that correct answer is code dependent, but some of them don’t define plastic strain limit at all. Is there any value (1%,2%,5%), that I can assume my structure is safe?

[u/Topher-22]

If you’re using a ductile material that would allowed to be used for a pressure vessel material, I think EN-13445-3 says 5% - 7%

Also based on your comments, I think you’re doing an “Elastic-Perfectly Plastic” material model

[u/Safe-Drama9784]

For pressure vessels, EN 13445-3, Annex B goes with 5%

[u/Maleficent_Play1092]

I use bilinear hardening model and I track plastic strain, not just strain

[u/Fresh_Librarian_2536 → u/Maleficent_Play1092]

Why do you specifically use bilinear and not multilinear hardening model, also what kind of hardening, iso, kine, combined?

[u/Maleficent_Play1092 → u/Fresh_Librarian_2536]

Its steel S355 so bilinear model with tangent modulus 0 seems to be enough, I do not define hardening as it’s not cyclic

[u/Partykongen → u/Maleficent_Play1092]

0, 0 0.00145631, 300 0.0033266, 350 0.003439, 360 0.0040484, 370 0.0059556, 380 0.011975, 390 0.03064, 400 0.087121, 410 0.25381, 420

That's the multilinear model I use for S355. For a single event, I would be quite comfortable with plastic strains at 0,05, mabye up to 0,1, depending on the consequences of failure. The stress/strain used in FEA is the true stress andlogarithmic strain, so the strain levels to failure is quite a bit higher than the engineering strain you'd see on most stress/strain diagrams.

[u/Key-Presence-9087]

Allowable up to half of total elongation is pretty common acceptance criteria

[u/nastran_]

If you know what the stress strain curve looks like, you can derive plastic strain from it. Elastic strain is usually 0.2% since Fty is defined using 0.2 offset strain. Technically the proportional limit is before that so there a tiny bit of plasticity at Fty but it’s not much. With that said if you know your strain to failure the plastic strain is just the difference between strain to failure and 0.2%. So for low ductile metals (maybe cast aluminum) I would expect 3 ish percent and highly ductile steels I would expect over 10%. You can get most of the numbers needed to do this exercise from mmpds or equivalent documents. To capture this in FEA you obviously need to do a nonlinear material run.

[u/martianfrog → u/nastran_]

"highly ductile steels I would expect over 10%" <- sounds right

[u/DistributionMean6322]

There is no general answer on allowable plastic strain. Is it in compression or tension? How ductile is the material? Is the part safety critical? What are the consequences of failure? How expensive is the repair? How localized is the plastic strain? Will that same area also be subject to fatigue loads after? The list of questions goes on and on without any context.

[u/randomlygrey]

Depends on which standard you are designing to, there will be a specification. Failing that the plastic strain limit for steel is 5% for eurocodes and similar. So if you're plastic but strain is less than 5% then you're not fracturing and that's good news.

[u/ImNotSanguinius]

Requires engineering judgement. Where’s the plastic strain? What does it look like? Concentrated? Through a plate? Also, you have to judge whether it’s something you can reasonably get rid of. Why gamble with this if you can just add a bit of extra strength? If you can’t, then you need to judge it and not just look at numbers.

[u/alettriste]

You should check the code. ASME VIII Div. 2 5.2.4 defines local failure as a function of plastic strain, but through consideration of the local stress state if I remember well. 5.3 protection against local failure.

[u/BisonDull9704]

Estimate the acceptable plastic strain by calibrating your model with a known solution. There are some good worked out examples in DNV C208

[u/lithiumdeuteride]

For a single-cycle worst-case load, I used 0.2% plastic strain to evaluate the yielding requirement, and 1/4 of the material's elongation rating for the ultimate failure requirement.

For example, if it were steel rated at 20% elongation at failure, I'd be using plastic strain allowables of 0.2% and 5%. The FEA would be nonlinear and would use a Ramberg-Osgood stress-strain curve with ~15 or so points, and isotropic hardening behavior.

That's not following a particular code, it's just as far as I felt comfortable pushing anything.

[u/wings314fire]

You cannot just do blanket x% plastic strain. If the geometry is notched then you will see failure in strains less than the one given by uniaxial tension test due to stress triaxiality. I will say, how much plastic deformation is ok for your use case. Are there load reversals? Are you going to use the structure once it gets plastically deformed ? Are there standards that suggest for a particular type of detail the allowable strain ?

[u/greenmonkies_13]

If you are looking at a single event, you probably want to stay well within the elastic limits of the material, unless you are doing something like crash. If there is not an obvious yield point in the stress-strain material curve, you can use 0.2% strain to define the elastic-plastic limit

[u/Partykongen → u/greenmonkies_13]

I'd argue the opposite. If it is a single event, he can accept a large amount of plastic strain for a ductile materials, as long as the deformed geometry is still usable. Then for subsequent events, the stresses would have to surpass the previously experienced stress before further plastic strain occur.

[u/greenmonkies_13 → u/Partykongen]

Fair point, the only other thing to consider is next time it is loaded, it is no longer being loaded to the original geometry, so potential for eccentricity that could cause stressed that weren't present in the initial loading

[u/Partykongen → u/greenmonkies_13]

If the high stresses is in some fillet at some corner, the geometry will likely not have changed enough to consider that but if it is the major bending stresses in a beam, then it will have deflected enough that the new configuration needs to be considered. While we usually use a geometric nonlinear model whenever we have material nonlinearity in a large strain model, it isn't strictly nessecary if the deformations are small, which they may be if the high strains are very concentrated.

[u/THBST666]

You need to have a validated material model for your solver first. Then you need a strain at break for that material, which can vary by thickness (if you model mid layer shells with thickness parameter). Then you check effective plastic strain for hotspots and P1 strain from mid layer scaled to maximum=strain at break for each material. Then you do a test comparison 1:1 and evaluate how close you got (test correlation) and how can you get closer next time. You have to have everything as close to reality as possible (earlier, similar models and old test comparisons are handy). And that's everything from meshing specs through CAD vs FEM model to things like time step and control cards... If you're not calculating with a strain limit then you have no idea when you cross from elastic to plastic deformation... You can use whatever % you want, the result is worthless... Nothing in = nothing out in FEA