Load until plastic collapse 1

[Doodler3D]

Hi,

I was going through some old FEA reports by a consultant as a part of my FEA training. Throughout the report, they mention "The plastic failure occurs at the load where the solver fails to converge". The structure in question is a rectangular steel plenum for an air cleaning process that is to be checked for a rapid over-pressurization event. (You can assume this to be a steel tank)

The confusion is that they describe their conclusions based on plots that have Von Mises contours limited to 30,000 psi (steel) and mention that the solver has failed, while the same plots indicate maximum stresses/stress concentrations/singularities that exceed 150,000 psi.

Question:

1. How do you determine whether plastic collapse has occurred if several sections within your model have already exceeded the proportional limit?

2. How can you 'load' a model till the solver fails to converge?

Thank you.

 

[GregLocock]

1) use non linear FEA, both materials and geometry

2) Depends on the solver. LS Dyna for example will cope with shattered fragments. I imagine a Mickey Mouse program won't understand things breaking.

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[rb1957]

why would you ever want your model not to converge ? Were they running Linear or Non-Linear ?

another day in paradise, or is paradise one day closer ?

 

[Doodler3D]

@rb1957, Greg

"The plastic collapse is said to occur when the solver cannot reach convergence". Confusing. They were using abaqus, non linear static analysis.

 

[SSCon]

This is the method from ASME BPVC Section VIII Div 2 Part 5, design by analysis.

There are two methods; limit analysis and plastic analysis (also elastic analysis).

Both use non-linear material models. Limit analysis uses an elastic perfectly plastic material model (bi-linear) with small displacement theory. Elastic plastic analysis uses a material curve with strain hardening and large displacements.

In both methods the loading is increased until the model fails to converge. As in, the loading is increased until there is structural instability in the model causing an error. The last successfully converged load step is the plastic collapse load.

This can be thought of as when all the material in the load path's critical cross section has reached the maximum strain from the material curve and any additional loading would cause infinitely more strain.

 

[rb1957]

ok ... that sort of makes sense ... drive the FEA off the rails, but jump off the train just before it goes ...

this is under pressure, yes? I wonder what's happening to the seams of the box ... how much pressure is venting in practice ?

If you're trying to protect from a bomb-like overpressure, why not have a blow-out door ? or intentionally leaky seams (once the load is well beyond service levels ??

another day in paradise, or is paradise one day closer ?

 

[Doodler3D]

@SSCon

I think I get what you mention. I allow the solution to progress till 1% strain on the ASME BPVC VIII Div 2 Annex 3-D stress-strain curve.
OR
Alternatively, could I run an iterative nonlinear simulation and observe the residuals at the different load steps. When I exceed elastic limit for the general stress away from discontinuities (defined by 5.2.2.2 of the BPVC VIII Div 2 code), the design has failed?

Also, I am using Elastic-plastic analysis.

@rb1957
Yes, vent door had been sized per NFPA 68. The design was complicated and Roark's/Blodgett/Troitsky etc. were not very helpful.Also, the design was evaluated with ASME FFS-1.

 

[SSCon]

You're conflating different methods, there are three for checking against plastic collapse. Elastic, Limit-Load & Elastic Plastic. You use one of them.

The report you referenced was using either Limit-Load or Elastic Plastic. 5.2.2 is the elastic (linear) method so not relevant.

With either limit-load or elastic-plastic you add a load case which is beyond the capacity of the design and then let the FE solver attempt to get a solution. It will iterate a solution, gradually increasing the load until it can't get a solution. The last successfully solved load step is the plastic collapse load (strain will be a lot more than 1%).

As this is just a training exercise have a look at the ASME example problem manual (ASME PTB-3) and attempt to replicate the results.

 

[Doodler3D]

@SSCon, My bad - I meant 5.2.4.3. Thank you for the hints

 

[rb1957]

if the box has a vent, how does it plastically collapse (or explode) ? Are you saying "incase the vent doesn't function properly ..." ?

another day in paradise, or is paradise one day closer ?

 

[Doodler3D]

@rb1957

The vent sizing was done correctly, but the customer requested last min addons after the dwgs were signed off and metal was cut. So they decided to do an FEA check and accommodate the modifications. I was not a part of the organization at that time, but it was interesting to go through the goofy stuff in the FEA report as a training exercise - like, they refer to 2004 ASME code numbers instead of 2013.

 

[TGS4]

rb1957 - the approach is to determine the load at which actual plastic collapse will occur, then apply a design margin from there. There is no intent to actually cause a collapse - think of it like a virtual test to failure.

 

[inline6]

i favour looking at the load vs displacent curve to determine actual collapse. failure to converge might be numerical issue due to solver settings not actual collapse even if there is quite a bit of plasticity may not have reeached its limit.

 

[Doodler3D]

Thank you all, for your advice!

 

[dik]

makes sense... on plastic failure, stiffness approaches 0... FEM should work if you can input a stress-strain curve that shows strain hardening... if elastic-perfectly plastic... then program may not address it.

Rather than think climate change and the corona virus as science, think of it as the wrath of God. Feel any better?

-Dik